Comsol Structural Mechanics Module User's guide

Structural Mechanics Module
User’s Guide
Structural Mechanics Module User’s Guide
© 1998–2023 COMSOL
Protected by patents listed on www.comsol.com/patents, or see Help>About COMSOL Multiphysics on the
File menu in the COMSOL Desktop for less detailed lists of U.S. Patents that may apply. Patents pending.
This Documentation and the Programs described herein are furnished under the COMSOL Software License
Agreement (www.comsol.com/sla) and may be used or copied only under the terms of the license
agreement.
COMSOL, the COMSOL logo, COMSOL Multiphysics, COMSOL Desktop, COMSOL Compiler,
COMSOL Server, and LiveLink are either registered trademarks or trademarks of COMSOL AB. All other
trademarks are the property of their respective owners, and COMSOL AB and its subsidiaries and products
are not affiliated with, endorsed by, sponsored by, or supported by those trademark owners. For a list of such
trademark owners, see www.comsol.com/trademarks.
Version: COMSOL 6.2
Contact Information
Visit the Contact COMSOL page at www.comsol.com/contact to submit general inquiries
or search for an address and phone number. You can also visit the Worldwide Sales Offices
page at www.comsol.com/contact/offices for address and contact information.
If you need to contact Support, an online request form is located on the COMSOL Access
page at www.comsol.com/support/case. Other useful links include:
• Support Center: www.comsol.com/support
• Product Download: www.comsol.com/product-download
• Product Updates: www.comsol.com/product-update
• COMSOL Blog: www.comsol.com/blogs
• Discussion Forum: www.comsol.com/forum
• Events: www.comsol.com/events
• COMSOL Video Gallery: www.comsol.com/videos
• Support Knowledge Base: www.comsol.com/support/knowledgebase
Part number: CM021101
C o n t e n t s
Chapter 1: Introduction
About the Structural Mechanics Module
34
A Quick Overview of the Structural Mechanics Module . . . . . . . . 34
What Problems Can It Solve? . . . . . . . . . . . . . . . . . . 35
The Structural Mechanics Module Physics Interface Guide . . . . . . . 38
Common Physics Interface and Feature Settings and Nodes
. . . . . . 49
Where Do I Access the Documentation and Application Libraries? . . . . 49
Overview of the User’s Guide
53
Chapter 2: Structural Mechanics Modeling
Study Types
61
Introduction
. . . . . . . . . . . . . . . . . . . . . . . . 61
Stationary Analysis . . . . . . . . . . . . . . . . . . . . . . 61
Eigenfrequency Analysis . . . . . . . . . . . . . . . . . . . . 63
Mode Analysis . . . . . . . . . . . . . . . . . . . . . . . . 68
Time-Domain Analysis . . . . . . . . . . . . . . . . . . . . . 69
Frequency-Domain Analysis . . . . . . . . . . . . . . . . . . . 70
Mode Superposition. . . . . . . . . . . . . . . . . . . . . . 73
Harmonic Perturbation . . . . . . . . . . . . . . . . . . . . 75
Modal Reduced-Order Models. . . . . . . . . . . . . . . . . . 78
Linearized Buckling Analysis. . . . . . . . . . . . . . . . . . . 83
Bolt Pretension Study . . . . . . . . . . . . . . . . . . . . . 84
Random Vibration (PSD) Study . . . . . . . . . . . . . . . . . 84
Response Spectrum Analysis Study . . . . . . . . . . . . . . . . 85
Selecting the Physics Interface
87
Solid Mechanics . . . . . . . . . . . . . . . . . . . . . . . 87
Elastic Waves, Time Explicit. . . . . . . . . . . . . . . . . . . 90
Shell and Plate . . . . . . . . . . . . . . . . . . . . . . . . 91
CONTENTS | 3
Membrane . . . . . . . . . . . . . . . . . . . . . . . . . 92
Beam . . . . . . . . . . . . . . . . . . . . . . . . . . . 92
Pipe Mechanics
. . . . . . . . . . . . . . . . . . . . . . . 93
Truss . . . . . . . . . . . . . . . . . . . . . . . . . . . 93
Wire . . . . . . . . . . . . . . . . . . . . . . . . . . . 94
Selecting Discretization
95
Shape Function Order . . . . . . . . . . . . . . . . . . . . . 95
Lagrange and Serendipity Shape Functions . . . . . . . . . . . . . 96
Choosing Shape Functions in Multiphysics Models . . . . . . . . . . 96
Implicit Shape Function Orders . . . . . . . . . . . . . . . . . 97
Coupling Different Element Types
99
Introduction to the Element Types . . . . . . . . . . . . . . . . 99
Coupling Techniques . . . . . . . . . . . . . . . . . . . . . 99
4 | CONTENTS
Applying Loads
108
Units, Orientation, and Visualization . . . . . . . . . . . . . .
108
Load Cases . . . . . . . . . . . . . . . . . . . . . . . .
110
Singular Loads . . . . . . . . . . . . . . . . . . . . . . .
112
Moments in the Solid Mechanics Interface . . . . . . . . . . . .
114
Pressure . . . . . . . . . . . . . . . . . . . . . . . . .
114
Acceleration Loads . . . . . . . . . . . . . . . . . . . . .
114
Temperature Loads — Thermal Expansion . . . . . . . . . . . .
115
Hygroscopic Swelling . . . . . . . . . . . . . . . . . . . .
115
Total Loads . . . . . . . . . . . . . . . . . . . . . . . .
116
Loads with a Spatial Variation . . . . . . . . . . . . . . . . .
116
Variables for Loads . . . . . . . . . . . . . . . . . . . . .
117
Defining Constraints
119
Rigid Body Motion . . . . . . . . . . . . . . . . . . . . .
119
Orientation . . . . . . . . . . . . . . . . . . . . . . . .
120
Prescribed Displacements, Velocities, and Accelerations . . . . . . .
121
Symmetry Constraints . . . . . . . . . . . . . . . . . . . .
122
Elemental and Nodal Constraints. . . . . . . . . . . . . . . .
125
Suppressing Constraints on Lower Dimensions . . . . . . . . . .
126
Kinematic Constraints . . . . . . . . . . . . . . . . . . . .
128
Rotational Joints . . . . . . . . . . . . . . . . . . . . . .
128
Attachments . . . . . . . . . . . . . . . . . . . . . . .
128
Calculating Reaction Forces
131
Using Predefined Variables to Evaluate Reaction Forces . . . . . . .
131
Using Weak Constraints to Evaluate Reaction Forces . . . . . . . .
133
Using Surface Traction to Evaluate Reaction Forces. . . . . . . . .
134
Evaluating Surface Traction Forces on Interior Boundaries . . . . . .
134
Introduction to Material Models
136
Material Models for Structural Mechanics
. . . . . . . . . . . .
136
Combination of Material Models . . . . . . . . . . . . . . . .
138
Entering Material Data . . . . . . . . . . . . . . . . . . . .
138
Introduction to Linear Elastic Materials . . . . . . . . . . . . .
139
Introduction to Viscoelastic Materials . . . . . . . . . . . . . .
139
Mixed Formulation . . . . . . . . . . . . . . . . . . . . .
140
Modeling Damage . . . . . . . . . . . . . . . . . . . . .
142
About the Material Databases for the Structural Mechanics Module
. .
143
Using External Materials . . . . . . . . . . . . . . . . . . .
144
References . . . . . . . . . . . . . . . . . . . . . . . .
157
Modeling Piezoelectric Problems
158
About Piezoelectric Materials . . . . . . . . . . . . . . . . .
158
Piezoelectric Material Orientation . . . . . . . . . . . . . . .
159
Piezoelectric Losses. . . . . . . . . . . . . . . . . . . . .
167
References for Piezoelectric Damping . . . . . . . . . . . . . .
174
Piezoelectric Coupling . . . . . . . . . . . . . . . . . . . .
175
Create the Piezoelectricity Interface and Define Domains . . . . . .
176
Complete Settings of Piezoelectric Materials . . . . . . . . . . .
177
Add Damping and Loss . . . . . . . . . . . . . . . . . . .
178
Define Material Properties . . . . . . . . . . . . . . . . . .
178
Coupling Piezoelectricity with Acoustics . . . . . . . . . . . . .
180
Modeling Electrostrictive and Ferroelectroelastic Materials
181
Electrostriction Coupling . . . . . . . . . . . . . . . . . . .
181
Ferroelectricity . . . . . . . . . . . . . . . . . . . . . .
181
Multiphysics Interfaces . . . . . . . . . . . . . . . . . . . .
181
CONTENTS | 5
Modeling Magnetostrictive Materials
183
Magnetostriction Coupling . . . . . . . . . . . . . . . . . .
183
Linear vs. Nonlinear Magnetostriction . . . . . . . . . . . . . .
183
Create the Magnetostriction Interface and Define Domains. . . . . .
184
Mechanical Damping and Losses
188
Damping Sources. . . . . . . . . . . . . . . . . . . . . .
188
About Damping . . . . . . . . . . . . . . . . . . . . . .
189
Rayleigh Damping
. . . . . . . . . . . . . . . . . . . . .
191
Loss Factor Damping . . . . . . . . . . . . . . . . . . . .
193
Viscous Damping . . . . . . . . . . . . . . . . . . . . . .
194
Equivalence Between Loss Factor, Rayleigh, and Viscous Damping . . .
194
Explicit Complex-Valued Damping . . . . . . . . . . . . . . .
195
Viscoelastic Damping . . . . . . . . . . . . . . . . . . . .
195
Piezoelectric Damping . . . . . . . . . . . . . . . . . . . .
195
Adding Damping in the Modal Solver . . . . . . . . . . . . . .
196
Modeling Geometric Nonlinearity
197
Geometric Nonlinearity, Frames, and the ALE Method . . . . . . .
197
Geometric Nonlinearity for the Solid Mechanics Interface . . . . . .
205
Geometric Nonlinearity for the Shell, Plate, Membrane, Beam, and
Truss Interfaces . . . . . . . . . . . . . . . . . . . . .
6 | CONTENTS
206
Solving Geometrically Nonlinear Problems . . . . . . . . . . . .
207
Prestressed Structures. . . . . . . . . . . . . . . . . . . .
207
Geometric Nonlinearity for the Piezoelectric Material. . . . . . . .
210
References . . . . . . . . . . . . . . . . . . . . . . . .
213
Contact Modeling
214
Overview. . . . . . . . . . . . . . . . . . . . . . . . .
214
Setting Up a Contact Problem . . . . . . . . . . . . . . . . .
215
Contact Pairs . . . . . . . . . . . . . . . . . . . . . . .
224
Meshing for Contact Analysis . . . . . . . . . . . . . . . . .
226
Settings for Contact Nodes . . . . . . . . . . . . . . . . . .
227
Quasistatic Contact Analysis . . . . . . . . . . . . . . . . .
237
Dynamic Contact Analysis . . . . . . . . . . . . . . . . . .
238
Multiphysics Contact Analysis . . . . . . . . . . . . . . . . .
239
Special Types of Contact Problems . . . . . . . . . . . . . . .
241
Fallback Conditions to Contact Regions . . . . . . . . . . . . .
242
Solver Settings for Contact Analysis. . . . . . . . . . . . . . .
243
Monitoring the Solution . . . . . . . . . . . . . . . . . . .
247
Dependent Variables in Contact Analysis. . . . . . . . . . . . .
248
Important Contact Variables . . . . . . . . . . . . . . . . .
251
References for Contact Modeling
253
. . . . . . . . . . . . . . .
Activating and Deactivating Material
254
Springs and Dampers
257
Defining Multiphysics Models
259
Thermal-Structure Interaction . . . . . . . . . . . . . . . . .
259
Acoustic–Structure Interaction . . . . . . . . . . . . . . . .
260
Thermal–Electric–Structural Interaction . . . . . . . . . . . . .
260
Thermally Coupled Problems
262
Temperature-Dependent Material Data . . . . . . . . . . . . .
262
Thermal Expansion . . . . . . . . . . . . . . . . . . . . .
264
Constraints and Thermal Expansion. . . . . . . . . . . . . . .
270
Thermoelastic Damping . . . . . . . . . . . . . . . . . . .
271
Fluid–Structure Interaction
273
Deforming Fluid Domains . . . . . . . . . . . . . . . . . .
273
Union or Assembly . . . . . . . . . . . . . . . . . . . . .
274
Contact and FSI . . . . . . . . . . . . . . . . . . . . . .
275
One-Way FSI . . . . . . . . . . . . . . . . . . . . . . .
276
Component Mode Synthesis
278
Introduction
. . . . . . . . . . . . . . . . . . . . . . .
278
COMSOL Implementation . . . . . . . . . . . . . . . . . .
278
Applications. . . . . . . . . . . . . . . . . . . . . . . .
279
Working with CMS Models . . . . . . . . . . . . . . . . . .
280
Computing Mass Properties
292
Effective Properties of Periodic Structures
295
Material Homogenization Using the Cell Periodicity Node . . . . . .
295
CONTENTS | 7
8 | CONTENTS
Modeling Pretensioned Bolts
298
Simplified Modeling of Bolt Threads
307
Modeling Embedded Structures and Reinforcements
309
Modeling Thin Layers
314
The Thin Layer Node . . . . . . . . . . . . . . . . . . . .
314
Interior and Exterior Boundaries . . . . . . . . . . . . . . . .
316
Material Models . . . . . . . . . . . . . . . . . . . . . .
317
Loads and Boundary Conditions . . . . . . . . . . . . . . . .
317
Result Evaluation and Visualization . . . . . . . . . . . . . . .
318
Modeling Cracks
320
The Crack Node . . . . . . . . . . . . . . . . . . . . . .
320
J-integrals. . . . . . . . . . . . . . . . . . . . . . . . .
321
Virtual Crack Extension Method . . . . . . . . . . . . . . . .
324
Stress Intensity Factors . . . . . . . . . . . . . . . . . . .
325
Contact Between Crack Faces . . . . . . . . . . . . . . . . .
326
Buckling Analysis
328
Linearized Buckling Analysis. . . . . . . . . . . . . . . . . .
328
Nonlinear Buckling Analysis . . . . . . . . . . . . . . . . . .
332
Modeling Imperfection in a Buckling Analysis . . . . . . . . . . .
332
Performing a Random Vibration Analysis
337
Performing a Response Spectrum Analysis
345
Stress Linearization
353
Evaluating Stresses in Welds
359
Solver Settings for Structural Mechanics
362
Symmetric Matrices . . . . . . . . . . . . . . . . . . . . .
362
Selecting Iterative Solvers . . . . . . . . . . . . . . . . . .
363
Solver Settings for Viscoelasticity, Creep, and Viscoplasticity . . . . .
364
Specifying Tolerances and Scaling for the Dependent Variables . . . .
365
Solver Settings . . . . . . . . . . . . . . . . . . . . . . .
365
Using Reduced Integration
367
Result Presentation
371
Local Orientations . . . . . . . . . . . . . . . . . . . . .
371
How an Expression Is Evaluated . . . . . . . . . . . . . . . .
374
Quality Settings . . . . . . . . . . . . . . . . . . . . . .
376
Gauss Point Evaluation. . . . . . . . . . . . . . . . . . . .
377
Postprocessing of Eigenmodes . . . . . . . . . . . . . . . . .
379
Plotting Applied Loads . . . . . . . . . . . . . . . . . . . .
381
Part Libraries
386
Parameter Estimation
389
Chapter 3: Structural Mechanics Theory
Solid Mechanics Theory
395
Introduction
395
. . . . . . . . . . . . . . . . . . . . . . .
Frames and Coordinate Systems
397
Material and Spatial Coordinates . . . . . . . . . . . . . . . .
397
Coordinate Systems. . . . . . . . . . . . . . . . . . . . .
398
Boundary System . . . . . . . . . . . . . . . . . . . . . .
399
Analysis of Deformation
400
Lagrangian Formulation . . . . . . . . . . . . . . . . . . .
400
Deformation Measures . . . . . . . . . . . . . . . . . . .
403
Invariants of Strain . . . . . . . . . . . . . . . . . . . . .
407
Inelastic Strain Contributions . . . . . . . . . . . . . . . . .
410
Deformed Geometry . . . . . . . . . . . . . . . . . . . .
414
Axial Symmetry . . . . . . . . . . . . . . . . . . . . . .
416
Plane Strain . . . . . . . . . . . . . . . . . . . . . . . .
419
Generalized Plane Strain . . . . . . . . . . . . . . . . . . .
420
CONTENTS | 9
Stresses
425
Invariants of the Stress Tensor
426
. . . . . . . . . . . . . . . .
Plane Stress . . . . . . . . . . . . . . . . . . . . . . . .
429
Initial Stresses and Strains . . . . . . . . . . . . . . . . . .
430
External Stress. . . . . . . . . . . . . . . . . . . . . . .
431
External Strain . . . . . . . . . . . . . . . . . . . . . . .
433
Axial Symmetry and Stresses . . . . . . . . . . . . . . . . .
434
Equation of Motion
435
Material Models
438
Linear Elastic Material . . . . . . . . . . . . . . . . . . . .
441
Mixed Formulation . . . . . . . . . . . . . . . . . . . . .
454
Nonlinear Elastic Materials . . . . . . . . . . . . . . . . . .
456
Linear Viscoelasticity . . . . . . . . . . . . . . . . . . . .
468
Large Strain Viscoelasticity . . . . . . . . . . . . . . . . . .
499
Hyperelastic Materials . . . . . . . . . . . . . . . . . . . .
501
Distributed Fiber Models . . . . . . . . . . . . . . . . . . .
530
Elastoplastic Materials . . . . . . . . . . . . . . . . . . . .
535
Failure Criteria for Concrete and Rocks . . . . . . . . . . . . .
575
Damage Models . . . . . . . . . . . . . . . . . . . . . .
582
Coupled Damage–Plasticity . . . . . . . . . . . . . . . . . .
592
Elastoplastic Soil Models . . . . . . . . . . . . . . . . . . .
603
Creep and Viscoplasticity. . . . . . . . . . . . . . . . . . .
621
Inelastic Strain Rate . . . . . . . . . . . . . . . . . . . . .
645
Shape Memory Alloy . . . . . . . . . . . . . . . . . . . .
647
Piezoelectricity
10 | C O N T E N T S
425
Defining Stress. . . . . . . . . . . . . . . . . . . . . . .
. . . . . . . . . . . . . . . . . . . . . .
655
Magnetomechanics . . . . . . . . . . . . . . . . . . . . .
665
Magnetostriction and Piezomagnetism . . . . . . . . . . . . . .
669
Electrostriction . . . . . . . . . . . . . . . . . . . . . .
681
Ferroelectroelasticity . . . . . . . . . . . . . . . . . . . .
683
Rigid Material . . . . . . . . . . . . . . . . . . . . . . .
686
Safety Factor Evaluation . . . . . . . . . . . . . . . . . . .
696
Formulation of the Equilibrium Equations
716
Equation Implementation . . . . . . . . . . . . . . . . . . .
716
Study Types
718
Frequency-Domain Studies . . . . . . . . . . . . . . . . . .
718
Eigenfrequency Studies
. . . . . . . . . . . . . . . . . . .
722
Random Vibration Theory . . . . . . . . . . . . . . . . . .
725
Response Spectrum Analysis Theory . . . . . . . . . . . . . .
732
Linear Buckling
750
. . . . . . . . . . . . . . . . . . . . . .
Damping
Rayleigh Damping
752
. . . . . . . . . . . . . . . . . . . . .
752
Loss Factor Damping . . . . . . . . . . . . . . . . . . . .
753
Viscous Damping . . . . . . . . . . . . . . . . . . . . . .
754
Maximum Loss Factor . . . . . . . . . . . . . . . . . . . .
755
Wave Attenuation . . . . . . . . . . . . . . . . . . . . .
756
Loads and Constraints
760
Distributed Loads . . . . . . . . . . . . . . . . . . . . .
760
Gravity and Base Excitation . . . . . . . . . . . . . . . . . .
761
Frame Acceleration Forces . . . . . . . . . . . . . . . . . .
762
Spring Foundation and Thin Elastic Layer . . . . . . . . . . . . .
764
Spring-Damper Theory . . . . . . . . . . . . . . . . . . .
768
Added Mass . . . . . . . . . . . . . . . . . . . . . . . .
773
Rigid Motion Suppression
774
. . . . . . . . . . . . . . . . . .
Inertia Relief . . . . . . . . . . . . . . . . . . . . . . .
775
Limited Displacement . . . . . . . . . . . . . . . . . . . .
777
Low-Reflecting Boundary Condition
. . . . . . . . . . . . . .
778
Cyclic Symmetry and Floquet Periodic Conditions . . . . . . . . .
779
Symmetry Condition with Translation . . . . . . . . . . . . . .
780
Roller Boundary Condition . . . . . . . . . . . . . . . . . .
781
Thermal Expansion of Constraints . . . . . . . . . . . . . . .
783
Fluid–Structure Interaction . . . . . . . . . . . . . . . . . .
785
Cell Periodicity . . . . . . . . . . . . . . . . . . . . . .
787
Rigid Connector . . . . . . . . . . . . . . . . . . . . . .
791
Continuity Condition . . . . . . . . . . . . . . . . . . . .
794
Contact Analysis Theory
798
Contact Search and Kinematics . . . . . . . . . . . . . . . .
798
Definition of Contact Tractions . . . . . . . . . . . . . . . .
802
Normal Contact . . . . . . . . . . . . . . . . . . . . . .
802
C O N T E N T S | 11
Tangential Contact with Friction . . . . . . . . . . . . . . . .
809
Unbiased Formulation and Self-Contact . . . . . . . . . . . . .
814
Adhesion . . . . . . . . . . . . . . . . . . . . . . . . .
815
Decohesion . . . . . . . . . . . . . . . . . . . . . . . .
817
Wear . . . . . . . . . . . . . . . . . . . . . . . . . .
828
Bolt Modeling Theory
830
Tightening Torque . . . . . . . . . . . . . . . . . . . . .
830
Stress Linearization
833
J-Integral Theory
836
Virtual Crack Extension Theory
840
Embedded Elements
843
Thin Layers
847
Deformation Gradient . . . . . . . . . . . . . . . . . . . .
847
Solid Approximation . . . . . . . . . . . . . . . . . . . .
848
Membrane Approximation . . . . . . . . . . . . . . . . . .
849
Spring Approximation . . . . . . . . . . . . . . . . . . . .
849
Material Models in Thin Layers
12 | C O N T E N T S
. . . . . . . . . . . . . . . .
850
Spring Material. . . . . . . . . . . . . . . . . . . . . . .
851
Enclosed Fluids
854
Volume Definition . . . . . . . . . . . . . . . . . . . . .
855
Symmetry Planes . . . . . . . . . . . . . . . . . . . . . .
856
Equation of State . . . . . . . . . . . . . . . . . . . . . .
857
Fluid Load . . . . . . . . . . . . . . . . . . . . . . . .
858
Reduced Integration and Hourglass Stabilization
860
Average Rotation
862
Warpage
864
Finding the Average Rotation . . . . . . . . . . . . . . . . .
864
Definition of Warping . . . . . . . . . . . . . . . . . . . .
867
Energy Quantities
868
Elastic Energy . . . . . . . . . . . . . . . . . . . . . . .
868
Kinetic Energy . . . . . . . . . . . . . . . . . . . . . . .
870
Dissipated Energy . . . . . . . . . . . . . . . . . . . . .
870
Mechanical Energy Flux . . . . . . . . . . . . . . . . . . .
871
Energy Variables . . . . . . . . . . . . . . . . . . . . . .
872
References
876
Chapter 4: Solid Mechanics
The Solid Mechanics Interface
890
Domain, Boundary, Edge, Point, and Pair Nodes for Solid Mechanics . .
900
Initial Values
. . . . . . . . . . . . . . . . . . . . . . .
906
Change Thickness . . . . . . . . . . . . . . . . . . . . .
907
Change Cross Section . . . . . . . . . . . . . . . . . . . .
907
Linear Elastic Material . . . . . . . . . . . . . . . . . . . .
908
Nonlinear Elastic Material . . . . . . . . . . . . . . . . . .
916
Elastoplastic Soil Material. . . . . . . . . . . . . . . . . . .
923
Hyperelastic Material . . . . . . . . . . . . . . . . . . . .
934
Shape Memory Alloy . . . . . . . . . . . . . . . . . . . .
946
Phase Transformation Direction . . . . . . . . . . . . . . . .
952
Piezoelectric Material . . . . . . . . . . . . . . . . . . . .
953
Piezomagnetic Material . . . . . . . . . . . . . . . . . . .
957
Magnetostrictive Material. . . . . . . . . . . . . . . . . . .
963
Viscoelasticity . . . . . . . . . . . . . . . . . . . . . . .
963
Mullins Effect . . . . . . . . . . . . . . . . . . . . . . .
970
Plasticity . . . . . . . . . . . . . . . . . . . . . . . . .
971
Set Variables . . . . . . . . . . . . . . . . . . . . . . .
979
Annealing. . . . . . . . . . . . . . . . . . . . . . . . .
981
Creep . . . . . . . . . . . . . . . . . . . . . . . . . .
982
Additional Creep . . . . . . . . . . . . . . . . . . . . . .
987
Viscoplasticity . . . . . . . . . . . . . . . . . . . . . . .
988
Polymer Viscoplasticity . . . . . . . . . . . . . . . . . . .
997
Porous Plasticity . . . . . . . . . . . . . . . . . . . . . . 1002
Soil Plasticity . . . . . . . . . . . . . . . . . . . . . . . 1007
C O N T E N T S | 13
Concrete . . . . . . . . . . . . . . . . . . . . . . . . . 1012
Rocks . . . . . . . . . . . . . . . . . . . . . . . . . . 1017
Fiber . . . . . . . . . . . . . . . . . . . . . . . . . . 1019
Thermal Expansion (Fiber) . . . . . . . . . . . . . . . . . . 1022
Thermal Expansion (for Materials) . . . . . . . . . . . . . . . 1024
Hygroscopic Swelling . . . . . . . . . . . . . . . . . . . . 1027
Intercalation Strain . . . . . . . . . . . . . . . . . . . . . 1029
Initial Stress and Strain. . . . . . . . . . . . . . . . . . . . 1030
External Stress. . . . . . . . . . . . . . . . . . . . . . . 1032
External Strain . . . . . . . . . . . . . . . . . . . . . . . 1035
Inelastic Strain Rate . . . . . . . . . . . . . . . . . . . . . 1039
Damage . . . . . . . . . . . . . . . . . . . . . . . . . 1042
Activation . . . . . . . . . . . . . . . . . . . . . . . . 1047
Safety . . . . . . . . . . . . . . . . . . . . . . . . . . 1048
Damping . . . . . . . . . . . . . . . . . . . . . . . . . 1054
Mechanical Damping . . . . . . . . . . . . . . . . . . . . 1060
Coupling Loss . . . . . . . . . . . . . . . . . . . . . . . 1062
Dielectric Loss. . . . . . . . . . . . . . . . . . . . . . . 1063
Conduction Loss (Time-Harmonic) . . . . . . . . . . . . . . . 1065
External Stress-Strain Relation. . . . . . . . . . . . . . . . . 1066
Rigid Material . . . . . . . . . . . . . . . . . . . . . . . 1069
Initial Values (Rigid Material) . . . . . . . . . . . . . . . . . 1073
Fixed Constraint (Rigid Material) . . . . . . . . . . . . . . . . 1074
Prescribed Displacement/Rotation . . . . . . . . . . . . . . . 1075
Applied Force (Rigid Material) . . . . . . . . . . . . . . . . . 1078
Location Nodes . . . . . . . . . . . . . . . . . . . . . . 1080
Applied Moment (Rigid Material) . . . . . . . . . . . . . . . . 1081
Mass and Moment of Inertia (Rigid Material) . . . . . . . . . . . 1082
Center of Mass Nodes. . . . . . . . . . . . . . . . . . . . 1084
Spring Foundation (Rigid Material) . . . . . . . . . . . . . . . 1085
Free. . . . . . . . . . . . . . . . . . . . . . . . . . . 1087
Prescribed Displacement . . . . . . . . . . . . . . . . . . . 1088
Prescribed Velocity . . . . . . . . . . . . . . . . . . . . . 1094
Prescribed Acceleration . . . . . . . . . . . . . . . . . . . 1096
Fixed Constraint . . . . . . . . . . . . . . . . . . . . . . 1098
Thermal Expansion (for Constraints) . . . . . . . . . . . . . . 1101
Roller . . . . . . . . . . . . . . . . . . . . . . . . . . 1103
Symmetry . . . . . . . . . . . . . . . . . . . . . . . . 1106
14 | C O N T E N T S
Symmetry Plane . . . . . . . . . . . . . . . . . . . . . . 1109
Antisymmetry . . . . . . . . . . . . . . . . . . . . . . . 1111
Rigid Motion Suppression
. . . . . . . . . . . . . . . . . . 1113
Body Load . . . . . . . . . . . . . . . . . . . . . . . . 1115
Gravity
. . . . . . . . . . . . . . . . . . . . . . . . . 1117
Base Excitation
. . . . . . . . . . . . . . . . . . . . . . 1119
Inertia Relief . . . . . . . . . . . . . . . . . . . . . . . 1120
Rotating Frame . . . . . . . . . . . . . . . . . . . . . . 1122
Linearly Accelerated Frame . . . . . . . . . . . . . . . . . . 1126
Boundary Load
. . . . . . . . . . . . . . . . . . . . . . 1127
Edge Load . . . . . . . . . . . . . . . . . . . . . . . . 1132
Point Load . . . . . . . . . . . . . . . . . . . . . . . . 1133
Point Load, Free . . . . . . . . . . . . . . . . . . . . . . 1137
Ring Load
. . . . . . . . . . . . . . . . . . . . . . . . 1139
Ring Load, Free . . . . . . . . . . . . . . . . . . . . . . 1140
Point Load (on Axis) . . . . . . . . . . . . . . . . . . . . 1142
Thin Layer . . . . . . . . . . . . . . . . . . . . . . . . 1144
Fiber (Thin Layer) . . . . . . . . . . . . . . . . . . . . . 1146
Prescribed Displacement (Thin Layer) . . . . . . . . . . . . . . 1148
Fixed Constraint (Thin Layer) . . . . . . . . . . . . . . . . . 1151
Roller (Thin Layer) . . . . . . . . . . . . . . . . . . . . . 1152
Face Load (Thin Layer)
. . . . . . . . . . . . . . . . . . . 1153
Boundary Load (Thin Layer)
. . . . . . . . . . . . . . . . . 1155
Spring Material. . . . . . . . . . . . . . . . . . . . . . . 1156
Damping (Spring Material) . . . . . . . . . . . . . . . . . . 1160
Spring Foundation . . . . . . . . . . . . . . . . . . . . . 1160
Thin Elastic Layer. . . . . . . . . . . . . . . . . . . . . . 1167
Predeformation . . . . . . . . . . . . . . . . . . . . . . 1170
Spring-Damper
. . . . . . . . . . . . . . . . . . . . . . 1171
Source Point (for Spring-Damper) . . . . . . . . . . . . . . . 1177
Destination Point (for Spring-Damper)
. . . . . . . . . . . . . 1177
Source Point Nodes. . . . . . . . . . . . . . . . . . . . . 1178
Destination Point Nodes . . . . . . . . . . . . . . . . . . . 1178
Added Mass . . . . . . . . . . . . . . . . . . . . . . . . 1178
Periodic Condition . . . . . . . . . . . . . . . . . . . . . 1181
Adiabatic Heating. . . . . . . . . . . . . . . . . . . . . . 1184
Cell Periodicity . . . . . . . . . . . . . . . . . . . . . . 1186
Boundary Pair . . . . . . . . . . . . . . . . . . . . . . . 1191
C O N T E N T S | 15
Low-Reflecting Boundary . . . . . . . . . . . . . . . . . . . 1192
Rigid Connector . . . . . . . . . . . . . . . . . . . . . . 1192
Center of Rotation Nodes . . . . . . . . . . . . . . . . . . 1203
Thermal Expansion (Rigid Connector) . . . . . . . . . . . . . . 1203
Applied Force (Rigid Connector) . . . . . . . . . . . . . . . . 1205
Applied Moment (Rigid Connector) . . . . . . . . . . . . . . . 1207
Mass and Moment of Inertia (Rigid Connector) . . . . . . . . . . 1209
Spring Foundation (Rigid Connector) . . . . . . . . . . . . . . 1210
Attachment . . . . . . . . . . . . . . . . . . . . . . . . 1213
Thermal Expansion (Attachment). . . . . . . . . . . . . . . . 1215
Reduced Flexible Components
. . . . . . . . . . . . . . . . 1216
Component Definition. . . . . . . . . . . . . . . . . . . . 1218
Fixed Joint . . . . . . . . . . . . . . . . . . . . . . . . 1219
Source Filter . . . . . . . . . . . . . . . . . . . . . . . 1220
Destination Filter. . . . . . . . . . . . . . . . . . . . . . 1221
Contact . . . . . . . . . . . . . . . . . . . . . . . . . 1221
Friction . . . . . . . . . . . . . . . . . . . . . . . . . 1234
Slip Velocity. . . . . . . . . . . . . . . . . . . . . . . . 1238
Adhesion . . . . . . . . . . . . . . . . . . . . . . . . . 1240
Decohesion . . . . . . . . . . . . . . . . . . . . . . . . 1243
Wear . . . . . . . . . . . . . . . . . . . . . . . . . . 1245
Stabilization . . . . . . . . . . . . . . . . . . . . . . . . 1248
Continuity . . . . . . . . . . . . . . . . . . . . . . . . 1250
Bolt Pretension . . . . . . . . . . . . . . . . . . . . . . 1252
Bolt Selection . . . . . . . . . . . . . . . . . . . . . . . 1255
Bolt Thread Contact . . . . . . . . . . . . . . . . . . . . 1258
Crack . . . . . . . . . . . . . . . . . . . . . . . . . . 1260
Crack Closure . . . . . . . . . . . . . . . . . . . . . . . 1262
Face Load (Crack) . . . . . . . . . . . . . . . . . . . . . 1264
J-Integral . . . . . . . . . . . . . . . . . . . . . . . . . 1265
Reverse Crack Front . . . . . . . . . . . . . . . . . . . . 1267
Virtual Crack Extension . . . . . . . . . . . . . . . . . . . 1268
Enclosed Cavity . . . . . . . . . . . . . . . . . . . . . . 1270
Prescribed Pressure (Enclosed Cavity) . . . . . . . . . . . . . . 1271
Fluid (Enclosed Cavity). . . . . . . . . . . . . . . . . . . . 1272
Port . . . . . . . . . . . . . . . . . . . . . . . . . . . 1274
Elastic Predeformation. . . . . . . . . . . . . . . . . . . . 1278
Phase . . . . . . . . . . . . . . . . . . . . . . . . . . 1280
16 | C O N T E N T S
Harmonic Perturbation . . . . . . . . . . . . . . . . . . . 1282
Stress Linearization . . . . . . . . . . . . . . . . . . . . . 1283
Section Forces . . . . . . . . . . . . . . . . . . . . . . . 1286
Test Material . . . . . . . . . . . . . . . . . . . . . . . 1290
Local System Results . . . . . . . . . . . . . . . . . . . . 1292
Average Rotation. . . . . . . . . . . . . . . . . . . . . . 1294
Warpage . . . . . . . . . . . . . . . . . . . . . . . . . 1296
Wave Speeds . . . . . . . . . . . . . . . . . . . . . . . 1298
Important Variables in the Solid Mechanics Interface . . . . . . . . 1299
Chapter 5: Shell and Plate
Modeling with Plates and Shells
Introduction
1304
. . . . . . . . . . . . . . . . . . . . . . . 1304
Dependent Variables . . . . . . . . . . . . . . . . . . . . 1305
Layered and Nonlayered Shells . . . . . . . . . . . . . . . . 1307
Working with Section Stiffness
. . . . . . . . . . . . . . . . 1309
Loads . . . . . . . . . . . . . . . . . . . . . . . . . . 1309
Theory for the Shell and Plate Interfaces
1311
General Theory for the Shell and Plate Interfaces . . . . . . . . . 1311
Theory for FSDT Laminated Shell . . . . . . . . . . . . . . . 1337
Theory for Hyperelastic Shells . . . . . . . . . . . . . . . . . 1353
Results Evaluation in a Laminate . . . . . . . . . . . . . . . . 1353
Theory for Section Stiffness . . . . . . . . . . . . . . . . . . 1354
References for the Shell Interface . . . . . . . . . . . . . . . 1355
The Shell and Plate Interfaces
1356
Domain, Boundary, Edge, Point, and Pair Nodes for the Shell and
Plate Interfaces . . . . . . . . . . . . . . . . . . . . . 1361
Initial Values
. . . . . . . . . . . . . . . . . . . . . . . 1365
Thickness and Offset . . . . . . . . . . . . . . . . . . . . 1365
Thickness Change . . . . . . . . . . . . . . . . . . . . . 1367
Linear Elastic Material . . . . . . . . . . . . . . . . . . . . 1368
Linear Elastic Material, Layered . . . . . . . . . . . . . . . . 1371
Shell Local System . . . . . . . . . . . . . . . . . . . . . 1376
C O N T E N T S | 17
Hyperelastic Material, Layered . . . . . . . . . . . . . . . . . 1377
Piezoelectric Material, Layered
. . . . . . . . . . . . . . . . 1379
Viscoelasticity . . . . . . . . . . . . . . . . . . . . . . . 1384
Plasticity . . . . . . . . . . . . . . . . . . . . . . . . . 1385
Set Variables . . . . . . . . . . . . . . . . . . . . . . . 1387
Creep . . . . . . . . . . . . . . . . . . . . . . . . . . 1387
Additional Creep . . . . . . . . . . . . . . . . . . . . . . 1389
Viscoplasticity . . . . . . . . . . . . . . . . . . . . . . . 1390
Fiber . . . . . . . . . . . . . . . . . . . . . . . . . . 1391
Thermal Expansion (Fiber) . . . . . . . . . . . . . . . . . . 1393
Thermal Expansion (for Materials) . . . . . . . . . . . . . . . 1395
Hygroscopic Swelling . . . . . . . . . . . . . . . . . . . . 1399
Initial Stress and Strain. . . . . . . . . . . . . . . . . . . . 1402
External Stress. . . . . . . . . . . . . . . . . . . . . . . 1405
External Strain . . . . . . . . . . . . . . . . . . . . . . . 1407
Inelastic Strain Rate . . . . . . . . . . . . . . . . . . . . . 1409
Damage . . . . . . . . . . . . . . . . . . . . . . . . . 1410
Mullins Effect . . . . . . . . . . . . . . . . . . . . . . . 1411
Safety . . . . . . . . . . . . . . . . . . . . . . . . . . 1412
Damping . . . . . . . . . . . . . . . . . . . . . . . . . 1413
Mechanical Damping . . . . . . . . . . . . . . . . . . . . 1415
Coupling Loss . . . . . . . . . . . . . . . . . . . . . . . 1416
Dielectric Loss. . . . . . . . . . . . . . . . . . . . . . . 1417
Section Stiffness . . . . . . . . . . . . . . . . . . . . . . 1418
Fixed Constraint . . . . . . . . . . . . . . . . . . . . . . 1421
Prescribed Displacement/Rotation . . . . . . . . . . . . . . . 1423
Thermal Expansion (for Constraints) . . . . . . . . . . . . . . 1428
Prescribed Velocity . . . . . . . . . . . . . . . . . . . . . 1429
Prescribed Acceleration . . . . . . . . . . . . . . . . . . . 1432
Pinned . . . . . . . . . . . . . . . . . . . . . . . . . . 1434
No Rotation . . . . . . . . . . . . . . . . . . . . . . . 1436
Simply Supported. . . . . . . . . . . . . . . . . . . . . . 1437
Symmetry . . . . . . . . . . . . . . . . . . . . . . . . 1438
Symmetry Plane . . . . . . . . . . . . . . . . . . . . . . 1441
Antisymmetry . . . . . . . . . . . . . . . . . . . . . . . 1443
Body Load . . . . . . . . . . . . . . . . . . . . . . . . 1444
Face Load . . . . . . . . . . . . . . . . . . . . . . . . 1446
Edge Load . . . . . . . . . . . . . . . . . . . . . . . . 1450
18 | C O N T E N T S
Point Load . . . . . . . . . . . . . . . . . . . . . . . . 1455
Point Load, Free . . . . . . . . . . . . . . . . . . . . . . 1459
Ring Load
. . . . . . . . . . . . . . . . . . . . . . . . 1461
Ring Load, Free . . . . . . . . . . . . . . . . . . . . . . 1463
Spring Foundation . . . . . . . . . . . . . . . . . . . . . 1466
Predeformation . . . . . . . . . . . . . . . . . . . . . . 1470
Added Mass . . . . . . . . . . . . . . . . . . . . . . . . 1470
Point Mass . . . . . . . . . . . . . . . . . . . . . . . . 1472
Periodic Condition . . . . . . . . . . . . . . . . . . . . . 1473
Adiabatic Heating, Layered . . . . . . . . . . . . . . . . . . 1478
Boundary to Boundary. . . . . . . . . . . . . . . . . . . . 1480
Edge to Boundary . . . . . . . . . . . . . . . . . . . . . 1482
Edge to Edge . . . . . . . . . . . . . . . . . . . . . . . 1484
Rigid Connector . . . . . . . . . . . . . . . . . . . . . . 1487
Thermal Expansion (Rigid Connector) . . . . . . . . . . . . . . 1495
Attachment . . . . . . . . . . . . . . . . . . . . . . . . 1496
Thermal Expansion (Attachment). . . . . . . . . . . . . . . . 1497
Phase . . . . . . . . . . . . . . . . . . . . . . . . . . 1498
Harmonic Perturbation . . . . . . . . . . . . . . . . . . . 1499
Chapter 6: Layered Shell
Theory for the Layered Shell Interface
1502
About Layered Shells . . . . . . . . . . . . . . . . . . . . 1502
Theory Background for the Layered Shell Interface . . . . . . . . . 1503
The Layered Shell Interface
1517
The Shell Properties and Interface Selection Sections . . . . . . . . 1521
Domain, Boundary, Edge, Point, and Pair Nodes for the Layered
Shell Interface. . . . . . . . . . . . . . . . . . . . . . 1522
Initial Values
. . . . . . . . . . . . . . . . . . . . . . . 1526
Linear Elastic Material . . . . . . . . . . . . . . . . . . . . 1527
Hyperelastic Material . . . . . . . . . . . . . . . . . . . . 1529
Piezoelectric Material . . . . . . . . . . . . . . . . . . . . 1531
Viscoelasticity . . . . . . . . . . . . . . . . . . . . . . . 1536
Mullins Effect . . . . . . . . . . . . . . . . . . . . . . . 1537
C O N T E N T S | 19
Plasticity . . . . . . . . . . . . . . . . . . . . . . . . . 1538
Set Variables . . . . . . . . . . . . . . . . . . . . . . . 1540
Creep . . . . . . . . . . . . . . . . . . . . . . . . . . 1541
Additional Creep . . . . . . . . . . . . . . . . . . . . . . 1542
Viscoplasticity . . . . . . . . . . . . . . . . . . . . . . . 1543
Thermal Expansion (for Materials) . . . . . . . . . . . . . . . 1544
Hygroscopic Swelling . . . . . . . . . . . . . . . . . . . . 1546
Initial Stress and Strain. . . . . . . . . . . . . . . . . . . . 1547
External Stress. . . . . . . . . . . . . . . . . . . . . . . 1549
External Strain . . . . . . . . . . . . . . . . . . . . . . . 1550
Inelastic Strain Rate . . . . . . . . . . . . . . . . . . . . . 1551
Damage . . . . . . . . . . . . . . . . . . . . . . . . . 1553
Activation . . . . . . . . . . . . . . . . . . . . . . . . 1554
Delamination . . . . . . . . . . . . . . . . . . . . . . . 1555
Safety . . . . . . . . . . . . . . . . . . . . . . . . . . 1558
Damping . . . . . . . . . . . . . . . . . . . . . . . . . 1560
Mechanical Damping . . . . . . . . . . . . . . . . . . . . 1561
Coupling Loss . . . . . . . . . . . . . . . . . . . . . . . 1562
Dielectric Loss. . . . . . . . . . . . . . . . . . . . . . . 1563
Rigid Material . . . . . . . . . . . . . . . . . . . . . . . 1564
Free. . . . . . . . . . . . . . . . . . . . . . . . . . . 1565
Prescribed Displacement . . . . . . . . . . . . . . . . . . . 1566
Prescribed Displacement, Interface . . . . . . . . . . . . . . . 1568
Prescribed Velocity . . . . . . . . . . . . . . . . . . . . . 1569
Prescribed Velocity, Interface . . . . . . . . . . . . . . . . . 1570
Prescribed Acceleration . . . . . . . . . . . . . . . . . . . 1571
Prescribed Acceleration, Interface . . . . . . . . . . . . . . . 1572
Fixed Constraint . . . . . . . . . . . . . . . . . . . . . . 1573
Fixed Constraint, Interface . . . . . . . . . . . . . . . . . . 1574
Thermal Expansion (for Constraints) . . . . . . . . . . . . . . 1575
Roller . . . . . . . . . . . . . . . . . . . . . . . . . . 1577
Roller, Interface . . . . . . . . . . . . . . . . . . . . . . 1578
Symmetry . . . . . . . . . . . . . . . . . . . . . . . . 1578
Antisymmetry . . . . . . . . . . . . . . . . . . . . . . . 1579
Rigid Motion Suppression
. . . . . . . . . . . . . . . . . . 1580
Body Load . . . . . . . . . . . . . . . . . . . . . . . . 1581
Face Load . . . . . . . . . . . . . . . . . . . . . . . . 1583
Rotating Frame . . . . . . . . . . . . . . . . . . . . . . 1584
20 | C O N T E N T S
Linearly Accelerated Frame . . . . . . . . . . . . . . . . . . 1585
Boundary Load
. . . . . . . . . . . . . . . . . . . . . . 1586
Edge Load . . . . . . . . . . . . . . . . . . . . . . . . 1588
Line Load. . . . . . . . . . . . . . . . . . . . . . . . . 1589
Point Load . . . . . . . . . . . . . . . . . . . . . . . . 1590
Phase . . . . . . . . . . . . . . . . . . . . . . . . . . 1591
Spring Foundation . . . . . . . . . . . . . . . . . . . . . 1592
Spring Foundation, Interface
. . . . . . . . . . . . . . . . . 1593
Thin Elastic Layer. . . . . . . . . . . . . . . . . . . . . . 1595
Thin Elastic Layer, Interface . . . . . . . . . . . . . . . . . . 1598
Predeformation . . . . . . . . . . . . . . . . . . . . . . 1599
Added Mass . . . . . . . . . . . . . . . . . . . . . . . . 1601
Added Mass, Interface . . . . . . . . . . . . . . . . . . . . 1602
Adiabatic Heating. . . . . . . . . . . . . . . . . . . . . . 1603
Rigid Connector . . . . . . . . . . . . . . . . . . . . . . 1605
Rigid Connector, Interface . . . . . . . . . . . . . . . . . . 1606
Thermal Expansion (Rigid Connector) . . . . . . . . . . . . . . 1607
Attachment . . . . . . . . . . . . . . . . . . . . . . . . 1608
Thermal Expansion (Attachment). . . . . . . . . . . . . . . . 1609
Continuity . . . . . . . . . . . . . . . . . . . . . . . . 1610
Chapter 7: Membrane
Theory for the Membrane Interface
1614
About Membranes . . . . . . . . . . . . . . . . . . . . . 1614
Theory Background for the Membrane Interface . . . . . . . . . . 1616
The Membrane Interface
1624
Boundary, Edge, Point, and Pair Nodes for the Membrane Interface. . . 1626
Linear Elastic Material . . . . . . . . . . . . . . . . . . . . 1628
Linear Elastic Material, Layered . . . . . . . . . . . . . . . . 1634
Viscoelasticity . . . . . . . . . . . . . . . . . . . . . . . 1639
Plasticity . . . . . . . . . . . . . . . . . . . . . . . . . 1640
Set Variables . . . . . . . . . . . . . . . . . . . . . . . 1641
Creep . . . . . . . . . . . . . . . . . . . . . . . . . . 1642
Additional Creep . . . . . . . . . . . . . . . . . . . . . . 1643
C O N T E N T S | 21
Viscoplasticity . . . . . . . . . . . . . . . . . . . . . . . 1645
Wrinkling
. . . . . . . . . . . . . . . . . . . . . . . . 1646
Fiber . . . . . . . . . . . . . . . . . . . . . . . . . . 1647
Thermal Expansion (for Materials) . . . . . . . . . . . . . . . 1650
Hygroscopic Swelling . . . . . . . . . . . . . . . . . . . . 1652
Initial Stress and Strain. . . . . . . . . . . . . . . . . . . . 1654
External Stress. . . . . . . . . . . . . . . . . . . . . . . 1656
Inelastic Strain Rate . . . . . . . . . . . . . . . . . . . . . 1658
Safety . . . . . . . . . . . . . . . . . . . . . . . . . . 1659
Damping . . . . . . . . . . . . . . . . . . . . . . . . . 1660
Symmetry . . . . . . . . . . . . . . . . . . . . . . . . 1662
Antisymmetry . . . . . . . . . . . . . . . . . . . . . . . 1664
Adiabatic Heating, Layered . . . . . . . . . . . . . . . . . . 1665
Chapter 8: Beam
Modeling with Beams
1670
About Beams . . . . . . . . . . . . . . . . . . . . . . . 1670
In-Plane Beams
. . . . . . . . . . . . . . . . . . . . . . 1670
3D Beam . . . . . . . . . . . . . . . . . . . . . . . . . 1671
Orientation of the Cross Section. . . . . . . . . . . . . . . . 1672
Geometric Variables . . . . . . . . . . . . . . . . . . . . 1673
Result Evaluation . . . . . . . . . . . . . . . . . . . . . . 1674
Geometric Nonlinearity . . . . . . . . . . . . . . . . . . . 1676
Modeling Stiffeners . . . . . . . . . . . . . . . . . . . . . 1677
Nonrigid Joints
. . . . . . . . . . . . . . . . . . . . . . 1678
Theory for the Beam Interface
1682
Shape Functions . . . . . . . . . . . . . . . . . . . . . . 1682
Geometric Nonlinearity . . . . . . . . . . . . . . . . . . . 1684
Strain-Displacement/Rotation Relation. . . . . . . . . . . . . . 1687
Stress-Strain Relation . . . . . . . . . . . . . . . . . . . . 1687
Thermal Strain . . . . . . . . . . . . . . . . . . . . . . . 1688
Hygroscopic Swelling . . . . . . . . . . . . . . . . . . . . 1688
Initial Load and Strain . . . . . . . . . . . . . . . . . . . . 1689
Implementation . . . . . . . . . . . . . . . . . . . . . . 1690
22 | C O N T E N T S
Theory for Section Stiffness . . . . . . . . . . . . . . . . . . 1692
Stress Evaluation . . . . . . . . . . . . . . . . . . . . . . 1694
Common Cross Sections . . . . . . . . . . . . . . . . . . . 1696
The Beam Interface
Boundary, Edge, Point, and Pair Nodes for the Beam Interface
Initial Values
1713
. . . . 1716
. . . . . . . . . . . . . . . . . . . . . . . 1718
Cross-Section Data . . . . . . . . . . . . . . . . . . . . . 1719
Section Orientation . . . . . . . . . . . . . . . . . . . . . 1724
Linear Elastic Material . . . . . . . . . . . . . . . . . . . . 1726
Thermal Expansion (for Materials) . . . . . . . . . . . . . . . 1728
Hygroscopic Swelling . . . . . . . . . . . . . . . . . . . . 1729
Initial Stress and Strain. . . . . . . . . . . . . . . . . . . . 1731
External Stress. . . . . . . . . . . . . . . . . . . . . . . 1732
Section Stiffness . . . . . . . . . . . . . . . . . . . . . . 1733
Prescribed Displacement/Rotation . . . . . . . . . . . . . . . 1736
Prescribed Velocity . . . . . . . . . . . . . . . . . . . . . 1739
Prescribed Acceleration . . . . . . . . . . . . . . . . . . . 1741
Pinned . . . . . . . . . . . . . . . . . . . . . . . . . . 1743
Thermal Expansion (for Constraints) . . . . . . . . . . . . . . 1744
No Rotation . . . . . . . . . . . . . . . . . . . . . . . 1746
Symmetry . . . . . . . . . . . . . . . . . . . . . . . . 1746
Antisymmetry . . . . . . . . . . . . . . . . . . . . . . . 1749
Edge Load . . . . . . . . . . . . . . . . . . . . . . . . 1750
Point Load . . . . . . . . . . . . . . . . . . . . . . . . 1753
Point Load, Free . . . . . . . . . . . . . . . . . . . . . . 1754
Point Mass . . . . . . . . . . . . . . . . . . . . . . . . 1756
Rigid Connector . . . . . . . . . . . . . . . . . . . . . . 1757
Attachment . . . . . . . . . . . . . . . . . . . . . . . . 1763
Beam End Release . . . . . . . . . . . . . . . . . . . . . 1764
Edge Group . . . . . . . . . . . . . . . . . . . . . . . . 1765
Phase . . . . . . . . . . . . . . . . . . . . . . . . . . 1766
Harmonic Perturbation . . . . . . . . . . . . . . . . . . . 1767
C O N T E N T S | 23
Chapter 9: Beam Cross Section
Using the Beam Cross Section Interface
1770
About Beams and Cross-Section Data . . . . . . . . . . . . . . 1770
Using the Beam Cross Section Interface . . . . . . . . . . . . . 1771
Theory for the Beam Cross Section Interface
1777
Cross-Section Properties. . . . . . . . . . . . . . . . . . . 1777
Computation of Stresses . . . . . . . . . . . . . . . . . . . 1791
The Beam Cross Section Interface
1794
Homogeneous Cross Section . . . . . . . . . . . . . . . . . 1795
Hole . . . . . . . . . . . . . . . . . . . . . . . . . . 1797
Safety . . . . . . . . . . . . . . . . . . . . . . . . . . 1799
Chapter 10: Truss
Modeling with Truss Elements
1802
Theory for the Truss Interface
1804
Theory Background for the Truss Interface . . . . . . . . . . . . 1804
The Truss Interface
Boundary, Edge, Point, and Pair Nodes for the Truss Interface
1813
. . . . 1814
Cross-Section Data . . . . . . . . . . . . . . . . . . . . . 1816
Straight Edge Constraint . . . . . . . . . . . . . . . . . . . 1819
Linear Elastic Material . . . . . . . . . . . . . . . . . . . . 1820
Set Variables . . . . . . . . . . . . . . . . . . . . . . . 1823
Thermal Expansion (for Linear Elastic Material) . . . . . . . . . . 1823
Thermal Expansion (for Shape Memory Alloy) . . . . . . . . . . . 1825
Hygroscopic Swelling . . . . . . . . . . . . . . . . . . . . 1826
Initial Stress and Strain. . . . . . . . . . . . . . . . . . . . 1827
External Stress. . . . . . . . . . . . . . . . . . . . . . . 1827
Spring-Damper Material . . . . . . . . . . . . . . . . . . . 1829
Pinned . . . . . . . . . . . . . . . . . . . . . . . . . . 1830
24 | C O N T E N T S
Thermal Expansion (for Constraints) . . . . . . . . . . . . . . 1831
Symmetry . . . . . . . . . . . . . . . . . . . . . . . . 1832
Antisymmetry . . . . . . . . . . . . . . . . . . . . . . . 1834
Edge Load . . . . . . . . . . . . . . . . . . . . . . . . 1836
Point Mass . . . . . . . . . . . . . . . . . . . . . . . . 1837
Chapter 11: Wire
Modeling Wires and Cables
1840
Theory for the Wire Interface
1841
Theory Background for the Wire Interface . . . . . . . . . . . . 1841
The Wire Interface
1844
Boundary, Edge, Point, and Pair Nodes for the Wire Interface. . . . . 1845
Elastic Wire . . . . . . . . . . . . . . . . . . . . . . . . 1847
Thermal Expansion (for Elastic Wire) . . . . . . . . . . . . . . 1848
Hygroscopic Swelling . . . . . . . . . . . . . . . . . . . . 1849
Initial Stress and Strain. . . . . . . . . . . . . . . . . . . . 1850
Pinned . . . . . . . . . . . . . . . . . . . . . . . . . . 1850
Thermal Expansion (for Constraints) . . . . . . . . . . . . . . 1851
Symmetry . . . . . . . . . . . . . . . . . . . . . . . . 1853
Antisymmetry . . . . . . . . . . . . . . . . . . . . . . . 1855
Edge Load . . . . . . . . . . . . . . . . . . . . . . . . 1856
Chapter 12: Pipe Mechanics
Theory for the Pipe Mechanics Interface
1860
About Pipes . . . . . . . . . . . . . . . . . . . . . . . . 1860
Effects of Internal Pressure . . . . . . . . . . . . . . . . . . 1861
Fluid Flow Forces. . . . . . . . . . . . . . . . . . . . . . 1865
Effects of Thermal Expansion . . . . . . . . . . . . . . . . . 1867
Stress Evaluation . . . . . . . . . . . . . . . . . . . . . . 1869
Connection Between Pipes and Structures . . . . . . . . . . . . 1874
Cross Sections. . . . . . . . . . . . . . . . . . . . . . . 1876
C O N T E N T S | 25
The Pipe Mechanics Interface
1881
Boundary, Edge, Point, and Pair Nodes for the Pipe Mechanics
Interface. . . . . . . . . . . . . . . . . . . . . . . . 1884
Pipe Cross Section . . . . . . . . . . . . . . . . . . . . . 1885
Section Orientation . . . . . . . . . . . . . . . . . . . . . 1889
Bend . . . . . . . . . . . . . . . . . . . . . . . . . . 1892
Fluid and Pipe Materials . . . . . . . . . . . . . . . . . . . 1894
Rigid Material . . . . . . . . . . . . . . . . . . . . . . . 1896
Thermal Expansion (for Materials) . . . . . . . . . . . . . . . 1898
Gravity
. . . . . . . . . . . . . . . . . . . . . . . . . 1900
Base Excitation
. . . . . . . . . . . . . . . . . . . . . . 1901
Linearly Accelerated Frame . . . . . . . . . . . . . . . . . . 1902
Fluid Load . . . . . . . . . . . . . . . . . . . . . . . . 1904
Chapter 13: Phase Field in Solids
Modeling with the Phase Field in Solids Interface
Introduction
1908
. . . . . . . . . . . . . . . . . . . . . . . 1908
Dependent Variables . . . . . . . . . . . . . . . . . . . . 1908
Phase Field Damage Modeling . . . . . . . . . . . . . . . . . 1909
Theory for the Phase Field in Solids Interface
1910
References . . . . . . . . . . . . . . . . . . . . . . . . 1912
The Phase Field in Solids Interface
1913
Domain and Boundary Nodes for the Phase Field in Solids Interface . . 1914
Phase Field Model . . . . . . . . . . . . . . . . . . . . . 1915
Bounds
. . . . . . . . . . . . . . . . . . . . . . . . . 1916
Prescribed Phase Field . . . . . . . . . . . . . . . . . . . . 1917
Source
. . . . . . . . . . . . . . . . . . . . . . . . . 1918
Initial Values
. . . . . . . . . . . . . . . . . . . . . . . 1918
No Flux . . . . . . . . . . . . . . . . . . . . . . . . . 1919
Symmetry . . . . . . . . . . . . . . . . . . . . . . . . 1919
26 | C O N T E N T S
Chapter 14: Transport in Solids
Modeling with the Transport in Solids Interface
Introduction
1922
. . . . . . . . . . . . . . . . . . . . . . . 1922
Dependent Variables . . . . . . . . . . . . . . . . . . . . 1922
Material and Spatial Variables . . . . . . . . . . . . . . . . . 1923
Mass Transfer Variables . . . . . . . . . . . . . . . . . . . 1924
Theory for the Transport in Solids Interface
1927
Mass Balance . . . . . . . . . . . . . . . . . . . . . . . 1927
Chemical Potential . . . . . . . . . . . . . . . . . . . . . 1928
The Transport in Solids Interface
1930
Domain and Boundary Nodes for the Transport in Solids Interface . . . 1932
Chemical Potential . . . . . . . . . . . . . . . . . . . . . 1933
External Chemical Potential . . . . . . . . . . . . . . . . . . 1935
External Flux . . . . . . . . . . . . . . . . . . . . . . . 1935
Initial Values
. . . . . . . . . . . . . . . . . . . . . . . 1936
No Flux . . . . . . . . . . . . . . . . . . . . . . . . . 1937
Prescribed Chemical Potential . . . . . . . . . . . . . . . . . 1937
Prescribed Transported Quantity
. . . . . . . . . . . . . . . 1938
Solid . . . . . . . . . . . . . . . . . . . . . . . . . . 1939
Flux . . . . . . . . . . . . . . . . . . . . . . . . . . . 1940
Source . . . . . . . . . . . . . . . . . . . . . . . . . . 1940
Symmetry . . . . . . . . . . . . . . . . . . . . . . . . 1941
C O N T E N T S | 27
Chapter 15: Multiphysics Interfaces and Couplings
The Thermal Stress, Solid Interface
1946
The Thermal Stress, Shell Interface
1948
The Thermal Stress, Layered Shell Interface
1950
The Thermal Stress, Membrane Interface
1952
The Joule Heating and Thermal Expansion Interface
1954
Overview of Fluid–Structure Interaction Interfaces
1957
The Fluid–Solid Interaction Interface
1959
The Fluid–Solid Interaction, Fixed Geometry Interface
1962
The Fluid–Shell Interaction Interface
1964
The Fluid–Shell Interaction, Fixed Geometry Interface
1966
The Fluid–Membrane Interaction Interface
1968
The Fluid–Membrane Interaction, Fixed Geometry Interface
1970
The Fluid–Pipe Interaction, Fixed Geometry Interface
1972
The Solid–Thin-Film Damping Interface
1973
The Shell–Thin-Film Damping Interface
1975
The Fluid–Solid Interaction, Viscoelastic Flow Interface
1977
The Fluid–Solid Interaction, Viscoelastic Flow, Fixed Geometry
28 | C O N T E N T S
Interface
1979
The Fluid–Solid Interaction, Conjugate Heat Transfer Interface
1981
The Fluid–Solid Interaction, Two-Phase Flow, Phase Field
Interface
1984
The Fluid–Solid Interaction, Two-Phase Flow, Phase Field,
Fixed Geometry Interface
1987
Overview of Poroelasticity Interfaces
1990
The Poroelasticity, Solid Interface
1991
The Poroelasticity, Solid Interface . . . . . . . . . . . . . . . 1991
Poroelasticity (Multiphysics Coupling) . . . . . . . . . . . . . . 1992
The Poroelasticity, Large Deformation, Solid Interface
1995
The Poroelasticity, Large Deformation, Solid Interface. . . . . . . . 1995
The Poroelasticity, Layered Shell Interface
1996
Poroelasticity, Layered (Multiphysics Coupling) . . . . . . . . . . 1998
The Unsaturated Poroelasticity Interface
2000
The Unsaturated Poroelasticity Interface . . . . . . . . . . . . . 2000
Unsaturated Poroelasticity (Multiphysics Coupling) . . . . . . . . . 2001
The Poroelasticity Interfaces . . . . . . . . . . . . . . . . . 2003
Overview of Electromagnetics–Structure Interaction Interfaces
2004
The Piezoelectricity Interface, Solid
2005
Coupling Piezoelectricity with Acoustics . . . . . . . . . . . . . 2008
C O N T E N T S | 29
The Piezoelectricity, Layered Shell Interface
2009
The Electrostriction Interface
2012
The Ferroelectroelasticity Interface
2013
The Magnetomechanics Interface
2014
The Magnetomechanics, No Currents Interface
2016
The Magnetic–Elastic Interaction in Rotating Machinery
Interface
2018
The Piezomagnetism Interface
2020
The Nonlinear Magnetostriction Interface
2023
Hygroscopic Swelling Coupling
2026
The Phase Field Damage Interface
2027
Phase Field Damage (Multiphysics Coupling) . . . . . . . . . . . 2028
Multiphysics Couplings
2032
Thermal Expansion . . . . . . . . . . . . . . . . . . . . . 2032
Thermal Expansion, Thin Layer . . . . . . . . . . . . . . . . 2035
Thermal Expansion, Layered . . . . . . . . . . . . . . . . . 2038
Hygroscopic Swelling . . . . . . . . . . . . . . . . . . . . 2041
Piezoelectricity
. . . . . . . . . . . . . . . . . . . . . . 2043
Piezoelectricity, Layered . . . . . . . . . . . . . . . . . . . 2045
Electrostriction . . . . . . . . . . . . . . . . . . . . . . 2046
Magnetomechanics . . . . . . . . . . . . . . . . . . . . . 2050
Magnetic Forces, Rotating Machinery . . . . . . . . . . . . . . 2053
Piezomagnetism . . . . . . . . . . . . . . . . . . . . . . 2056
Nonlinear Magnetostriction . . . . . . . . . . . . . . . . . . 2058
Magnetostriction . . . . . . . . . . . . . . . . . . . . . . 2061
Fluid–Structure Interaction . . . . . . . . . . . . . . . . . . 2061
Fluid–Structure Interaction, Pair . . . . . . . . . . . . . . . . 2063
Fluid–Structure Interaction, Fixed Geometry . . . . . . . . . . . 2065
30 | C O N T E N T S
Fluid–Pipe Interaction . . . . . . . . . . . . . . . . . . . . 2066
Structure–Thin-Film Flow Interaction . . . . . . . . . . . . . . 2068
Shell–Thin-Film Flow Interaction . . . . . . . . . . . . . . . . 2069
Couplings Between Structural Mechanics Interfaces
2071
Solid–Thin Structure Connection. . . . . . . . . . . . . . . . 2071
Solid–Beam Connection . . . . . . . . . . . . . . . . . . . 2074
Shell–Beam Connection . . . . . . . . . . . . . . . . . . . 2079
Layered Shell–Structure Transition . . . . . . . . . . . . . . . 2081
Layered Shell–Structure Cladding
. . . . . . . . . . . . . . . 2082
Layered Shell–Shell Connection . . . . . . . . . . . . . . . . 2083
Structure–Pipe Connection . . . . . . . . . . . . . . . . . . 2084
Embedded Reinforcement . . . . . . . . . . . . . . . . . . 2085
Beam Cross Section–Beam Coupling . . . . . . . . . . . . . . 2088
Beam–Beam Cross Section Coupling . . . . . . . . . . . . . . 2089
Chapter 16: Glossary
Glossary of Terms
2092
Index
2099
C O N T E N T S | 31
32 | C O N T E N T S
1
Introduction
This guide describes the Structural Mechanics Module, an optional add-on
package that extends the COMSOL Multiphysics modeling environment with
customized physics interfaces that solve problems in the fields of structural and
solid mechanics, including special physics interface for modeling of shells,
membranes, beams, plates, trusses, wires, and pipes.
This chapter introduces you to the capabilities of this module and includes a
summary of the physics interfaces as well as information about where you can find
additional documentation and model examples. The last section is a brief overview
with links to each chapter in this guide.
• About the Structural Mechanics Module
• Overview of the User’s Guide
33
About the Structural Mechanics
Module
In this section:
• A Quick Overview of the Structural Mechanics Module
• What Problems Can It Solve?
• The Structural Mechanics Module Physics Interface Guide
• Common Physics Interface and Feature Settings and Nodes
• Where Do I Access the Documentation and Application Libraries?
The Physics Interfaces and Building a COMSOL Multiphysics Model in
the COMSOL Multiphysics Reference Manual
A Quick Overview of the Structural Mechanics Module
The Structural Mechanics Module solves problems in the fields of structural and solid
mechanics, adding special physics interfaces for modeling shells and beams, for
example.
The physics interfaces in this module are fully multiphysics enabled, making it possible
to couple them to any other physics interfaces in COMSOL Multiphysics or the other
modules. Available physics interfaces include:
• Solid mechanics for 1D and 2D plane stress, plane strain, and generalized plane
strain, 2D axial symmetry, and 3D solids
• Beams in 2D and 3D, Euler and Timoshenko theory
• Pipes in 2D and 3D
• Truss elements in 2D and 3D
• Wires in 2D and 3D
• Shells and plates, Mindlin theory, 3D and 2D axial symmetry
• Membranes, 3D and 2D axial symmetry
• With the Composite Materials Module, the Layered Shell interface is also available.
34 |
CHAPTER 1: INTRODUCTION
The module’s study capabilities include static, eigenfrequency, time dependent
(transient), frequency response, buckling, response spectrum, random vibration, and
parametric studies.
There are several material models:
• Linear Elastic Materials can be isotropic, orthotropic, or fully anisotropic, and you
can use local coordinate systems to specify material properties.
• Linear Viscoelastic Materials
• Piezoelectric Materials
• Magnetostrictive Materials are available when used together with the AC/DC
module.
• Material models for hyperelasticity, metal plasticity, porous plasticity, creep,
viscoplasticity, nonlinear elasticity, soil plasticity, concrete, rocks, and clay are
available with the optional Nonlinear Structural Materials Module and
Geomechanics Module.
Large deformations, as well as contact and friction, can also be modeled.
Coupling structural analysis with thermal analysis is one example of multiphysics easily
implemented with the module, which provides predefined multiphysics couplings for
thermal stress and other types of multiphysics. Piezoelectric materials, coupling the
electric field and strain in both directions are fully supported inside the module
through special multiphysics couplings solving for both the electric potential and the
displacements. Structural mechanics couplings are common in simulations done with
COMSOL Multiphysics and occur in interaction with, for example, fluid flow (fluid–
structure interaction, FSI), chemical reactions, acoustics, electric fields, magnetic
fields, and optical wave propagation.
What Problems Can It Solve?
The Structural Mechanics Module contains a set of physics interfaces adapted to a
broad category of structural-mechanics analyses. The module serves as an excellent
tool for the professional engineer, researcher, and teacher. In education, the benefit of
the short learning curve is especially useful because educators need not spend excessive
time learning the software and can instead focus on the physics and the modeling
process.
A short summary is given below.
ABOUT THE STRUCTURAL MECHANICS MODULE
|
35
STATIC ANALYSIS
In a static analysis, the load and constraints are fixed in time.
EIGENFREQUENCY ANALYSIS
An eigenfrequency analysis finds the damped or undamped eigenfrequencies and
mode shapes of a structure, sometimes referred to as the free vibration of a structure.
Prestress effects and damping can also be taken into account.
TRANSIENT ANALYSIS
A transient analysis finds the transient response for a time-dependent model, taking
into account mass and mass moment of inertia. The transient analysis can be either
direct or using a modal solution.
FREQUENCY RESPONSE ANALYSIS
A frequency response analysis finds the steady-state response to harmonic loads. The
frequency-response analysis can be either direct or using a modal solution. Effects of
prestress can be included.
LINEAR BUCKLING STUDY
A linear buckling analysis uses the stiffness coming from stresses and material to
define an eigenvalue problem where the eigenvalue is a load factor that, when
multiplied with the actual load, gives the critical load in a linear context.
PARAMETRIC ANALYSIS
A parametric analysis finds the solution dependence due to the variation of a specific
parameter, which could be, for instance, a material property or the position of a load.
RESPONSE SPECTRUM ANALYSIS
Response spectrum analysis provides a method to estimate peak values of, for example,
displacements and stresses when a structure is subjected to a short, nondeterministic
event like an earthquake or a shock.
RANDOM VIBRATION ANALYSIS
For steady-state random dynamic loading, like wind or waves, it is possible to perform
random vibration analysis where the input is given in terms of a power spectrum
density (PSD).
36 |
CHAPTER 1: INTRODUCTION
THERMAL STRESS
In a transient thermal stress study, the program neglects mass effects, assuming that
the time scale in the structural mechanics problem is much smaller than the time scale
in the thermal problem.
LARGE DEFORMATIONS
You can also enable geometric nonlinearity for all structural mechanics interfaces. The
engineering strain is then replaced with the Green–Lagrange strain and the stress with
the second Piola–Kirchhoff stress. To solve the problem, the program uses a total
Lagrangian formulation.
ELASTOPLASTIC MATERIALS
An elastoplastic analysis involves a nonlinear material with or without hardening.
Several isotropic and kinematic hardening models are available.
The material models allow large strains.
The elastoplastic material models are available in the Solid Mechanics, Shell, Layered
Shell, Membrane, and Truss interfaces.
CREEP AND VISCOPLASTIC MATERIALS
A number of different material models for creep and viscoplasticity are available. In
these materials, the rate of strain depends on the stress.
HYPERELASTIC MATERIALS
In hyperelastic materials, the stresses are computed from a strain energy density
function. They are often used to model rubber and biological tissue, but are also used
in acoustic elasticity. Many different models are available.
The hyperelastic materials are available in the Solid Mechanics, Shell, Layered Shell,
and Membrane interfaces.
NONLINEAR ELASTIC MATERIALS
The nonlinear elastic materials are intended for materials that exhibit a nonlinear
behavior already at small strains. Some brittle material as well as soils show this
behavior.
ABOUT THE STRUCTURAL MECHANICS MODULE
|
37
VISCOELASTIC MATERIALS
Viscoelastic materials have a time-dependent response, even if the loading is constant.
Viscoelasticity is available in the Solid Mechanics, Shell, Layered Shell, and Membrane
interfaces.
• Hyperelastic, elastoplastic, creep, viscoplastic, and nonlinear elastic
material models are available with the Nonlinear Structural Materials
Module.
• Additional functionality and material models for geomechanics and soil
mechanics — nonlinear elasticity, soil plasticity, concrete, rock, and clay
material models — is available with the Geomechanics Module.
CONTACT MODELING
You can model contact between parts of a structure. The Solid Mechanics, Shell,
Layered Shell, and Membrane interfaces support contact with or without friction.
Three contact algorithms are available: penalty, augmented Lagrangian, and Nitsche
methods. The contact models can be augmented with adhesion and decohesion.
SPECIAL MODELING TECHNIQUES
In the Structural Mechanics Module, you will find support for many important special
modeling techniques. Some examples are:
• Bolt pretension
• Bolt thread modeling
• Stress linearization
• Rigid connectors
• Transitions between solid, shell, and beam elements
The Structural Mechanics Module Physics Interface Guide
The Poroelasticity interface requires and is coupled with the Structural
Mechanics Module, and is discussed in the Subsurface Flow Module
User’s Guide.
38 |
CHAPTER 1: INTRODUCTION
At any time, a new model can be created or physics interfaces added. Right-click the
Root (top) node and select Add Component or right-click a Component node and select
Add Physics.
Depending on the physics interface, specify parameters defining a problem on points,
edges (3D), boundaries, and domains. It is possible to specify loads and constraints on
all available geometry levels, but material properties can only be specified for the
domains, except for shells, membranes, beams, and trusses, where they are defined on
the boundary or edge level.
In the COMSOL Multiphysics Reference Manual:
• Studies and Solvers
• The Physics Interfaces
• For a list of all the core physics interfaces included with a COMSOL
Multiphysics license, see Physics Interface Guide.
PHYSICS INTERFACE
ICON
TAG
SPACE
DIMENSION
AVAILABLE STUDY TYPE
Elastic Waves, Time
Explicit
elte
3D, 2D, 2D
axisymmetric
time dependent
Piezoelectric Waves,
Time Explicit
—
3D, 2D, 2D
axisymmetric
time dependent
all dimensions
stationary; time dependent
Acoustics
Elastic Waves
Chemical Species Transport
Transport in Solids
ts
ABOUT THE STRUCTURAL MECHANICS MODULE
|
39
PHYSICS INTERFACE
ICON
TAG
SPACE
DIMENSION
AVAILABLE STUDY TYPE
Fluid Flow
Fluid-Structure Interaction
40 |
Fluid–Solid
Interaction2
—
3D, 2D, 2D
axisymmetric
stationary; time dependent
Fluid–Shell Interaction2
—
3D, 2D
axisymmetric
stationary; time dependent
Fluid–Shell Interaction,
Fixed Geometry
—
3D, 2D
axisymmetric
stationary; stationary, one
way; time dependent; time
dependent, one way
Fluid–Membrane
Interaction2
—
3D, 2D
axisymmetric
stationary; time dependent
Fluid–Membrane
Interaction, Fixed
Geometry2
—
3D, 2D
axisymmetric
stationary; stationary, one
way; time dependent; time
dependent, one way
Fluid–Pipe Interaction,
Fixed Geometry2,7
—
3D, 2D
stationary; time dependent
Conjugate Heat
Transfer, Fluid–Solid
Interaction2
—
3D, 2D, 2D
axisymmetric
stationary; time dependent;
Fluid–Solid Interaction,
Viscoelastic Flow2,10
—
3D, 2D, 2D
axisymmetric
time dependent; time
dependent with phase
initialization
Fluid–Solid Interaction,
Two-Phase Flow, Phase
Field2,6
—
3D, 2D, 2D
axisymmetric
time dependent; time
dependent with phase
initialization
CHAPTER 1: INTRODUCTION
PHYSICS INTERFACE
ICON
TAG
SPACE
DIMENSION
AVAILABLE STUDY TYPE
Solid–Thin-Film
Damping2
—
3D, 2D, 2D
axisymmetric
stationary; eigenfrequency;
time dependent; time
dependent, modal; time
dependent, modal
reduced-order model;
frequency domain;
frequency domain, modal;
frequency domain, modal
reduced-order model; time
dependent; response
spectrum; random
vibration (PSD)
Shell–Thin-Film
Damping2
—
3D, 2D
axisymmetric
stationary; eigenfrequency;
time dependent; time
dependent, modal; time
dependent, modal
reduced-order model;
frequency domain;
frequency domain, modal;
frequency domain, modal
reduced-order model; time
dependent; response
spectrum; random
vibration (PSD)
ABOUT THE STRUCTURAL MECHANICS MODULE
|
41
PHYSICS INTERFACE
ICON
TAG
SPACE
DIMENSION
AVAILABLE STUDY TYPE
Solid Mechanics1
solid
3D, 2D, 2D
axisymmetric,
1D, 1D
axisymmetric
stationary; eigenfrequency;
eigenfrequency,
prestressed; mode analysis;
time dependent; time
dependent, modal; time
dependent, modal
reduced-order model;
frequency domain;
frequency domain, modal;
frequency domain,
prestressed; frequency
domain, prestressed,
modal; frequency domain,
modal reduced-order
model; frequency domain,
AWE reduced-order
model; response spectrum;
random vibration (PSD);
linear buckling; bolt
pretension
Shell
shell
3D, 2D
axisymmetric
stationary; eigenfrequency;
eigenfrequency,
prestressed; time
dependent; time
dependent, modal; time
dependent, modal
reduced-order model;
frequency domain;
frequency domain, modal;
frequency domain,
prestressed; frequency
domain, prestressed,
modal; frequency domain,
modal reduced-order
model; response spectrum;
random vibration (PSD);
linear buckling
Structural Mechanics
42 |
CHAPTER 1: INTRODUCTION
PHYSICS INTERFACE
ICON
TAG
SPACE
DIMENSION
AVAILABLE STUDY TYPE
Plate
plate
2D
stationary; eigenfrequency;
eigenfrequency,
prestressed; time
dependent; time
dependent, modal; time
dependent, modal
reduced-order model;
frequency domain;
frequency domain, modal;
frequency domain,
prestressed; frequency
domain, prestressed,
modal; frequency domain,
modal reduced-order
model; response spectrum;
random vibration (PSD);
linear buckling
Beam
beam
3D, 2D
stationary; eigenfrequency;
time dependent, modal;
time dependent, modal
reduced-order model;
frequency domain;
frequency domain, modal;
frequency domain, modal
reduced-order model; time
dependent; response
spectrum; random
vibration (PSD); linear
buckling
Beam Cross Section
bcs
3D, 2D
stationary
ABOUT THE STRUCTURAL MECHANICS MODULE
|
43
PHYSICS INTERFACE
44 |
TAG
SPACE
DIMENSION
AVAILABLE STUDY TYPE
Truss
truss
3D, 2D
stationary; eigenfrequency;
eigenfrequency,
prestressed; time
dependent; time
dependent, modal; time
dependent, modal
reduced-order model;
frequency domain;
frequency domain, modal;
frequency domain,
prestressed; frequency
domain, prestressed,
modal; frequency domain,
modal reduced-order
model; response spectrum;
random vibration (PSD);
linear buckling
Wire
wire
3D, 2D
stationary; eigenfrequency;
eigenfrequency,
prestressed; time
dependent; time
dependent, modal; time
dependent, modal
reduced-order model;
frequency domain;
frequency domain, modal;
frequency domain,
prestressed; frequency
domain, prestressed,
modal; frequency domain,
modal reduced-order
model; response spectrum;
random vibration (PSD);
linear buckling
CHAPTER 1: INTRODUCTION
ICON
PHYSICS INTERFACE
ICON
TAG
SPACE
DIMENSION
AVAILABLE STUDY TYPE
Membrane
mbrn
3D, 2D
axisymmetric
stationary; eigenfrequency;
eigenfrequency,
prestressed; time
dependent; time
dependent, modal; time
dependent, modal
reduced-order model;
frequency domain;
frequency domain, modal;
frequency domain,
prestressed; frequency
domain, prestressed,
modal; frequency domain,
modal reduced-order
model; response spectrum;
random vibration (PSD)
Pipe Mechanics
pipem
3D, 2D
stationary; eigenfrequency;
time dependent, modal;
time dependent, modal
reduced-order model;
frequency domain;
frequency domain, modal;
frequency domain, modal
reduced-order model; time
dependent; response
spectrum; random
vibration (PSD)
Phase Field Damage,2,11
—
3D, 2D, 2D
axisymmetric
stationary; time dependent
Thermal–Structure Interaction
Thermal Stress, Solid2
—
3D, 2D, 2D
axisymmetric
stationary; time dependent
Thermal Stress,
Shell2,4
—
3D, 2D
axisymmetric
stationary; time dependent
Thermal Stress,
Membrane2,4
—
3D, 2D
axisymmetric
stationary; time dependent
ABOUT THE STRUCTURAL MECHANICS MODULE
|
45
PHYSICS INTERFACE
ICON
TAG
SPACE
DIMENSION
AVAILABLE STUDY TYPE
—
3D, 2D, 2D
axisymmetric
stationary; time dependent
Piezoelectricity, Solid2
—
3D, 2D, 2D
axisymmetric
stationary; eigenfrequency;
eigenfrequency,
prestressed; time
dependent; time
dependent, modal;
frequency domain;
frequency domain, modal;
frequency domain,
prestressed; frequency
domain, prestressed,
modal; small-signal analysis,
frequency domain; linear
buckling
Piezoelectricity,
Layered Shell2,5
—
3D
stationary; eigenfrequency;
time dependent; frequency
domain
Piezomagnetism2,3
—
3D, 2D, 2D
axisymmetric
stationary; eigenfrequency;
time dependent; frequency
domain; small-signal
analysis, frequency domain;
eigenfrequency,
prestressed; frequency
domain, prestressed
Nonlinear
Magnetostriction2,3
—
3D, 2D, 2D
axisymmetric
stationary; eigenfrequency;
time dependent; frequency
domain; small-signal
analysis, frequency domain;
eigenfrequency,
prestressed; frequency
domain, prestressed
Joule Heating and
Thermal Expansion2
Piezoelectricity
Magnetomechanics
46 |
CHAPTER 1: INTRODUCTION
PHYSICS INTERFACE
ICON
TAG
SPACE
DIMENSION
AVAILABLE STUDY TYPE
Magnetomechanics2,3
—
3D, 2D, 2D
axisymmetric
stationary; eigenfrequency;
time dependent; frequency
domain; small-signal
analysis, frequency domain;
eigenfrequency,
prestressed; frequency
domain, prestressed
Magnetomechanics,
No Currents2,3
—
3D, 2D, 2D
axisymmetric
stationary; eigenfrequency;
time dependent; frequency
domain; small-signal
analysis, frequency domain;
eigenfrequency,
prestressed; frequency
domain, prestressed
Magnetic–Elastic
Interaction in Rotating
Machinery2,3
—
3D, 2D
stationary; time dependent;
frequency domain;
Ferroelectroelasticity2,
—
3D, 2D, 2D
axisymmetric
stationary; time dependent;
frequency domain
Electrostriction2,9
—
3D, 2D, 2D
axisymmetric
stationary; time dependent;
frequency domain
—
3D
stationary; time dependent;
time dependent, modal;
frequency domain;
frequency domain, modal;
small-signal analysis,
frequency domain;
eigenfrequency,
prestressed; frequency
domain, prestressed
Electrostriction
9
Piezoresistivity
Piezoresistivity,
Shell2,12
ABOUT THE STRUCTURAL MECHANICS MODULE
|
47
PHYSICS INTERFACE
TAG
SPACE
DIMENSION
AVAILABLE STUDY TYPE
—
3D
stationary; time dependent;
time dependent, modal;
frequency domain;
frequency domain, modal;
small-signal analysis,
frequency domain;
eigenfrequency,
prestressed; frequency
domain, prestressed
Poroelasticity, Large
Deformation, Solid2,8
—
3D, 2D, 2D
axisymmetric
stationary; time dependent
Unsaturated
Poroelasticity2,8
—
3D, 2D, 2D
axisymmetric
stationary; time dependent
pfs
3D, 2D, 2D
axisymmetric
stationary, time dependent
Piezoresistivity,
Layered Shell2,5,12
ICON
Poroelasticity
Mathematics
Moving Interface
Phase Field in Solids
1
This physics interface is included with the core COMSOL Multiphysics software but has
added functionality for this module.
2 This physics interface is a predefined multiphysics coupling that automatically adds all the
physics interfaces and coupling features required.
3
Requires the addition of the AC/DC Module.
4 Requires the addition of the Heat Transfer Module.
5
Requires the addition of the Composite Materials Module.
6 Requires the addition of the CFD Module, or the Polymer Flow, or the Microfluidics
Module.
7
48 |
Requires the addition of the Pipe Flow Module.
CHAPTER 1: INTRODUCTION
PHYSICS INTERFACE
ICON
TAG
SPACE
DIMENSION
AVAILABLE STUDY TYPE
8 Requires the addition of the Porous Media Flow Module.
9
Requires the addition of the AC/DC Module or the MEMS Module.
10 Requires the addition of the Polymer Flow Module.
11
Requires the addition of the Nonlinear Structural Materials Module or the Geomechanics
Module.
12 Requires the addition of the MEMS Module.
Common Physics Interface and Feature Settings and Nodes
There are several common settings and sections available for the physics interfaces and
feature nodes. Some of these sections also have similar settings or are implemented in
the same way no matter the physics interface or feature being used. There are also some
physics feature nodes that display in COMSOL Multiphysics.
In each module’s documentation, only unique or extra information is included;
standard information and procedures are centralized in the COMSOL Multiphysics
Reference Manual.
In the COMSOL Multiphysics Reference Manual, see Table 2-4 for
links to common sections and Table 2-5 to common feature nodes.
You can also search for information: press F1 to open the Help
window or Ctrl+F1 to open the Documentation window.
Where Do I Access the Documentation and Application Libraries?
A number of online resources have more information about COMSOL, including
licensing and technical information. The electronic documentation, topic-based (or
ABOUT THE STRUCTURAL MECHANICS MODULE
|
49
context-based) help, and the Application Libraries are all accessed through the
COMSOL Desktop.
If you are reading the documentation as a PDF file on your computer,
the blue links do not work to open an application or content
referenced in a different guide. However, if you are using the Help
system in COMSOL Multiphysics, these links work to open other
modules, application examples, and documentation sets.
THE DOCUMENTATION AND ONLINE HELP
The COMSOL Multiphysics Reference Manual describes the core physics interfaces
and functionality included with the COMSOL Multiphysics license. This book also has
instructions on how to use COMSOL Multiphysics and how to access the electronic
Documentation and Help content.
Opening Topic-Based Help
The Help window is useful as it is connected to the features in the COMSOL Desktop.
To learn more about a node in the Model Builder, or a window on the Desktop, click
to highlight a node or window, then press F1 to open the Help window, which then
displays information about that feature (or click a node in the Model Builder followed
). This is called topic-based (or context) help.
by the Help button (
To open the Help window:
• In the Model Builder, Application Builder, or Physics Builder, click a node
or window and then press F1.
• On any toolbar (for example, Home, Definitions, or Geometry), hover the
mouse over a button (for example, Add Physics or Build All) and then
press F1.
• From the File menu, click Help (
).
• In the upper-right corner of the COMSOL Desktop, click the Help (
button.
50 |
CHAPTER 1: INTRODUCTION
)
To open the Help window:
• In the Model Builder or Physics Builder, click a node or window and then
press F1.
• In the main toolbar, click the Help (
) button.
• From the main menu, select Help>Help.
Opening the Documentation Window
To open the Documentation window:
• Press Ctrl+F1.
• In the main toolbar, click the Documentation (
) button.
• From the main menu, select Help>Documentation.
THE APPLICATION LIBRARIES WINDOW
Each model or application includes documentation with the theoretical background
and step-by-step instructions to create a model or application. The models and
applications are available in COMSOL Multiphysics as MPH-files that you can open
for further investigation. You can use the step-by-step instructions and the actual
models as templates for your own modeling. In most models, SI units are used to
describe the relevant properties, parameters, and dimensions, but other unit systems
are available.
Once the Application Libraries window is opened, you can search by name or browse
under a module folder name. Click to view a summary of the model or application and
its properties, including options to open it or its associated PDF document.
Opening the Application Libraries Window
To open the Application Libraries window (
):
CONTACTING COMSOL BY EMAIL
For general product information, contact COMSOL at [email protected].
COMSOL ACCESS AND TECHNICAL SUPPORT
To receive technical support from COMSOL for the COMSOL products, please
contact your local COMSOL representative or send your questions to
[email protected]. An automatic notification and a case number will be sent to you
ABOUT THE STRUCTURAL MECHANICS MODULE
|
51
by email. You can also access technical support, software updates, license information,
and other resources by registering for a COMSOL Access account.
COMSOL ONLINE RESOURCES
52 |
COMSOL website
www.comsol.com
Contact COMSOL
www.comsol.com/contact
COMSOL Access
www.comsol.com/access
Support Center
www.comsol.com/support
Product Download
www.comsol.com/product-download
Product Updates
www.comsol.com/product-update
COMSOL Blog
www.comsol.com/blogs
Discussion Forum
www.comsol.com/forum
Events
www.comsol.com/events
COMSOL Application Gallery
www.comsol.com/models
COMSOL Video Gallery
www.comsol.com/videos
Support Knowledge Base
www.comsol.com/support/knowledgebase
CHAPTER 1: INTRODUCTION
Overview of the User’s Guide
The Structural Mechanics Module User’s Guide gets you started with modeling using
COMSOL Multiphysics. The information in this guide is specific to this module.
Instructions how to use COMSOL in general are included with the COMSOL
Multiphysics Reference Manual.
As detailed in the section Where Do I Access the Documentation and
Application Libraries?, this information can also be searched from the Help
menu in COMSOL Multiphysics.
TABLE OF CONTENTS, GLOSSARY, AND INDEX
To help you navigate through this guide, see the Contents, Glossary, and Index.
MODELING WITH THE STRUCTURAL MECHANICS MODULE
The Structural Mechanics Modeling chapter gives you an insight on how to approach
the modeling of various structural mechanics problems.
STRUCTURAL MECHANICS THEORY
The Structural Mechanics Theory chapter introduces the general theory on which the
physics interfaces in the Structural Mechanics Module are based.
THE SOLID MECHANICS INTERFACE
The Solid Mechanics chapter describes The Solid Mechanics Interface, which is used
to model 3D solids, plane strain and plane stress 2D and 1D models, and 2D
axisymmetric models.
THE SHELL AND PLATE INTERFACES
The Shell and Plate chapter describes The Shell and Plate Interfaces, which are used to
model thin 3D structures (shell) and out-of-plane loaded plates (plate). The
underlying theory is described in Theory for the Shell and Plate Interfaces.
THE BEAM INTERFACE
The Beam chapter describes The Beam Interface, which contains Euler (Euler–
Bernoulli) and Timoshenko beams for modeling slender 3D and 2D structures.
Typical examples are frameworks and latticeworks. The underlying theory for the
physics interface is described in Theory for the Beam Interface.
OVERVIEW OF THE USER’S GUIDE
|
53
THE BEAM CROSS SECTION INTERFACE
The Beam Cross Section chapter describes The Beam Cross Section Interface, which
is used for computing cross section properties for beams. It can also be used for a
detailed evaluation of stresses in a beam when the section forces to which it is subjected
are known. The first section discusses Using the Beam Cross Section Interface, and the
underlying theory is described in Theory for the Beam Cross Section Interface.
THE TRUSS INTERFACE
The Truss chapter describes The Truss Interface, which models slender 3D and 2D
structures with components capable to withstand axial forces only. Typical applications
are latticeworks, but it can also be used for modeling cables. In the section Modeling
with Truss Elements, you will find a discussion about how to set up models using this
interface. The underlying theory for the physics interface is described in Theory for the
Truss Interface.
THE MEMBRANE INTERFACE
The Membrane chapter describes The Membrane Interface, which can be used for
modeling prestressed membranes, cladding on solids, and balloons, for example. The
underlying theory for the physics interface is also included in Theory for the
Membrane Interface.
THE WIRE INTERFACE
The Wire chapter describes The Wire Interface, which is mainly intended for modeling
pretensioned or sagging wires or cables. The underlying theory for the physics
interface is also included in Theory for the Wire Interface.
THE PIPE MECHANICS INTERFACE
The Pipe Mechanics chapter describes The Pipe Mechanics Interface, which is used for
studying the stresses and deformations in piping systems. The underlying theory for
the physics interface is also included in Theory for the Pipe Mechanics Interface.
THE PHASE FIELD IN SOLIDS INTERFACE
The Phase Field in Solids chapter describes The Phase Field in Solids Interface, which
is used to determine the degradation of material properties in the damaged regions.
The underlying theory for the physics interface is also included in Theory for the Phase
Field in Solids Interface.
54 |
CHAPTER 1: INTRODUCTION
THE TRANSPORT IN SOLIDS INTERFACE
The Transport in Solids chapter describes The Transport in Solids Interface, which can
be used to model transport phenomena in solids. The underlying theory for the physics
interface is also included in Theory for the Transport in Solids Interface.
THE MULTIPHYSICS INTERFACES
The Multiphysics Interfaces and Couplings chapter describes these physics interfaces
found under the Structural Mechanics branch when adding a physics interface:
• The Thermal Stress, Solid Interface combines a Solid Mechanics interface with a
Heat Transfer interface. The coupling appears on the domain level, where the
temperature from the Heat Transfer interface acts as a thermal load for the Solid
Mechanics interface, causing thermal expansion.
• The Thermal Stress, Shell Interface combines a Shell interface with a Heat Transfer
in Shells interface. The coupling appears on the boundary level, where the
temperature from the Heat Transfer in Shells interface acts as a thermal load for the
Shell interface, causing thermal expansion.
• The Thermal Stress, Layered Shell Interface combines a Layered Shell interface with
a Heat Transfer in Shells interface. The coupling appears on the boundary level,
where the temperature from the Heat Transfer in Shells interface acts as a thermal
load for the Layered Shell interface, causing thermal expansion.
• The Thermal Stress, Membrane Interface combines a Membrane interface with a
Heat Transfer in Shells interface. The coupling appears on the boundary level,
where the temperature from the Heat Transfer in Shells interface acts as a thermal
load for the Membrane interface, causing thermal expansion.
• The Joule Heating and Thermal Expansion Interface combines solid mechanics
using a thermal linear elastic material with an electromagnetic Joule heating model.
This is a multiphysics combination of solid mechanics, electric currents, and heat
transfer for modeling of, for example, thermoelectromechanical (TEM)
applications.
• The Piezoelectricity Interface, Solid combines a Solid Mechanics interface with an
Electrostatics interface. Piezoelectric materials in 3D, 2D plane strain and plane
stress, and 2D axial symmetry can be modeled.
• The Piezoelectricity, Layered Shell Interface combines a Layered Shell interface with
an Electric Currents in Layered Shells interface. This makes it possible to model
piezoelectric effects in thin layered structures.
OVERVIEW OF THE USER’S GUIDE
|
55
• The Piezoelectricity, Layered Shell Interface combines a Layered Shell interface with
an Electric Currents in Layered Shells interface. This makes it possible to model
piezoelectric effects in thin layered structures.
• The Electrostriction Interface combines a Solid Mechanics with an Electrostatics
interface. Using this interface, you can solve problems where strains are caused by
electrostrictive effects.
• The Ferroelectroelasticity Interface combines a Solid Mechanics with an
Electrostatics interface. Using this interface, you can solve problems involving
ferroelectric materials, for example within nonlinear piezoelectricity.
• Hygroscopic Swelling Coupling combines a Solid Mechanics with a Magnetic Fields
interface. Using this interface, you can solve problems in the magnetostrictive field
with linear as well as nonlinear material models.
• The Fluid–Solid Interaction Interface combines fluid flow with the Solid Mechanics
interface to capture the interaction between the fluid and the solid in a situation
where the fluid domain has significant deformation. The solid material exists on
domains which are adjacent to the fluid.
• The Fluid–Shell Interaction Interface combines fluid flow with the Shell interface to
capture the interaction between the fluid and the solid in a situation where the fluid
domain has significant deformation. The shell is modeled on the boundary of the
fluid.
• The Fluid–Membrane Interaction Interface combines fluid flow with the Membrane
interface to capture the interaction between the fluid and the membrane in a
situation where the fluid domain has significant deformation. The membrane is
modeled on the boundary of the fluid.
• The Fluid–Solid Interaction, Fixed Geometry Interface combines fluid flow with
the Solid Mechanics interface to capture the interaction between the fluid and the
solid in a situation where the fluid domain can be considered to be nondeforming.
The solid material exists on domains which are adjacent to the fluid.
• The Fluid–Shell Interaction, Fixed Geometry Interface combines fluid flow with the
Shell interface to capture the interaction between the fluid and the solid in a
situation where the fluid domain can be considered to be nondeforming. The shell
is modeled on the boundary of the fluid
• The Fluid–Membrane Interaction, Fixed Geometry Interface combines fluid flow
with the Membrane interface to capture the interaction between the fluid and the
membrane in a situation where the fluid domain can be considered to be
nondeforming. The membrane is modeled on the boundary of the fluid.
56 |
CHAPTER 1: INTRODUCTION
• The Fluid–Pipe Interaction, Fixed Geometry Interface combines flow computed
using the Pipe Flow interface with structural analysis in the Pipe Mechanics
interface. Different types of fluid loads are transferred to the structural analysis.
• The Fluid–Solid Interaction, Conjugate Heat Transfer Interface combines fluid flow
with the Solid Mechanics interface and the Heat Transfer in Solids and Fluids
interface. It combines fluid-structure interaction modeling with a nonisothermal
flow. Heat transfer is considered both in the fluid and in the solid in order to capture
thermal expansion effects.
• The Fluid–Solid Interaction, Two-Phase Flow, Phase Field Interface combines
two-phase fluid flow with the Solid Mechanics interface to capture the interaction
between the fluid and the solid in a situation where the fluid domain has significant
deformation. The solid material exists on domains which are adjacent to the fluid.
• The Fluid–Solid Interaction, Two-Phase Flow, Phase Field, Fixed Geometry
Interface combines two-phase fluid flow with the Solid Mechanics interface to
capture the interaction between the fluid and the solid in a situation where the fluid
domain can be considered to be nondeforming. The solid material exists on
domains which are adjacent to the fluid.
• The Fluid–Solid Interaction, Viscoelastic Flow Interface combines the Viscoelastic
Flow interface with a Deforming Domain feature and the Solid Mechanics interface
to capture the interaction between a viscoelastic fluid and solids in a situation where
the fluid domain has significant deformation.
• The Fluid–Solid Interaction, Viscoelastic Flow, Fixed Geometry Interface combines
the Viscoelastic Flow interface with a Deforming Domain feature and the Solid
Mechanics interface to capture the interaction between a viscoelastic fluid and solids
in a situation where the fluid domain can be considered to be nondeforming.
• The Solid–Thin-Film Damping Interface combines the Thin-Film Flow interface
and the Solid Mechanics interface to model phenomena where a thin-film fluid and
a deformable solid affect each other. The fluid can be either a liquid or a gas, with
the possibility to include cavitation in liquids.
• The Shell–Thin-Film Damping Interface combines the Thin-Film Flow interface
and the Shell interface to model phenomena where a thin-film fluid and a
deformable shells affect each other. The fluid can be either a liquid or a gas, with the
possibility to include cavitation in liquids.
• The Poroelasticity, Solid Interface combines a transient formulation of Darcy’s law
with a quasistatic formulation of Solid Mechanics. The coupling occurs on the
domain level, where the pore pressure from the Darcy’s Law interface acts as a load
OVERVIEW OF THE USER’S GUIDE
|
57
for the Solid Mechanics interface, causing swelling or shrinking. Changes in
volumetric strain affect the pore space, acting as a mass source or sink in Darcy’s
Law.
• The Poroelasticity, Large Deformation, Solid Interface combines a transient
formulation of Darcy’s law with a quasistatic formulation of Solid Mechanics, where
large strains and geometric nonlinear effects are considerable.
• The Poroelasticity, Layered Shell Interface combines the Layered Darcy’s Law
formulation with the Layered Shell interface for structural mechanics. This
multiphysics interface is only available for 3D simulations and it can be active on
boundaries where a layered material is present.
• The Unsaturated Poroelasticity Interface combines a transient formulation of
Moisture Transport in Solids with a quasistatic formulation of Solid Mechanics. The
coupling occurs on the domain level, where the pore pressure from the Moisture
Transport in Solids interface acts as a load for the Solid Mechanics interface, causing
swelling or shrinking. Changes in volumetric strain affect the pore space, impacting
the transport of moist air and liquid water in the porous solid.
• The Phase Field Damage Interface combines the Solid Mechanics and Phase Field
in Solids interfaces to model the evolution of damage and cracks in deforming
solids. The coupling occurs on the domain level, where the driving force for damage
depends on the state of deformation in the solid, which governs the evolution of the
phase field. In turn, the phase field determines the degradation of the solid
properties in the damaged regions.
58 |
CHAPTER 1: INTRODUCTION
2
Structural Mechanics Modeling
The goal of this chapter is to give you an insight on how to approach the modeling
of various structural mechanics problems.
Some physics interfaces and features discussed in this chapter are only available with
certain products. For a detailed overview of the functionality available in each
product, visit https://www.comsol.com/products/specifications/
59
In this chapter:
• Study Types
• Component Mode Synthesis
• Selecting the Physics Interface
• Computing Mass Properties
• Selecting Discretization
• Coupling Different Element Types
• Effective Properties of Periodic
Structures
• Applying Loads
• Modeling Pretensioned Bolts
• Defining Constraints
• Simplified Modeling of Bolt
Threads
• Calculating Reaction Forces
• Introduction to Material Models
• Modeling Piezoelectric Problems
• Modeling Electrostrictive and
Ferroelectroelastic Materials
• Modeling Magnetostrictive
Materials
• Mechanical Damping and Losses
• Modeling Geometric Nonlinearity
• Contact Modeling
• Activating and Deactivating
Material
• Springs and Dampers
• Defining Multiphysics Models
• Thermally Coupled Problems
• Fluid–Structure Interaction
60 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
• Modeling Embedded Structures
and Reinforcements
• Modeling Thin Layers
• Modeling Cracks
• Buckling Analysis
• Performing a Random Vibration
Analysis
• Performing a Response Spectrum
Analysis
• Stress Linearization
• Solver Settings for Structural
Mechanics
• Using Reduced Integration
• Result Presentation
• Part Libraries
• Parameter Estimation
Study Types
Introduction
In this section, you will find information about when and how to apply the study types
which are available for structural mechanics problems:
• Stationary Analysis
• Eigenfrequency Analysis
• Mode Analysis
• Time-Domain Analysis
• Frequency-Domain Analysis
• Mode Superposition
• Harmonic Perturbation
• Modal Reduced-Order Models
• Linearized Buckling Analysis
• Bolt Pretension Study
• Random Vibration (PSD) Study
• Response Spectrum Analysis Study
For general information about study types and solvers, see Studies and
Solvers in the COMSOL Multiphysics Reference Manual
Stationary Analysis
You can consider a structural mechanics problem as stationary if the following two
criteria are fulfilled:
• The loads vary so slowly that inertial forces are negligible. Problems of this type are
referred to as quasi static.
• There are no explicit time dependencies in the material model. Viscoelasticity and
creep have such time dependencies.
To perform this type of analysis, you use a Stationary study step.
STUDY TYPES
|
61
In many cases, there is a variation in the load, even though the solution for each value
of the load can be considered as stationary. There are three conceptually different
cases:
• The load values are independent; it is just a number of different load cases you want
to compute. The load case handling functionality described in Load Cases is well
suited for this purpose.
• You want to study a nonlinear problem where the solution is path dependent, or
where the load must be increased in small increments in order to obtain a converged
solution. In this case you should use the parametric continuation solver. Create a
parameter under Global Definitions>Parameters, which you use to control the
variation of the load. Then select Auxiliary sweep under Study Extensions in the
settings for the Stationary solver. In the table for the auxiliary sweep parameters, add
the load controlling parameter, and define its range of variation.
• In a multiphysics problem, another physical quantity might be truly time dependent
but on a time scale that is “slow” from the structural mechanics point of view. This
is usually the case with, for example, problems coupled to heat transfer or diffusion.
If the problem also is such that the structural deformations do not affect the other
physics, it will be unnecessarily expensive to solve also the structural problem in the
time domain, irrespective of whether it is linear or nonlinear. In this situation, you
should first solve the other physics in a time-dependent study and then the structural
mechanics problem in a subsequent stationary study step using the time t as the
parameter in the auxiliary sweep.
For an example of how to set up such a study sequence, see
Fluid-Structure Interaction in a Network of Blood Vessels: Application
Library path Structural_Mechanics_Module/Fluid-Structure_Interaction/
blood_vessel.
CONSTRAINTS
A stationary problem is solvable only if the structure is sufficiently constrained. There
must not be any possible rigid body modes. Thus, no stress-free deformation states are
allowed.
For a more detailed discussion about sufficient constraints, see Rigid
Body Motion.
62 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Eigenfrequency Analysis
An Eigenfrequency study solves for the eigenfrequencies (natural frequencies) and the
shapes of the corresponding eigenmodes.
When performing an eigenfrequency analysis, you can specify whether to look at the
mathematically more fundamental eigenvalue, , or the eigenfrequency, f, which is
more commonly used in a structural mechanics context. The relation between the two
is
f = – -------2i
where i is the imaginary unit.
The undamped eigenvalue problem is commonly written as
2
 K –  M u = 0
where K is the stiffness matrix, M is the mass matrix, u is the eigenmode displacement
vector, and   f is the angular frequency. If damping is present, the eigenvalue
equation is expanded to
2
 K + iC –  M u = 0
(2-1)
where C is the viscous damping matrix, and K can be complex-valued.
Because only the shape and not the size of the modes (eigenvectors) have physical
significance, the computed modes can be scaled arbitrarily. You can select the method
for scaling in the Eigenvalue Solver node of the solver sequence. If Scaling of eigenvectors
is set to Mass matrix, the eigenmodes u are orthogonalized with respect to the mass
matrix M so that
T
u i Mu i = 1
(2-2)
This is a common choice for the scaling of eigenvectors within the structural mechanics
field. The choice of eigenvector scaling does not affect for example the results of a
subsequent mode superposition analysis, but it will affect the interpretation of an
exported modal representation of the system.
STUDY TYPES
|
63
MODAL PARTICIPATION FACTORS
Modal (or mass) participation factors are useful tools when working with the modal
representation of a structure. Through them, you can get the following information:
• The fraction of the total mass of a structure that a certain number of modes
represent is a result. This can be important when judging if a set of modes forms a
good enough base for a mode superposition.
• The main direction of vibration for a certain mode can be seen from the relation
between the participation factors.
• When you have a large set of modes, an examination of the participation factors can
give information about the dominant modes.
To compute modal participation factors, a Participation Factors node must be present
under Definitions in the current component. When you add an Eigenfrequency study
from the Add Study window, such a node is automatically created.
You can also add it manually under Definitions>Physics Utilities. If you do that after an
eigenfrequency study has been run, you need to do an Update Solution in order to get
access to the variables containing the participation factors.
The modal participation factors are available as global variables, and these can for
example be displayed in a table using a Global Evaluation node under Derived Values in
the Results branch. The participation factor results are available as predefined variables
in the Definitions submenu for the component. In Table 2-1, the variables created from
a Participation Factors node is listed (assuming the default tag mpf1).
TABLE 2-1: PARTICIPATION FACTOR VARIABLES.
VARIABLE
DESCRIPTION
mpf1.mass
Total mass
mpf1.CMJ
Center of mass, J coordinate
mpf1.mEffLJ
Effective mass, translation along J-axis
mpf1.mEffRJ
Effective mass, rotation around J-axis
mpf.pfLJ
Participation factor, translation along J-axis
mpf.pfRJ
Participation factor, rotation around J-axis
mpf.pfLnormJ
Normalized participation factor, translation along J-axis
mpf.pfRnormJ
Normalized participation factor, rotation around J-axis
The normalized participation factors are those that would be obtained if mass matrix
scaled eigenmodes would have been used.
64 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
If a Participation Factors node is present in the model when an eigenfrequency study is
run, an evaluation group named Participation Factors is automatically generated. It
contains a table with the translational and rotational modal participation factors for all
computed eigenfrequencies.
• If you would compute all eigenmodes of a structure, and sum all modal
masses, they will usually not exactly match the total mass of the
structure. The reason is that any mass which is associated with
constrained degrees of freedom is lost. This effect is discretization
dependent. The mass lost is a fraction of the mass of the elements
having constrained nodes.
• The computation of participation factors is a feature at the component
level. For a case where there are couplings between two or more
components that affect the eigenvalue problem, an evaluation of the
participation factors and modal masses may give unpredictable results.
For an example showing how to compute modal participation factors and
modal mass, see In-Plane Framework with Discrete Mass and Mass
Moment of Inertia: Application Library path
Structural_Mechanics_Module/Verification_Examples/
inplane_framework_freq.
In the COMSOL Multiphysics Reference Manual:
• Eigenvalue Solver
• Studies and Solvers
• Postprocessing of Eigenmodes
• Derived Values, Evaluation Groups, and Tables
In the theory chapter of the Structural Mechanics User’s Guide:
• Modal Participation Factors
It is possible to compute eigenfrequencies for structures which are not fully
constrained; this is sometimes referred to as free-free modes. For each possible rigid
STUDY TYPES
|
65
body mode, there is one eigenvalue which in theory is zero. The number of possible
rigid body modes for different geometrical dimensions is shown in the table below.
TABLE 2-2: NUMBER OF POSSIBLE RIGID BODY MODES.
DIMENSION
NUMBER OF RIGID BODY MODES
3D
6 (3 translations + 3 rotations)
2D axisymmetric
1 (Z-direction translation)
2D (solid, beam, truss)
3 (2 translations + 1 rotation)
2D (plate)
3 (1 translation + 2 rotations)
The computed rigid body modes will in general not be recognizable as having pure
translation or rotation. Rather, they will contain linear combinations of all the
fundamental rigid body motions.
In a piezoelectric model, one more zero eigenfrequency could appear if you have not
set a reference value for the electric potential.
In practice, the natural frequencies of the rigid body modes are not computed as
exactly zero, but can appear as small numbers which may even be negative or complex.
If rigid body modes are present in the model, then it is important to use a nonzero
value in the Search for eigenfrequencies around text field in the settings for the
Eigenfrequency study step. The value should reflect the order of magnitude of the first
important nonzero eigenfrequency.
For an example showing an eigenfrequency computation in a model
having a rigid body mode, see Eigenfrequency Analysis of a Free
Cylinder: Application Library path Structural_Mechanics_Module/
Verification_Examples/free_cylinder.
DAMPING
If any type of damping is included in the model, an eigenfrequency solution
automatically returns the damped eigenvalues. The eigenfrequencies and, in general,
also the mode shapes are complex in this case. A complex-valued eigenfrequency can
be interpreted so that the real part represents the actual frequency, and the imaginary
part represents the damping. The damping ratio of the corresponding eigenmode can
be defined as
imag   i  imag   i 
 i = -------------------------  ------------------------real   i 
i
66 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
where the approximate expression is valid with high accuracy (within 2%) as long as the
damping is less than 0.2.
In a complex mode shape, there are phase shifts between different parts of the
structure, so that not all points reach the maximum at the same time under free
vibration.
Some damping types will still give real-valued eigenmodes, this is the case for Rayleigh
damping and loss factor damping.
If an eigenfrequency study is performed as a first step of a mode
superposition analysis, then all features that supply damping should be
disabled in this step. This can be done in the Physics and Variables Selection
section in the settings for the Eigenfrequency study step.
The damping is taken into account in the mode superposition studies.
See also the discussion under Mode Superposition.
PRESTRESSED ANALYSIS
In a loaded structure, the natural frequencies may be shifted due to stress stiffening.
To do a prestressed analysis, Include geometric nonlinearity must be selected in the
Eigenfrequency study step. This is automatic when you add the Eigenfrequency,
Prestressed study type.
The prestress loading can include a contact analysis, in which case the subsequent
eigenfrequency analysis provide as linearization around the current contact state.
Prestressed Structures
FREQUENCY DEPENDENT MATERIAL PROPERTIES
If the material data (stiffness or damping) is frequency dependent, the eigenvalue
problem will become nonlinear. This can, for example, occur for some viscoelastic
materials. In this case, the eigenvalue equation Equation 2-1 becomes
2
 K    + iC    –  M u = 0
(2-3)
The eigenvalue solver as such assumes that the matrices involved are constant, so they
must be evaluated at a certain frequency, the linearization point.
STUDY TYPES
|
67
2
 K   L  + iC   L  –  M u = 0
(2-4)
In order to get a correct solution to Equation 2-3, the linearization point L must be
close to the actual eigenvalue . This is in general possible only for one single
eigenfrequency at a time. You must solve this problem either by manual iteration, or
by using some type of scripting, for example through a model method.
Eigenmodes of a Viscoelastic Structural Damper: Application Library
path Structural_Mechanics_Module/Dynamics_and_Vibration/
viscoelastic_damper_eigenmodes.
The built-in viscoelastic materials use a special formulation that do not
generate a nonlinear eigenvalue problem, as long fractional derivatives are
not used.
Mode Analysis
The Mode Analysis study type (
2D plane strain.
) is available with the Solid Mechanics interface in
Elastic waves can propagate over large distances in structures like rails and pipes, with
a generic name referred to as waveguides. After some distance of propagation in a
waveguide of uniform cross section, such guided waves can be described as a sum of
just a few discrete propagating modes, each with its own shape and phase speed. The
equation governing these modes can be obtained as a spatial Fourier transform of the
linearized time-harmonic equation in the waveguide axial z direction or by inserting
the assumption that the mode is harmonic in space,
u = ue – ikz z
and eliminating all out-of-plane z dependence.
Similar to the full time-harmonic equation, the transformed equation can be solved at
a given frequency with a nonzero excitation for most axial wave numbers kz. But at
certain discrete values the equation breaks down. These values are the propagation
constants or wave numbers of the propagating or evanescent waveguide modes. The
68 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
eigenvalue solver can solve for these propagation constants together with the
corresponding mode shapes.
The propagating wave number is a function of the frequency. The relation
between the two is commonly referred to as a dispersion curve.
The most common use for mode analysis is to define sources for a subsequent
time-harmonic simulation. If there is a component with one or more waveguide
connections, its behavior can be described by simulating its response to the discrete set
of propagating modes on the waveguide opening cross sections.
• Out-of-Plane Waves in the Structural Mechanics Theory chapter.
• Studies and Solvers and Mode Analysis in the COMSOL Multiphysics
Reference Manual.
Time-Domain Analysis
There are two classes of problems where a stationary solution cannot be used:
• When the inertial forces no longer are negligible, the full problem as given by
Newton’s first law must be solved.
• When there are time dependencies in the material model, as for creep or
viscoelasticity.
The most general way of handling time-dependent problems is to use a Time Dependent
study. In this type of analysis, you can incorporate any type of nonlinearity, and there
are no limitations on the time dependence of the loads.
A time-domain solution can be preceded by a stationary study, if, for example, prestress
effects are needed.
For a linear problem including inertia, using the mode superposition method is often
much more efficient than using the standard direct method.
SOLVER SELECTION
The two classes of dynamic problems presented above have quite different properties.
The inertial forces in the full structural dynamics problem contain second-order time
derivatives of the displacements, whereas creep and viscoelasticity only have first-order
STUDY TYPES
|
69
derivatives. The physical and numerical properties of these equations differ
significantly.
There are two general solvers for time-dependent problems in COMSOL
Multiphysics.
• The Generalized alpha method, which is recommended for structural dynamics
problems. This is the default solver if Structural Transient Behavior is set to Include
inertial terms in the physics interface settings.
• The BDF method, which is recommended for first-order problems. This is the
default solver if Structural Transient Behavior is set to Quasistatic in the physics
interface settings.
In the COMSOL Multiphysics Reference Manual:
• Time-Dependent Solver
• Studies and Solvers
Frequency-Domain Analysis
In a frequency-domain analysis, you study the response to a harmonic steady state
excitation for certain frequencies. Such a steady state can prevail once all transient
effects have been damped out.
The response must be linear, so that the single frequency harmonic excitation gives a
pure harmonic response with the same frequency. The model may, however, contain
nonlinearities. The harmonic response is computed around a certain linearization
point. In such a case, the frequency-domain analysis can be considered as a very small
perturbation around that linearization point.
Harmonic Perturbation
70 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
All loads and responses in a frequency-domain analysis are in general complex-valued
quantities. If all loads do not have the same phase, you can describe the phase of a
certain load in two ways:
• Add a Phase subnode to the load, in which you directly give the phase angle.
• Enter the load as a complex value, for example as
100[N]*(1+0.3*i)/sqrt(1+0.3^2).
Most results from a frequency-domain analysis are complex valued. In many results
evaluation nodes, the real value of any result quantity will be shown. Assuming that
you want to display for example the displacement in the x direction, u, you have the
following options:
• Plot u or real(u). This gives the displacement at current (default zero) phase angle.
• Plot imag(u). This gives the displacement at a phase angle shifted 90 degrees from
the current value.
• Plot abs(u). This gives the amplitude of the displacement.
• Plot arg(u). This gives the phase angle of the displacement.
The reference phase, with respect to which the results above are reported can be
entered in the settings for the dataset.
STUDY TYPES
|
71
Result quantities that are nonlinear in terms of the displacements, such as principal
stresses, should be interpreted with great care in frequency domain. They will in
general not be harmonic, so the information about amplitude and phase is not reliable.
Some extra variables for postprocessing are created in a frequency-domain
analysis. As an example, in a Solid Mechanics interface with the name
solid, the following variables are defined:
• solid.disp — norm of displacement (at current phase angle)
• solid.vel — norm of velocity (at current phase angle)
• solid.acc — norm of acceleration (at current phase angle)
• solid.disp_rms — RMS displacement over a cycle
• solid.vel_rms — RMS velocity over a cycle
• solid.acc_rms — RMS acceleration over a cycle
• solid.uAmpX — amplitude of displacement in the X direction
• solid.uAmp_tX — amplitude of velocity in the X direction
• solid.uAmp_ttX — amplitude of acceleration in the X direction
• solid.uPhaseX — phase of X displacement, in radians
• solid.uPhase_tX — phase of X velocity, in radians
• solid.uPhase_ttX — phase of X displacement, in radians
• solid.mises — von Mises equivalent stress at current phase angle.
• solid.mises_peak — maximum von Mises equivalent stress over a
cycle.
The components in other coordinate directions are obtained by replacing
X by another coordinate name.
PRESTRESSED ANALYSIS
The shift in the natural frequencies in a prestressed structure may have a significant
effect on the frequency response. This is particularly important when the frequencies
of the load are close to any of the natural frequencies of the structure.
To do a prestressed analysis, Include geometric nonlinearity must be selected in the
Frequency Domain study step. This is automatic when you add the Frequency Domain,
Prestressed study type.
72 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
The prestress loading can include a contact analysis, in which case the subsequent
frequency domain analysis provides a linearization around the current contact state.
• Prestressed Structures
• Harmonic Perturbation
OBTAINING A TIME HISTORY
Sometimes you want to study the time history over a period for the results of a
frequency domain analysis. You can do that by adding a Frequency to Time FFT study
step. The frequency response results are then viewed as terms in a Fourier series, which
can be transformed to time domain. It is possible combine the results for several
frequencies into a single time history, under the assumption that they are all multiples
of the same fundamental frequency.
For examples showing how to obtain a time history from frequency
domain results, see
• Viscoelastic Structural Damper: Application Library path
Structural_Mechanics_Module/Dynamics_and_Vibration/
viscoelastic_damper_frequency.
• Vibration Analysis of a Deep Beam: Application Library path
Structural_Mechanics_Module/Verification_Examples/
vibrating_deep_beam.
Mode Superposition
Analyzing forced dynamic response for large models can be very time consuming. You
can often improve the performance dramatically by using the mode superposition
technique. The following requirements must be met for a modal solution to be
possible:
• The analysis is linear. It is possible, however, that the structure has been subjected
to a preceding nonlinear history. The modal response can then be a linear
perturbation around that state.
• There are no nonzero prescribed displacements.
• The important frequency content of the load is limited to a range that is small when
compared to all the eigenfrequencies of the model, so that its response can be
STUDY TYPES
|
73
approximated with a small number of eigenmodes. In practice, this excludes wave
and shock type problems.
• If the modal solution is performed in the time domain, all loads must have the same
dependency on the time. This requirement can be relaxed if you use a reduced-order
model to represent the system, rather than using one of the mode superposition
studies.
When using the Structural Mechanics Module, there are three predefined study types
for mode superposition:
• Time Dependent, Modal
• Frequency Domain, Modal
• Frequency Domain, Prestressed, Modal
The two first of these study types consist of two study steps: One step for computing
the eigenfrequencies and one step for the modal response. The last one has three study
steps. Before the eigenfrequency step, you solve a static load case in order to get a
prestress state used in the eigenfrequency computation.
In practice, you have often computed the eigenfrequencies already, and then want to
use them in a mode superposition. In this case, start by adding an empty study, and
then add a Time Dependent, Modal or Frequency Domain, Modal study step to it. After
having added the study step this way, you must point the modal solver to the solution
containing the eigenfrequencies and eigenmodes. You do this by first selecting Show
default solver at the study level, and then selecting the eigenfrequency solution to be
used in the Eigenpairs section of the generated modal solver.
In a mode superposition, the deformation of the structure is represented by a linear
combination of its eigenmodes. The amplitudes of these modes are the degrees of
freedom of the reduced problem. You must select which eigenmodes to include in the
analysis. This choice is usually based on a comparison between the eigenfrequencies of
the structure and the frequency content of the load. As a rule of thumb, select
eigenmodes up to approximately twice the highest frequency of the excitation.
In the mode superposition formulation in COMSOL Multiphysics, the full model is
projected onto the subspace spanned by the eigenmodes. A problem having the
number of degrees equal to the number of included modes is then solved. Note that
this differs from many implementations of mode superposition, where it often is
assumed that the modal equations are totally decoupled.
74 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
An implication of this, is that it is not necessary to assume a certain structure of the
damping matrix. Any type of damping which is allowable in the corresponding analysis
of the full system can also be used in the modal based analysis.
For many common cases, the mode superposition analysis is not sensitive to whether
the eigenmodes were computed using damping or not. The reason is that the
eigenmodes of problems with Rayleigh damping and loss factor damping can be shown
to be identical to those of the undamped problem, so that the projection to the
subspace spanned by the eigenmodes is the same in both cases. For more general
damping, it is however recommended that you suppress all contributions to the
damping during the eigenfrequency step, and thus base the mode superposition on the
solution to the undamped eigenfrequency problem.
FREQUENCY DOMAIN ANALYSIS
All loads are assumed to have a harmonic variation. This is a perturbation type analysis,
so only loads having the Harmonic perturbation property selected are then included in
the analysis.
TIME-DEPENDENT ANALYSIS
Only the factor of the load which is independent of time should be specified in the load
features. The dependency on time is specified as Load factor under the Advanced section
of the modal solver. This factor is then applied to all loads.
• Modal Solver and Studies and Solvers in the COMSOL Multiphysics
Reference Manual
• Mechanical Damping and Losses
Harmonic Perturbation
Analyses in the frequency domain assume that the problem your study is linear, at least
with respect to the response to the harmonic excitation. There may be other
nonlinearities, such that the structure has responded nonlinearly to a previous loading.
This loading could, for example, have caused a large rotations or prestress of a rubber
membrane.
The concept of harmonic perturbation is in COMSOL Multiphysics used for
distinguishing the linear harmonic analysis from a possible prestress analysis. The most
important implication is that if a load has the Harmonic Perturbation selection, it is
applied only in a study that is of the perturbation type. A load without this selection is,
STUDY TYPES
|
75
on the other hand, ignored in such a study. In this way two sets of loads can be
distinguished from each other. Technically speaking, the effect of marking a load as
Harmonic Perturbation is that the linper() operator is applied to the value of the load.
The default settings for the different structural mechanics study types in the frequency
domain are summarized in Table 2-3.
TABLE 2-3: DEFAULT PERTURBATION SETTINGS FOR STRUCTURAL MECHANICS STUDY TYPES.
STUDY TYPE
STUDY STEP
PERTURBATION
Frequency Domain
Frequency Domain
No
Frequency Domain, Prestressed
Stationary
Frequency Domain, Perturbation
No
Yes
Frequency Domain, Modal
Eigenfrequency
Frequency Domain, Modal
N/A
Yes
Frequency Domain, Prestressed,
Modal
Stationary
Eigenfrequency
Frequency Domain, Modal
N/A
N/A
Yes
Note the following:
• With the default settings you cannot use the same set of loads for a Frequency Domain
and a Frequency Domain, Modal study because only the latter responds to
perturbation loads.
• You can change the behavior of a Frequency Domain study to be of the perturbation
type by modifying the solver sequence. In the General section of the settings for the
Stationary Solver, change Linearity to Linear perturbation.
• A solver that does not have Linearity set to either Linear perturbation or Linear may
respond to nonlinear effects. There are multiphysics problems where this is wanted
because there may be a nonlinearity in another physics, even though the harmonic
solution within structural mechanics is linear. But if there are nonlinearities within
76 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
the structural mechanics parts of the model, you must be careful with the solver
settings.
In a Frequency-Domain, Perturbation study step, that is when Linearity is set
to Linear perturbation, geometric nonlinearity will be incorporated in the
sense that there is a split between the material and spatial frames. This
makes it possible to take for example stiffness from follower loads into
account, and to use a contact solution as linearization point.
This frame split was introduced in version 5.3. As an effect, models
created in an earlier version, in which some expressions have a frame
dependency, may produce results that differ from before. Examples of
such cases are:
• Pressure loads
• Loads defined in coordinate systems with deformation dependent axis
orientation
• User-defined expressions containing spatial (“lowercase”) coordinates
In the COMSOL Multiphysics Reference Manual:
• Frequency-Domain Perturbation Study Step
• Harmonic Perturbation — Exclusive and Contributing Nodes
• Built-In Operators (linper() operator)
For most load types, the use of Harmonic Perturbation is straightforward, but some
cases need a more detailed discussion:
• A Rigid Connector can be assigned a Harmonic Perturbation subnode in which you can
prescribe harmonic perturbation values to constrained degrees of freedom. If you
have added Applied Force or Applied Moment nodes under a Rigid Connector, you can
independently assign Harmonic Perturbation to these nodes, so that the loads are
considered as being of the perturbation type.
STUDY TYPES
|
77
• Even though initial stresses and strains are not usually considered as loads, you can
assign Harmonic Perturbation also to the Initial Stress and Strain nodes.
• Rather assigning Harmonic Perturbation to a load, you can write the load value
enclosed in the linper() operator. This is particularly useful when the feature that
provide the loading does not have the Harmonic Perturbation option.
For an example showing how to use harmonic perturbation, see Bracket
— Frequency-Response Analysis: Application Library path
Structural_Mechanics_Module/Tutorials/bracket_frequency.
Modal Reduced-Order Models
Reduced-order modeling seeks to reduce the number of degrees of freedom in a
physical model whilst still retaining the essential physics. For a lightly damped resonant
system driven at one of its resonant frequencies, it is reasonable to consider only the
contributions to the system of a small number (m) of modes within the signal
bandwidth. In some cases, a single mode is sufficient. A system with n degrees of
freedom has mass, stiffness, and damping matrices of size n-by-n. A reduced-order
representation of the system considering m modes has size m-by-m. The reduction in
complexity of the system, and the computational speed up is therefore significant when
m « n. This section describes the theory of the reduced-order system and gives
guidelines on how to obtain reduced-order models from a COMSOL model.
This can be employed in two different ways: Either you can use the built-in modal
solvers for the time or frequency domain, or you can export the small equivalent system
and analyze it outside COMSOL Multiphysics, for example, as a component in a larger
system simulation.
THE MODAL COORDINATE SYSTEM
Consider a mechanical system, with n degrees of freedom, described by an equation of
the form
ꞏꞏ + Duꞏ + Ku = F
Mu
where u is the displacement vector (size: n-by-1), K is the stiffness matrix (size:
n-by-n), D is the damping matrix (size: n-by-n), and M is the mass matrix (size:
n-by-n). In the frequency domain the problem takes the form
78 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
(2-5)
2
–  M u 0 + iDu 0 + Ku 0 = F
where u = u0eit.
Initially consider the system in the absence of damping and forces. The undamped
system has n eigenvalues i, which satisfy the equation
2
Kû i =  i Mû i
(2-6)
These eigenvectors can be shown to be orthogonal with respect to both M and K:
T
i  j , i  j
(2-7)
T
i  j , i  j
(2-8)
û j Mû i = 0
û j Kû i = 0
Next the following n-by-n matrix is constructed, with columns taken from the n
eigenvectors:
U = û 1 , û 2  û n
Then consider the following matrix:
T
T
T
T
û 1 Mû 1 û 1 Mû 2
T
û 2 Mû 1 û 2 Mû 2
U MU =
T
T
û n – 1 Mû n – 1 û n – 1 Mû n
T
û n Mû n – 1
T
û n Mû n
From Equation 2-7 it is clear that this is a diagonal matrix. Similarly, from
Equation 2-8 it is clear that UTKU is also diagonal.
From the properties of the eigenvectors it is possible to expand any function in terms
of the eigenvectors. Thus, the displacement u can be written as:
n
u =
 ai ûi
i=1
This equation can also be expressed in the form:
STUDY TYPES
|
79
u = Ua
(2-9)
where a is a column vector containing the coefficients ai as rows. In general a is
time dependent.
Now consider the original equation: Equation 2-5. First substitute for u using
Equation 2-9. Then transform the equation to the modal coordinate system by
premultiplying by UT. This gives:
T
ꞏꞏ + U T DUaꞏ + U T KUa = U T F
U MUa
(2-10)
It has already been established that the matrices UTMU and UTKU are diagonal and
frequently a damping model is chosen that results in a diagonal damping matrix. For
example, in Rayleigh damping D  M + K, where  and  are constants. For a
general damping, the transformed damping matrix is however not diagonal. As an
alternative, a damping ratio, i, can be assigned to each mode.
EIGENVALUE SCALING
The precise form of Equation 2-10 is determined by the normalization adopted for the
eigenfunctions. In structural applications the eigenfunctions are often normalized such
that UTMU  I. This is referred to as mass matrix scaling in the eigenvalue solver. In
this case Equation 2-6 gives
T
2
T
û i Kû i =  i û i Mû i =  i
2
so that
T
2
U KU = diag   i 
where diag(i2) is the diagonal matrix with diagonal elements i2. Similarly, if
damping ratios for each mode are defined, the damping matrix can be expressed in the
form
T
U DU = diag  2 i  i 
Thus, if mass matrix scaling is used Equation 2-10 takes the form
ꞏꞏ + diag  2  aꞏ + diag   2 a = U T F
a
i i
i
(2-11)
It is also possible to scale the eigenvectors so that the point of maximum displacement
has given displacement. This is referred to as max scaling in the eigenvalue solver. For
80 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
an individual mode this scaling has a simple physical interpretation — the
corresponding component of a, ai, is the amplitude of the i:th mode, measured at the
point of maximum displacement, when the mode is driven by the force F. In this case
Equation 2-10 takes the form
T
ꞏꞏ + diag  c
ꞏ
diag  m eff , i a
eff , i a + diag  k eff , i a = U F
(2-12)
Here meff,i is the effective mass of the i:th mode, ceff,i = 2meff,iii is the effective
damping parameter for the mode, and keff,i is the effective spring constant. Each
element of the vector UTF gives the force component that acts on each of the
respective modes.
When using max scaling, it is the largest value of a degree of freedom
which is scaled to 1. The total displacement in that node will thus be
between 1 and 3 times the given scaling factor.
If degrees of freedom other than displacements are active in the
eigenfrequency problem, the maximum value may occur in another type
of degree of freedom such as electric potential or pressure. Consequently,
the peak displacement in that mode can then be less than the scaling
factor.
REDUCED-ORDER MODELS
The preceding discussion did not consider how to reduce the number of degrees of
freedom in the system. For systems in which the vector UTF has only a few significant
components (for example, components i = 1, …, m where m « n) the following
approximation can be made:
m
u
 ai ûi
i=1
The expression for u in matrix becomes:
u = U'a'
where U' is now an m-by-n and a' is a vector with m components. The equation
system in modal coordinates now takes the form
T
ꞏꞏ + U' T DU'a'
ꞏ + U' T KU'a' = U' T F
U' MU'a'
(2-13)
STUDY TYPES
|
81
The matrices U'TMU', U'TDU', and U'TKU' now have dimensions m-by-m.
Similarly, the vector U'TF has m components. This results in a significant reduction in
the system complexity.
REDUCED-ORDER MODELS WITH PHYSICAL DAMPING
If physically relevant damping is present in the system, the above theory must be
modified as the damping matrix is no longer diagonal in the modal coordinate system.
COMSOL can still handle this case as the modal solver does not assume that any of the
matrices are diagonal. In this case the eigenvalues become complex and the
eigenvectors split into right and left eigenvectors. The right eigenvectors Ur are
solutions of the equation:
2
–  i M û r ,i + i i Dû r ,i + Kû r ,i = F
As in the previous section, for a reduced set of modes, it is assumed that:
u = U' r a'
where U'r is the n-by-m matrix containing the right eigenvectors chosen for the modal
analysis. Once again a' is a vector with m components. The system in modal
coordinates takes the form
ꞏꞏ + U' DU' a'
ꞏ
U' l MU' r a'
l
r + U' l KU' r a' = U' l F
T
T
T
T
where U'l is the n-by-m matrix containing the left eigenvectors chosen for the modal
analysis.
The matrices U'lTMU'r, U'lTDU'r, and U'lTKU'r are no longer necessarily diagonal.
The modal solver accepts any linearly independent set of vectors to project the solution
vector and equations onto and constructs the reduced-order system accordingly.
ACCESSING THE REDUCED-ORDER MODEL MATRICES
The Model Reduction and Modal Reduced-Order Model study steps have the property that
they can assemble the modal matrices and make them available for output. In the Model
Reduction node, the Store reduced matrices check box must be selected.
After the model has solved, right-click the Results>Derived Values node and select
System Matrices. In the output section choose the Matrix to display in the list. The mass
matrix corresponds to the matrix U'lTMU'r the stiffness matrix corresponds to
U'lTKU'r, and the damping matrix corresponds to U'lTDU'r. The vector U'lTF is
available as the load vector. These matrices are given in a format that respects the
82 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
normalization of the preceding Eigenvalue Solver. To change this, select the Eigenvalue
Solver node, and change the Scaling of Eigenvectors setting under the Output section.
Use the Max setting if an equivalent Mass-Spring-Damper system is required, in which
case the modal amplitude corresponds to the maximum displacement of the mode.
Linearized Buckling Analysis
A linearized buckling analysis can be used to estimate the critical load at which a
structure becomes unstable. This is a predefined study type that consists of two study
steps: An initial step in which a unit load is applied to the structure, and a second step
in which an eigenvalue problem is solved for the critical buckling load.
COMSOL reports a critical load factor, ,which is the multiplier to the initial load at
which the structure becomes unstable. The corresponding eigenmode is the shape of
the structure in its buckled state.
The level of the initial load used is immaterial since a linear problem is solved. If the
initial load actually was larger than the buckling load, then the critical value of  is
smaller than 1. It is also possible that the computed value of  is negative. This signifies
that a reversed load will give the critical case.
When performing a linearized buckling study, it is possible to discriminate between live
and dead loads, where the former are the ones with respect to which the critical load
factor is computed, and the latter are assumed to be constant. In this case, two
different basic load cases need to be solved before the eigenvalue solution.
The buckling computed buckling modes can be used to provide an initial imperfection
for a subsequent nonlinear buckling analysis,
• For more details about how to model buckling, see Buckling Analysis.
• The numerical formulation is described in the section Linear Buckling
in the Structural Mechanics Theory chapter.
• Settings for the solvers are described in Studies and Solvers, Linear
Buckling, and Buckling Imperfection in the COMSOL Multiphysics
Reference Manual.
STUDY TYPES
|
83
• Bracket — Linear Buckling Analysis: Application Library path
Structural_Mechanics_Module/Tutorials/bracket_linear_buckling
• Buckling Analysis of a Truss Tower: Application Library path
Structural_Mechanics_Module/Buckling_and_Wrinkling/
truss_tower_buckling
Bolt Pretension Study
The Bolt Pretension study step is a special case of a Stationary study step, where the
special degrees of freedoms used for modeling prestressed bolts are solved for. In all
other study types, these degrees of freedom are inactive. Typically, you include a Bolt
Pretension study step as the first step in a study in order to simulate the state after the
assembly of a bolted joint. You can then add any other types of study steps for
computing the effects of the service loads.
In a Bolt Pretension study step, it is possible to tension the bolts sequentially, or to
change the bolt prestress more than once, if an auxiliary sweep over some history
parameter is used.
Modeling Pretensioned Bolts
• Modeling of Pretensioned Bolts: Application Library path
Structural_Mechanics_Module/Tutorials/bolt_pretension_tutorial
• Prestressed Bolts in a Tube Connection: Application Library path
Structural_Mechanics_Module/Contact_and_Friction/tube_connection
Random Vibration (PSD) Study
A random vibration study is used to analyze the response of a structure subjected to
loads that randomly vary in time, but their statistical properties do not change with
time.
The input to a random vibration analysis is given in terms of power spectral densities
(PSD) and, in the case of several loading sources, the load cross-correlations.
84 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
The results of this type of analysis can only be interpreted in a statistical sense. Usually,
the root mean square (RMS) of the result quantities is studied.
The analysis is based on a mode superposition and the reduced-order model (ROM)
functionality. Except from the computation of eigenfrequencies and corresponding
eigenmodes, and the creation of the reduced model, the core of the computation is
performed during result evaluation.
The Random Vibration (PSD) study is mainly an entry point when adding studies. When
you select it, you actually get two studies and a number of nodes under Global
Definitions added to the model.
• See Performing a Random Vibration Analysis for a detailed description
of how to study random vibration.
• The theory is described in Random Vibration Theory.
• Bracket — Random Vibration Analysis: Application Library path
Structural_Mechanics_Module/Tutorials/bracket_random_vibration
• Random Vibration Test of a Motherboard: Application Library path
Structural_Mechanics_Module/Dynamics_and_Vibration/
motherboard_random_vibration
• Random Vibration Analysis of a Deep Beam: Application Library
path Structural_Mechanics_Module/Verification_Examples/
random_vibration_deep_beam
Response Spectrum Analysis Study
Response spectrum analysis is used for computing an approximation of the structural
response to transient, nondeterministic events, such as earthquakes or shocks.
The Response Spectrum Analysis study is mainly an entry point when adding studies.
What you actually get when you add such study is an Eigenfrequency study step together
with a Response Spectrum node under Definitions.
The actual response is computed on demand during result evaluation, using the
computed eigenfrequencies and modes. The settings for the evaluation are done in the
Response Spectrum 2D and Response Spectrum 3D datasets.
STUDY TYPES
|
85
If your response spectrum evaluation requires inclusion of missing mass correction,
you need also to compute a set of stationary load cases. To set up that analysis, use the
Create missing mass correction study button (
) on the header of the Response
Spectrum section the in the Response Spectrum node settings.
• See Performing a Response Spectrum Analysis for a detailed
description of how to work with response spectrum evaluations.
• The theory is described in Response Spectrum Analysis Theory.
• The settings for the special datasets are described in Response
Spectrum 2D and Response Spectrum 3D in the COMSOL
Multiphysics Reference Manual.
• The Response Spectrum node is described in the COMSOL
Multiphysics Reference Manual.
• Earthquake Analysis of a Building: Application Library path
Structural_Mechanics_Module/Dynamics_and_Vibration/
building_response_spectrum
• Shock Response of a Motherboard: Application Library path
Structural_Mechanics_Module/Dynamics_and_Vibration/
motherboard_shock_response
86 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Selecting the Physics Interface
The structural mechanics products contain a number of physics interfaces for a wide
range of applications. This section contains some guidelines for how to select an
appropriate physics interface for your analysis.
The basic physics interfaces for structural mechanics are:
• Solid Mechanics — General modeling of solid objects with extension in all
directions.
• Elastic Waves, Time Explicit — For efficient analysis of linear elastic wave
propagation in solid domain.
• Shell and Plate — For objects which are thin in one direction, but have significant
bending stiffness
• Membrane — For objects which are thin in one direction, and have negligible
bending stiffness
• Beam — For objects where two directions have significantly smaller dimensions
than the third; significant bending stiffness
• Pipe Mechanics — For analysis of pipes with internal pressure. This interface is
similar to the Beam interface, but specialized for analysis of pipes.
• Truss — For objects where two directions have significantly smaller dimensions than
the third; only axial forces can be transmitted
• Wire — Similar to Truss, but only tensile forces can be transmitted
For a detailed overview of the functionality available in each product, visit
https://www.comsol.com/products/specifications/
Solid Mechanics
The Solid Mechanics interface offers the most general modeling of structural
mechanics problems and is based on general principles of continuum mechanics. It is
the interface which contains the largest number of material models, and the most
advanced boundary conditions.
SELECTING THE PHYSICS INTERFACE
|
87
The drawback with using solid elements is that the models can become
computationally expensive, especially in 3D. For structures which are thin or slender,
you should consider using one of the specialized physics interfaces.
3D SOLID GEOMETRY
The degrees of freedom (dependent variables) in 3D are the global displacements u, v,
and w in the global x, y, and z directions, respectively.
Figure 2-1: Loads and constraints applied to a 3D solid using the Solid Mechanics
interface.
2D GEOMETRY
Plane Stress
The plane stress variant of the 2D physics interface is useful for analyzing thin in-plane
loaded plates. For a state of plane stress, the out-of-plane components of the stress
tensor are zero.
Figure 2-2: Plane stress is used to model plates where the loads are only in the plane; it does
not include any out-of-plane stress components.
The 2D physics interface for plane stress allows loads in the x and y directions, and
assumes that these are constant throughout the material’s thickness, which can vary
with x and y. The plane stress condition prevails in a thin (compared to the in-plane
88 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
dimensions) flat plate in the xy-plane loaded only in its own plane and without any
z direction restraint.
Plane Strain
The plane strain variant of the 2D physics interface that assumes that all out-of-plane
strain components of the total strain tensor z, yz, and xz are zero.
Figure 2-3: A geometry suitable for plane strain analysis.
Loads in the x and y directions are allowed. The loads are assumed to be constant
throughout the thickness of the material, but the thickness can vary with x and y.
Formally, the plane strain condition requires that the ends of the object are constrained
in the z direction, but it is often also used for central parts of an object that is long in
the z direction (compared to the in-plane dimensions). One example is a long tunnel
along the z-axis where it is sufficient to study a unit-depth slice in the xy-plane.
Generalized Plane Strain
Generalized plane strain is similar to plane strain in the sense that transverse stresses
can develop in the 2D cross section of a long object. The requirement that the
out-of-plane strain is zero, is however relaxed. Instead, an assumption about zero
resulting force in the transverse direction is used. Optionally, assumptions about zero
bending moments over the cross section can be added. Generalized plane strain
conditions prevail in the inner parts of a long object with free ends. For many cases,
generalized plane strain conditions is the 2D approximation that is closest to a full 3D
solution.
For an in-depth discussion of different aspects of 2D solid mechanics, see
https://www.comsol.com/blogs/
what-is-the-difference-between-plane-stress-and-plane-strain
SELECTING THE PHYSICS INTERFACE
|
89
AXISYMMETRIC GEOMETRY
The axisymmetric variant of the Solid Mechanics interface uses cylindrical coordinates
r,  (phi), and z. All properties are independent of the azimuthal angle .
In the default version of the interface, displacements occur only in the rz-plane, and
there are two degrees of freedom, u and w. By selecting the Include circumferential
displacement option, you can model also torsion around the axis of rotational
symmetry. The azimuthal rotation degree of freedom v is then included. In addition,
many features, such as load features, allow values to be entered in the  direction.
The 2D axisymmetric geometry is viewed as the intersection between the original
axially symmetric 3D solid and the half plane   0, r  0. Therefore, the geometry is
drawn only in the half plane r  0, and it recovers the original 3D solid by rotating the
2D geometry about the z-axis.
Figure 2-4: Rotating a 2D geometry to recover a 3D solid.
• Axisymmetric Twist and Bending: Application Library path
Structural_Mechanics_Module/Verification_Examples/
axisymmetric_twist_and_bending
Elastic Waves, Time Explicit
The Elastic Waves, Time Explicit is used to compute the velocity and strain field in
solids with propagating linear elastic waves. In the Add Physics dialog, it is found in
the Acoustics branch, under Elastic Waves.
In general, the interface is suited for modeling the propagation of waves over large
distances relative to the wavelength, for example, ultrasound propagation for
nondestructive testing (NDT), or seismic waves. The interface exists in 2D
(generalized plane strain) and 3D.
90 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
The interface is based on the discontinuous Galerkin (dG or dG-FEM) method and
uses a time explicit solver. The method is very memory efficient and can solve problems
with many million degrees of freedom (DOFs). The method is also well suited for
distributed computing on clusters.
In the Acoustics Module User’s Guide:
• The Elastic Waves, Time Explicit Interface
• Theory for the Elastic Waves, Time Explicit Interface
Shell and Plate
The Shell interface is useful when the object is thin in one direction. Structures built
from welded or bolted flat plates are archetypal shell structures and so are pressure
vessels. The Shell interface is available in 3D and 2D axisymmetry.
The Plate interface is a specialization of the Shell interface, used for 2D modeling in
the XY-plane. A plate model has its main action in bending out of the plane, but can
optionally also treat in-plane forces. If the loads act only in the plane, using Solid
Mechanics with the Plane Stress option is a better choice.
Shells are modeled on boundaries, and the transverse direction is represented only by
the mathematical model. The degrees of freedom consist of displacements and
rotations at the modeled boundary. This results in an assumption where the in-plane
strains vary linearly through the thickness, and the stress in the thickness direction is
zero. The thickness of a shell does not have to be constant, although this is by far the
most common case.
When the Composite Materials Module is available, it is possible to model also
multilayered shells.
For nonlinear material models, a layered approach with a single layer is used. There is
a virtual mesh in the thickness direction, in order to accommodate the potential
variation of the material properties in the thickness direction.
Rather than computing the shell stiffness from material properties and thickness, you
can also directly enter that stiffness properties in tension, bending, and shear.
The Shell and Plate interfaces can be used both for “thin” and “thick” shells. Shear
deformations are taken into account; this is usually called Mindlin theory. The material
model is linear elastic.
SELECTING THE PHYSICS INTERFACE
|
91
When modeling with shells, it is important to keep track of “top” and “bottom” side
when applying loads and interpreting the results.
The in-plane stiffness of an elastic shell is proportional to the thickness h, while the
bending stiffness is proportional to h3. The difference in stiffness along different
directions can thus become very large. When an object is very thin, a shell model may
be numerically ill-posed due to the negligible bending stiffness. It is then better to use
the Membrane interface.
Membrane
The Membrane interface can be used for very thin objects, like cloth, where only
in-plane forces are important. Membranes can be considered as plane stress elements
but with an arbitrary, possibly curved configuration in space. The Membrane interface
is available in 3D and 2D axisymmetry.
In most applications, a membrane must be pretensioned in order to have a stable
configuration, so it will almost invariably be used in a geometrically nonlinear analysis.
The main exception is when it is used as a “cladding” on top of a solid, since it will
then be stabilized by the solid.
You can study configurations when there is local wrinkling in a membrane by adding
a special nonlinear material model.
In the Membrane interface a large number of different material models can be used.
When the Composite Materials Module is available, it is possible to model also
multilayered membranes.
Beam
A beam is an abstract model where only the extension in the axial direction is modeled
explicitly on an edge. The cross section is usually specified in terms of geometrical
properties such as area and moments of inertia. Several predefined cross-section types
are also available. The Beam interface is available in 3D and 2D.
The exact stress distribution in the beam is not explicitly modeled. It is actually not
even fully determined by the cross-sectional properties. Instead, six (in 3D) resultant
section forces are used: axial force, shear forces in two perpendicular directions, two
bending moments, and one twisting moment.
The Beam interface assumes linear elasticity.
92 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Two formulations are available in the Beam interface:
• The classical Euler–Bernoulli beam theory, which is applicable for slender beams.
• Timoshenko theory, where also shear deformations are considered. This theory
makes it possible to use the Beam interface to model rather thick beams.
Pipe Mechanics
Pipes are similar to beams, and many properties of the Pipe Mechanics interface are
shared with the Beam interface. The most distinguishing feature is that the internal
pressure usually causes a significant part of the stresses in a pipe. Also, temperature
gradients usually occur through the pipe wall, rather than across the entire section.
The loads from internal pressure and drag forces can be taken directly from results in
the Pipe Flow interface. Similarly, the temperature in the pipe walls can be taken from
the Heat Transfer in Pipes interface.
In the Pipe Flow Module User’s Guide:
• The Pipe Flow Interface
• The Heat Transfer in Pipes Interface
Truss
The Truss interface has two main purposes:
• Modeling of trusses, consisting of straight bars carrying only axial forces
• As reinforcements, used in conjunction with other physics interfaces
The Truss interface is available in 3D and 2D.
For a truss model, only one geometrical property is needed, the cross-section area. The
material model can be linear elastic, elastoplastic, or a shape memory alloy. There is also
a special material model for creating spring/damper data.
The truss element has no stiffness in the directions perpendicular to its extension. For
trusses, this is usually not a problem since they are designed such that each member is
stabilized by its neighbors.
SELECTING THE PHYSICS INTERFACE
|
93
Wire
The Wire interface intended for modeling of cables and wires. The structures are often
prestressed, but also cables sagging under, for example, self-weight can be modeled.
The main difference between the Truss interface and the Wire interface is that the
wires cannot sustain any compressive forces. In reality the wire will wrinkle.
Numerically, this is handled by using a very low stiffness in compression.
94 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Selecting Discretization
Shape Function Order
In structural mechanics analysis, the focus is often on the stresses and strains rather
than on the displacements. Since the strains are derivatives of the displacement field,
the accuracy of the strains will be one order less than the accuracy of the displacements.
For this reason, second-order shape functions are used as default in most of the
structural mechanics interfaces. Often this gives the best tradeoff between model size
and accuracy.
It is well known that using first-order shape functions in solid mechanics will give an
overly stiff solution, unless a very fine mesh is used. This is especially noticeable for
triangular and tetrahedral elements. This can, to some extent, be counteracted by using
reduced integration, see Using Reduced Integration.
If the purpose of the analysis is only to compute stiffness, rather than stresses, the use
of linear shape functions can still be justified. This is the default choice in the
Multibody Dynamics interface, available with the Multibody Dynamics Module.
If the solution contains discontinuities, for example when some type of front is moving
through the material, first-order elements and a fine mesh is often a good choice, since
the advantage of the higher-order elements lies in their ability to represent smooth
gradients.
TRUSS ELEMENTS
In the Truss interface the default is to use first-order shape functions, since the
elements are mainly used in a context where the axial force in each element is constant.
When truss elements share an edge with other structural elements, you should choose
the same discretization in both interfaces, usually quadratic.
BEAM ELEMENTS
The beam elements have only one set of shape functions, which cannot be changed.
The axial displacement and the twist are represented by first-order shape functions,
while the bending is represented by cubic Hermitian shape functions. This element can
then represent a constant axial force, a constant twisting torque, a linear bending
moment, and a constant shear force. This is the exact solution for a beam having no
distributed loads.
SELECTING DISCRETIZATION
|
95
A consequence of this formulation is that it may not possible to obtain a perfectly
conforming approximation if a beam shares an edge with elements from another
physics interface.
Lagrange and Serendipity Shape Functions
In the Solid Mechanics and Membrane interfaces, you can choose between two
families of shape functions: Lagrange and serendipity. The default is to use serendipity
shape functions.
The serendipity elements have the advantage of generating significantly fewer degrees
of freedom for structured meshes. The accuracy is in most cases almost as good as for
the Lagrange elements. The Lagrange elements are however less sensitive to strong
mesh distortions.
The serendipity shape functions differ from the Lagrange shape functions only for the
following element shapes:
• 2D: Quadrilateral elements of discretization order higher than 1
• 3D: Hexahedral, prism, and pyramid elements of discretization order higher than 1
In the COMSOL Multiphysics Reference Manual:
• The Lagrange Element (shlag)
• The Nodal Serendipity Element (shnserp)
When coupling two structural mechanics physics interfaces, the same type of shape
functions should be used in both interfaces to ensure conformity in displacement shape
functions. Since there is no difference between the two families of shape functions in
1D, this is not an issue when connecting edges.
Choosing Shape Functions in Multiphysics Models
In problems where several physics fields participate, the accuracy can sometimes be
improved by considering how the different fields interact. In structural mechanics, it
is common that other physics fields directly affect the inelastic strains. This is the case
in, for example, thermal expansion and hygroscopic swelling.
96 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
In thermal expansion, the elastic strain used in most constitutive relations is the
difference between the total strain, which is computed from derivatives of the
displacement field, and the thermal strain:
 el =  tot –  th =  tot –   T – T ref 
Since the thermal strain is directly proportional to the temperature, a consistent
approximation would be to use one step lower discretization order for the temperature
than for the displacements. When using built-in couplings, such as Thermal Expansion,
such a modification is not necessary. Any mismatch is automatically taken care of by
reinterpolating the thermal strains to an order that matches the general strain field.
Another type of coupling appears on the boundary between two domains having
different physics, as in Fluid–Structure interaction and Acoustic–Structure interaction.
When, for example, Thermoviscous Acoustics is coupled to Solid Mechanics, then the
time derivative of the displacement in the solid is set equal to the velocity in the
acoustic medium on the shared boundary. In this case, it makes sense to have the same
shape function order for these two fields.
Implicit Shape Function Orders
Some solid mechanics formulations contain other degrees of freedom in addition to
the displacements. The shape functions are then selected internally based on your
choice of displacement discretization.
VISCOELASTIC STRESS AND STRAIN
When using a viscoelastic material model, auxiliary degrees of freedom are added either
for the viscoelastic strains or the viscoelastic stresses, depending on whether a linear or
a nonlinear formulation is used. These degrees of freedom are local to the element, and
you can select either the discontinuous Lagrange or Gauss point data type.
The discontinuous Lagrange shape functions will have an order that is one below what
is used for the displacement shape functions.
If Gauss point data is used, the same integration points as used for the numerical
integration of the stiffness matrix are used. This order depends on the selected
displacement discretization order and whether reduced integration is used or not.
INELASTIC STRAINS
For material models like plasticity and creep, the inelastic strains are formally degrees
of freedom. They will be allocated at the same integration points as used for the
SELECTING DISCRETIZATION
|
97
numerical integration of the stiffness matrix. This order depends on the selected
displacement discretization order and whether reduced integration is used or not.
98 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Coupling Different Element Types
In this section:
• Introduction to the Element Types
• Coupling Techniques
Introduction to the Element Types
In some engineering structures, the optimal idealization is a mixture of different
element types. Some examples are:
• Structures that are thin in large regions, but more three-dimensional at certain
locations. A mixture of solids and shells can then significantly reduce the model size.
• Plates or shells having beams as stiffeners.
• Truss elements acting as reinforcement bars in a concrete structure.
• A thin layer of one material on top of another material. In this case, an idealization
with shells or membranes covering the boundary of a solid can be useful.
When several physics interfaces are added in COMSOL Multiphysics, the default is
always that each physics interface has individual and unique degrees of freedom. In
structural mechanics, the first physics interface has the displacement variables (u, v, w),
then the second physics interface has (u2, v2, w2), and so on. This means that the
physics interfaces initially are independent, even when defined on the same geometrical
part. To get the intended interaction requires that a coupling is established between
the physics interfaces.
Various methods to couple different element types are discussed in this section.
Coupling Techniques
The following basic techniques to connect physics interfaces with displacement
degrees of freedom are discussed in this section:
• Renaming Degrees of Freedom
• Using Customized Coupling Features
• Using General Coupling Operators
COUPLING DIFFERENT ELEMENT TYPES
|
99
RENAMING DEGREES OF FREEDOM
The easiest coupling method is to rename the displacement degrees of freedom so that
these are the same for all physics interfaces. This is sufficient, for example, when using
membranes as cladding on a solid boundary or truss elements as reinforcement bars in
a solid.
In the Beam, Pipe Mechanics, Shell, and Plate interfaces, the deformation is described
also by rotational degrees of freedom. In the general case, these degrees of freedom
interact with the translational degrees of freedom in a connection.
In some special cases — for example, when a thin shell acts as cladding on a solid — it
is sufficient to make the degree of freedom names for the displacements common; the
rotational degrees of freedom are not important. If, however, a shell edge is connected
to a solid, it acts as a “hinge”, which in most cases is not the intended behavior. You
then need to use the more sophisticated techniques described next.
The default shape functions in the Solid Mechanics interface are of the
serendipity type, whereas Lagrange shape functions are used in the Shell
interface. If you are placing a shell element on the boundary of a solid
element, you must select Lagrange shape functions also in the Solid
Mechanics interface so that the two physics interfaces share the same node
points.
The shape functions used in the Beam and Pipe Mechanics interfaces have
special properties, and a beam cannot have the same degrees of freedom
as another physics interface if the same edge is shared.
Also, the representation of rotations differs between the Shell and Plate
interfaces (displacement of normal) and the Beam and Pipe Mechanics
interfaces (rotation angle). It is therefore not possible to use common
degree of freedom names for the rotational degrees of freedom.
USING CUSTOMIZED COUPLING FEATURES
There are a number of built-in couplings, by which you can add connections that are
nontrivial to set up manually:
• Shell Edge to Solid Boundary (3D)
• Shell Boundary to Solid Boundary (3D)
• Membrane Boundary to Solid Boundary (3D)
100 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
• Beam Point to Solid Boundary (2D)
• Beam Point to Solid (3D)
• Beam Edge to Solid Boundary (2D)
• Beam Edge to Solid Boundary (3D)
• Beam Edge to Shell Edge (3D)
• Beam Point to Shell Boundary (3D)
• Beam Point to Shell Edge (3D)
• Pipe Point to Solid Boundary (3D)
• Pipe Point to Shell Edge (3D)
• Embedded Reinforcement
Shell Edge to Solid Boundary (3D)
A shell can be coupled to a solid by adding a Solid–Thin Structure Connection
multiphysics coupling. In the settings, set Connection type to Solid boundaries to shell
edges. This situation typically occurs when you want to make a transition from a thin
region to one that is thicker. Usually, shell assumptions should be valid on both sides
of the transition. The solid geometry is expected to have the same thickness as the
thickness given in the Shell interface.
You can choose between two different formulations, by setting Method to either Rigid
or Flexible. The flexible version is significantly more accurate locally at the connected
solid boundary, but it comes with a cost in terms of some extra degrees of freedom.
Also, this method requires a large enough number of degrees of freedom in the
thickness direction of the solid. For second-order elements, typically three elements are
required.
Shell Boundary to Solid Boundary (3D)
A shell can also be coupled to a solid by adding a Solid–Thin Structure Connection
multiphysics coupling with Connection type set to Shared boundaries or Parallel
boundaries. This connection is used to add a shell on top of a solid as a ‘cladding’. It is
possible to include an offset distance. The boundaries may be coincident or parallel.
Membrane Boundary to Solid Boundary (3D)
A membrane can be coupled to a solid by adding a Solid–Thin Structure Connection
multiphysics coupling with Connection type set to Shared boundaries. When the thin
structure is a membrane, this is the only available connection type. It is used to add a
membrane on top of a solid as a ‘cladding’.
COUPLING DIFFERENT ELEMENT TYPES
|
101
Beam Point to Solid Boundary (2D)
A beam in 2D can be coupled to a solid by adding a Solid–Beam Connection
multiphysics coupling. In the settings, set Connection type to Solid boundaries to beam
points. This connection is intended for modeling a transition from a beam to a solid,
where beam assumptions are valid on both sides of the connection.
You can choose between two different formulations, by setting Method to either Rigid
or Flexible. The flexible version is significantly more accurate locally at the connected
solid boundary, but it comes with a cost in terms of some extra degrees of freedom.
Also, this method requires a large enough number of degrees of freedom in the
thickness direction of the solid. For second-order elements, typically three elements are
required.
Beam Point to Solid (3D)
A beam in 3D can be coupled to a solid by adding a Solid–Beam Connection
multiphysics coupling. In the settings, set Connection type to either Solid boundaries to
beam points, general. or Solid boundaries to beam points, transition. These two
couplings are fundamentally different.
The Solid boundaries to beam points, general connection is used for modeling a beam
with one end “welded” to the face of the solid. You can specify the size of the area on
the solid boundary that is connected to the endpoint of the beam in several different
ways.
The Solid boundaries to beam points, transition coupling is intended for modeling a
transition from a beam to a solid where beam assumptions are valid on both sides of
the connection. Thus, the geometry of the solid at the transition should match the
cross-section data given to the beam.
This connection type can include warping of the solid cross section. In order to
compute the warping properties, an extra PDE is solved over the cross-section
boundaries. To improve the performance, you should preferably solve for these
variables once in a separate stationary study or study step. In that study step, clear all
physics interfaces except the Solid–Beam Connection multiphysics coupling in the Physics
and Variables Selection section.
You can manually control whether to include warping or not. If not included, the setup
of the solver sequence is simplified, but there will be significant stress disturbances
close to the connection boundaries if the cross section is susceptible to warping.
There are four warping variables: one named Warping function and three named
Warping constant. In the successive study steps, you need to manually suppress
102 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
them. You can do so under the Dependent Variables node, where you first set Defined
by study step to User Defined. Then, for each of these four variables, clear the Solve for
this field check box.
Beam Edge to Solid Boundary (2D)
A beam in 2D can also be coupled to a solid by adding a Solid–Beam Connection
multiphysics coupling with Connection type set to Shared boundaries or Parallel
boundaries. This connection is used for adding a beam on top of a solid as a “cladding”.
It is possible to include an offset distance. The boundaries may be coincident or
parallel.
Beam Edge to Solid Boundary (3D)
A beam in 3D can also be coupled to a solid by adding a Solid–Beam Connection
multiphysics coupling with Connection type set to Solid boundaries to beam edges. This
connection is used for adding a beam that is “welded” along the surface of the solid.
Beam Edge to Shell Edge (3D)
A beam can be coupled to a shell by adding a Shell–Beam Connection multiphysics
coupling with Connection type set to either Shared boundaries or Parallel boundaries.
This connection is used for adding beams as stiffeners to shells. The edges may be
coincident or parallel. It is possible to prescribe that the beam has an offset from the
shell when a coincident edge is used.
Beam Point to Shell Boundary (3D)
A beam can be coupled to a shell by adding a Shell–Beam Connection multiphysics
coupling with Connection type set to Shell boundaries to beam points. This connection
is used for modeling a beam with one end “welded” to the face of the shell. You can
specify the size of the area on the shell boundary that is connected to the end point of
the beam in several different ways.
Beam Point to Shell Edge (3D)
A beam can be coupled to a shell by adding a Shell–Beam Connection multiphysics
coupling with Connection type set to Shell edges to beam points. This connection is
used for modeling a beam with one end “welded” to the edge of the shell. You can
specify the part of the shell edge that is connected to the end point of the beam in
several different ways.
Pipe Point to Solid Boundary (3D)
A pipe in 3D can be coupled to a solid by adding a Structure–Pipe Connection
multiphysics coupling. The coupling is intended for modeling a transition from a pipe
to a solid where beam assumptions are valid on both sides of the connection. Thus, the
COUPLING DIFFERENT ELEMENT TYPES
|
103
geometry of the solid at the transition should match the cross-section data given to the
pipe. The connection assumes that the pipe cross section is circular; if another cross
section is used, it is converted to an equivalent circular cross section. This means that
warping is not considered.
The connection can be considered an extension of the Solid boundaries to beam points,
transition coupling in Solid–Beam Connection to also account for radial deformation
of the pipe caused by the fluid pressure and the temperature difference over the cross
section.
Pipe Point to Shell Edge (3D)
A pipe in 3D can be coupled to a shell by adding a Structure–Pipe Connection
multiphysics coupling. The coupling is intended for modeling a transition from a pipe
to a shell where beam assumptions are valid on both sides of the connection. Thus, the
geometry of the shell at the transition should match the cross-section data given to the
pipe. The connection assumes that the pipe cross section is circular; if another cross
section is used, it is converted to an equivalent circular cross section. This means that
warping is not considered.
The connection can be considered an extension of the Shell edges to beam points
coupling in Shell–Beam Connection to also account for radial deformation of the pipe
caused by the fluid pressure and the temperature difference over the cross section.
Embedded Reinforcement
Lower dimension structural elements can be connected to a solid domain by adding
an Embedded Reinforcement multiphysics coupling. This connection supports
coupling truss, wire, beam, and membrane elements to a Solid Mechanics interface.
The connection can either be rigid, or made by attaching springs between points on
the embedded structure and points in the solid. A more detailed discussion about this
type of modeling is given in Modeling Embedded Structures and Reinforcements.
The underlying theory and more details about the built-in couplings can
be found in
• Connection Between Shells and Solids
• Connection Between Shells and Beams
• Embedded Elements
104 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
• Examples of all types of couplings between shells and beams are shown
in Connecting Shells and Beams: Application Library path
Structural_Mechanics_Module/Beams_and_Shells/shell_beam_connection
• An example of couplings between shells and solids is shown in
Connecting Shells and Solids: Application Library path
Structural_Mechanics_Module/Beams_and_Shells/shell_solid_connection
• An example of couplings between beams and solids is shown in
Connecting Beams and Solids: Application Library path
Structural_Mechanics_Module/Beams_and_Shells/beam_solid_connection
USING GENERAL COUPLING OPERATORS
The most general method of connecting parts modeled with different physics
interfaces is by using a General Extrusion operator. In this case the parts need not even
be in contact, so the connection is an abstraction.
An example could be a shell stiffened by beams. In practice, you would probably use
the built-in coupling described in Beam Edge to Shell Edge (3D) for this case, but the
example shows the principles.
In structure like this, the beam is usually placed at one side of the shell, so that the
centerline of the beam and the midsurface of the shell do not coincide. This difference
COUPLING DIFFERENT ELEMENT TYPES
|
105
must be taken into account, so the edges representing the beam are geometrically
disconnected from the midsurface of the shell.
Beam centerline
Mathematically, the connection between the beam and the shell can be expressed as

 u beam = u shell +    X beam – X shell 

  beam =  shell

or equivalently as

 u beam = u shell +   X beam – X shell   n a

  beam =  shell

Here,  is the rotation vector, which contains the rotational degrees of freedom in the
Beam interface. The rotation vector is also available as a variable in the Shell interface,
where it is derived from the rotational degrees of freedom a. The shell normal is
denoted by n. Small rotations are assumed.
To create the coupling:
1 Add a General Extrusion node under Definitions>Nonlocal Couplings. Select the line on
the shell midsurface as source. Enter data in the Destination Map.
106 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
2 Add a Prescribed Displacement/Rotation node in the Beam interface and select the
corresponding edge.
3 Enter data for the prescribed displacements and rotations, for example
genext1(u)+genext1(shell.thy)*zdist, where zdist is some expression
defining the distance from the beam axis to the shell midsurface.
Because a shell does not have a valid rotation degree of freedom around
its normal, the rotation of the beam should not be connected in that
direction.
In the COMSOL Multiphysics Reference Manual:
• Nonlocal Couplings and Coupling Operators and General Extrusion
• About Nonlocal Couplings
COUPLING DIFFERENT ELEMENT TYPES
|
107
Applying Loads
An important aspect of structural analysis is the formulation of the forces applied to
the modeled structure. You can use custom expressions, predefined or user-defined
coordinate systems, and even variables from other modeling physics interfaces.
Loads can be applied in the structural mechanics interfaces on the body, face, edge, or
point levels. You can also apply loads to special features like Rigid Material or Rigid
Connector. There is also an option to apply point loads to given coordinates, which do
not have to coincide with a geometrical point or a mesh node.
In this section:
• Units, Orientation, and
Visualization
• Acceleration Loads
• Load Cases
• Temperature Loads — Thermal
Expansion
• Singular Loads
• Hygroscopic Swelling
• Moments in the Solid Mechanics
Interface
• Total Loads
• Pressure
• Variables for Loads
• Loads with a Spatial Variation
Units, Orientation, and Visualization
USING UNITS
Enter loads in any unit, independently of the base SI unit system in the model, because
COMSOL automatically converts any unit to the base SI unit system. To use the
feature for automatic unit conversion, enter the unit in square brackets, for example,
100[lbf/in^2].
The exception is random vibration analysis. In that case, no automatic unit conversions
are available, so you must enter loads in the base units of the model.
PREDEFINED AND CUSTOM COORDINATE SYSTEMS
In this module, different predefined coordinate systems are available when materials or
boundary conditions are specified. There is always the global coordinate system.
Depending on the dimensionality of the part being worked with, there can also be
108 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
predefined coordinate systems such as the local tangent and normal coordinate system
for boundaries.
Custom coordinate systems are also available and are useful, for example, to specify a
load in any direction without splitting it into components. From the Definitions
) from the menu.
toolbar, select a Coordinate System (
Some coordinate systems can have solution dependent axis directions. If
you use such a system for defining a load, the directions of the load follow
the moving coordinate axis directions if the Include geometric nonlinearity
check box is selected under the Study settings section of the current study
step.
VISUALIZATION
If you have switched on the physics symbols (see Displaying Physics Symbols in the
Graphics Window — An Example in the COMSOL Multiphysics Reference Manual),
then an applied load is indicated by a symbol together with a coordinate system
indicator displaying the definition directions for the load. The actual direction or
magnitude of the load you enter is not, however, reflected by the symbol. As a load in
COMSOL Multiphysics can be a function of parameters, variables, the solution, or
results from other physics interfaces, it is not possible to display it with only the
information available in the individual load feature.
Once you have turned on the physics symbols for a certain physics interface, you can
fine-tune the display. Every feature which has associated physics symbols will now have
a check box Show physics symbols, by which you can control the display of the symbols
for that specific feature.
Loads are among the results for which predefined plots are generated, so you will
always have access to a visual feedback of the loads after the solution. How to work
with the default load plots is described in detail in the Plotting Applied Loads section.
Sometimes, especially if you have entered complicated load expressions in a large
model, it is important to inspect the load distribution before you run the analysis. You
will then need to generate a dataset and the predefined plots. The fastest way to do that
APPLYING LOADS
|
109
is to click Get Initial Value in the Study toolbar. Note that if you change the loads, you
will have to delete the dataset and generate it again.
In the COMSOL Multiphysics Reference Manual:
• Physics Symbols
• Using Units
• Coordinate Systems
• Plotting Applied Loads
For an example showing how to examine the load distribution, see
Bracket — Static Analysis: Application Library path
Structural_Mechanics_Module/Tutorials/bracket_static. This is also the first
example used in the Introduction to the Structural Mechanics Module.
Load Cases
For a Stationary or Frequency Domain study, you can define load cases and constraint
cases. Any load or constraint can be assigned to a load or constraint group, and then
be used conditionally.
For most load types, the load case acts as a simple multiplier, but some cases need a
more detailed discussion:
• A Prescribed Displacement or Prescribed Displacement/Rotation node can be assigned
both a constraint group and a load group. You can use the constraint group to
switch on and off the whole constraint. The load group acts as a multiplier to any
nonzero prescribed values of displacement and rotations, and will not have any
effect unless the constraint is active.
• When a load case multiplier is used for Thermal Expansion, the multiplier is applied
not to the actual temperature, but to the difference between the temperature and
the strain free reference temperature. The temperature difference, and thus the
thermal strain, is proportional to the load case multiplier.
• Since Thermal Expansion nodes are exclusive (only the last one given gives a
contribution for a certain domain), you cannot switch between different Thermal
Expansion nodes only by assigning them to different load cases.
• Hygroscopic Swelling behaves analogously to Thermal Expansion.
110 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
• For External Stress, the given stress values are multiplied by the load case multiplier.
• A Spring Foundation or Thin Elastic Layer node can be assigned a constraint group,
which you can use to switch the whole boundary condition on and off. If there is
also a Predeformation subnode, then you can assign a load group to that subnode.
The prescribed predeformation is then multiplied by the load case multiplier.
Predeformation nodes are exclusive, you cannot switch between them by assigning
them to different load cases.
• A Rigid Connector can be assigned both a constraint group and a load group. You can
use the constraint group to switch off the prescribed displacements and rotations.
The load group acts as a multiplier to nonzero prescribed values of displacement and
rotations.
• If you have added Applied Force or Applied Moment nodes under a Rigid Connector,
you can assign individual load groups to these nodes.
• If you have added Applied Force or Applied Moment nodes under a Rigid Material, you
can assign individual load groups to these nodes.
Any expression that acts purely as a load, that is, contributes only to the
right-hand side of the system of equations, can be part of the load case
handling. This is true even if, for example, the corresponding feature does
not have a setting for load cases, or if it is a contribution you have created
using equation based modeling.
To do this, you can modify any such expression expr to
if(group.<lgName>,group.<lgName>*expr). Here, <lgName> is the
parameter name you have chosen in the settings for the load group.
In most cases, the expression group.<lgName>*expr is sufficient. The
only reason to use the longer version with the if() statement if you want
to avoid that expr is evaluated for load cases in which it is not used.
For example, if you have a boundary load which partially is always active,
and partially is conditional, you can write 20[MPa]+group.lg1*10[MPa]
in the input field for the pressure.
In particular, this approach is useful for features that override each other,
like Thermal Expansion, since you can then accommodate several load
cases in a single node in the Model Builder.
APPLYING LOADS
|
111
In the COMSOL Multiphysics Reference Manual:
• About Load Cases
• Defining Load Groups and Constraint Groups
• Load Group
• Constraint Group
For an example about how to set up expressions for controlling position
and distribution of loads using load cases, see Tapered Cantilever with
Two Load Cases: Application Library path COMSOL_Multiphysics/
Structural_Mechanics/tapered_cantilever.
Singular Loads
In reality, loads always act on a finite area or over a volume. However, in a model loads
are sometimes defined on points or edges, which leads to a singularity. The reason for
this is that points and lines have no area, so the stress becomes infinite. Because of the
stress singularity, there are high stress values in the area surrounding the applied load.
The size of this area and the magnitude of the stress depend on both the mesh and the
material properties. The stress distribution at locations far from these singularities is
unaffected according a to a well-known principle in solid mechanics, the St. Venant’s
principle. It states that for an elastic body, statically equivalent systems of forces
produce the same stresses in the body, except in the immediate region where the loads
are applied.
Figure 2-5 shows a plate with a hole in plane stress loaded with a distributed load and
a point load of the same magnitude. The mesh consists of triangular elements with
quadratic shape functions. The high stress around the point load is dissipated within
the length of a few elements for both mesh cases. The stresses in the middle of the plate
and around the hole agree for the distributed load and the point load. The problem is
that due to the high stress around the singular load it is easy to overlook the high stress
region around the hole. When the point load is applied, the range must be manually
set for the stress plot to get the same visual feedback of the high stress region around
the hole in the two cases. This is because the default plot settings automatically set the
range based on the extreme values of the expression that is plotted.
Despite these findings it is good modeling practice to avoid singular loads because it is
difficult to estimate the size of the singular region. In the Structural Mechanics
112 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Module, it is possible to define loads on all boundary types. However, avoid singular
loads altogether with elastoplastic or creep materials.
The Plasticity and Creep nodes are available as a subnode to Linear Elastic
Material nodes with the Nonlinear Structural Materials Module or the
Geomechanics Module.
normal mesh size
finer mesh size
Figure 2-5: A plate with a hole subject to a distributed load (left) and a point load (right).
For more details about singularities, see also
https://www.comsol.com/blogs/
singularities-in-finite-element-models-dealing-with-red-spots/
https://www.comsol.com/blogs/
applying-and-interpreting-saint-venants-principle/
APPLYING LOADS
|
113
Moments in the Solid Mechanics Interface
The Solid Mechanics interface, as opposed to the Beam, Pipe Mechanics, Plate, and
Shell interfaces, does not have rotational degrees of freedom. This makes the direct
specification of moment loads somewhat more complicated. To specify moments, you
can attach a Rigid Connector to the loaded area. The rigid connector has rotational
degrees of freedom, and it is possible to apply moments directly. For load application,
the flexible formulation of the rigid connector is particularly useful, since it avoids
artificial stiffening of the boundary where the load is applied.
Pressure
A pressure is a load acting toward the normal of a face of the structure. If there are
large deformations in the model and the Include geometric nonlinearity check box is
selected under the Study settings section of the current study step, the pressure acts as
a follower load. The pressure is then defined with respect to the geometry and, as the
geometry deforms locally, the orientation of the load changes. The size of the loaded
area can also change as an effect of straining.
Acceleration Loads
Within the structural mechanics interfaces, you will find four different types of loads
to describe acceleration loads:
• Gravity
• Base Excitation
• Rotating Frame
• Linearly Accelerated Frame
The two first nodes have are of a global type. They will be applied to all features in the
physics interface, and cannot have a spatial variation.
The Rotating Frame and Linearly Accelerated Frame nodes have a domain selection. They
can be applied selectively, and also depend on the coordinates. When applied to a set
of selected domains, such loads are applied also to lower dimensional objects, for
example, a point mass or an added mass on an edge.
All acceleration loads share the property that they are not applied to mass contributions
that belong to global features such as rigid connectors. There, you must add loads
explicitly.
114 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
When a structure is subjected to an acceleration which is applied to all its support
points, then it often more convenient to replace the support acceleration by an
acceleration force, using a Base Excitation node. In particular, this is necessary when
using modal based dynamic analyses, in which nonzero prescribed displacements
cannot be used. Changing to a frame acceleration load does not affect the distribution
of forces and stresses. It will however imply that displacements, velocities, and
accelerations are measured relative to the supports, and not relative to a room fixed
coordinate system. The Base Excitation node does however also define absolute
acceleration variables, which are what would be measured by an accelerometer.
Temperature Loads — Thermal Expansion
When performing thermal expansion analysis, temperature loads are specified by
entering a temperature and a reference temperature in a thermal expansion subnode
which is available from the context menu (right-click the parent node, a Linear Elastic
Material node, for example) or from the Physics toolbar, Attributes menu. Enter a
constant temperature or an analytic expression that can depend on the coordinates or
dependent variables. For beams, plates, and shells it is also possible to specify bending
temperature loads. More details are available in the descriptions for each physics
interface.
When a separate physics interface is used to model heat transfer in the material, the
entry for the temperature is the dependent variable for the temperature from that
physics interface, typically T. In most cases, possible temperature variables from other
physics interfaces can be directly selected from a list.
• For more information about how to couple heat transfer analysis with
structural mechanics analysis, see Thermal-Structure Interaction. This
module also includes The Thermal Stress, Solid Interface.
• For a detailed discussion about thermal effects in structural mechanics
models, see Thermally Coupled Problems.
Hygroscopic Swelling
Some materials have the capability to absorb significant amounts of moisture through
diffusion processes. Changes in the moisture content may then cause volume changes.
To include the effects of hygroscopic swelling, the Hygroscopic Swelling subnode is
available from the context menu (right-click the parent node, Linear Elastic Material
APPLYING LOADS
|
115
node, for example) or from the Physics toolbar, Attributes menu. Enter a constant
concentration or an analytic expression that can depend on the coordinates or
dependent variables. For beams, plates, and shells it is also possible to specify bending
swelling loads caused by concentration gradient in the transverse direction. More
details are available in the descriptions for each physics interface.
When a separate physics interface is used to model the moisture diffusion in the
material, the entry for the concentration is the dependent variable for the
concentration from that physics interface, typically c. In most cases, possible
concentration variables from other physics interfaces can be directly selected from a
list.
The diffusion of the moisture into the material also adds to the mass density. You can
choose to automatically include this effect in a dynamic analysis, and also in mass
proportional loads, such as gravity and rotating frame loads.
Total Loads
You can specify a load either as a distributed load per unit length, area, or volume, or
as a total force to be distributed on a boundary. In the case of a total load, the applied
distributed load is the given load divided by the area (or length, or volume) on which
its acts. Thus, entering a total load is usually only meaningful when its orientation is
given by a Cartesian coordinate system.
Loads with a Spatial Variation
Since you can write any type of expression in an input text field, it is easy to describe
loads having a spatial variation.
HYDROSTATIC LOAD
Hydrostatic loading is a common special case of spatial variation. In this case, there is
often a fluid surface, above which there is no load. Such a load you can describe with
an expression like if(Z<ZSurf,rhoFluid*g_const*(ZSurf-Z),0). Here, ZSurf
and rhoFluid are assumed to be parameters containing the Z-coordinate of the fluid
surface and the mass density of the fluid respectively.
LOADS WITH A FAST SPATIAL VARIATION
If a load has a spatial variation which is fast relative to the element size, you may need
to increase the accuracy of the numerical integration used to compute the load
contribution. As a default, a load which varies no faster than the polynomial order of
116 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
the displacement shape functions can be integrated exactly. To change the integration
order, enable Equation View. In the Equation View node under the current load node
in the Model Builder tree, you can then increase the integration order.
The local stress state within the loaded element is still limited by what can be described
by the shape functions, but the total load applied on the structure will be more
accurate it you increase the integration order.
TRAVELING LOADS
Loads that are moving along the structure with time can be modeled using an
expression X-v*t, where v is the velocity of the load. The mesh independent point
load of the type Point Load, Free is particularly well suited for this type of modeling. If
a distributed load is modeled using this approach, it is often necessary to increase the
integration order as discussed in the previous section, since the load patch will typically
cover partial element faces.
Variables for Loads
Each node in which a load is given, such as Boundary Load or Point Load, creates a
number of variables which you have access to, for example during postprocessing.
These variables have standardized names. The names are constructed using the
following pattern: <phys>.<loadTag>_<loadType>_<geom><dir>, for example
solid.bndl1.F_Ax.
TABLE 2-4: THE LOAD VARIABLE NAMING SCHEME.
DESCRIPTION
EXAMPLES
<phys>
Physics interface tag
solid, truss2
<loadTag>
Tag of the load feature
bndl1, el2
<loadType>
Force or moment
F (force)
<geom>
The type of object to which
the load is applied
M (moment)
P (point)
L (line)
A (area)
V (volume)
<dir>
Orientation
x, y, z, r (vector
components)
_Mag (magnitude of
the vector)
APPLYING LOADS
|
117
For loads which are do not have a geometrical selection, such as loads on Rigid
Connector and Rigid Material, the _<geom> part of the name is omitted. As an example,
a load created through an Applied Force node under a Rigid Connector, is contained in
a variable such as solid.rig2.rf4.Fy.
118 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Defining Constraints
Defining the proper constraints for structural mechanics models is just as important as
defining the loads as together they make up the model boundary conditions. There are
many useful predefined physics features to define the constraints or to create
user-defined expressions that define constraints.
In this section:
• Rigid Body Motion
• Orientation
• Prescribed Displacements, Velocities, and Accelerations
• Symmetry Constraints
• Elemental and Nodal Constraints
• Suppressing Constraints on Lower Dimensions
• Kinematic Constraints
• Rotational Joints
• Attachments
Rigid Body Motion
In most cases, a structure must have a set of constraints which is sufficient to suppress
any rigid body motions. A stationary problem is solvable only if the structure is
sufficiently constrained. There must not be any possible rigid body modes. Thus, no
stress-free deformation states are allowed. In a dynamic analysis, rigid body motions
are admissible. The inertial forces will then balance the external forces.
The number of possible rigid body modes for different geometrical dimensions is
shown in the table below.
TABLE 2-5: NUMBER OF POSSIBLE RIGID BODY MODES.
DIMENSION
NUMBER OF RIGID BODY MODES
3D
6 (3 translations + 3 rotations)
2D axisymmetric
1 (Z-direction translation)
2D (solid, beam, truss)
3 (2 translations + 1 rotation)
2D (plate)
3 (1 translation + 2 rotations)
DEFINING CONSTRAINTS
|
119
If the model is under constrained, you may encounter the following problems:
• The solver reports that the stiffness matrix is singular.
• The solver reports that the stiffness matrix is ill-conditioned. Theoretically, the
matrix is singular for a structure with rigid body modes, but because of the roundoff
errors during the solution this is not exactly determined.
• A nonlinear analysis fails to converge.
• An iterative linear equation solver fails to converge.
• You get a solution with an extremely large displacement, orders of magnitude larger
than what is expected.
For a single body, it is seldom difficult to see whether it is fully constrained or not, but
for a more complex assembly, including several physics interfaces, or advanced
couplings and boundary conditions, it may not be trivial. If you suspect that rigid body
modes are a problem in your model, you can run an eigenfrequency analysis, and check
for modes with zero eigenfrequency as described in Eigenfrequency Analysis.
If there are no constraints which are dictated by the physical boundary conditions of
the structure, you can use the Rigid Motion Suppression feature to automatically
remove the rigid body motions. When you do this, the assumption is that the external
loads are in equilibrium. If not, reaction forces and stress concentrations will appear at
seemingly arbitrary points where the automatic constraints were placed.
As an alternative to applying constraints, you can also add elastic supports through a
Spring Foundation node to suppress rigid body motion.
Rigid Motion Suppression in the Structural Mechanics Theory chapter.
Orientation
You can specify constraints in global as well as in any previously defined local
coordinate system.
Coordinate Systems in the COMSOL Multiphysics Reference Manual
120 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Prescribed Displacements, Velocities, and Accelerations
The most fundamental constraint is the prescribed displacement, where the individual
components of displacement or rotation can be prescribed to zero or nonzero values
for points, edges, boundaries, or domains.
For dynamic analysis, you can also directly prescribe the velocity or acceleration. The
conditions for prescribing displacements, velocities, or accelerations are mutually
exclusive for the same geometrical object since they prescribe the same degree of
freedom.
FREQUENCY DOMAIN
In frequency domain, a prescribed velocity vp or prescribed acceleration ap can be
directly interpreted as a prescribed displacement up:
v
u p = -----pi
–a
u p = --------p2

where  is the angular frequency.
A prescribed velocity with zero phase is assumed to have its peak at the
reference phase. As an effect, the corresponding peak displacement is
shifted by 90°. Similarly, a positive prescribed acceleration with zero phase
corresponds to a negative value of the displacement.
These definitions are particularly important if you mix prescribed velocity
or acceleration conditions with other boundary conditions.
TIME DOMAIN
In the case of a time-dependent analysis, the prescribed displacement is obtained as
t

u p  t  = u 0  t 0  + v p    d
t0
or
DEFINING CONSTRAINTS
|
121




u p  t  = u 0  t 0  + v 0  t 0  + a p    d d



t0 
t0
t


where u0 and v0 are is given by the initial conditions. It is not possible to set explicit
initial conditions, but if initial values are taken from a previous study, they will be
respected. In order to compute the integrals, up is introduced as a separate degree of
freedom which is solved for by adding an extra ODE.
As prescribing the velocity or acceleration in time domain comes with an extra cost,
you should always consider using a prescribed displacement instead. As long as the
time history of the velocity or acceleration is a known a priori and does not depend on
the solution itself, this is possible.
• When the velocity or acceleration has a simple time dependence, you can integrate
it analytically one or two times to obtain the displacement, and directly prescribe the
displacement instead.
• When you have complicated known velocity or acceleration histories, for example
from measurements, you can use the integrate() operator. In this case, you enter
the prescribed displacement as integrate(my_data(tau),tau,0,t). Here
my_data is the measured data as function of time, and tau is a dummy integration
variable
When a local coordinate system is used for prescribing a prescribed velocity or
acceleration, the axis directions must be fixed in space. As an example, you cannot use
a Boundary System rotating with the deformation.
STATIONARY ANALYSIS
In a stationary analysis, the prescribed velocity and acceleration nodes can have two
different behaviors. As a default, they are ignored, but you can also select that the
degrees of freedom having a prescribed velocity or acceleration in a dynamic analysis
should be constrained to zero in a static analysis.
Symmetry Constraints
In many cases symmetry of the geometry and loads can be used to your advantage in
modeling. Symmetries can often greatly reduce the size of a model and hence reduce
the memory requirements and solution time. When a structure exhibits axial
symmetry, use the axisymmetric physics interfaces. A solid that is generated by rotating
a planar shape about an axis is said to have axial symmetry. In order to make use of
122 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
the axisymmetric physics interfaces, all loads and constraints must also be the same
around the circumference.
For other types of symmetry, use the predefined symmetry and antisymmetry
constraints. This means that no expressions need to be entered — instead just add the
type of constraint to apply to the model.
Physics Interface Axial Symmetry Node in the COMSOL Multiphysics
Reference Manual
If the geometry exhibits two symmetry planes (Figure 2-6), model a quarter of the
geometry by using the Symmetry node for the two selected surfaces.
Symmetry planes
Apply symmetry constraints
Figure 2-6: If the geometry exhibits two symmetry planes, model a quarter of the geometry
by using the Symmetry feature for the two selected surfaces.
Both geometric symmetry and loads are important when selecting the
correct constraints for a model.
In an eigenfrequency or buckling analysis, the eigenmodes might be
nonsymmetric even if the structure is symmetric.
Figure 2-7 shows symmetric and antisymmetric loading of a symmetric geometry.
When modeling half of the geometry, the correct constraint for the face at the middle
DEFINING CONSTRAINTS
|
123
of the object would be Antisymmetry in the case of antisymmetric loading and
Symmetry in the case of symmetric loading of the object.
Symmetry plane
Antisymmetry plane
Figure 2-7: Symmetry plane (left) and antisymmetry plane (right).
SYMMETRY IN 2D AXISYMMETRY
In an axisymmetric model, the only possible symmetry is when the symmetry plane is
normal to the Z-axis. For models in 2d axisymmetry, the Symmetry Plane node is used
for prescribing this type of symmetry.
Antisymmetry cannot exist in this case.
TRANSLATION OF THE SYMMETRY PLANE
In some situations, you may want to use a symmetry condition, in which the symmetry
boundary actually can move along its normal. This may for example the case when you
use symmetry conditions to terminate your modeled region even though the situation
is not truly symmetric. The best approximation may then be that the boundary remains
planar, but that there is no resultant reaction force from the boundary condition.
You can modify the symmetry condition, so that it can translate in various ways by
using the controls in the Normal Direction Condition section of the settings for the
Symmetry constraint. You can model the following cases:
• Reaction force free translation.
• Prescribed total force acting on the constrained part.
• The displacement in the normal direction is prescribed.
124 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Note that allowing translation in the symmetry constraint is only meaningful if the
geometry selection corresponds to a single symmetry plane.
For an example showing how to force a boundary to remain plane, but
still allow it to translate in its normal direction using this special version
of Symmetry, see Thermo-Mechanical Analysis of a Surface-Mounted
Resistor: Application Library path Structural_Mechanics_Module/
Thermal-Structure_Interaction/surface_resistor.
Symmetry Condition with Translation in the Structural Mechanics
Theory chapter.
Elemental and Nodal Constraints
For most constraints, you can select between using elemental and nodal constraints.
To do this, select Advanced Physics Options, so that the Constraint Settings section is
displayed.
When using nodal constraints, one constraint is generated for each node within the
selection a certain constraint feature. With elemental constraints, the number of
constraints added at a node equals the number of elements connected to that node.
This means that if some values used in the constraints differ between the elements,
then different constraints will be generated by the elemental method, whereas with the
nodal method an average is computed at the node before adding the constraint.
When several constraints are present at a node, the internal constraint elimination
algorithm is responsible for reducing them to a minimum unique set. Using elemental
constraints will clearly put an extra burden on this algorithm, so whenever possible you
should use nodal constraints.
The two different options exist, since under some circumstances the actual constraints
can differ between the two methods. Consider for example a symmetry constraint,
where the displacement in the direction normal to the boundary is constrained by the
equation
un = 0
where n is the unit normal vector.
DEFINING CONSTRAINTS
|
125
If there are several intersecting symmetry planes, like in Figure 2-6, using nodal
constraints could cause a problem:
• If both boundaries are selected in the same Symmetry node, then only a single
constraint is applied for each node along the common edge, while you actually want
constraints along the normals of both planes. The normal used would be pointing
somewhere between the two planes, since a nodal constraint uses averaging of the
values from the adjacent elements.
• If two Symmetry nodes are used, so that the selection in any one of them only
contains boundaries without a normal direction discontinuity, the intended
constraints are added. On the common edge, there will be two contributions, one
from each Symmetry node, and each using the normal direction of its boundary. If
you want to use nodal constraints, you must set up your model in this way if the
constraints are orientation dependent.
Elemental constraints, on the other hand, can cause problems if the constraints added
by adjacent elements are not exactly the same. This could for example happen if the
normal orientation differs between neighboring elements. In such a case, a boundary
could behave as if it were fixed when a Symmetry, Antisymmetry, or Roller constraint is
applied. Such a situation could occur when the component consists of an imported
mesh, so that no underlying geometry exists.
The default type of the constraint, nodal or elemental, differs between different
constraint features. A nodal formulation is the default whenever it is considered safe,
like for a Fixed Constraint. Whenever the constraint can have a dependency on the
surface orientation, the default value is elemental.
See also Constraint Settings in the COMSOL Multiphysics Reference
Manual.
Suppressing Constraints on Lower Dimensions
Sometimes, boundary conditions on two adjacent objects can come into conflict on a
shared object.
For most constraints in the structural mechanics interfaces, you have the possibility to
select that certain objects of lower dimensions should be excluded from the main
selection. To do this, you must first select Advanced Physics Options. In the settings for
a constraint, like for example Prescribed Displacement, new sections named Excluded
126 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Surfaces, Excluded Edges, and Excluded Points will then appear. In these sections, you
can select geometrical objects which should be excluded from the main selection when
the constraint is applied.
In the structural mechanics interfaces, there are many types of complex constraints,
and sometimes you may get conflicts or duplicates which makes the model either
overconstrained, or problematic for the automatic constraint elimination algorithm. If
you are aware of such situations, it is good practice to remove one of the potentially
conflicting constraints. One example of such a situation is when you have a Solid–Shell
Connection meeting a symmetry plane, as shown in Figure 2-8.
Figure 2-8: Example of potentially conflicting constraints.
Here you would add a Symmetry condition on a boundary in the Solid Mechanics
interface, as well as a Symmetry condition on an edge in the Shell interface. But at the
same time, the displacements on whole boundary where the solid meets the shell are
controlled by shell degrees of freedom as an effect of the Solid–Shell Connection. As a
result, on the edge marked with Conflict in the sketch, the displacements will be
controlled both by the symmetry condition is Solid Mechanics, and implicitly through
the coupling, by the symmetry condition in the Shell interface. Particularly if the
geometry is curved, there is a risk that these constraints are not identical from a
numerical point of view. In this case, excluding the conflicting edge from the selected
boundary in the Solid Mechanics interface will make the behavior unique and fully
predictable.
Another example where constraints will come in conflict is if you want to constrain the
displacement on parts of the geometry using weak constraints, while keeping the
default pointwise constraints on other parts. If the same mesh node has both types of
DEFINING CONSTRAINTS
|
127
constraints, the solution will fail, so you must exclude any common geometrical objects
from the selection in one of the constraints.
See also Excluded Surfaces, Excluded Edges, and Excluded Points in the
COMSOL Multiphysics Reference Manual.
Kinematic Constraints
Kinematic constraints are equations that control the motion of solids, faces, edges, or
points. Add a Prescribed Displacement constraint to enter expressions for constraints.
You can define the equations using predefined coordinate systems as well as custom
coordinate systems. Special constraints, for instance to keep an edge of body straight
or to make a boundary rotate, require such constraint equations.
In the 3D and 2D Solid Mechanics interfaces and in the Shell and Beam
interface there is a special constraint called a Rigid Connector. A rigid
connector is applied to one or more boundaries, edges, or points and force
them to behave as connected to a common rigid body. The rigid
connector can be given prescribed displacements and rotations and thus
simplifies the realization of some constraints.
Rotational Joints
Joints between elements in The Truss Interface are automatically rotational joints
because the truss elements have no rotational degrees of freedom. For beams, however,
the rotational degrees of freedom are by default coupled between elements. To create
a rotational joint between two beam elements, add one additional Beam interface to a
geometry. Make sure that it is only active for the edge that includes the point where
the joint is positioned and that no other physics interface is active here. Couple the
translational degrees of freedom and leave the rotational degrees of freedom
uncoupled at the joint.
Attachments
An Attachment is a set of boundaries, edges, or points on a flexible or rigid component
used to connect it to another flexible or rigid component through a joint or spring. An
128 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
attachment can be defined on the boundaries of a solid element, on the edges of a shell
element, and on the points of a beam element.
When an attachment is connected to a flexible body, you can use two different
formulations: rigid or flexible.
In the rigid attachment formulation, all selected boundaries or edges behave as if they
were connected to a common rigid body. This may cause an unrealistic stiffening and
local stress concentrations.
In the flexible version, the boundaries are allowed to deform, and the rigid body
constraints are enforced only in an average sense.
The attachment formulation is similar to that of a rigid connector. In the rigid case,
the only degrees of freedom needed to represent this assembly are the ones needed to
describe the movement of a rigid body. In 2D this is just two in-plane translations, and
the rotation around the out-of-plane axis.
In 3D the situation is more complex. Six degrees of freedom are necessary, usually
selected as three translations and three parameters for the rotation. For finite rotations
any choice of three rotation parameters is singular at some specific set of angles. For
this reason, a four-parameter quaternion representation is used.
Some extra degrees of freedom are added for each attachment where the flexible
formulation is used.
When an attachment is defined on a rigid component, it does not create any degrees
of freedom of its own and directly picks the degrees of freedom of the rigid
component.
The formulation of the attachment feature is same as the rigid connector
formulation, which is discussed in Rigid Connector in the Structural
Mechanics Module User’s Guide.
Some useful information about the attachment feature:
• The attachment can be defined either on a flexible or on a rigid component. It is not
possible to select the boundaries from both types of components in a single
attachment. The reason is the different formulation of attachment for flexible or
rigid components.
DEFINING CONSTRAINTS
|
129
• The attachment’s center of rotation is the centroid of its selected boundaries, edges,
or points. In a joint, it is possible to select the attachment center of rotation as the
center of the joint.
• If the attachment is connected to a flexible domain, the forces and moments on an
attachment with a boundary selection are computed by summing the reaction forces
on the selected boundaries. There is an option to use these forces and moments to
evaluate the joint forces.
• For an attachment in the Shell interface, the selection consists of edges. The forces
and moments on an attachment are then computed by summing the reaction forces
and reaction moments on the selected edges. There is an option to use these forces
and moments to evaluate the joint forces.
• For an attachment in the Beam interface, the selection consists of points. The forces
and moments on an attachment are then computed by summing the reaction forces
and reaction moments on the selected points. There is an option to use these forces
and moments to evaluate the joint forces.
• When an attachment is defined in the Shell or Beam interface, the normal force
cannot be defined through Attachment reaction forces in the Friction subnode of a
joint.
• In a joint you select attachments to establish its connection with flexible, or
optionally, rigid bodies. This is accomplished by setting up a relation between the
source attachment and destination attachment degrees of freedom. Thus, the
motion of an attachment is governed by the joints where this attachment is used.
• An attachment which is not referenced by any joint acts as an unconstrained rigid
connector.
• The Multibody Dynamics Interface
• The Solid Mechanics Interface, The Shell and Plate Interfaces, and The
Beam Interface in the Structural Mechanics Module User’s Guide.
130 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Calculating Reaction Forces
There are different ways to evaluate reaction forces and these are discussed in this
section.
• Using Predefined Variables to Evaluate Reaction Forces
• Using Weak Constraints to Evaluate Reaction Forces
• Using Surface Traction to Evaluate Reaction Forces
• Evaluating Surface Traction Forces on Interior Boundaries
The following sections describe the merits and costs of these methods.
Using Predefined Variables to Evaluate Reaction Forces
The results analysis capabilities include easy access to the reaction forces and moments.
They are available as predefined variables. The reaction force variables are available
only at the nodes, and not as a continuous field, so they are not suitable for graphic
presentation.
To compute the sum of the reaction forces over a region, use
Volume Integration, Surface Integration, or Line Integration under Results>
Derived Values or under an Evaluation Group node. The integration
method discovers that the reaction forces are discrete values and applies a
summation instead of an integration.
If you create an integration operator under Component>Definitions>
Nonlocal Couplings>Integration to sum reaction forces, you must explicitly
set Method to Summation over nodes.
Reaction forces are computed as the sum of the nodal values over the selected volume,
face, or edge. Reaction moments are calculated as the sum of the moment from the
reaction forces with respect to a reference point, and any explicit reaction moments (if
CALCULATING REACTION FORCES
|
131
there are rotational degrees of freedom). During postprocessing, you can modify the
coordinates of the reference point in the Parameters section of a result feature.
• Reaction forces are not available for eigenfrequency analysis or when
weak constraints are used.
• Reaction force variables are computed where there are constraints, that
is Dirichlet conditions like Fixed Constraint, or Prescribed Displacement.
Reaction force variables are found in the Reactions folder in the result
menus, and have names like solid.RFx and solid.RMz for an
x-directed force and a moment around the z-axis, respectively.
• From the physical point of view, there can be other sources of reaction
forces, such as the elastic and viscous forces from a Spring Foundation.
Such forces are not included in the reaction force variables, but are
placed in separate variables. You will find them in the Spring and
damping forces folder in the result menus.
• Total reaction force variables are available. In these variables, reaction
forces, spring forces, and damping forces have been integrated over the
whole physics interface. These variables are found in the Reactions
folder in the result menus, and have names like solid.RFtotalx and
solid.RMtotalz for an x-directed force and a moment around the
z-axis, respectively. These variables should thus, for a stationary
analysis, be equal to the total applied load.
• The ordinary reaction forces are not computed for domains having a
Rigid Material. The reactions to constraints applied to such domains are,
however, included in the total reaction force variables.
• If reaction forces are summed independently for two adjacent
boundaries, the total sum is not the same as if the reaction forces were
summed for both boundaries in one operation. The values of the nodes
at the common edge always contain contributions from the elements
at both sides of the edge.
Derived Values, Evaluation Groups, and Tables in the COMSOL
Multiphysics Reference Manual
132 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Using Weak Constraints to Evaluate Reaction Forces
In the Constraint Settings section, Select Weak constraints from the Constraint list in
order to compute accurate distributed reactions. Extra variables that correspond to the
reaction traction distribution are automatically added to the solution components.
With weak constraints activated, COMSOL Multiphysics adds the reaction forces to
the solution components. The variables are denoted X_lm, where X is the name of the
constrained degree of freedom (as, for example, u_lm and v_lm). The extension lm
stands for Lagrange multipliers. It is only possible to evaluate reaction forces on
constrained boundaries in the directions of the constraints.
To compute the total reaction force on a boundary, integrate one of the
variables X_lm using Volume Integration, Surface Integration, or Line
Integration under Derived Values or under an Evaluation Group node.
If the constraint is defined in a local coordinate system, the degrees of
freedom for the weak constraint variables are defined along the directions
of that system.
Since the reaction force variables are added to the solution components, the number
of DOFs for the model increases slightly, depending on the mesh size for the
boundaries in question. Boundaries that are adjacent to each other must have the same
constraint settings. The reason for this is that adjacent boundaries share a common
node.
Using weak constraints affects the structure of the equation system to be solved, and
is not suitable for all types of equation solvers.
In the COMSOL Multiphysics Reference Manual:
• Weak Constraints
• Constraint Settings
• Derived Values, Evaluation Groups, and Tables
• Symmetric and Nonsymmetric Constraints
CALCULATING REACTION FORCES
|
133
Using Surface Traction to Evaluate Reaction Forces
As an alternative method, you can obtain values of the reaction forces on constrained
boundaries by using boundary integration of the relevant components of the surface
traction vector.
For 2D and 1D axisymmetric components, multiply the surface traction
by the cross-section thickness, and for 1D components multiply the
surface traction by the cross-section area before integrating to calculate
the total reaction force.
Two different types of surface traction results can be computed in COMSOL
Multiphysics:
The first type, contained in the variables interface.Tax, is computed from the
stresses. It is always available. Since the surface traction vector is based on computed
stress results, this method is less accurate for computing reactions than the other
methods.
The second type, contained in the variables interface.Tracx, is computed using a
method similar to the weak constraints, but without introducing the Lagrange
multipliers as extra degrees of freedom. The accuracy is high, but there is an extra
computational cost. These traction variables are computed only if the Compute
boundary fluxes check box in the Discretization section is selected for the Solid
Mechanics interface.
In case of geometric nonlinearity, the two types of traction variables are
interpreted differently. The interface.Tax variables are based on
Cauchy stress, and contains a force per current area. If you integrate them
you must use the spatial frame. The interface.Tracx variables are based
on First Piola–Kirchhoff stresses and contains a force per undeformed
area. An integration must then be done on the material frame.
Evaluating Surface Traction Forces on Interior Boundaries
As opposed to the other methods for reaction force computation, the boundary flux
based tractions are computed not only on external boundaries, but also on interior
boundaries. On interior boundaries, there are then two traction fields: One acting
from each of the domains sharing the boundary. These internal traction fields are
134 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
contained in the variables interface.iTracux and interface.iTracdx. The letters
u and d in the variable names indicate the upside and downside of the boundary,
respectively. If you need the value of the total force acting on an internal section
through your model, these variables can be integrated. The interface.iTracux and
interface.iTracdx variables are only available if the Compute boundary fluxes check
box is selected in the Discretization section of the physics interface, and there are
interior boundaries in your model.
Computing Accurate Fluxes in the COMSOL Multiphysics Reference
Manual
CALCULATING REACTION FORCES
|
135
Introduction to Material Models
In this section:
• Material Models for Structural Mechanics
• Entering Material Data
• Introduction to Linear Elastic Materials
• Introduction to Viscoelastic Materials
• Mixed Formulation
• Modeling Damage
• About the Material Databases for the Structural Mechanics Module
• Using External Materials
Material Models for Structural Mechanics
The Structural Mechanics Module without any add-on modules provides the Linear
Elastic material with Viscoelasticity and Thermal Expansion modeling capabilities. It
also provides access to piezoelectric and magnetostrictive materials.
If you have the optional products Nonlinear Structural Materials Module or
Geomechanics Module, many other classes of nonlinear materials are also available.
These models can be modified and extended, and custom material models can be
defined.
You can also add a material model which you have coded yourself and made available
as a binary library file using an External Stress-Strain Relation.
• Modeling Piezoelectric Problems
• Modeling Magnetostrictive Materials
In the COMSOL Multiphysics Reference Manual:
• Working with External Materials
• External Material
136 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
In Table 2-6 and Table 2-7 you can find an overview of the families of materials, and
their applicability in the various structural mechanics interfaces.
TABLE 2-6: MATERIAL MODELS IN THE PHYSICS INTERFACES ON DOMAINS AND BOUNDARIES.
MATERIAL
MODEL
SOLID
MECHANICS
ELASTIC
WAVES,
TIME
EXPLICIT
Linear Elastic Material
X
—
Linear Elastic
Material, Layered
—
—
Section Stiffness
—
Elastic Waves, Time
Explicit Model
Nonlinear Elastic
Material
SHELL/
PLATE
LAYERED
SHELL
MEMBRANE
X
X
X
X
—
X
—
X
—
—
—
X
—
—
—
X
—
—
—
X
Hyperelastic Material
X
—
—
X
X
Hyperelastic Material,
Layered
—
—
X
—
—
Shape Memory Alloy
X
—
—
—
—
Piezoelectric Material
X
—
—
X
—
Piezomagnetic
Material
X
—
—
—
—
Viscoelasticity
X
—
X
X
X
Plasticity
X
—
X
X
X
Soil Plasticity
X
—
—
—
—
Creep
X
—
X
X
X
Elastoplastic Soil
Material
X
—
—
—
—
Viscoplasticity
X
—
X
X
X
Porous Plasticity
X
—
—
—
—
Concrete
X
—
—
—
—
Rocks
X
—
—
—
—
Damage
X
—
—
—
—
External Stress-Strain
Relation
X
—
—
—
X
Rigid Material
X
—
X
X
—
INTRODUCTION TO MATERIAL MODELS
|
137
TABLE 2-7: MATERIAL MODELS IN THE PHYSICS INTERFACES ON EDGES.
MATERIAL
MODEL
BEAM
PIPE
MECHANICS
TRUSS
Linear Elastic Material
X
—
X
Fluid and Pipe
Materials
—
X
—
Section Stiffness
X
—
—
Plasticity
—
—
X
Rigid Material
X
X
—
Spring-Damper
Material
—
—
X
Many of the material models can be augmented by effects like thermal expansion,
hygroscopic swelling, initial stresses and strains, external stress, and activation.
Combination of Material Models
It is possible to combine many of the effects in an additive manner. The models based
on elasticity all have the same structure where
1 An elastic strain is computed by removing all inelastic strains (for example, plastic or
thermal strains) from the total strain.
2 An “elastic stress” is computed from the elastic strains.
3 Any additional stresses (for example viscous stresses, or initial stresses) are added to
form the total stress.
This concept will give you a great freedom in combining effects. Some such useful
combinations are
• Plasticity and thermal expansion
• Plasticity and creep
• Thermal expansion and hygroscopic swelling
• Viscoelasticity and creep
Entering Material Data
For most material data, you have the option to choose between From material and
User defined. The preferred way of supplying the material data, is through the Materials
138 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
node. If you are using data from the Material Library, this is the only option, but also
when supplying your own data this will improve clarity of model.
Constitutive matrices, such as the elasticity matrix for an anisotropic material, are in
many cases per definition symmetric. Only the upper diagonal of the matrix given as
input is used for forming the matrix used, so you need not enter the lower diagonal
part.
Introduction to Linear Elastic Materials
Linear elasticity forms the basis for the majority of structural mechanics simulations.
For isotropic linear elasticity, two parameters are enough to describe the material
behavior. The number of parameters increases to (at most) 21 for the fully anisotropic
case in 3D. When setting up a model, make sure that the material parameters are
defined in agreement with the type of relationship used. If necessary, transform the
material data before entering it in the physics interface. For example, for orthotropic
materials calculate the Poisson’s ratio xy by
Ex
 xy =  yx -----Ey
In the theory section Linear Elastic Material
Introduction to Viscoelastic Materials
The generalized Maxwell, standard linear solid (SLS) and Kelvin–Voigt viscoelastic
materials are available. All the models are linear, and the corresponding materials can
be described as consisting of one or more branches with a spring and a dashpot acting
in parallel to a linear elastic material. For each viscoelastic branch, the shear modulus
and the relaxation time (or viscosity) are entered.
• Linear Viscoelasticity
• Viscoelasticity
INTRODUCTION TO MATERIAL MODELS
|
139
Mixed Formulation
Nearly and fully incompressible materials can cause numerical problems if only
displacements are used in the interpolating functions. Small errors in the evaluation of
volumetric strain, due to the finite resolution of the discrete model, are exaggerated by
the high bulk modulus. This leads to an unstable representation of stresses, and in
general to underestimation of the deformation, because spurious volumetric stresses
might balance also applied shear and bending loads.
In several material models you will find settings named Use mixed formulation or
Compressibility, by which you can introduce a mixed formulation.
Use a mixed formulation when the material data is such that the deformation is close
to being incompressible. For an isotropic elastic material, this happens when Poisson’s
ratio approaches 0.5.
There are different approaches to assess which combinations of displacement shape
function types and auxiliary variable shape function types yield numerically sound and
effective elements. In general, the shape function order of the auxiliary variable should
be lower than for the displacement field, to avoid locking. However, this is not a
sufficient requirement. The inf-sup condition (Ref. 1) can be used to analytically or
numerically identify sound mixed element formulations. In general, the outcome of
such a test will depend not only on the shape function type combination, but also on
the element type. For instance, a sound and effective combination of shape function
types for a tetrahedral element is not necessarily suitable for a hexahedral element.
COMSOL Multiphysics provides four types of shape functions for the auxiliary
pressure or auxiliary volumetric strain variable. The different shape function types for
the auxiliary variable are described below. Depending on the particular context, one of
these types is implicitly selected using Automatic.
Note that in the case of a mixed mesh, you may have to subdivide the
domain by element type, to be able to control the shape functions for the
auxiliary variable.
DISCONTINUOUS LAGRANGE
If this shape function type is selected, the auxiliary variable shape function is
discontinuous across element boundaries, and it is one order lower than the shape
function order of the displacements.
140 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
CONTINUOUS
If this shape function type is selected, the auxiliary variable shape function is
continuous across element boundaries. It will be of the same type (Lagrange or
Serendipity) as that of the displacements, but one order lower. A special case is for a
linear displacement field, for which a discontinuous, constant, shape function is used.
LINEAR
If this shape function type is selected, the auxiliary variable is regarded as a linearly
interpolated field in the element. In the case of an auxiliary pressure, the interpolation
in a 3D isoparametric element is
p = p0 + 1  p1 – p0  + 2  p2 – p0  + 3  p3 – p0 
where p0, p1, p2, and p3 are auxiliary pressure coefficients, and 1, 2, and 3 are
isoparametric coordinates. Note that the field is linear in the local element coordinates,
and that it is not continuous across element boundaries.
The linear shape function type is not available for layered material
features.
CONSTANT
This shape function type represents a constant auxiliary variable in the element, p = p0.
The mixed formulation is useful not only for linear elastic materials but
also for nonlinear elastic materials, elastoplastic materials, hyperelastic
materials, and viscoelastic materials.
Note that some iterative solvers do not work well together with mixed
formulation because the stiffness matrix becomes indefinite.
For more details, see Mixed Formulation in the Structural Mechanics
Theory chapter.
INTRODUCTION TO MATERIAL MODELS
|
141
Modeling Damage
Modeling problems with strain localization might turn into unstable behavior and
convergence difficulties. The following techniques can be used to help in such
situations:
• Use a displacement-controlled loading scheme, since damage is often associated
with a reduction in load carrying capacity, see the Cracking of a Notched Beam
example in the Geomechanics Module and Nonlinear Structural Materials Module
Application Libraries.
• Better convergence is often obtained when the Nonlinear method is set to Constant
(Newton) with a Damping factor equal to 1, and a Jacobian update on every iteration.
• Reduce the smallest and/or largest allowable step size in an Auxiliary sweep, or
restrict the time steps in a time-dependent study.
• Introducing a soft spot where a crack is expected can make the localization of strains
more stable, see the Brittle Damage in Uniaxial Tension example in the
Geomechanics Module Application Library and Nonlinear Structural Materials
Module Application Libraries. Alternatively, a random spatial distribution of the
material parameters could be employed to obtain a more stable solution.
When using the crack band method or no regularization at all, the following steps are
recommended:
• The size of the biggest mesh element h should not exceed 2EGf/ts2, where E is
the Young’s modulus, Gf is the fracture energy per unit area, and ts is the tensile
strength. Larger values of h will cause a snap-back of the stress-strain curve at the
material point level.
• Use linear shape functions for the displacement field. When using higher-order
shape functions, strains may localize in either rows of Gauss points, or entire
elements, depending on the stress state and numerical rounding errors.
• If cracks are located on a symmetry plane, the model parameters should be modified
so that the amount of dissipated energy is reduced by one half in the elements
adjacent to the symmetry plane. This can be achieved, for example, by reducing the
fracture energy in that row of elements.
When using the implicit gradient method, the element size should be sufficiently small
to resolve damaged zones. The same applies to the Phase field damage model, where it
is recommended that size of the mesh elements in the expected crack path follows
h < lint/2 for a linear displacement field, otherwise h < lint.
142 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
While it is possible to solve brittle fracture problems with the Phase field damage model
by applying a fully coupled strategy, this can often exhibit poor or slow convergence.
An alternative and often more stable approach is to use a segregated solution strategy,
by splitting the evolution of the crack phase field and the displacement field in two
groups. This type of algorithmic operator split can conceptually be summarized as
follows for step n+1:
1 Initialization. The crack phase field, displacement field and state variables are
known at step n.
2 Update state variables. Update internal state variables used by the phase field
model with values from step n.
3 Solve for the Crack Phase Field. Compute the crack phase field variable in a Newton
step, with the displacement field frozen at step n.
4 Solve for the Displacement field. Compute displacement field variables in a Newton
step with the updated crack phase field.
This leads to a single-pass algorithm that is accurate only for sufficiently small
parameter or time steps.
The default solver will suggest the above single-pass algorithm for the
Phase field damage model when it is feasible to perform the operator split.
Cases where this is not possible include when some multiphysics
couplings are present in the model and when a segregated contact
algorithm has to be used.
An improvement to the method is to add a multipass correction by iterating over steps
3 and 4 in each increment; either until convergence is achieved or for a predefined
number of iterations. This type of strategy is demonstrated in the Brittle Fracture of
a Holed Plate example in the Geomechanics Module and Nonlinear Structural
Materials Module Application Libraries, where a multipass algorithm with a maximum
of 3 outer iterations is used. Note that although the solution is accepted without
requiring convergence of the outer problem, each subgroup locally fulfills the defined
convergence criterion. Hence the displacement field can be considered as a converged
solution given the current crack phase field.
About the Material Databases for the Structural Mechanics Module
The Structural Mechanics Module includes these material databases: Liquids and
Gases, with temperature-dependent fluid dynamic and thermal properties, MEMS, an
INTRODUCTION TO MATERIAL MODELS
|
143
extended solid materials library with metals, semiconductors, insulators, and polymers
common in MEMS devices, and a Piezoelectric database with over 20 common
piezoelectric materials. The materials include temperature-dependent fluid dynamic
and thermal properties.
In the COMSOL Multiphysics Reference Manual:
• MEMS Material Library
• Piezoelectric Materials Library
• Liquids and Gases Material Library
• Materials
For an example of the MEMS materials database and Piezoelectric
materials database, see Piezoelectric Shear-Actuated Beam: Application
Library path Structural_Mechanics_Module/Piezoelectric_Effects/
shear_bender.
Using External Materials
If you need to use a constitutive model which is not available among the built-in
material models, it is possible to program it yourself. Such a material function, termed
an external material, is coded in C. If you already have an existing code in another
language like Fortran or C++, it is however possible to write a wrapper function to it.
Before moving to implementing your own material model, there are however two
other options to consider:
• Many material models like hyperelasticity, creep, and plasticity have User defined as
one of the options in addition to the standard models. Any material model which
you can describe using built-in variables is most conveniently described here.
• A material model which can partially described in terms of a PDE can often be
implemented using one of the mathematical interfaces. Stresses or strains computed
in that interface are then injected in an existing material model using the External
Stress and External Strain subnodes.
There are two basic types of external material functions: those which completely
replace other material definitions in a domain, and those that just compute an inelastic
strain contribution to be used as part of an existing material model. The former is
144 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
referenced from an External Stress-Strain Relation node, whereas the latter is
referenced from an External Strain subnode.
During the solution, an external material routine is always called for each Gauss point
during evaluation of stiffness matrices and computation of residuals. During result
presentation, the external material can be called from any location in the geometry, as
requested by for example graphs and point evaluations.
Almost invariably, you need to store state variables in the external material, such as for
example plastic strains. The state variables are stored at the Gauss points. If an external
material is called at another location, the state variables will be interpolated to that
location. This means that the state of the material may not be exactly consistent there,
which can lead to some artifacts during result presentation. You can avoid this problem
by using the gpeval operator.
In the COMSOL Multiphysics Reference Manual:
• Working with External Materials
• External Material
LIBRARY OF UTILITY FUNCTIONS
In order to simplify the task of writing the code for an external material, a library of
utility routines is provided. It provides a toolkit for operations common in solid
mechanics such as various tensor operations or computing principal stresses and
equivalent stresses.
LIST OF UTILITY FUNCTIONS
csext_add: Function that adds two matrices
/*
* Function: csext_add
* ------------------* Description:
*
Adds two (3 x 3) matrices 'A' and 'B' and stores the
*
result 'A + B' in 'C'.
*
* Arguments:
*
double A[3][3]
*
double B[3][3]
*
double C[3][3] (output)
*
* Return value:
INTRODUCTION TO MATERIAL MODELS
|
145
*
void
*/
void csext_add(double A[3][3],double B[3][3], double C[3][3]);
csext_det: Function that computes the matrix determinant
/*
* Function: csext_det
* ------------------* Description:
*
Computes the determinant of a (3 x 3) matrix 'A' and
*
returns the value.
*
* Arguments:
*
double A[3][3]
*
* Return value:
*
double
*
*/
double csext_det(double A[]3[3]);
csext_dev: Function that computes the deviator of a matrix
/*
* Function: csext_dev
* ------------------* Description:
*
Computes the deviator of a (3 x 3) matrix 'A'
*
and stores the value in 'dev'.
*
* Arguments:
*
double A[3][3]
*
double dev[3][3] (output)
*
* Return value:
*
void
*
*/
void csext_dev(double A[3][3], double dev[3][3]);
csext_dot: Function that computes the inner product of two matrices
/*
* Function: csext_dot
* ------------------* Description:
*
Computes the inner product of (3 x 3) matrices 'A' and 'B',
146 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
*
and returns 'A : B'.
*
* Arguments:
*
double A[3][3]
*
double B[3][3]
*
* Return value:
*
double
*
*/
double csext_dot(double A[3][3],double B[3][3]);
csext_eig: Function that computes the spectral decomposition of a symmetric matrix
/*
* Function: csext_eig
* ------------------* Description:
*
Computes the eigenvalues and eigenvectors of a
*
symmetric (3 x 3) matrix 'A'.
*
The eigenvalues are stored in 'vals', sorted with the
*
largest value in vals[0].
*
The eigenvectors are stored column-wise in 'vecs' with
*
the same ordering as the eigenvalues.
*
Normal execution returns 0. nonzero means that the
*
computation failed.
*
* Arguments:
*
double A[3][3]
*
double vals[3]
(output)
*
double vecs[3][3] (output)
*
* Return value:
*
int
*
*/
int csext_eig(double A[3][3], double vals[3], double vecs[3][3]);
csext_gl: Function that computes the Green–Lagrange strain tensor
/*
* Function: csext_gl
* -----------------* Description:
*
Computes the Green–Lagrange strain tensor 'egl' based on
*
the Right Cauchy–Green deformation tensor 'rcg'.
*
* Arguments:
*
double rcg[3][3]
INTRODUCTION TO MATERIAL MODELS
|
147
*
double egl[3][3] (output)
*
* Return value:
*
void
*
*/
void csext_gl(double rcg[3][3],double egl[3][3]);
csext_inv: Function that computes the matrix inverse
/*
* Function: csext_inv
* ------------------* Description:
*
Computes the inverse of a (3 x 3) matrix 'A'.
*
The inverse, if it exists, is stored in 'inv'.
*
0 is returned if successful, -1 if 'A' is numerically
*
singular. The matrix 'A' is considered singular if
*
abs(det(A))<tol.
*
* Arguments:
*
double A[3][3]
*
double tol
*
double inv[3][3] (output)
*
* Return value:
*
int
*
*/
int csext_inv(double A[3][3], double tol, double inv[3][3]);
csext_lcg: Function that computes the Left Cauchy–Green deformation tensor
/*
* Function: csext_lcg
* ------------------* Description:
*
Computes the Left Cauchy–Green deformation 'lcg' tensor
*
based on the deformation gradient 'defgrad'.
*
*
* Arguments:
*
double defgrad[3][3]
*
double lcg[3][3] (output)
*
* Return value:
*
void
*
*/
148 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
void csext_lcg(double defgrad[3][3], double lcg[3][3]);
csext_linsolv: Function to solve a linear system of equations
/*
* Function: csext_linsolv
* ------------------* Description:
*
Solves a linear system of equations, 'Ax = b', for 'x',
*
where 'A' is (n x n), and 'b' is (n x 1).
*
The maximum allowed size of the system is n = 6.
*
*
The solution vector 'x' is stored in 'b' as output.
*
The elements of matrix 'A' are not preserved.
*
*
If successful, 0 is returned.
*
If the solution cannot be determined, -1 is returned.
*
If n < 1 or n > 6, -2 is returned.
*
* Arguments:
*
double *A
*
double *b
(input/output)
*
* Return value:
*
int
*
*/
CSEXTUTILS_SYMBOLS int csext_linsolv(int n, double *A, double *b);
csext_lpolar: Function that computes the Left polar decomposition of a matrix
/*
* Function: csext_lpolar
* ------------------* Description:
*
Computes the Left polar decomposition F = VR,
*
such that the deformation gradient 'defgrad' is
*
multiplicatively decomposed into a rotation, 'R',
*
and a stretch tensor, 'V'.
*
If the polar decomposition fails, -1 is returned.
*
If successful, 0 is returned.
*
* Arguments:
*
double defgrad[3][3]
*
double V[3][3]
(output)
*
double R[3][3]
(output)
*
* Return value:
*
int
INTRODUCTION TO MATERIAL MODELS
|
149
*
*/
int csext_lpolar(double defgrad[3][3], double V[3][3],
double R[3][3]);
csext_mises: Function that computes the von Mises equivalent stress
/*
* Function: csext_mises
* --------------------* Description:
*
Computes and returns the von Mises equivalent stress based
*
on a stress tensor 'sig'.
*
* Arguments:
*
double sig[3][3]
*
* Return value:
*
double
*
*/
double csext_mises(double sig[3][3]);
csext_mul: Function that multiplies two matrices
/*
* Function: csext_mul
* ------------------* Description:
*
Multiplies two (3 x 3) matrices 'A' and 'B'.
*
The result 'AB' is stored in 'C'.
*
* Arguments:
*
double A[3][3]
*
double B[3][3]
*
double C[3][3] (output)
*
* Return value:
*
void
*
*/
void csext_mul(double A[3][3], double B[3][3], double C[3][3]);
csext_rcg: Function that computes the Right Cauchy–Green deformation tensor
/*
* Function: csext_rcg
* -------------------
150 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
* Description:
*
Computes the Right Cauchy–Green deformation tensor 'rcg'
*
based on the deformation gradient 'defgrad'.
*
* Arguments:
*
double defgrad[3][3]
*
double rcg[3][3]
(output)
*
* Return value:
*
void
*
*/
void csext_rcg(double defgrad[3][3], double rcg[3][3]);
csext_rpolar: Function that computes the Right polar decomposition of a matrix
/*
* Function: csext_rpolar
* ------------------* Description:
*
Computes the Right polar decomposition F = RU,
*
such that the deformation gradient 'defgrad' is
*
multiplicatively decomposed into a rotation, 'R',
*
and a stretch tensor, 'U'.
*
If the polar decomposition fails, -1 is returned.
*
If successful, 0 is returned.
*
* Arguments:
*
double defgrad[3][3]
*
double R[3][3]
(output)
*
double U[3][3]
(output)
*
* Return value:
*
int
*
*/
int csext_rpolar(double defgrad[3][3], double R[3][3],
double U[3][3]);
csext_spect: Function that computes a matrix based on its spectral decomposition
/*
* Function: csext_spect
* ------------------* Description:
*
Computes a symmetric (3 x 3) matrix 'A' based on
*
its spectral decomposition A=Q*diag*Q^T.
*
The matrix 'diag' is diagonal and stores the
*
eigenvalues of 'A'. The matrix 'Q' stores the
INTRODUCTION TO MATERIAL MODELS
|
151
*
eigenvectors (column-wise) of 'A', with the ordering
*
corresponding to the eigenvalues in 'diag'.
*
The vector 'd' stores the diagonal elements of 'diag'.
*
* Arguments:
*
double Q[3][3]
*
double d[3]
*
double A[3][3]
(output)
*
* Return value:
*
void
*
*/
void csext_spect(double Q[3][3], double d[3], double A[3][3]);
csext_trace: Function that computes the matrix trace
/*
* Function: csext_trace
* --------------------* Description:
*
Computes and returns the trace of a (3 x 3) matrix 'A'.
*
* Arguments:
*
double A[3][3]
*
* Return value:
*
double
*
*/
double csext_trace(double A[3][3]);
csext_transp: Function that computes the matrix transpose
/*
* Function: csext_transp
* ---------------------* Description:
*
Computes the transpose of a (3 x 3) matrix 'A'.
*
The result is stored in 'transp'.
*
* Arguments:
*
double A[3][3]
*
double transp[3][3] (output)
*
* Return value:
*
void
*
*/
152 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
void csext_transp(double A[3][3], double transp[3][3]);
csext_add_voigt: Function that adds two matrices
/*
* Function: csext_add_voigt
* --------------------------* Description:
*
Adds two matrices 'A' and 'B' stored on Voigt form.
*
The result is stored in 'C'.
*
* Arguments:
*
double A[6]
*
double B[6]
*
double C[6] (output)
*
* Return value:
*
void
*/
void csext_add_voigt(double A[6], double B[6], double C[6]);
csext_dev_voigt: Function that computes the deviator of a symmetric matrix
/*
* Function: csext_dev_voigt
* --------------------------* Description:
*
Computes the deviator of a (symmetric) matrix 'A' stored on
Voigt form.
*
The result is stored in 'dev'.
*
* Arguments:
*
double A[6]
*
double dev[6] (output)
*
* Return value:
*
void
*/
void csext_dev_voigt(double A[6], double dev[6]);
csext_dot_voigt: Function that computes the inner product of symmetric matrices
/*
* Function: csext_dot_voigt
* --------------------------* Description:
*
Computes and returns the dot product (inner product) of two
*
symmetric (3 x 3) matrices 'A' and 'B' stored on Voigt form.
INTRODUCTION TO MATERIAL MODELS
|
153
*
* Arguments:
*
double A[6]
*
double B[6]
*
* Return value:
*
double
*/
double csext_dot_voigt(double A[6], double B[6]);
csext_mises_voigt: Function that computes the von Mises equivalent stress
/*
* Function: csext_mises_voigt
* --------------------* Description:
*
Computes and returns the von Mises equivalent stress based
*
on a stress tensor 'sig' on Voigt form.
*
* Arguments:
*
double sig[6]
*
* Return value:
*
double
*
*/
double csext_mises_voigt(double sig[6]);
csext_utils_trace_voigt: Function that computes the matrix trace
/*
* Function: csext_trace_voigt
* --------------------------* Description:
*
Computes and returns the trace of a symmetric (3 x 3) matrix
*
'A' stored on Voigt form.
*
* Arguments:
*
double A[6]
*
* Return value:
*
double
*/
double csext_trace_voigt(double A[6]);
csext_from_voigt: Function to change from Voigt notation
/*
154 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
* Function: csext_from_voigt
* ------------------* Description:
*
Converts a symmetric (3 x 3) matrix 'A' stored
*
on Voigt form to matrix form. The result is stored in 'B'.
*
If 'def' = 1, the values of last three elements of 'A' are
*
un-altered when passed into 'B'.
*
If 'def' = 2, the values of last three elements of 'A' are
*
halved when passed into 'B'.
*
Returns -1 if the value of 'def' is invalid, 0 otherwise.
*
* Arguments:
*
double A[6]
*
int def
*
double B[3][3] (output)
*
* Return value:
*
int
*
*/
int csext_from_voigt(double A[6], int def, double B[3][3]);
csext_to_voigt: Function to change to Voigt notation
/*
* Function: csext_to_voigt
* ------------------* Description:
*
Converts a symmetric (3 x 3) matrix 'A' to Voigt form.
*
The result is stored in 'B'.
*
If 'def' = 1, the values of the off-diagonal components
*
of 'A' are unaltered when passed into 'B'.
*
If 'def' = 2, the values of the off-diagonal components
*
of 'A' are doubled when passed into 'B'.
*
Returns -1 if the value of 'def' is invalid, 0 otherwise.
*
* Arguments:
*
double A[3][3]
*
int def
*
double B[6] (output)
*
* Return value:
*
int
*
*/
int csext_to_voigt(double A[3][3], int def, double B[6]);
INTRODUCTION TO MATERIAL MODELS
|
155
csext_jac_conv: Function to convert the Jacobian
/*
* Function: csext_jac_conv
* -----------------------* Description:
*
Converts a Jacobian from 'dSde' to 'dSdF' using the deformation
*
gradient 'defgrad', where:
*
- 'S' is the 2:nd Piola–Kirchhoff stress tensor,
*
- 'e' is the Green–Lagrange strain tensor,
*
- 'F' is the deformation gradient.
*
If 'def' = 1, dSde is defined using tensor shears.
*
If 'def' = 2, dSde is defined using engineering shears.
*
Returns -1 if the value of 'def' is invalid.
*
* Arguments:
*
double dSde[6][6]
*
int def
*
double defgrad[3][3]
*
double dSdF[6][9]
(output)
*
* Return value:
*
int
*
*/
int csext_jac_conv(double dSde[6][6], int def,
double defgrad[3][3], double dSdF[6][9]);
csext_unit: Function to define a unit matrix
/*
* Function: csext_unit
* ------------------* Description:
*
Initializes an (n x n) matrix 'A' to the identity matrix.
*
Returns -1 if n < 1,
*
0 otherwise.
*
* Arguments:
*
int n
*
double *A (output)
*
* Return value:
*
int
*
*/
int csext_unit(int n, double *A);
156 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
csext_zero: Function to initialize a matrix
/*
* Function: csext_zero
* ------------------* Description:
*
Initializes an (m x n) matrix 'A' to zero.
*
Returns -1 if m < 1 or n < 1,
*
0 otherwise.
*
* Arguments:
*
int m
*
int n
*
double *A (output)
*
* Return value:
*
void
*
*/
int csext_zero(int m, int n, double *A);
References
1. D. Chapelle and K.J. Bathe, The Inf-Sup test, Comp. Struct., Vol. 47, No. 4/5, pp.
537–545, 1993.
INTRODUCTION TO MATERIAL MODELS
|
157
Modeling Piezoelectric Problems
In this section:
• About Piezoelectric Materials
• Piezoelectric Coupling
• Create the Piezoelectricity Interface and Define Domains
• Complete Settings of Piezoelectric Materials
• Add Damping and Loss
• Define Material Properties
• Multiphysics Modeling Workflow in the COMSOL Multiphysics
Reference Manual.
• Piezoelectric Coupling
• Piezoelectricity in the theory section
About Piezoelectric Materials
Piezoelectric materials become electrically polarized when strained. From a
microscopic perspective, the displacement of atoms within the unit cell (when the solid
is deformed) results into electric dipoles within the medium. In certain crystal
structures, this combines to give an average macroscopic dipole moment or electric
polarization. This effect, known as the direct piezoelectric effect, is always
accompanied by the converse piezoelectric effect, in which the solid becomes strained
when placed in an electric field.
Within a piezoelectric, there is a coupling between the strain and the electric field,
which is determined by the constitutive relation:
T
S = sE T + d E
D = dT +  T E
(2-14)
Here, the naming convention used in piezoelectricity theory is assumed: S is the strain,
T is the stress, E is the electric field, and D is the electric displacement field. The
material parameters sE, d, and T, correspond to the material compliance, the coupling
properties and the permittivity. These quantities are tensors of rank 4, 3, and 2,
158 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
respectively. The tensors, however, are highly symmetric for physical reasons, and they
can be represented as matrices within an abbreviated subscript notation, which is
usually more convenient. In the Piezoelectricity interface, the Voigt notation is used,
which is a standard in the literature for piezoelectricity but which differs from the
defaults in the Solid Mechanics interface.
The Piezoelectric Material uses the structural mechanics nomenclature.
The strain is named  (instead of S) and the stresses are denoted by either
 or S (instead of T). This makes the names consistent with those used in
the other structural mechanics interfaces.
Equation 2-14 will, using the notation from structural mechanics, then read
T
 = sE + d E
D = d +  0  rT E
(2-15)
Equation 2-14 (or Equation 2-15) is known as the strain-charge form of the
constitutive relations. The equation can be rearranged into the stress-charge form,
which relates the material stresses to the electric field:
T
 = cE  – e E
D = e +  0  rS E
(2-16)
The material properties, cE, e, and S are related to sE, d, and T. It is possible to use
either form of the constitutive relations. In addition to Equation 2-14 or
Equation 2-16, the equations of solid mechanics and electrostatics must also be solved
within the material.
• Piezoelectric Coupling
• Modeling Piezoelectric Problems
• Piezoelectricity in the theory section
Piezoelectric Material Orientation
The orientation of a piezoelectric crystal cut is frequently defined by the system
introduced by the IRE standard of 1949 (Ref. 8). This standard has undergone a
number of subsequent revisions, with the final revision being the IEEE standard of
MODELING PIEZOELECTRIC PROBLEMS
|
159
1987 (Ref. 9). Unfortunately, the 1987 standard contained a number of serious errors
and the IEEE subsequently withdrew it. COMSOL therefore adopts the preceding
1978 standard (Ref. 10), which is similar to the 1987 standard, for material property
definitions. Most of the material properties in the material library are based on the
values given in the book by Auld (Ref. 11), which uses the 1978 IEEE conventions.
This is consistent with general practice except in the specific case of quartz, where it is
more common to use the 1949 IRE standard to define the material properties.
COMSOL therefore provides additional sets of material properties consistent with this
standard for the case of quartz. Note that the material properties for quartz are based
on Ref. 12, which uses the 1949 IRE standard (the properties are appropriately
modified according to the different standards).
The stiffness, compliance, coupling, and dielectric material property matrices are
defined with the crystal axes aligned with the local coordinate axes. Note that the signs
of several matrix components differ between the 1949 and the 1978 standards (see
Table 2-8). In the absence of a user-defined coordinate system, the local system
corresponds to the global X, Y, and Z coordinate axes. When an alternative coordinate
system is selected this system defines the orientation of the crystal axes. This is the
mechanism used in COMSOL to define a particular crystal cut, and typically it is
necessary to calculate the appropriate Euler angles for the cut (given the thickness
orientation for the wafer). All piezoelectric material properties are defined using the
Voigt form of the abbreviated subscript notation, which is universally employed in the
literature (this differs from the standard notation used for the Solid Mechanics
interface material properties). The material properties are defined in the material
frame, so that if the solid rotates during deformation the material properties rotate
with the solid. See Modeling Geometric Nonlinearity.
Crystal cuts are usually defined by a mechanism introduced by the IEEE/IRE
standards. Both standards use a notation that defines the orientation of a virtual slice
(the plate) through the crystal. The crystal axes are denoted X, Y, and Z and the plate,
which is usually rectangular, is defined as having sides l, w, and t (length, width, and
thickness). Initially the plate is aligned with respect to the crystal axes and then up to
three rotations are defined, using a right-handed convention about axes embedded
along the l, w, and t sides of the plate. Taking AT cut quartz as an example, the IEEE
1978 standard defines the cut as: (YXl) 35.25°. The first two letters in the bracketed
expression always refer to the initial orientation of the thickness and the length of the
plate. Subsequent bracketed letters then define up to three rotational axes, which move
with the plate as it is rotated. Angles of rotation about these axes are specified after the
bracketed expression in the order of the letters, using a right-handed convention. For
160 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
AT cut quartz only one rotation, about the l axis, is required. This is illustrated in
Figure 2-10. Note that within the 1949 IRE Standard AT cut quartz is denoted as:
(YXl) 35.25°, since the X-axis is rotated by 180° in this convention and positive
angles therefore correspond to the opposite direction of rotation (see Figure 2-9).
Table 2-9 summarizes the differences between the standards for different crystal cuts.
When defining the material properties of Quartz, the orientation of the
X, Y, and Z axes with respect to the crystal differs between the 1987 IEEE
standard and the 1949 IRE standard. Figure 2-9 shows the alignment of
the axis for the case of right-handed quartz. A consequence of this is that
both the material property matrices and the crystal cuts differ between the
two standards. Table 2-8 summarizes the signs for the important matrix
elements under the two conventions. Table 2-9 shows the different
definitions of the crystal cuts under the two conventions.
TABLE 2-8: SIGNS FOR THE MATERIAL PROPERTIES OF QUARTZ, WITHIN THE TWO STANDARDS COMMONLY
EMPLOYED.
IRE 1949 STANDARD
IEEE 1978 STANDARD
MATERIAL
PROPERTY
RIGHT HANDED
QUARTZ
LEFT HANDED
QUARTZ
RIGHT HANDED
QUARTZ
LEFT HANDED
QUARTZ
s14
+
+
-
-
c14
-
-
+
+
d11
-
+
+
-
d14
-
+
-
+
e11
-
+
+
-
e14
+
-
+
-
TABLE 2-9: CRYSTAL CUT DEFINITIONS FOR QUARTZ CUTS WITHIN THE TWO STANDARDS COMMONLY
EMPLOYED AND THE CORRESPONDING EULER ANGLES FOR DIFFERENT ORIENTATIONS OF THE CRYSTAL
THICKNESS.
STANDARD
REPRESENTATION
AT CUT
IRE 1949
Standard
(YXl) +35.25
(YXl) 49
Y-thickness Euler
angles
(ZXZ: 035.250)
(ZXZ: 0490)
Z-thickness Euler
angles
(ZXZ: 0°,125.250)
(ZXZ: 0 410)
Standard
(YXl) 35.25
(YXl) +49
IEEE 1978
BT CUT
MODELING PIEZOELECTRIC PROBLEMS
|
161
TABLE 2-9: CRYSTAL CUT DEFINITIONS FOR QUARTZ CUTS WITHIN THE TWO STANDARDS COMMONLY
EMPLOYED AND THE CORRESPONDING EULER ANGLES FOR DIFFERENT ORIENTATIONS OF THE CRYSTAL
THICKNESS.
STANDARD
REPRESENTATION
AT CUT
BT CUT
Y-thickness Euler
angles
(ZXZ: 0 35.250)
(ZXZ: 0 490)
Z-thickness Euler
angles
(ZXZ: 0 54.750)
(ZXZ: 0 1390)
When defining the material orientation, it is necessary to consider the orientation of
the plate with respect to the global coordinate system in addition to the orientation of
the plate with respect to the crystallographic axes. Consider the example of AT cut
quartz in Figure 2-10. The definition of the appropriate local coordinate system
depends on the desired final orientation of the plate in the global coordinate system.
One way to set up the plate is to orient its normal parallel to the Y-axis in the global
coordinate system. Figure 2-11 shows how to define the local coordinate system in this
case. Figure 2-12 shows how to define the local system such that the plate has its
normal parallel to the global Z-axis. In both cases it is critical to keep track of the
orientation of the local system with respect to the global system, which is defined
depending on the desired orientation of the plate in the model.
There are also a number of methods to define the local coordinate system with respect
to the global system. Usually, it is most convenient to define the local coordinates with
a Rotated System node, which defines three Euler angles according to the ZXZ
convention (rotation about Z, then X, then Z again). Note that these Euler angles
define the local (crystal) axes with respect to the global axes — this is distinct from the
approach of defining the cut (global) axes with respect to the crystal (local) axes.
162 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Figure 2-9: Crystallographic axes defined for right-handed quartz in COMSOL and the
1978 IEEE standard (color). The 1949 standard axes are shown for comparison (gray).
Figure 2-9 is reproduced with permission from: IEEE Std 176-1987 IEEE Standard on Piezoelectricity, reprinted with permission from
IEEE, 3 Park Avenue, New York, NY 10016-5997 USA, copyright 1987,
by IEEE. This figure must not be reprinted or further distributed without
prior written permission from the IEEE.
MODELING PIEZOELECTRIC PROBLEMS
|
163
Figure 2-10: Definition of the AT cut of quartz within the IEEE 1978 standard. The AT
cut is defined as: (YXl) 35.25°. The first two bracketed letters specify the initial
orientation of the plate, with the thickness direction, t, along the crystal Y-axis and the
length direction, l, along the X-axis. Then up to three rotations about axes that move with
the plate are specified by the corresponding bracketed letters and the subsequent angles. In
this case only one rotation is required about the l-axis, of 35.25° (in a right-handed
sense).
164 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Figure 2-11: Defining an AT cut crystal plate within COMSOL, with normal in the
global Y direction. Within the 1978 IEEE standard the AT cut is defined as (YXl)
-35.25°. Start with the plate normal or thickness in the Ycr direction (a) and rotate the
plate 35.25° about the l-axis (b). The global coordinate system rotates with the plate.
Finally rotate the entire system so that the global coordinate system is oriented as it appears
in COMSOL (c). The local coordinate system should be defined with the Euler angles
(ZXZ: 0, 35.25°, 0). (d) shows a coordinate system for this system in COMSOL.
MODELING PIEZOELECTRIC PROBLEMS
|
165
Figure 2-12: Defining an AT cut crystal plate within COMSOL, with normal in the
global Z direction. Within the 1978 IEEE standard the AT cut is defined as (YXl)
35.25°. Begin with the plate normal in the Zcr direction, so the crystal and global systems
are coincident. Rotate the plate so that its thickness points in the Ycr direction (the starting
point for the IEEE definition), the global system rotates with the plate (b). Rotate the plate
35.25° about the l-axis (d). Finally rotate the entire system so that the global coordinate
system is oriented as it appears in COMSOL (d). The local coordinate system should be
defined with the Euler angles (ZXZ: 0, -54.75°, 0). (e) shows a coordinate system for this
system in COMSOL.
166 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Piezoelectric Losses
Losses in piezoelectric materials can be generated both mechanically and electrically.
In the frequency domain, these can be represented by introducing complex material
properties in the elasticity and permittivity matrices. Taking the mechanical case as an
example, this introduces a phase lag between the stress and the strain, which
corresponds to a Hysteretic Loss. These losses can be added to the Piezoelectric
Material by three subnodes: Mechanical Damping, Coupling Loss, and Dielectric Loss.
The losses typically defined as loss factors (see below).
The hysteretic electrical losses are usually used to represent high-frequency electrical
losses that occur as a result of friction impeding the rotation of the microscopic dipoles
that produce the material permittivity.
Low-frequency losses, corresponding to a finite material conductivity, can be added to
the model through an Electrical Conductivity (Time Harmonic) subnode. This feature
operates only in the frequency domain.
In the time domain, the losses can be added by:
• Using the Rayleigh Damping option in the Mechanical Damping and Coupling Loss
subnodes to the Piezoelectric Material,.
Rayleigh Damping
• Using either the Dispersion, or Complex permittivity, or Maximum Loss Tangent option
in the Dielectric Loss subnode to the Piezoelectric Material.
These types of damping are also available in the frequency domain.
Rayleigh Damping
HYSTERETIC LOSS
In the frequency domain, the dissipative behavior of the material can be modeled using
complex-valued material properties, irrespective of the loss mechanism. Such hysteretic
losses can be applied to model both electrical and mechanical losses. For more
information about hysteretic losses, see Ref. 1 to Ref. 4.
MODELING PIEZOELECTRIC PROBLEMS
|
167
For the case of piezoelectric materials, this means that the constitutive equations are
written as follows.
For the stress-charge formulation
T
T = c̃ E S – ẽ E
D = ẽT +  0 ̃ rS E
where T is the stress tensor, and S is the strain tensor.
For the strain-charge formulation,
T
S = s̃ E T + d˜ E
D = d˜ S +  0 ̃ rT E
All constitutive matrices in the above equation can be complex-valued matrices, where
the imaginary parts define the dissipative function of the material.
Both the real and complex parts of the material data must be defined so as to respect
the symmetry properties of the material being modeled and with restrictions imposed
by the laws of physics.
A key requirement is that the dissipation density is positive; that is, there
is no power gain from the passive material. This requirement sets rules for
the relative magnitudes for all material parameters. This is important
when defining the coupling losses.
In COMSOL, you can enter the complex-valued data directly or by means of loss
˜ is represented as pairs of a
factors. When loss factors are used, the complex data X
real-valued parameter
˜
X = real  X
and a loss factor
˜   real  X
˜
 X = imag  X
the ratio of the imaginary and real part, and the complex data is then:
˜ = X  1  j 
X
X
168 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
where the sign depends on the material property used. The loss factors are specific to
the material property, and thus they are named according to the property they refer to,
for example, cE. For a structural material without coupling, simply use s, the
structural loss factor.
The loss factors are defined so that a positive loss factor value usually corresponds to a
positive loss. The complex-valued data is then based on sign rules.
By default, there is no damping until at least one of the damping and losses related
subnodes is added.
For the Piezoelectric Material node, the following equations apply via the
corresponding three subnodes:
Mechanical Damping
m n
c̃ E
m n
s̃ E
m n
 1 + j cE 
m n
 1 – j sE 
= cE
= sE
m n
m n
where m and n refer to components of each matrix.
Coupling Loss
ẽ
m n
˜ m n
d
=e
m n
=d
m n
 1 + j e
m n

m n
 1 + j d 
Dielectric Loss
m n
m n
m n
m n
m n
m n
̃ rS =  rS  1 – j S 
̃ rT =  rT  1 – j T 
Note that the multiplication is applied component-wise.
The loss factors can also be entered as scalar isotropic factors independently of the
material and the other coefficients.
A good check on the chosen values is to compute a number of eigenfrequencies,
possibly using some different sets of boundary conditions. All computed
eigenfrequencies must have a positive imaginary part in order to represent a damped
motion.
MODELING PIEZOELECTRIC PROBLEMS
|
169
In practice, it is often difficult to find complex-valued data for each of the matrix
elements in the literature. Measuring the losses independently is a challenging task.
Two important particular cases are available in COMSOL, for which the
dielectric loss data can be entered based on experimentally measurable
quantities:
• Complex Permittivity
• Maximum Loss Tangent
DIELECTRIC DISPERSION
The Dielectric Loss subnode can be set to use the Dispersion option. In such case, the
following equations need to be solved in the time domain:
   D + J p = 0
t

Jp + d
J p
E
=  0  rS
t
t
(2-17)
(2-18)
where you can specify two material parameters: the relaxation time d and the relative
permittivity increment rS. The latter can be either a matrix or a scalar quantity. This
model is a one-term version of the more general Debye dispersion model, Ref. 13.
The constitutive relation is assumed as
D = eS +  0   E
(2-19)
where S is the strain tensor, and  is the relative permittivity in the high-frequency
limit (that is, for excitations with a characteristic time much shorter than the relaxation
time d).
The parent Piezoelectric Material node has an input for the relative
permittivity, rS, which is used in stationary studies. You can choose how
this input will be interpreted in the dispersion computations. The options
are:
• High-frequency limit. In this case,   rS is used.
• Low-frequency limit. In this case,   rS  rS is used. Note that for
consistency,  must always be positive valued.
170 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
With the absence of free electric charges, Equation 2-17 and Equation 2-18 can be
combined and integrated in time to yield the following equation:
D
   D +  d
+  0  rS E = 0
t
This is the equation form used in COMSOL Multiphysics for time-dependent analysis.
For the eigenfrequency and frequency domain analyses, the corresponding equation is:
    1 + j d  jD +  0  rS jE  = 0
In most cases, i can be factored out, so that the following equation is solved:
   D + j d  D +  0  rS E  = 0
This equation, together with the constitutive relation Equation 2-19 gives
   eS +  0  ' – j'' E  = 0
(2-20)
where
 rS
' =   + -------------------------2
1 +  d  
and
 d  0  rS
'' = --------------------------2
1 +  d  
Equation 2-20 shows how the dispersion parameters contribute to the polarization
and losses. Thus, the effective relative permittivity decreases with the excitation
frequency from the low-frequency limit   rS down to the high-frequency limit .
The damping effect vanishes for both large and small frequencies, and it reaches the
maximum for   1d.
If your license includes either the AC/DC Module or MEMS Module,
more options for modeling dielectric dispersion can be found in
Dispersion section in the AC/DC Module User’s Guide.
The following two sections present two cases, for which the dielectric dispersion data
can be related to other experimentally measurable quantities. Both cases, can be used
MODELING PIEZOELECTRIC PROBLEMS
|
171
in Eigenfrequency, Frequency Domain, and Time Dependent study. The software will
apply the dispersion model equations, for which the effective relaxation time and
relative permittivity increment are computed automatically based on the node input
parameters.
Complex Permittivity
In this case, the complex relative permittivity is known at a certain reference frequency
'  f ref  – j''  f ref 
The relaxation time and relative permittivity contribution cane be computed as
–1
 d =  ref ''  ' –   
–1
2
 rS = ' –   +  ''   ' –   
–1
where ref  2fref.
If the relative permittivity rS (input on the Piezoelectric Material parent node) is
selected to represent the low-frequency limit, one has
2
  = ' –  ''    rS – ' 
–1
If rS is selected to represent the high-frequency limit, one can simply use   rS
instead.
Maximum Loss Tangent
The loss tangent is defined as a function of the frequency
  f  = tan  = ''  '
so that the complex relative permittivity can be written as
 r  f  = '  I – j 
For many materials, the loss tangent reaches a maximum at certain frequency fref
within the frequency range of interested
 max = max  f  =   f ref 
The relaxation time cane be computed as
–1
2
 d =  ref   max +   max + I 
172 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
12

where ref  2fref.
If the relative permittivity rS (input on the Piezoelectric Material parent node) is
selected to represent the low-frequency limit, the relative permittivity contribution is
computes as
 rS =  rS –  
where   dref2rS.
If the relative permittivity rS is selected to represent the high-frequency limit, it is
computed as
2
 rS =    d  ref  – I  
where   rS.
ELECTRICAL CONDUCTIVITY (TIME HARMONIC)
For frequency domain and eigenfrequency analyses, the effect of electrical conductivity
of the piezoelectric material (see Ref. 2, Ref. 5, and Ref. 6) can be included. Thus, in
addition to the displacement current, the conduction electric current term is used:
   jD + J e  = 0
Je = e E
where e is the material electrical conductivity, and E is the electric field. The above
form of the equation is used for the eigenfrequency analysis in COMSOL
Multiphysics.
When the conduction loss is applied, the default eigenvalue analysis will
in most cases return a number of pure imaginary eigenfrequencies. To
avoid this, you can configure the solver to search for eigenvalues with real
part larger than zero.
Do not use any dielectric loss factor damping together with the
conduction loss in an eigenfrequency analysis.
MODELING PIEZOELECTRIC PROBLEMS
|
173
In the COMSOL Multiphysics Reference Manual:
• Selecting a Stationary, Time-Dependent, or Eigenvalue Solver
• Eigenvalue Solver
For the frequency domain analysis, the angular frequency is just a parameter, and the
equation can be transformed into
–1
   D – j  e E  = 0
which allows you to use both a dielectric loss factor and electrical conductivity in a
frequency response study. In such case, ensure that the loss factor refers to the
alternating current loss tangent, which dominates at high frequencies, where the effect
of ohmic conductivity vanishes (Ref. 7).
Conduction loss can be combined with Dielectric Dispersion for both eigenfrequency
and frequency domain analyses. The following equation forms are used, respectively,
in the frequency domain:
–1
   D + j d  D +  0  rS E +   d – j J e  = 0
and in eigenfrequency analyses:
    1 + j d  jD +  0  rS jE +  1 + j d  J e  = 0
References for Piezoelectric Damping
1. R. Holland and E.P. EerNisse, Design of Resonant Piezoelectric Devices, Research
Monograph No. 56, The M.I.T. Press, 1969.
2. T. Ikeda, Fundamentals of Piezoelectricity, Oxford University Press, 1990.
3. A.V. Mezheritsky, “Elastic, Dielectric, and Piezoelectric Losses in Piezoceramics:
How it Works all Together,” IEEE Transactions on Ultrasonics, Ferroelectrics, and
Frequency Control, vol. 51, no. 6, 2004.
4. K. Uchino and S. Hirose, “Loss Mechanisms in Piezoelectrics: How to Measure
Different Losses Separately,” IEEE Transactions on Ultrasonics, Ferroelectrics, and
Frequency Control, vol. 48, no. 1, pp. 307–321, 2001.
174 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
5. P.C.Y. Lee, N.H. Liu, and A. Ballato, “Thickness Vibrations of a Piezoelectric Plate
With Dissipation,” IEEE Transactions on Ultrasonics, Ferroelectrics, and Frequency
Control, vol. 51, no. 1, 2004.
6. P.C.Y. Lee and N.H. Liu, “Plane Harmonic Waves in an Infinite Piezoelectric Plate
With Dissipation,” Frequency Control Symposium and PDA Exhibition, pp. 162–
169, IEEE International, 2002.
7. C.A. Balanis, “Electrical Properties of Matter,” Advanced Engineering
Electromagnetics, John Wiley & Sons, chapter 2, 1989.
8. “Standards on Piezoelectric Crystals, 1949”, Proceedings of the I. R. E.,vol. 37,
no.12, pp. 1378–1395, 1949.
9. IEEE Standard on Piezoelectricity, ANSI/IEEE Standard 176-1987, 1987.
10. IEEE Standard on Piezoelectricity, ANSI/IEEE Standard 176-1978, 1978.
11. B.A. Auld, Acoustic Fields and Waves in Solids, Krieger Publishing, 1990.
12. R. Bechmann “Elastic and Piezoelectric Constants of Alpha-Quartz,” Physical
Review B, vol. 110 no. 5, pp. 1060–1061, 1958.
13. N.S. Stoykov, T.A. Kuiken, M.M. Lowery, and A. Taflove, “Finite-element
time-domain algorithms for modeling linear Debye and Lorentz dielectric dispersions
at low frequencies,” IEEE Transactions on Biomedical Engineering, vol. 50, no. 9,
pp. 1100–1107, 2003.
Piezoelectric Coupling
The piezoelectric effect is an interaction between the mechanical and electrical physics,
where a stress applied on a piezoelectric material generates a voltage (direct effect) or
a voltage applied on it generates the deformation of the material (inverse effect). In
COMSOL Multiphysics, the Piezoelectricity interface is constituted of one Solid
Mechanics and one Electrostatics interface, which are coupled together by a
Piezoelectricity multiphysics feature. Hence a piezoelectric problem contains solid and
electrostatic domains, with at least one domain shared by the two physics interfaces
and with the piezoelectric coupling defined on it.
MODELING PIEZOELECTRIC PROBLEMS
|
175
Create the Piezoelectricity Interface and Define Domains
A piezoelectric problem can be set up in different ways:
• By selecting Piezoelectricity from the Model Wizard,
• By choosing Piezoelectricity from the Add Physics menu when working in an existing
model, or
• By adding the corresponding features to create the coupling manually.
In the first two cases, by default all the domains in the model are assumed to be
piezoelectric materials.
When setting up the problem manually (that is, by adding single physics interfaces one
at a time) both Solid Mechanics and Electrostatics interfaces should be added. Then, you
have to specify which domains are in each physics, and which domains are to be
modeled as piezoelectric materials.
1 On the Solid Mechanics interface Settings window, locate the Domain Selection
section. Select the domains which undergo structural deformation, including the
piezoelectric material domains.
2 Go to the Solid Mechanics>Piezoelectric Material node (if it is not yet available, add
it). Select the domains where the piezoelectric effect applies. Domains which are not
piezoelectric can be modeled using other available material models.
3 Go to the Electrostatics node and under Domain Selection select the domains the
electrostatics equations must be solved. These domains include all the piezoelectric
domains, and any other insulating domains.
Since metals usually have a conductivity several orders of magnitude
higher than other materials, it is normal not to solve the electrostatics
equations in their corresponding domains, but instead the surfaces of the
material are represented as isopotentials with an appropriate boundary
condition (usually a terminal or floating potential).
4 Go to the Electrostatics>Charge Conservation, Piezoelectric node (if it is not yet
available, add it). Select the domains where the piezoelectric effect has to be
modeled.
5 A Multiphysics>Piezoelectricity node is already present if the coupling was added
using either the Model Wizard or Add Physics window. If the model is set up manually
176 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
(that is, single physics interfaces are added), right-click the Multiphysics Couplings
node to add a Piezoelectricity coupling.
6 Confirm that all the domains where the piezoelectric material is present are selected.
Only domains that have both Charge Conservation, Piezoelectric selected in
the Electrostatics interface and Piezoelectric Material selected in the Solid
Mechanics interface are selected. The selection of this feature cannot be
edited. If several Solid Mechanics or Electrostatics interfaces are present,
select the correct ones.
7 Confirm that remaining domains are well assigned:
- Solid and electrostatic domains: In these domains, the electrostatics and
structural problems are solved independently without any piezoelectric coupling.
This is the case for insulators.
- Solid–only domains: In these domains, only mechanical phenomena are modeled,
and the electrostatics phenomena are neglected. Metals are typically modeled in
this way, because their conductivity is so high that their surfaces can be treated as
isopotential surfaces within the electrostatics problem. In some cases, insulators
are modeled using these settings, for example, when there is no potential applied
across the domain, and correspondingly solving the electrostatics equations
would produce a constant potential and waste computing resources.
- Electrostatics-only domains: Those domains are nonsolid. This is typically the
case of air, in which the electrostatics is solved but not mechanics.
- Nonsolid and nonelectrostatic domains: In those domains, another physics is
solved. A typical example is an acoustic domain in the case of piezoacoustic
modeling.
Complete Settings of Piezoelectric Materials
Go to the Solid Mechanics>Piezoelectric Material node. In the Settings window,
complete these settings:
• Coordinate System Selection section: The material is poled in the x3 direction of the
coordinate system (x1, x2, x3) specified in this section. By default, it is set to the
global coordinate system. If the piezoelectric material is poled along another
direction, you need to define a coordinate system so that its third direction is aligned
MODELING PIEZOELECTRIC PROBLEMS
|
177
with the poling direction. Then, assign it as the coordinate system which orients the
material in the Coordinate System Selection section.
If a given piezoelectric material is present with several orientations (such
as stacked piezoelectric disks) you need to define several Piezoelectric
Material nodes and to assign a different coordinate system for each of
them.
• Piezoelectric Material Properties: Select whether the constitutive relation of
piezoelectric material is in Stress-charge or in Strain-charge form. This choice
defines the type of material properties that will be used.
• Geometric Nonlinearity: select the check box to force strains to be linear.
• Energy Dissipation: Select the check box to enable the calculation of the dissipated
energy.
Add Damping and Loss
In the physics toolbar you can add attributes to the Piezoelectric Material node,
especially the following damping and loss contributions:
• Mechanical Damping: Specify the domains of application, then choose if you want to
define a loss factor for cE, a loss factor for sE (in Strain-charge form), an isotropic
loss factor, or a Rayleigh damping.
• Dielectric Loss: Specify the domains of application, then choose if you want to define
a loss factor for rS, a loss factor for rT (in Strain-charge form), or dispersion.
• Coupling Loss: Specify the domains of application, then choose if you want to define
a loss factor for e, a loss factor for d (in Strain-charge form), or Rayleigh damping.
• Conduction Loss (Time-Harmonic): Specify the domains of application, then choose
how you want to define the Electrical conductivity.
Define Material Properties
Define material properties for the piezoelectric materials. The material library contains
several common piezoelectric materials under the piezoelectric section. If you want to
define your own piezoelectric material, you need to specify its properties by hand. The
required properties depend on whether the constitutive relations are in Stress-charge
or Strain-charge form, and which damping and loss attributes are created. Defining all
178 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
piezoelectric settings before materials preselects the required properties and makes the
completion easier:
MECHANICAL PROPERTIES
3
• Density rho (SI unit: kg/m )
• Elasticity matrix cE (SI unit: Pa) in Stress-charge form.
• Compliance Matrix sE (SI unit: 1/Pa) in Strain-charge form.
ELECTROSTATIC PROPERTIES
• Relative Permittivity rS (dimensionless) in Stress-charge form.
• Relative Permittivity rT (dimensionless) in Strain-charge form.
COUPLING PROPERTIES
• Coupling matrix eES (SI unit: C/m2) in Stress-Charge form.
• Coupling matrix dET (SI unit: C/N) in Strain-charge form.
DAMPING AND LOSS PROPERTIES
• Either loss factor cE for elasticity matrix cE, or the loss factor sE for compliance
matrix sE: required when Mechanical Damping is present. Both are dimensionless,
the latter is valid only in Strain-Charge form.
• Either loss factor  S for electrical permittivity matrix rS, or loss factor  T for
electrical permittivity matrix rT: required when Dielectric Loss is present. TBoth
are dimensionless, the latter is valid only in Strain-Charge form.
• Either loss factor e for coupling matrix e, or loss factor d for coupling matrix d:
required when Coupling Loss is present. Both are dimensionless, the latter is valid
only in Strain-Charge form.
• Electrical conductivity e (SI unit: S/m): required when Conduction Loss is
present.
Working with Materials and Piezoelectric Materials Library in the
COMSOL Multiphysics Reference Manual.
MODELING PIEZOELECTRIC PROBLEMS
|
179
Coupling Piezoelectricity with Acoustics
Using piezoelectric materials for an acoustic application is common, such as in sonars,
microphones, sensors, and so forth. This is why coupling piezoelectric devices with
acoustic domains is of particular interest for these applications.
Compared to a single piezoelectric model, you need to add a pressure acoustics
interface, for example, Pressure Acoustics, Frequency Domain or Pressure Acoustics,
Transient (depending on which study type you want to use) plus an Acoustic–Structure
Boundary coupling under the Multiphysics Couplings node. You can also directly create
the nodes that are needed for coupling by adding an Acoustic-Piezoelectric Interaction
interface from the Model Wizard or Add Physics windows. If solid and acoustic domains
are correctly defined, then the right coupling boundaries are automatically selected.
Then specify domains of application for each physics.
• Select solid domains and Piezoelectric Material domains in Solid Mechanics.
• Select electrostatic domains and Charge Conservation, Piezoelectric domains in
Electrostatics.
• Select acoustic domains in a Pressure Acoustics node.
• Under the Multiphysics branch, confirm that selections for Piezoelectricity and
Acoustic–Structure Boundary are the right ones. If several Pressure Acoustics, Solid
Mechanics, or Electrostatics interfaces are present, select the right ones that need to
be coupled in the multiphysics interfaces.
• Continue the modeling process by entering the settings for each physics interface
and feature and define materials.
180 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Modeling Electrostrictive and
Ferroelectroelastic Materials
Electrostriction Coupling
Electrostriction is an interaction between the mechanical and electric physics, where an
electric field applied on electrostrictive material generates the deformation of the
material (direct effect), and a stress applied on it changes the material polarization
(inverse effect). In contrast to linear piezoelectricity, the electrostrictive strain induced
in the polarized material is proportional to the square of the polarization. Thus, the
strain will remain the same if the direction of the applied electric field is changed to the
opposite.
Ferroelectricity
The ferroelectroelasticity and ferroelectricity phenomena are related to phase
transitions in materials. In its ferroelectric phase, the material exhibits spontaneous
polarization, so that it is constituted of domains with nonzero polarization even at zero
applied field. This is similar to permanent magnetism in ferromagnetics, which explains
the name used for such materials. Electrostriction in ferroelectroelastic materials can
be related to the domain rotation. Thus, the applied electric field can both rearrange
the domains resulting into the net polarization and rotate the domains mechanically.
Thus, the material extends in the direction of the electric field and contracts in the
direction perpendicular to the field. The domain rotation can be affected by an applied
mechanical stress, which also results into the effective polarization. At very large
electric fields, the electrostrictive effect saturates, as all ferroelectric domains in the
material are aligned along the direction of the applied field. Domain wall interactions
can also lead to a significant hysteresis in the polarization and strain.
Many piezoelectric materials exhibit such nonlinear ferroelectroelastic behavior at large
applied electric fields.
Multiphysics Interfaces
In COMSOL Multiphysics, the electrostrictive effect can be modeled using two
multiphysics interfaces: Electrostriction and Ferroelectroelasticity. Both interfaces are
constituted of one Solid Mechanics and one Electrostatics interface, which are coupled
MODELING ELECTROSTRICTIVE AND FERROELECTROELASTIC MATERIALS
|
181
together via an Electrostriction multiphysics feature. However, in case of
Ferroelectroelasticity, the corresponding Electrostatics interface will contain a dedicated
feature Charge Conservation, Ferroelectric.
The Electrostriction interface electrostatically can be used for modeling electrostatically
actuated structures in regimes when the electric polarization can be assumed to vary
linear with the applied electric field.
The Ferroelectroelasticity can be used for modeling nonlinear electromechanical
interaction in ferroelectric and piezoelectric materials at high applied electric fields.
Electric polarization in such materials depends nonlinearly on the applied electric field
including possible hysteresis and saturation effects.
Ferroelectricity in the AC/DC Module User’s Guide.
Electrostriction and Ferroelectroelasticity in the Structural Mechanics
Module User’s Guide.
182 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Modeling Magnetostrictive Materials
Magnetostriction Coupling
Magnetostriction is an interaction between the mechanical and magnetic physics,
where a magnetic field applied on magnetostrictive material generates the deformation
of the material (direct effect or Joule effect), while a mechanical stress applied on it
changes the material magnetization (inverse effect or Villari effect).
The magnetostrictive strain has a nonlinear dependence on the magnetic field and the
mechanical stress in the material. However, the effect can be modeled using linear
coupled constitutive equations if the response of the material consists of small
deviations around an operating point (bias point). This type of coupling is reffed to as
Piezomagnetism.
In COMSOL Multiphysics, there are two multiphysics interfaces for modeling either
linear or nonlinear magnetostriction, respectively:
• The Piezomagnetism Interface
• The Nonlinear Magnetostriction Interface
Both multiphysics interfaces, the Magnetostriction interfaces are constituted of one
Solid Mechanics and one Magnetic Fields interface, which are coupled together via either
Piezomagnetism or Nonlinear Magnetostriction multiphysics coupling feature. Hence
a magnetostriction problem contains solid and magnetic domains, with at least one
domain shared by the two physics interfaces and with the magnetostriction coupling
defined on it.
Linear vs. Nonlinear Magnetostriction
For piezomagnetic model, it is possible to express the relation between the stress S,
strain , magnetic field H, and magnetic flux density B in either a stress-magnetization
form or strain-magnetization form. In COMSOL Multiphysics, both constitutive
forms can be used; simply select one, and the software will make all necessary
transformations if needed. You find all the necessary material data inputs within the
Piezomagnetic Material selected in the Solid Mechanics interface.
The nonlinear model of magnetostrictive strain can be used for the whole range from
full demagnetization to saturation magnetization. In case of nonlinear
magnetostriction, the magnetization model can be selected. The following options are
MODELING MAGNETOSTRICTIVE MATERIALS
|
183
available: Langevin function, Hyperbolic tangent, User defined, and Linear. The last
option will make it possible to find an explicit expression for the magnetization. Note
however that such model does not have a proper saturation behavior, and thus it
should be used only in the operating range far from saturation. For all other choices,
the magnetization vector components will be treated as extra dependent variables.
For more details, see the corresponding theory section in Magnetostriction and
Piezomagnetism.
Create the Magnetostriction Interface and Define Domains
A magnetostriction problem can be set up in different ways:
• By selecting either Piezomagnetism or Nonlinear Magnetostriction from the Model
Wizard,
• By choosing either Piezomagnetism or Nonlinear Magnetostriction from the Add
Physics menu when working in an existing model, or
• By adding the corresponding coupling features to create the coupling manually.
In the first two cases, by default all the domains in the model are assumed to be
magnetostrictive materials.
PIEZOMAGNETISM
When setting up the problem manually (that is, by adding single physics interfaces one
at a time) both Solid Mechanics and Magnetic Fields interfaces should be added. Then,
you have to specify which domains are in each physics, and which domains are to be
modeled as piezomagnetic materials.
1 On the Solid Mechanics interface Settings window, locate the Domain Selection
section. Select the domains which undergo structural deformation, including the
piezomagnetic material domains.
2 Go to the Solid Mechanics>Piezomagnetic Material node. If it is not yet available, add
such node. Select the domains where the piezomagnetic effect applies. You find all
the necessary material data inputs within the Piezomagnetic Material. This includes
the elasticity, magnetic permeability and coupling matrices. Nonpiezomagnetic
domains can be modeled using any other available structural material model.
3 Go to the Magnetic Fields node and under Domain Selection select the domains the
magnetics equations must be solved. These domains include all the piezomagnetic
domains, and any other magnetic domains.
184 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
4 Go to the Magnetic Fields>Ampere’s Law, Piezomagnetic node. If it is not yet available,
add such node. Select the domains where the piezomagnetic effect needs to be
modeled.
5 A Multiphysics>Piezomagnetism node is already present if the coupling was added
using either the Model Wizard or Add Physics window. If the model is set up manually
(that is, single physics interfaces are added), right-click the Multiphysics Couplings
node to add a Piezomagnetism coupling. If several Solid Mechanics or Magnetic Fields
interfaces are present, select the correct ones. By default, the model will be solved
as fully coupled. Alternatively, on the Piezomagnetism coupling node, you can select
to include only either Joule effect or Villari effect. Confirm that all the domains
where the piezomagnetic material is present are selected.
Only domains that have both Ampere’s Law, Piezomagnetic selected in the
Magnetic Fields interface and Piezomagnetic Material selected in the Solid
Mechanics interface are applicable in the selection for Piezomagnetism
coupling. The selection of this multiphysics coupling node cannot be
edited directly.
6 Confirm that remaining domains are well assigned:
- Solid and magnetic domains: In these domains, the magnetics and structural
problems are solved independently without any piezomagnetic coupling. This
represents deformable magnetic materials for which such coupling is negligible.
Exclude such domains from the selections for all Ampere’s Law, Piezomagnetic, and
Piezomagnetic Material nodes under the corresponding interfaces.
- Solid–only domains: In these domains, only mechanical phenomena are modeled,
and the magnetics phenomena are neglected. This represents deformable solid
nonmagnetic materials. Exclude such domains from the selection in the Magnetic
Fields interface.
- Magnetics-only domains: Those domains are nonsolid. This is typically the case
of air, in which the magnetics is solved but not mechanics. Exclude such domains
from the selection in the Solid Mechanics interface.
- Nonsolid and nonmagnetic domains: In those domains another physics is solved.
Typical examples are acoustic domains and fluid flow domains, which might be
MODELING MAGNETOSTRICTIVE MATERIALS
|
185
present in certain multiphysics application. Exclude such domains from the
selections on both Magnetic Fields and Solid Mechanics interface nodes.
• Piezomagnetic Material
• Ampère’s Law, Piezomagnetic
NONLINEAR MAGNETOSTRICTION
When setting up the problem manually (that is, by adding single physics interfaces one
at a time) both Solid Mechanics and Magnetic Fields interfaces should be added. Then,
you have to specify which domains are in each physics, and which domains are to be
modeled as magnetostrictive materials.
Instead of Magnetic Fields interface, you can also use Rotating Machinery,
Magnetic interface.
1 On the Solid Mechanics interface Settings window, locate the Domain Selection
section. Select the domains which undergo structural deformation, including the
magnetostrictive material domains. The following structural material nodes are
supported to represent the magnetostrictive domains: Linear Elastic Material and
Hyperelastic Material (available with the Nonlinear Structural Materials Module).
2 Go to the Magnetic Fields node and under Domain Selection select the domains the
magnetics equations must be solved. These domains include all the magnetostrictive
domains, and any other magnetic domains.
3 Go to the Magnetic Fields>Ampere’s Law, Nonlinear Magnetostrictive node. If it is not
yet available, add such node. Select the domains where the magnetostriction effect
needs to be modeled. You can specify the magnetization model and enter the related
material data on the node.
4 A Multiphysics>Nonlinear Magnetostriction node is already present if the coupling was
added using either the Model Wizard or Add Physics window. If the model is set up
manually (that is, single physics interfaces are added), right-click the Multiphysics
Couplings node to add a Nonlinear Magnetostriction coupling. If several Solid
Mechanics or Magnetic Fields interfaces are present, select the correct ones. On the
coupling node, you can also select the magnetostriction model depending on the
material symmetry and enter the corresponding coupling data. By default, the
model will be solved as fully coupled. Alternatively, on the Nonlinear Magnetostriction
186 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
coupling node, you can select to include only either Joule effect or Villari effect.
Select only the domains where the magnetostrictive effect needs to be modeled.
On the Nonlinear Magnetostriction coupling node, the applicable domains
in the selection are only domains that have both Ampere’s Law, Nonlinear
Magnetostrictive selected in the Magnetic Fields interface and Linear Elastic
Model (or Hyperelastic Model) selected in the Solid Mechanics interface.
5 Confirm that remaining domains are well assigned:
- Solid and magnetic domains: In these domains, the magnetics and structural
problems are solved independently without any magnetostriction coupling. This
represents deformable magnetic materials for which such coupling is negligible.
Exclude such domains from the selection in the Nonlinear Magnetostriction
coupling node.
- Solid–only domains: In these domains, only mechanical phenomena are modeled,
and the magnetics phenomena are neglected. This represents deformable solid
nonmagnetic materials. Exclude such domains from the selection in the Magnetic
Fields interface.
- Magnetics-only domains: Those domains are nonsolid. This is typically the case
of air, in which the magnetics is solved but not mechanics. Exclude such domains
from the selection in the Solid Mechanics interface.
- Nonsolid and nonmagnetic domains: In those domains another physics is solved.
Typical examples are acoustic domains and fluid flow domains, which might be
present in certain multiphysics applications. Exclude such domains from the
selections in both Magnetic Fields and Solid Mechanics interfaces.
• Ampère’s Law, Nonlinear Magnetostrictive
MODELING MAGNETOSTRICTIVE MATERIALS
|
187
Mechanical Damping and Losses
Damping and losses are important factors for determining the response in
time-dependent and frequency domain studies, and sometimes also when computing
eigenfrequencies. This section describes how to model damping and loss using
different damping models. In this section:
In this section:
• About Damping
• Rayleigh Damping
• Loss Factor Damping
• Viscoelastic Damping
• Explicit Complex-Valued Damping
• Equivalence Between Loss Factor, Rayleigh, and Viscous Damping
• Piezoelectric Damping
• Adding Damping in the Modal Solver
Damping Sources
There are many sources of damping in a system. Some of them are:
• Dissipation in the material. This dissipation can be for example be proportional to
the amplitude of the strain rate (viscous damping) or to the amplitude of the strain
itself (hysteretic damping).
• Thermoelastic damping, which is a thermodynamic effect which is related not only
to the state in a point, but also to the gradients of the temperature field.
• Damping caused by the surrounding medium, often air or water.
• Friction between joined parts.
• Components intended to supply damping like a dashpot in a car suspension.
It is often difficult to separate and quantify these effects, so damping modeling is one
of the biggest challenges in structural dynamics.
188 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
About Damping
Phenomenological damping models are typically invoked to model the intrinsic
frictional damping present in most materials (material damping). These models are
easiest to understand in the context of a system with a single degree of freedom. The
following equation of motion describes the dynamics of such a system with viscous
damping:
2
d u
du
m ---------2- + c ------- + ku = f  t 
dt
dt
(2-21)
In this equation u is the displacement of the degree of freedom, m is its mass, c is the
damping parameter, and k is the stiffness of the system. The time (t) dependent forcing
term is f(t). This equation is often written in the form:
2
2
d
u- + 2 du
ft
--------------0 dt +  0 u = --------2
m
dt
(2-22)
where   c2m0 and 02  km. In this case  is the damping ratio (  1 for
critical damping) and 0 is the undamped resonant frequency of the system. In the
literature it is more common to give values of  than c. The damping ratio  can also
be readily related to many of the various measures of damping employed in different
disciplines. These are summarized in Table 2-10.
TABLE 2-10: RELATIONSHIPS BETWEEN MEASURES OF DAMPING.
DAMPING
PARAMETER
DEFINITION
RELATION TO
DAMPING RATIO
Damping ratio
 = c  c critical
–
Logarithmic
decrement
u  t0 
 d = ln  ----------------------
u  t0 +  
 d  2
 « 1
where t0 is a reference time and  is the period
of vibration for a decaying, unforced degree of
freedom.
MECHANICAL DAMPING AND LOSSES
|
189
TABLE 2-10: RELATIONSHIPS BETWEEN MEASURES OF DAMPING.
DAMPING
PARAMETER
DEFINITION
RELATION TO
DAMPING RATIO
Quality factor
Q =   
Q  1   2 
where  is the bandwidth of the amplitude
resonance measured at 1  2 of its peak.
 « 1
1 Qh
 = ------  --------
2  W h
At the resonant
frequency:
Loss factor
  2
where Qh is the energy lost per cycle and Wh is
the maximum potential energy stored in the
cycle. The variables Qh and Wh are available as
solid.Qh and solid.Wh.
 « 1
In the frequency domain, the time dependence of the force and the displacement can
be represented by introducing a complex force term and assuming a similar time
dependence for the displacement. The equations
f  t  = Re  Fe
jt
 and u  t  = Re  Ue
jt

are written where  is the angular frequency and the amplitude terms U and F can in
general be complex (the arguments provide information on the relative phase of
signals). Usually the real part is taken as implicit and is subsequently dropped.
Equation 2-21 takes the following form in the frequency domain:
2
–  mU + jcU + kU = F
(2-23)
where the time dependence has canceled out on both sides. Alternatively, this equation
can be written as:
2
2
F–  U + 2j 0 U +  0 U = ---m
(2-24)
There are three basic damping models available in the structural mechanics interfaces
for explicit modeling of material damping — Rayleigh damping, viscous damping,
and loss factor models based on introducing complex quantities into the equation
system. There are also other phenomena which contribute to the damping. Some
material models, such as viscoelasticity and plasticity are inherently dissipative. It is also
possible to model damping in spring conditions.
190 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Rayleigh Damping
A common method of modeling damping is Rayleigh damping, where two damping
coefficients are specified. This type of damping is not directly related to any physical
process, but must be seen as a way to take the total damping of a structure into
account.
Rayleigh damping introduces damping in a form based on Equation 2-21. This means
that the method can be applied generally in either the time or frequency domain. The
parameter c in Equation 2-21 is defined as a fraction of the mass and the stiffness using
two parameters, dM and dK, such that
c =  dM m +  dK k
(2-25)
Substituting this relationship into Equation 2-21 and rearranging into the form of
Equation 2-22 gives:
2
2 du
2
d
u- +  
ft
--------------dM +  dK  0  dt +  0 u = --------2
m
dt
When there are many degrees of freedom m, k, and c become matrices and the
technique can be generalized.
Rayleigh damping can therefore be identified as equivalent to the damping ratio at
resonance of:
1  dM
 = ---  ---------- +  dK  0

2 
(2-26)
0
Note that Equation 2-26 holds separately for each vibrational mode in the system at
its resonant frequency. In the frequency domain it is possible to use frequency
dependent values of dM and dK. For example, setting dM  0 and dK  2/0
produces an equivalent viscous damping model at the resonant frequency 0.
While Rayleigh damping is numerically convenient, the model does not agree with
experimental results for the frequency dependence of material damping over an
extended range of frequencies. This is because the material damping forces behave
more like frictional forces (which are frequency independent) than viscous damping
forces (which increase linearly with frequency as implied by Equation 2-23). In the
frequency domain it is possible to introduce loss factor damping, which has the desired
property of frequency independence.
MECHANICAL DAMPING AND LOSSES
|
191
A complication with the Rayleigh damping model is to obtain good values for the
damping parameters dM and dK. A more physical damping measure is the damping
ratio, the ratio between actual and critical damping, often expressed as a percentage of
the critical damping. Commonly used values of the damping ratio can be found in the
literature.
Using Equation 2-26, this relationship at two frequencies, f1 and f2, with different
damping ratio, 1 and 2, results in an equation system that can be solved for dM and
dK:
1 ----------f
4f 1 1  dM
1  dK
----------f
4f 2 2
=
1
2
The damping ratios are then
1 f2 – 2 f1
 dM = 4f 1 f 2 --------------------------2
2
f2 – f1
2 f2 – 1 f1
 dK = --------------------------2
2
  f2 – f1 
Damping ratio
Using the same damping ratio, 1 = 2 = 0, does not result in a constant damping
factor inside the interval f1  f  f2. It can be shown that the damping factor is lower
inside the interval, as Figure 2-13 shows.
Rayleigh damping
(f)
0
Specified damping
f1
f2
Figure 2-13: An example of Rayleigh damping.
192 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
f
Since the coefficients dM and dK should not be negative, the damping ratios are
constrained by the respective frequencies as
f1 2 f2
----  -----  ---f2 1 f1
For many applications it is sufficient to leave dM as zero and to define damping only
using the dK coefficient. Then, according to Equation 2-26, a damping which
increases linearly with frequency is obtained. If the damping ratio f0 or loss factor
f0 is known at a given frequency f0, the appropriate value for dK is:
 dK =    f 0  =    2f 0 
In order to visualize the damping ratio as a function of frequency, click
Damping Ratio Preview (
).
Loss Factor Damping
Loss factor damping (sometimes referred to as material damping, structural damping,
or hysteretic damping) can be applied in the frequency domain.
The loss factor is a measure of the inherent damping in a material when it is
dynamically loaded. It is typically defined as the ratio of energy dissipated in unit
volume per radian of oscillation to the maximum strain energy per unit volume.
In COMSOL Multiphysics the loss information appears as a multiplier to the elastic
constitutive matrix Dc
c
D =  1 + j s D
For a nonlinear elastic material, this applies to the tangential stiffness.
The use of loss factor damping traditionally refers to a scalar-valued loss factor s. But
there is no reason that s must be scalar. Because the loss factor is a value deduced from
true complex-valued material data, it can be represented by a matrix of the same
dimensions as the anisotropic stiffness matrix. Especially for orthotropic materials,
there should be a set of loss factors of all normal and shear elasticity modulus
components, and COMSOL allows all these options, so a more general expression is.
c
D mn =  1 + j s mn D mn
MECHANICAL DAMPING AND LOSSES
|
193
For hyperelastic materials the loss information appears as a stress contribution to the
second Piola–Kirchhoff stress, S:
W s
S q = j s ---------E
Loss factor damping is available for frequency response analysis and damped
eigenfrequency analysis in all interfaces.
Viscous Damping
You can add an explicit viscous damping to several material models. Viscous damping
can be used both in time domain and frequency domain. In the viscous damping
model, and extra contribution, proportional to the strain rate, is added to the stress
tensor, as described in Viscous Damping.
You can specify the viscous damping for volumetric strains and shear strains
independently.
Equivalence Between Loss Factor, Rayleigh, and Viscous Damping
In frequency domain, it is possible to use Rayleigh damping in order to specify an
equivalent viscous damping. Set the stiffness damping parameter dK, to the loss
factor, , divided by the excitation frequency:
 - = -- dK = -------2f

The mass damping factor, dM, should be set to zero.
If, on the other hand, you would want to use a viscous damping, corresponding to a
certain Rayleigh stiffness damping, the conversion to bulk and shear viscosity can be
made using the expressions
 b = K dK
 v = G dK
where K and G are the bulk and shear moduli, respectively. Equivalently, you can
transform between loss factor damping and viscous damping,
194 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
 b = K
-------
G
 v = -------
Explicit Complex-Valued Damping
In frequency domain, it is possible to define damping by modeling the dissipative
behavior of the material using complex-valued material properties. In COMSOL
Multiphysics, you can enter the complex-valued data directly, using i or sqrt(-1) for
the imaginary unit.
However, entering complex-valued data directly into the material parameters is
incompatible with the built-in damping and viscoelasticity features.
Viscoelastic Damping
In some cases, damping is included implicitly in the material model. This is the case for
a viscoelastic material, where damping operates on the shear components of stress and
strain.
When viscoelasticity is modeled in the frequency domain, it will act as a loss factor
damping. The complex modulus G*() is the frequency-domain representation of the
stress relaxation function of viscoelastic material. It is defined as
G = G + jG =  1 + j s G
where G' is the storage modulus, G'' is the loss modulus, and their ratio sG''G' is
the loss factor. The term G' defines the amount of stored energy for the applied strain,
whereas G'' defines the amount of energy dissipated as heat; G', G'', and s can all be
frequency dependent.
Piezoelectric Damping
Piezoelectric losses are more complex and include coupling and electrical losses in
addition to the material terms. For damping in piezoelectric materials, see Piezoelectric
Losses.
For piezoelectric materials, dK is only used as a multiplier of the structural
contribution to the stiffness matrix when building-up the damping matrix as given by
MECHANICAL DAMPING AND LOSSES
|
195
Equation 2-25. In the frequency domain studies, you can use the coupling and
dielectric loss factors equal to dK to effectively achieve the Rayleigh damping
involving the whole stiffness matrix.
Adding Damping in the Modal Solver
In COMSOL it is possible to solve a problem for a set of modes in the absence of
damping, and then to use those solutions as a modal basis to solve a problem in the
time (using a time domain modal study) or frequency domain (using a Frequency
Domain, Modal study). In both of these cases it is possible to manually assign a
damping ratio to the computed modes in the time or frequency domain study. To do
that, right click on the study and choose Show Default Solver, then expand the solver
sequence until the Modal Solver node is visible. In the Settings window for that node,
add damping ratios for each of the modes.
For more details, see the section Modal Solver in the COMSOL
Multiphysics Reference Manual.
196 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Modeling Geometric Nonlinearity
This section discusses how to model problems where displacements or strains are of a
size where the deformation of the structure has to be taken into account when
formulating the equations. Examples of the type of problems where this feature is
useful include:
• Thin structures, where the deflection is of the same order of magnitude as the
thickness.
• Where the structure exhibits large rotations. A rigid body rotation of only a few
degrees causes significant strains and stresses in a material where a linear strain
representation is used.
• Where the strains are larger than a few percent.
• Contact problems.
• Where a prestress must be taken into account for computing the dynamic response
of a structure.
• Buckling problems.
• Where a deformed mesh is used.
• Fluid–Structure interaction problems.
• Contact Modeling
• Fluid–Structure Interaction
• The more formal theory is described in Analysis of Deformation
Geometric Nonlinearity, Frames, and the ALE Method
Consider the bending of a beam in the general case of a large deformation (see
Figure 2-14). In this case the deformation of the beam introduces an effect known as
geometric nonlinearity into the equations of solid mechanics.
Figure 2-14 shows that as the beam deforms, the shape, orientation, and position of
the element at its tip changes significantly. Each edge of the infinitesimal cube
undergoes both a change in length and a rotation that depends on position.
Additionally, the three edges of the cube are no longer orthogonal in the deformed
MODELING GEOMETRIC NONLINEARITY
|
197
configuration (although typically for practical strains the effect of the
nonorthogonality can be neglected in comparison to the rotation).
From a simulation perspective it is possible to solve the equations of solid mechanics
on either a fixed domain (this is often called a Total Lagrangian formulation), or on
a domain that changes continuously with the deformation. The latter approach is often
called an Updated Lagrangian formulation. These two approaches also stand in
contrast to the Eulerian formulation, which is often used for fluid mechanics. In an
Eulerian formulation, the flow through a domain fixed in space is considered, while in
the Lagrangian formulation, a fixed volume of material is considered.
In COMSOL Multiphysics, the concepts of a material frame and a
spatial frame are used. Equations formulated in the material frame will
give a Total Lagrangian formulation, while equations formulated in the
spatial frame will give an Eulerian formulation.
See Frames and Coordinate Systems in the Structural Mechanics Theory
chapter for more details.
Solid mechanics in COMSOL Multiphysics is formulated on the material frame. This
is achieved by defining a displacement field for every point in the solid, usually with
the components u, v, and w. At a given coordinate (X, Y, Z) in the reference
configuration (on the left of Figure 2-14), the value of u describes the displacement of
the point relative to its original position. The displacement is considered as a function
of the material coordinates (X, Y, Z), but it is not explicitly a function of the spatial
coordinates (x, y, z). The spatial coordinates give the current location in space of a
point in the deformed solid. As a consequence, it is only possible to compute
derivatives with respect to the material coordinates.
Taking derivatives of the displacement with respect to X, Y, and Z enables the
definition of a strain tensor. There are possible representations of the deformation. Any
reasonable representation must however be able to represent a rigid rotation of an
unstrained body without producing any strain. The engineering strain fails here, thus
it cannot be used for general geometrically nonlinear cases. One common choice for
representing large strains is the Green–Lagrange strain. It contains derivatives of the
displacements with respect to the original configuration. The values therefore
represent strains in material directions. This choice allows a physical interpretation, but
it must be realized that even for a uniaxial case, the Green–Lagrange strain is strongly
nonlinear with respect to the displacement. If an object is stretched to twice its original
198 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
length, the Green–Lagrange strain is 1.5 in the stretching direction. If the object is
compressed to half its length, the strain would read 0.375.
An even more fundamental quantity is the deformation gradient, which contains the
derivatives of the deformed coordinates with respect to the original coordinates:
x- = u + I
F = -----X
The deformation gradient contains all information about the local deformation in the
solid, and can be used to form many other strain quantities. As an example, the Green–
Lagrange strain is
1 T
 = ---  F F – I 
2
An element at a point (X, Y, Z) specified in the material frame moves with a single
piece of material throughout a solid mechanics simulation. It is often convenient to
define material properties in the material frame as these properties move and rotate
naturally together with the volume element at the point at which they are defined as
the simulation progresses. In Figure 2-14 this point is illustrated by the small cube
highlighted at the end of the beam, which is stretched, translated, and rotated as the
beam deforms. The three mutually perpendicular faces of the cube in the Lagrange
MODELING GEOMETRIC NONLINEARITY
|
199
frame are no longer perpendicular in the deformed (spatial) frame. The deformed
frame coordinates in this frame are denoted (x, y, z) in COMSOL.
Figure 2-14: An example of the deformation of a beam showing the undeformed state
(left) and the deformed state (right) of the beam itself with an element near its tip
highlighted (top), of the element (center), and of lines parallel to the x-axis in the
undeformed state (bottom).
It is important to note that, as the solid deforms, the Lagrangian frame
becomes a nonorthogonal curvilinear coordinate system (see the lower
part of Figure 2-14 to see the deformation of the X-axis). Particular care
is therefore required when defining physics in this coordinate system.
FRAME CONTROL CONFLICTS
Under geometric nonlinearity, a Solid Mechanics interface (or a similar structural
mechanics interface such as Multibody Dynamics) will assume control over the spatial
frame in the domains where it is active. However, the definition of the spatial frame
must be unique, and there may be conflicts. Some examples are:
• A Solid Mechanics interface and a moving mesh feature (for example, Deforming
Domain or Rotating Domain) have a common selection. In this case, the selection in
200 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
the Solid Mechanics interface will be marked as “not applicable”. Thus, it is not
possible to solve a structural mechanics problem on such a domain.
• There are more than one frame-controlling physics interfaces active on the same
domain.
When two physics interfaces are competing for frame control, you will get the error
message “Multiple moving frame specifications on the same selection” when trying to
run the study. To identify the problem, go to the settings for the study step, and select
Modify model configuration for study step. There, you will get an overview of the frame
control in the model. Note that it is quite possible that several features control the
spatial frame, as long as it is on different geometric selections.
When you select a physics interface in the tree view, you can click the Control Frame
) to toggle whether that interface should control the spatial
frame or not.
Deformation button (
MODELING GEOMETRIC NONLINEARITY
|
201
STRESS MEASURES
For example, in the spatial frame it is easy to define forces per unit area (known as
tractions) that act within the solid and to define a stress tensor that represents all of
these forces that act on a volume element. Such forces could be physically measured,
for example, using an implanted piezoresistor. The stress tensor in the spatial frame is
called the Cauchy or true stress tensor (in COMSOL Multiphysics this is referred to as
the spatial stress tensor). To construct the stress tensor in the Lagrangian frame a
tensor transformation must be performed on the Cauchy stress. This produces the
second Piola–Kirchhoff (or material) stress, which can be used with the material strain
to solve the solid mechanics problem in the (fixed) material frame. This is how the
Solid Mechanics interface works when geometric nonlinearities are enabled.
For the Cauchy stress tensor, both the force components and the normal to the area
on which the force is acting have fixed directions in space. This means that if a stressed
body is subjected to a pure rotation, the actual values of the stress components will
change. What was originally a uniaxial stress state might be transformed into a full
tensor with both normal and shear stress components. In many cases, this is neither
what you want to use nor what you would expect.
Consider for example an orthotropic material with fibers having a certain orientation.
It is much more plausible that you want to see the stress in the fiber direction, even if
the component is rotated. The Second Piola–Kirchhoff stress has this property as it is
defined along the material directions. In the figure below, an originally straight
cantilever beam has been subjected to bending by a pure moment at the tip. The
xx-component of the Cauchy stress and Second Piola–Kirchhoff stress are shown.
Since the stress is physically directed along the beam, the xx-component of the Cauchy
stress (which is related to the global x direction) decreases with the deflection. The
Second Piola–Kirchhoff stress, however, has the same through-thickness distribution
all along the beam, even in the deformed configuration.
202 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Figure 2-15: xx-components of the Cauchy stress tensor (top) and the second Piola–
Kirchhoff stress tensor for an initially straight beam.
Another stress measure available in COMSOL Multiphysics is the First Piola–Kirchhoff
stress. It is a multiaxial generalization of the nominal (or engineering) stress. The stress
is defined as the force in the current configuration acting on the original area. The First
Piola–Kirchhoff stress is an unsymmetric tensor, and is for that reason less attractive to
work with. Sometimes you may also encounter the Kirchhoff stress, although it is not
used in COMSOL Multiphysics. The Kirchhoff stress is just the Cauchy stress scaled
by the volume change. It has little physical significance, but can be convenient in some
mathematical and numerical operations.
Unfortunately, even without a rotation, the actual values of all these stress
representations are not the same. All of them scale differently with respect to local
volume changes and stretches. This is illustrated in the graph below. The
xx-component of four different stress measures are plotted at the fixed end of the beam
from the example above. At this point, the beam axis coincides with the x-axis, so the
directions of all stress tensor components coincide. In the center of the beam, where
strains, and thereby volume changes are small, all values approach each other. For a
case with large rotation but small strains, the different stress representations can be
seen as pure rotations of the same stress tensor.
MODELING GEOMETRIC NONLINEARITY
|
203
Figure 2-16: Stress distribution across the beam at the constrained end.
If you want to compute the resulting force or moment on a certain boundary based on
the stresses, there are in practice only two possible choices: Either integrate the Cauchy
stress over the deformed boundary, or integrate the First Piola–Kirchhoff stress over
the same boundary in the undeformed configuration. In COMSOL Multiphysics this
corresponds to selecting either Spatial frame or Material frame in the settings for the
integration operator.
ALE METHOD
In the case of solid mechanics, the material and spatial frames are associated directly
with the Lagrangian and Eulerian frames, respectively. In a more general case (for
example, when tracking the deformation of a fluid, such as a volume of air surrounding
a moving structure) tying the Lagrangian frame to the material frame becomes less
desirable. Fluid must be able to flow both into and out of the computational domain,
without taking the mesh with it. The arbitrary Lagrangian-Eulerian (ALE) method
allows the material frame to be defined with a more general mapping to the spatial or
Eulerian frame. In COMSOL Multiphysics, a separate equation is solved to produce
this mapping — defined by the mesh smoothing method (Laplacian, Winslow,
hyperelastic, or Yeoh) with boundary conditions that determine the limits of
204 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
deformation (these are usually determined by the physics of the system, whilst the
domain level equations are typically being defined for numerical convenience). The
ALE method offers significant advantages since the physical equations describing the
system can be solved in a moving domain.
Deformed Geometry and Moving Mesh in the COMSOL Multiphysics
Reference Manual
Geometric Nonlinearity for the Solid Mechanics Interface
In the settings for each material model in the Solid Mechanics interface, you can select
a Formulation — From study step (default), Total Lagrangian, or Geometrically linear to
set the kinematics of the deformation and the definition of strain.
When From study step is selected, the study step controls the kinematics and the strain
definition. In this situation, you can force a geometrically nonlinear analysis for a
certain study step by selecting the Include geometric nonlinearity check box in the Study
Settings section of the study step.
To have full control of the formulation, select either Total Lagrangian, or Geometrically
linear. When Total Lagrangian is selected, the physics will force the Include geometric
nonlinearity check box in all study steps.
If any active feature in the model requires the analysis to be geometrically nonlinear,
the Include geometric nonlinearity check box in the study step is selected automatically,
and it cannot be cleared. The following physics features force this behavior:
• Contact, because the deformation between the contacting boundaries is part of the
solution.
• Moving mesh (when at least one deforming domain is active).
• Hyperelastic materials, which are always formulated for large strains.
For geometrically nonlinear analysis, the behavior of several features differs from the
geometrically linear case:
• There is an important difference between using uppercase (X, Y, Z, R) and
lowercase (x, y, z, r) coordinates in expressions. The lowercase coordinates
represent the deformed position, and this introduces a dependency on the solution.
• Many features, such as coupling operators, can be specified as operating in either the
material (X, Y, Z) or the spatial (x, y, z) frame. This setting does not make a
MODELING GEOMETRIC NONLINEARITY
|
205
difference unless a geometrically nonlinear analysis is performed. In most cases you
would want to do the operation in the material frame.
• The strain representation changes from using engineering strains to Green–
Lagrange strains, unless Geometrically linear is selected in the Formulation list of a
certain material.
• Where Green–Lagrange strains are used, Second Piola–Kirchhoff stresses are also
used. This means that material data must be given in terms of these quantities. This
distinction is important only when the strains are actually large.
• For each material model, the Strain decomposition list determines how inelastic
deformations are treated. It is possible to choose an additive decomposition of
strains or a multiplicative decomposition of deformation gradients. This option is
not available when the formulation is set to Geometrically linear, for which an
additive strain decomposition is used.
• Pressure loads are interpreted as follower loads, so that the direction of the load as
well as the loaded area depend on deformation.
• Rigid connectors take finite rotations into account.
Studies and Solvers in the COMSOL Multiphysics Reference Manual
Geometric Nonlinearity for the Shell, Plate, Membrane, Beam, and
Truss Interfaces
For the Shell, Plate, Membrane, and Truss interfaces, geometrically nonlinear analysis
is handled in the same way described above. For the Membrane and Truss interfaces,
geometric nonlinearity must almost always be used, because nonlinear effects supply
stiffness in the transverse direction. The geometric nonlinearity in the Beam interface
is limited to large rotations and displacements, but small strains. It is possible to force
a geometrically linear formulation in the beam interface.
206 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Solving Geometrically Nonlinear Problems
Depending on the geometrically nonlinear effects that appear in your model, you may
have to use different solution strategies. Some problems in this class are strongly
nonlinear, while others show only a weak deviation from linearity. Some guidelines are:
• If the problem has a path dependent solution, then it must be solved in an
incremental way in order to give a correct solution. Problems including for example
plasticity or friction belong to this class. If you do the analysis in time domain, then
the solution is inherently incremental. If the analysis is stationary, invoke the
parametric continuation solver by adding an Auxiliary Sweep, and ramp up some
loading parameter. In either case, make sure that the step size is not too large.
• Problem that have a unique solution, like an elastic model subjected to large
rotations or strains can be solved in a single static load step without loss of accuracy.
It is however possible that such an approach will not converge, in which case a
parametric continuation solver must be used.
• In problems involving large rotations, the default settings of the nonlinear solver
will sometimes give a too conservative solution strategy. You can often decrease the
solution time significantly by modifying the settings under Method and Termination
in the settings for the Fully Coupled or Segregated Step node in the solver sequence.
Set Nonlinear method to Constant (Newton) and use a rather high Damping factor. In
most cases the value 1 will work.
• If you model a situation which to a large extent is a rigid rotation, it is often
necessary to use tighter tolerances than usual in order to avoid spurious stresses.
Since the strains are computed from the differences of the displacements in an
element, even a small relative error in the displacements (which are large) can cause
significant strains. This will be visible in a case where the actual stresses are small.
Prestressed Structures
You can analyze eigenfrequency, frequency domain, or time-dependent problems
where the dynamic properties of the structure are affected by a preload, such as a
tensioned string.
Usually, a study of a prestressed problem includes using two study steps. The first step
is a Stationary step in which the static preload is applied. The preload step can be
computed with or without taking geometric nonlinearity into account. In the second
study step, where you compute the eigenfrequency or the frequency response, it is
MODELING GEOMETRIC NONLINEARITY
|
207
necessary to take geometric nonlinearity into account. Even if the displacements and
strains are small, this is what gives the prestress contribution to the equations.
There are three predefined study sequences for prestressed dynamic analysis:
• Eigenfrequency, Prestressed
• Frequency Domain, Prestressed
• Frequency Domain, Prestressed, Modal
The prestressed study types assume that the loading causes small perturbations around
the prestressed state.
In a general nonlinear analysis, like a Stationary or Time Dependent study step, the full
combined effect of the prestress and other loads will automatically be included.
The same principles apply also to a linear buckling analysis, except that both study steps
should be geometrically linear. The nonlinear contribution is included in the
formulation of the buckling eigenvalue itself.
FOLLOWER LOADS
Loads that change orientation with deformation, such as a pressure, actually contribute
not only to the load but also to the stiffness. This is a physical effect and not just a
numerical artifact. Whether such loads are included or not in an Eigenfrequency study
step will affect the computed eigenfrequencies. If you for some reason do not want this
effect, you must suppress the load in the Physics and Variables section of the
Eigenfrequency node.
If you use a local coordinate system for describing a load, you must, in
case of geometric nonlinearity, pay attention to whether that coordinate
system has constant axis orientations or not. As an example, the default
boundary system has Frame set to Deformed Configuration, so that a load
represented in that system will behave as a follower load. Change to
Reference Configuration if the load should act in fixed directions.
In more general terms, any feature in which there is a dependency on the
choice of frame (material or spatial) can potentially affect the outcome of
a prestressed analysis.
CONTACT AND PRESTRESSED ANALYSIS
If a contact is included in the prestress load case, you can perform a subsequent
eigenfrequency or frequency-domain analysis in which the linearization will be made
208 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
around the computed contact state. The connection between the two boundaries is
elastic, using the penalty factor as stiffness, both for the penalty method and the
augmented Lagrangian method. If the augmented Lagrangian method is used for the
contact modeling, then the penalty factor must be constant and not dependent on the
iteration number.
The contact state is considered as fixed, so there is no harmonic perturbation in contact
quantities, such as the contact pressure.
The gap distance in a contact analysis is computed from the coordinates
of the contacting boundaries in the spatial frame. The spatial frame is
defined by the displacements in the preload step and is not affected by the
displacements in a subsequent perturbation step.
INELASTIC STRESSES AND STRAINS
When inelastic stresses and strains are part of the problem description, you need to
make some extra considerations. Such contributions are formally part of the
constitutive model but generate load vector contributions.
There are three Preset study types which can be used to set up these two
study steps: Eigenfrequency, Prestressed; Frequency Domain, Prestressed;
and Linear Buckling.
If you want to explicitly prescribe the stress field for a prestressed analysis
rather than solving for it, you should not use the two study step
procedure. In such a case, prescribe the stress field using an Initial Stress
and Strain, External Stress, or External Strain node. Then add a separate
Eigenfrequency or Frequency Domain study and select Include Geometric
Nonlinearity in the settings for the study step.
Eigenfrequency, Prestressed, Frequency Domain, Prestressed, and Linear
Buckling in the COMSOL Multiphysics Reference Manual
MODELING GEOMETRIC NONLINEARITY
|
209
• For an example of a general prestressed eigenfrequency analysis see
Bracket — Eigenfrequency Analysis: Application Library path
Structural_Mechanics_Module/Tutorials/bracket_eigenfrequency.
• For an example of an analysis where the stress state is explicitly
prescribed, see Vibrating Membrane: Application Library path
Structural_Mechanics_Module/Verification_Examples/
vibrating_membrane.
Geometric Nonlinearity for the Piezoelectric Material
PIEZOELECTRIC MATERIALS WITH LARGE DEFORMATIONS
The linear piezoelectric equations as presented in About Piezoelectric Materials with
engineering strains are valid if the model undergoes only relatively small deformations.
As soon as the model contains larger displacements or rotations, these equations
produce spurious strains that result in an incorrect solution. To overcome this
problem, so-called large deformation piezoelectric equations are required.
The Piezoelectric Material implements the large deformation piezoelectric equations
according to Yang (Ref. 1). Key items of this formulation are:
• The strains are calculated as the Green–Lagrange strains, ij:
1  u u
 ij = ---  --------i + --------j +
2  X j X i
u k u k
- ---------
 -------X i X j 
(2-27)
k
Green–Lagrange strains are defined with reference to an undeformed geometry.
Hence, they represent a Lagrangian description. In a small-strain, large rotational
analysis, the Green–Lagrange strain corresponds to the engineering strain in
directions that follow the deformed body.
• Electrical field variables are calculated in the material directions, and the electric
displacement relation is replaced by an expression that produce electric polarization
in the material orientation of the solid.
• In the variational formulation, the electrical energy is split into two parts: The
polarization energy within the solid and the electric energy of free space occupied
by the deformed solid.
The first two items above result in another set of constitutive equations for large
deformation piezoelectricity:
210 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
T
S = cE  – e Em
P m = e +  0   rS – I E m
where S is the second Piola–Kirchhoff stress;  is the Green–Lagrange strain, Em and
Pm are the electric field and electric polarization in the material orientation; I is the
identity matrix; and cE, e, and rS are the piezoelectric material constants. The
expression within parentheses equals the dielectric susceptibility of the solid:
 =  rS – I
The electric displacement field in the material orientation results from the following
relation
–1
D m = P m +  0 JC E m
where C is the right Cauchy–Green tensor
T
C = F F
Fields in the global orientation result from the following transformation rules:
E = F
–T
Em
–1
P = J FP m
(2-28)
–1
D = J FD m
v = V J
–1
where F is the deformation gradient; J is the determinant of F; and v and V are the
volume charge density in spatial and material coordinates, respectively. The
deformation gradient is defined as the gradient of the present position of a material
point x  X + u:
xF = -----X
Finally, one can rewrite the constitutive equations as
T
S = cE  – e Em
D m = e +  0  rS E m +  0  JC
–1
– I E m
MODELING GEOMETRIC NONLINEARITY
|
211
DECOUPLED MATERIALS WITH LARGE DEFORMATIONS
The large deformation formulation described in the previous section applies directly to
materials not being piezoelectric if the coupling term is set to zero: e  0. In that case,
the structural part corresponds to the large deformation formulation described for the
solid mechanics interfaces.
The electrical part separates into two different cases: For solid domains, the electric
energy consists of polarization energy within the solid and the electric energy of free
space occupied by the deformed solid — the same as for the piezoelectric materials.
For nonsolid domains this separation does not occur, and the electric displacement in
these domains directly results from the electric field — the electric displacement
relation:
D = 0 r E
The Electrostatics Interface in the COMSOL Multiphysics Reference
Manual
LARGE DEFORMATION AND DEFORMED MESH
The Piezoelectricity Interface, Solid can be coupled with the Moving Mesh (ALE)
interface in a way so that the electrical degrees of freedom are solved in an ALE frame.
This feature is intended to be used in applications where a model contains nonsolid
domains, such as modeling of electrostatically actuated structures. This functionality is
not required for modeling of piezoelectric or other solid materials.
The use of ALE has impacts on the formulation of the electrical large deformation
equations:
• The first impact is that with ALE, the gradient of the electric potential directly
results in the electric field in the global orientation, and the material electric field
results after transformation.
• The most visible impact is on the boundary conditions. With ALE, any surface
charge density or electric displacement is defined per the present deformed
boundary area, whereas for the case without ALE, they are defined per the
undeformed reference area.
Deformed Geometry and Moving Mesh in the COMSOL Multiphysics
Reference Manual
212 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
References
1. J. Yang, An Introduction to the Theory of Piezoelectricity, Springer Science and
Business Media, N.Y., 2005.
2. A.F. Bower, Applied Mechanics of Solids, CRC Press, Boca Raton, FL (http://
www.solidmechanics.org), 2010.
MODELING GEOMETRIC NONLINEARITY
|
213
Contact Modeling
Overview
Situations where objects come into contact with each other occur frequently in
mechanical simulations. Setting up and solving such contact problems can be a
challenging task, and this section contains information about important aspects of
creating models involving contact.
In a contact analysis, you solve for the contact state and the contact forces. The most
fundamental quantity in a contact analysis is the distance between the objects which
may come into contact, the gap. If the gap is positive then there is no interaction. The
task of the contact algorithm is to ensure that the gap never becomes negative; that is,
to avoid overclosure. In order to accomplish this task, contact forces must be
introduced.
For normal contact, the state only consists of being in contact or not, and the force
variable is the contact pressure in the normal direction. With friction included, there
are two possible states for the relative tangential displacement when in contact:
sticking or sliding. The tangential force vector is added as force variable.
The contact analysis functionality in COMSOL Multiphysics also includes the
possibility to prescribe adhesion and decohesion between the contacting objects, and
to model removal of material by wear when the objects are sliding relative to each
other.
In this section:
• Setting Up a Contact Problem
• Special Types of Contact Problems
• Contact Pairs
• Meshing for Contact Analysis
• Fallback Conditions to Contact
Regions
• Settings for Contact Nodes
• Solver Settings for Contact Analysis
• Quasistatic Contact Analysis
• Monitoring the Solution
• Dynamic Contact Analysis
• Dependent Variables in Contact
Analysis
• Multiphysics Contact Analysis
• Important Contact Variables
214 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Setting Up a Contact Problem
Mechanical contact can be modeled between boundaries in the Solid Mechanics,
Multibody Dynamics, Shell, Layered Shell, and Membrane interfaces. You can model
contact not only within a single physics interface, but also between two physics
interfaces, or even between a physics interface and any boundary having a mesh.
To model a mechanical contact problem, you must do the following fundamental
steps:
• In the finalization step of the geometry sequence, you should normally have Action
set to Form an assembly. If Form a union is used, then the contacting boundaries must
be geometrically separated in the initial configuration.
• Add Contact Pair nodes under Definitions. A contact pair consists of two sets of
boundaries, which are called the source and destination boundaries. Contact pairs
can also be added automatically, based on boundary adjacency when the Form an
assembly action is used. The geometric gap distance is a variable set up by the
contact pair, which also define operators for mapping variables or expressions
between the selected boundaries.
• Use the default Contact node or add new Contact nodes in the physics interface. In
the Contact node, you select the contact pairs to be used, and provide the settings
for the physical and numerical properties of the contact model.
• If relevant, add Friction, Slip Velocity, Adhesion, Decohesion, or Wear subnodes to
Contact.
CONTACT MODELING
|
215
• Select a suitable study type. You can analyze contact using the following types of
study steps:
- Stationary; commonly using an auxiliary sweep.
- Bolt Pretension
- Time Dependent
- Any type of prestressed analysis. In this case, the full contact problem is solved in
the preload step, and in the subsequent perturbation step the contact state is
considered as fixed.
• Documentation of the Contact, Friction, Slip Velocity, Adhesion,
Decohesion, and Wear nodes.
• Contact Analysis Theory.
• Identity and Contact Pairs in the COMSOL Multiphysics Reference
Manual.
In a multiphysics analysis, a contact problem can also incorporate for example changes
in the heat flux or electric current through the contacting boundaries. You will then
also need to add corresponding features in the other participating interfaces, like a
Thermal Contact node in the Heat Transfer in Solids interface. The contact state and
contact pressure used by other physics interfaces are always supplied by the structural
mechanics interface.
Because of the multiphysics capabilities, the setup of a contact problem is
split into two parts. The definition of the contact pair is made under
Definitions, and can be shared between several physics interfaces. This part
of the contact problem defines the geometric properties of the contact,
such as search and mapping operations between the selected boundaries.
The physics related definitions of the contact properties are then made in
the respective physics interfaces.
The fact that you add a Contact node to your model will automatically make all study
steps geometrically nonlinear. For the default Contact node, this requirement can be
removed by selecting Disconnect pair.
216 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
INCLUDING FRICTION
In real life, there is always some friction between contacting objects, but this is
sometimes ignored when setting up the mechanical contact problem. There are several
reasons to do this simplification:
• In many cases, only the normal forces are significant for the general force
distribution in the structure, while the frictional forces only cause minor local
effects.
• The values of the friction coefficients are difficult to obtain, and unless the structure
is assembled under well controlled conditions, the magnitude of the friction can
vary a lot. If there is a large degree in uncertainty in the input data, it can be argued
that the inclusion of friction does not add much to the quality of the results.
• Adding friction to a contact problem will often increase the computation time
significantly, or even cause convergence problems.
There are a number of situations when friction modeling cannot be avoided. Some of
them are:
• When a significant portion of the load is carried by shear tractions acting on the
contact boundaries.
• When a tangential force is necessary to maintain stability and to avoid rigid body
motions. In many cases, it is however possible to replace the friction by a suitable
boundary condition instead, as long as there are no resultant forces being resisted
by such a constraint.
• When modeling wear.
• When the frictional dissipation is an important component of a dynamics problem,
or when it is needed as a heat source in a thermal analysis.
In some cases, such as when a brake pad slides along a brake disc, the size and
orientation of the slip velocity is known. You can then employ a simplified form of
friction modeling by assuming the tangential contact to always be in a slip state, which
simplifies the computation of the friction forces. This is done using the Slip Velocity
node. This is particularly useful for wear modeling.
INCLUDING ADHESION AND DECOHESION
You can also specify that the contacting boundaries stick to each other, so that they will
not separate or slide. The onset of adhesion, when the boundaries become
permanently attached to each other, can be based on several criteria:
• When a certain contact pressure is exceeded.
CONTACT MODELING
|
217
• When the gap distance between the contact boundaries is smaller than a certain
value.
• When a user specified logical expression is fulfilled. This can for example be used if
an adhesive cures when a certain temperature is exceeded.
• From the start of the analysis. This case is particularly useful if you are interested in
modeling the subsequent tearing of a thin glue layer by decohesion.
If adhesion is active between the contact boundaries, it is possible to break the bond
by adding a decohesion model. You can choose between several different decohesion
models.
Adhesion and friction can be combined, but during the time that two boundaries are
bonded to each other through adhesion, any settings for friction are ignored.
INCLUDING WEAR
It is possible to model adhesive or abrasive wear of the material when the contacting
boundaries are sliding along each other. The removal of material from the domain
adjacent to the contact boundary can be modeled using three, fundamentally different,
approaches.
For the Solid Mechanics and the Multibody Dynamics interfaces, the most general
approach relies on the deformed geometry concept, where material is actually removed
by using an adaptive mesh technique. In the second, simplified, approach wear is
incorporated as an offset in the contact condition. This approach is computationally
less expensive, and is suitable as long as only small amounts of material are removed,
and wear does not change the orientation of the normal to the boundary significantly.
In the Shell and Membrane interfaces the structural domain is represented by only a
meshed surface. Therefore, a different, more suitable approach is used, in which the
thickness variable and the midsurface offset to the meshed boundary are modified.
Computing the amount of wear involves solving a rate equation, hence, it is only
possible to compute wear in time-dependent studies. The wear rate is typically a
function of the contact pressure and the relative slip velocity between the contacting
boundaries.
The Wear subnode is not available in the Layered Shell interface.
218 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
SELECTING THE CONTACT METHOD
In COMSOL Multiphysics, there are three classes of methods available for solving
contact problems: the penalty method, the augmented Lagrangian method, and the
Nitsche method. For all methods, the contact pair is asymmetric, that is, the
destination contact boundary is constrained not to penetrate the source boundary, but
not vice versa. However, it is possible to set up a symmetric formulation for the contact
problem by selecting the same boundaries as source and destination.
Penalty Method
The default penalty method is rather simple and robust method to introduce the
contact conditions. Roughly speaking, it is based on inserting a stiff distributed spring,
active only in compression, between the contacting boundaries. In addition to the
robustness, it has the advantage that no special solver is required, which makes it easier
to set up multiphysics problems and time-dependent studies. However, the penalty
method only enforces the contact conditions approximately. The contact forces
computed are thus less accurate than when using, for example, the augmented
Lagrangian method, and there is always some overclosure between the contacting
surfaces. For stick friction, there is also an “elastic” deformation due to the
penalization of the constraint.
When using the penalty method, there is always a tradeoff between accuracy and
stability. While a large penalty factor will reduce unphysical overclosures, the problem
may become ill-conditioned and unstable if it is too large. It might therefore be
beneficial to accept some penetration between the contacting objects. Note, however,
that if the penalty factor is too small, the contact condition may be violated.
Augmented Lagrangian Method
The augmented Lagrangian method provides better accuracy, but at a higher
computational cost, and is often less stable from a convergence point of view. All
contact conditions are enforced in a weak or integral sense, and thus evaluated in the
integration points on the destination boundary. For normal contact, it is thus possible
for a node to have a small penetration into the source boundary, even for a well
converged solution. Both, the contact pressure and the friction forces are added as
extra degrees of freedom to enforce the contact constraints.
When using the augmented Lagrangian method, it is possible to choose between a
segregated and a coupled solution method. The segregated solution method sets up
special type of segregated solver sequence, where the extra degrees of freedom related
to contact are updated in a separate segregated solver step. As its name implies, there
is no such need when using the coupled solution method, and you can more freely set
CONTACT MODELING
|
219
up the solver sequence. This less restrictive solver requirement can be particularly
useful for multiphysics problems where the penalty method does not provide sufficient
accuracy.
Nitsche Method
The Nitsche method for contact is an extension of the general method suggested by
J. Nitsche in 1971 to weakly impose Dirichlet conditions. Conceptually, it can be
viewed as an enhancement of the penalty method where the surface traction of the
adjacent domains is used to improve the accuracy of the contact condition. Also, as for
the penalty method, it has the advantage that no special solver is required, which makes
it easier to set up multiphysics problems and time-dependent studies.
The Nitsche method is intended as an alternative to the augmented Lagrangian
method for problems where the penalty method lacks sufficient accuracy. Relevant
examples where this might be the case includes:
• Large deformation problems with hyperelasticity
• Self-contact
• Problems where the structural stiffness of the global system is of importance
For the first two problems in particular, the accuracy and stability can be further
improved by increasing the quadrature order for the contact equations, see also
Quadrature Settings. Hence, the Nitsche method uses a higher quadrature order by
default than the other contact methods.
COMSOL Multiphysics supports three different formulations of the Nitsche method:
• Symmetric
• Skew-symmetric
• Incomplete
The default incomplete formulation is recommended for the majority of cases and
provides a good tradeoff between performance and stability. In cases where the default
formulation fails, the skew-symmetric formulation can be an alternative, but it includes
additional equations that are expensive to evaluate that can increase the solution time.
The Nitsche method is available in the Solid Mechanics and Multibody
Dynamics interfaces.
220 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Dynamic Methods
Both the penalty and the augmented Lagrangian methods are additionally available in
a specialized formulation intended for dynamic contact problems. Both of these are
based on a viscous formulation that for the normal contact constrains the rate of the
gap to be zero, rather than the gap. Since the formulations are viscous, the duration of
the contact should be small, otherwise the overclosure will eventually grow and violate
the nonpenetration condition. This is especially the case for the dynamic penalty
method, where the gap rate is only approximately zero.
CONTACT DETECTION
The contact search is made only toward one side of the source and destination
boundaries, determined by the positive direction of the contact normal of the selected
boundary. For contact to be detected, this means that the source and destination
contact normals must point toward each other. Generally, the contact normal coincides
with the geometry normal that is determined by the direction of the boundary.
However, there are situations where this is not the case, or where the Contact node can
control the sign of the contact normal. Some common situations are summarized in
the following:
• If the contact boundary is on the exterior of a domain, then the geometry normal
always point outward from the domain. This is the most common case, and then no
other considerations are needed.
• In some cases, like Fluid–Structure interaction, there may be a domain with a
moving mesh between the two contacting objects. The source and destination
boundaries will then, in the geometrical sense, be interior boundaries. In this case,
the physics interface (Solid Mechanics or Multibody Dynamics) defines a normal
vector which is pointing outward from the boundaries that are external to the
physics interface. Thus, this case is also handled automatically.
• When a boundary without an adjacent domain is selected, you need to be careful so
that the normal is pointing in the intended direction.
• When using the Shell, Layered Shell or Membrane interfaces, contact can potentially
occur on both sides of the boundary. In a single Contact node, you can only model
contact on one side. In the Contact Surface section, you can select whether the
contact should occur on the top side or bottom side. The ‘top’ and ‘bottom’ sides
are defined by the orientation of the physics interface normal, which may differ from
the geometry normal. In these interfaces, the orientation of the physics normal is
controlled by the Boundary System that is attached to each boundary through the
CONTACT MODELING
|
221
material models. The normal direction can be reversed using the settings in the
Boundary System node.
The actual normal vector used in the contact search algorithm can be
visualized by plotting <pair_tag>.n<coord_label>. For example, the
variable p1.nx gives the x-component of the spatial normal used by
contact pair p1. Plotting the contact normal vector can be useful to verify
that the source and destination normals point toward each other.
Visualizing the Orientation of Boundaries
In 2D, a boundary is represented by a line. If you follow the line from its start point
to its endpoint, the positive normal points to the left. The line orientations can be
visualized by selecting the Show edge direction arrows check box in the appropriate View
node under Definitions.
In 3D, the rules for the orientation of a boundary are more complicated. In general,
you have to visualize the normals, in order to check its orientation. This can be done
in different ways:
• For a mesh without physics, you will need to use the general result presentation
tools. Follow these steps:
- Run Get Initial Values for an arbitrary study in order to create data for result
presentation.
- Add a 3D Plot Group under Results.
- Add an Arrow Surface plot to the new plot group.
- In the Replace Expression (
222 |
) dialog, select the geometry normal.
CHAPTER 2: STRUCTURAL MECHANICS MODELING
• When working with the Shell or Membrane interfaces, select Enable physics symbols
in the settings for the interface. You will then see the physics normals plotted if you
select a material model like Linear Elastic Material in the Model Builder.
CONTACT BETWEEN PHYSICS INTERFACES
Contact can seamlessly be modeled between Solid Mechanics, Shell, and Membrane
interfaces. Equation are only added to Contact nodes that have an applicable
destination boundary, that is, a destination boundary that intersects with the selection
of the physics interface. Properties such as contact surface offset can, however, be
considered as long as either a source or a destination boundary is applicable in the
Contact node. Shell and Membrane offsets are automatically considered on both source
and destination boundaries.
SOURCE SELECTION OUTSIDE PHYSICS INTERFACES
In most cases, the source and destination boundaries belong to the same physics
interface. The only strict rule, however, is that the destination side belongs to the
physics interface in which the Contact node resides. The source side only needs to have
a mesh and can optionally have one or more physics interfaces attached to it.
If the source boundary is not part of the a physics interface with a Contact node, the
gap is computed using only the current location of its mesh, ignoring any physical
properties that may exist there. In this case, the Contact node has no control of the
contact normal used by the source boundary. Care must therefore be taken to ensure
CONTACT MODELING
|
223
that the contact normal of the source and destination points toward each other for the
contact detection to work.
There are two main scenarios where you may want to use a source selection that is not
in the current physics interface:
Fixed Rigid Wall
If one side of a contact pair can be considered as rigid and fixed in space, then it is
sufficient to add a meshed boundary at that location without any physics.
Moving Rigid Wall
This case is similar to the previous. In order to prescribe the path of the rigid wall, add
Moving Mesh with a Prescribed Deformation node under Definitions.
Contact Pairs
SELECTING SOURCE AND DESTINATION
To decide which boundaries to assign as source and destination in a contact pair,
consider the following guidelines:
• If there is a significant difference in the stiffness in the normal direction between the
source and destination boundaries, select the stiffer side as source. This is especially
important if the difference in stiffness is quite large (for example, more than a factor
of ten).
• When the contacting parts have approximately the same stiffness, consider the
geometry of the boundaries instead. Make a concave boundary the source and a
convex boundary the destination rather than the opposite.
• If one of the boundaries belongs to a part that is rigid it should be selected as the
source boundary. Rigid boundaries can be created in several ways, for example
- The underlying domain has the Rigid Material material model.
- The boundary or its underlying domain is constrained by, for example, Fixed
Constraint or Prescribed Displacement.
- The source boundary is meshed, but has no physics attached.
- The source boundary position is controlled by Prescribed Deformation under
Moving Mesh.
• If only one side of the contact pair is within a physics interface that has a Contact
node, that side must be the destination side.
224 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
For efficiency, include only those boundaries that can potentially come in contact in
the destination selection. All equations are formed on the destination boundary, and
includes performing the contact search which can be expensive.
If it is difficult to follow the above guidelines, the same boundaries can be selected as
both source and destination. Doing so results in an unbiased (or symmetric)
formulation that is less sensitive to, for example, difference in stiffness or mesh density
between the contacting boundaries. However, such a formulation involves evaluating
equation and contact mapping at additional points and can thus be more expensive to
use.
STRATEGIES FOR SELECTING CONTACT PAIRS
A Contact node can reference any number of contact pairs.
A contact pair is just a definition, and does not have to be referenced by any Contact
node.
Neither the source, nor the destination, in a contact pair has to be geometrically
contiguous. In practice, this means that you often only need a few contact pairs in a
model. The number of pairs actually needed will be determined by how many different
settings that are required in the Contact Pair and Contact nodes.
If you have many contact pairs in your model, it is a good idea to manually set the Label
of each pair in order to simplify the identification during subsequent selections in the
Contact nodes.
AUTOMATIC GENERATION OF CONTACT PAIRS
Contact pairs can be automatically generated during the finalization of the geometry
sequence. When Action is set to Form an assembly, you can select Create pairs, and use
Contact pair as Pair type. Boundaries which are in geometrical contact with each other
will then be placed in contact pairs. All contact pairs created are automatically added
to the default Contact node. If you do not want to use all pairs, either delete the pairs
from the model or disconnect the default Contact node in the relevant physics interface
by selecting Disconnect pair. For the latter alternative, add new Contact nodes in the
CONTACT MODELING
|
225
physics interface, and select which of available pairs to actually use for the contact
analysis.
The automatic pair generation will not know which side to use as source
or destination. Based on the suggestions in Selecting Source and
Destination above, you may need to switch selections using the Swap
Source and Destination (
) button in the Source Boundaries section of the
contact pair settings.
SMALL SLIDING CONTACT
In some situations, the relative sliding between the contacting boundaries is small. This
is, for example, often the case for shrink fit simulations, when mounting a component
using prestressed bolts, or for partial decohesion of two components. The sliding
distance can be considered as small if it is significantly less than the length of a mesh
element edge.
In such cases, it is possible to simplify the problem by selecting the Mapping Method to
be Initial Configuration in the Contact Pair node. With this setting, a material point on
the destination boundary will see the same material point on the source boundary
throughout the entire simulation; that is, the mapping is constant. This setting will
make the contact analysis run faster and convergence to be more stable.
The analysis is geometrically nonlinear also when using this option, and the contact
region can still have arbitrarily large displacements and rotations.
Friction can be modeled. Even though there is no sliding in a geometrical sense, the
difference in tangential displacement is computed.
You cannot mix contact pairs with the two different types of Mapping
Method within the same Contact node.
Meshing for Contact Analysis
Once the source and destination boundaries are chosen, you should mesh the
destination finer than the source. Do not make the destination mesh just barely finer
than the source because this can cause unphysical oscillations in the contact pressure.
Make the element size on the destination at least two times finer than on the source.
The reason is that the algorithm is asymmetric; the points on the destination side
226 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
connects to the source side, and not vice versa. With a coarse mesh on the destination
side, a large portion of an element (or even a whole element) on the source side could
be without connection to the destination.
It is always important that the geometry is well resolved, so that a curved contact
boundary actually is seen as curved rather than “faceted”. The density of the mesh
often needs to be finer than what would be needed to resolve stresses on a similar
boundary without the contact conditions. If the normal to the contact boundary
changes much from one element to the next, there is a risk that the contact analysis
does not converge.
If the source boundary is rigid, there are no requirements on the mesh size of the
destination boundary. In this case, you may use a significantly finer mesh on the source
boundary than on the destination boundary. This is sometimes necessary in order to
resolve the geometry well. On the other hand, if you have a flat rigid boundary, you
only need to mesh it with a single element.
Settings for Contact Nodes
THE CONTACT NODE
Penalty Factor
An important parameter in the settings for the Contact node is the penalty factor.
When running into convergence problems, check the penalty factor settings and
consider changing the current value. It is used by all contact methods, but its
interpretation differs:
• In the penalty method, the penalty factor has a straightforward interpretation as the
stiffness of a distributed spring connecting the two contacting boundaries. A higher
value will decrease the unphysical penetration, but can be detrimental to the
numerical conditioning of the stiffness matrix. A too small value can, however, result
in violation of the contact condition.
• In the augmented Lagrangian method, the penalty factor is a numerical parameter,
which affects the convergence properties of the algorithm. Its interpretation is
different depending on the chosen solution method. For a segregated method, the
penalty factor mainly affects the rate of convergence of the outer iteration loop; a
higher value typically leads to faster convergence, but can decrease the stability of
the algorithm for certain problems. For the coupled method, the penalty factor
mainly affects the structure of the underlying equations, and the solution is typically
CONTACT MODELING
|
227
less sensitive to the value of the penalty factor. However, the convergence properties
can be improved by tuning the penalty factor.
• In the Nitsche method, the penalty factor is a stabilization parameter which can
affect the robustness of the solution, but to a lesser extent the accuracy. The suitable
value of the penalty factor depends on the chosen formulation, where the
skew-symmetric and incomplete formulation are typically less sensitive than the
symmetric formulation.
In the augmented Lagrangian method and the Nitsche method, the value
of the penalty factor does not affect the accuracy of the final solution, like
it does in the penalty method.
High values of the penalty factor can lead to an ill-conditioned stiffness matrix and
convergence problems in the Newton iterations. This is often identified by that the
damping factor reported by the solver becomes less than 1 for many Newton iterations,
or by that the structure “jumps” into an unphysical state. Large errors returned from
the linear solver are also an indication that the stiffness matrix is ill-conditioned. If this
occurs, decrease the penalty factor.
The default value for the penalty factor is based on a characteristic stiffness. The
default is an “equivalent” Young’s modulus (Eequ) of the material on the destination
side. For linear elastic isotropic materials, Eequ is the actual Young’s modulus. For
other types of materials, Eequ is defined by an estimate of a similar stiffness at zero
strain. For materials that are user defined or in other ways nonstandard (for example,
anisotropic with large differences in stiffness in different directions), Eequ might need
to be replaced with another estimate.
For nonlinear materials in general, and for elastoplastic materials in
particular, there can be a significant change in stiffness during the solution
process. Choose the source and destination boundaries accordingly. You
may even have to adjust the penalty factor as the solution progresses when
such materials form a contact boundary.
When using the augmented Lagrangian formulation with a segregated solution
method, having a well-tuned penalty factor is important for the performance of the
outer contact iterations. The default value is selected as a compromise between speed
and stability, but with more weight on stability. The strategy is for each new step
(parametric step or time step) to start with a softened penalty factor, which is then
228 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
increased over the first four iterations. The purpose is to stabilize the problem in case
there are large overclosures during the first iterations. This is called relaxation.
In a situation where the contact is well established, using relaxation will however cost
extra iterations, and it may even lead to a loss of convergence.
For this method, the penalty factor can be tuned in several ways. You have three basic
choices, ranging from simple to advanced:
• With a Preset penalty factor, you can choose having it tuned for Stability, Speed, or
Bending. With Stability, relaxation is used in every step. With Speed, a constant
penalty factor is used, and the value that is used is equal to the final value obtained
when using Stability. For Bending, a constant and low penalty factor is used in all
iterations. The value corresponds to the initial value when using Stability. As the
name implies, this option is intended for bending dominated problems where the
structural stiffness is much lower than the bulk stiffness of the material.
• With Manual tuning, you can adjust the magnitude of the penalty factor, and also the
relaxation strategy.
• With User defined, you can enter any expression for the penalty factor.
For details about these settings, see the documentation of the settings for
the Contact node.
Some hints for selecting the penalty factor for the segregated augmented Lagrangian
method:
• Use relaxation only when large changes in the contact state is expected.
• If an analysis takes a long time, check the convergence graphs. If the contact
variables show a steady, but slow, convergence it may help to increase the penalty
factor. Increase by a factor of 2 – 5.
• If a model fails to converge, and the contacting parts appear to have moved far from
each other, it is probable that the penalty factor is too high. You can then either
decrease the total stiffness or add more relaxation.
Trigger Cutback
If, during the iterations, a contact problem comes into a state where it is far from the
converged solution, it is unlikely that the solution will ever converge. In such a case,
much computing time can be spent before the maximum number of iterations is
reached, and the solver makes an attempt with a smaller time or parameter step. To
CONTACT MODELING
|
229
speed up this process, you can select the Trigger cutback check box when using the
augmented Lagrangian method. You can then enter a logical expression that will force
the solver to immediately abandon the iterations and try a smaller step when fulfilled.
Such an expression can, for example, be a maximum displacement (like solid.disp >
5[mm]), based on what is physically realizable for the structure. The expression is
evaluated in all points on the boundary, but you can also use a global value, like an
average or a maximum.
Contact Surface Offset and Adjustment
It is possible to assign an offset to both the source and destination boundaries. When
an offset is given, the boundary used in the computations is not the geometrical
boundary, but a virtual boundary displaced by the offset value. You can use this option
for several purposes:
• When analyzing problems with for example shrink fit, nominal dimensions can be
used for the geometry, and the overclosure included in the gap by using a positive
offset.
• When there is a small clearance between two boundaries, a negative offset can be
used instead of changing the geometry.
• If geometries are such that a large overclosure exists in the initial configuration, the
contact algorithms may not converge. You can then add a negative offset, which is
slowly removed by letting it depend on time or on the parameter in the parametric
continuation solver.
• A positive offset can be used to avoid a complete collapse of a mesh that exists
between the source and destination boundaries. This is discussed in more detail in
Multiphysics Contact Analysis.
When the source and destination boundaries are curved, the discretization introduced
by the meshing may lead to small variations in the computed distance between the
source and destination boundaries, even though the geometrical shapes of the two
objects are ideal. When modeling for example a shrinkage fit, this effect can cause
significant fluctuations in the contact pressure. If you select Force zero initial gap, the
computed distance from destination to source will be adjusted by the initial gap
distance detected by the contact search. Positive gap distances smaller than the
tolerance gap are adjusted to be zero. By default, gap is set to Inf, which means that
all gaps and overclosures detected are adjusted to be zero. This adjustment can be
combined with an offset. The offset is applied to the adjusted gap value.
230 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
It is only the gap computation that is affected by this setting, the mesh as such is not
adjusted. This type of adjustment is most useful when the sliding is small, so that the
gap distance is always computed between the same points on source and destination.
You can only apply an offset to the source boundaries if they belong to the same physics
interface as the destination boundaries.
Initial Value
In the augmented Lagrangian method, where the contact pressure is a dependent
variable, it can be given an initial value. In force-controlled contact problems where no
other stiffness than the contact prohibits the deformation, the initial contact pressure
is crucial for convergence. If it is too low, the parts might pass through each other in
the first iteration. If it is too high, they will never come into contact.
Discretization
When using the augmented Lagrangian method it is possible to change the type and
order of the shape functions used for the contact pressure and friction force degrees of
freedom. The default is linear shape functions, which ensures that there are no
over-constraints in the contact interface. It is allowed to use a shape function order that
is equal to or lower than the order of the displacement field. Increasing the order of
the contact variables from the default can increase the accuracy of how well the contact
conditions are enforced, but can impair convergence and increase the computational
cost.
For a discretization other than Linear, the lumped solver is no longer optimal for the
contact pressure update when using a segregated solution method. In such cases, a
standard segregated step should be used. The default solver generation takes this into
account, but if you later modify the discretization, you should update the solver
sequence.
Quadrature Settings
The weak equations set up by the Contact node and its subnodes typically involve
discontinuous functions. These originate from the contact mapping, where the source
and destination meshes, in most cases, are nonconforming. The default quadrature
used in the numerical integration of these integrals is equal to the order used by the
displacement field. For a quadratic displacement field, this means integration order
equal to four.
In most situations, the default quadrature provides sufficient accuracy of the numerical
integration. However, it is sometimes necessary to increase the integration order for
the contact weak equations. This can improve the stability of the contact model since
CONTACT MODELING
|
231
it reduces numerical errors that might occur during assembly of the system matrices.
Note that using a too high integration order can significantly increase the cost of
assembling the matrices.
Jacobian Contribution
In the Advanced section of the Contact node, there is an option to specify the type of
Jacobian contribution from the contact equations. The default Automatic option will
choose a suitable setting depending on the mapping method used by the contact pair.
However, if controlled manually the Nonsymmetric option is the preferable choice
especially when the source boundaries undergoes large deformations, since it is more
robust. The Symmetric option can be attractive for large models since it preserves the
symmetry of the global stiffness matrix, as long as no other features cause it to be
nonsymmetric. This can decrease the solution time and memory requirements when
solving the model.
THE FRICTION NODE
When adding a Friction node, you can specify a constitutive model (friction model) for
the behavior of the tangential contact. This model includes conditions for switching
between sticking and sliding, as well as computation of the current friction forces.
Friction Parameters
The friction model specifies the threshold for the friction force in the contact pair. If
the computed (trial) friction force is above this threshold value, the contact is in a stick
state; if the (trial) friction force is above the threshold, the contact is in a slip (or
sliding) state.
Two predefined friction models are available based on the classical Coulomb law,
where the friction force is proportional to the contact pressure through the friction
coefficient. Both Coulomb laws are additionally generalized by allowing specification
of minimum (cohesion) sliding resistance and a cap that sets the maximum tangential
traction.
It is also possible to define the threshold for the friction force as an arbitrary expression
that may depend on any quantity in the model, for example temperature or position.
The only limitation is that the expression may not implicitly depend on the current
value of the friction force.
Friction Force Penalty Factor Control
This section provides similar settings as described in Penalty Factor of the Contact
node, but the penalty factor is here used to regularize the stick constraint. However,
232 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
the same considerations for how to set an appropriate value apply. For convenience, it
is also possible to utilize the penalty factor set in the parent contact node.
This section is not available when the Nitsche method is used. The same penalty factor
as set in the parent Contact node will be used for friction as well.
THE SLIP VELOCITY NODE
The Slip Velocity node facilitates a simplified form of slip friction modeling, which can
be used in the case that the direction and speed of the sliding is known. The same
friction models as for the Friction node are available. However, it is here assumed that
the tangential contact is in a sliding state, and that the slip velocity is known
beforehand. The latter is supplied to the feature as a user input in the local coordinate
system.
Knowing the slip velocity greatly simplifies the computation of friction forces. There is
no need to determine the transition between stick and slip contact, which can be
difficult.
THE ADHESION NODE
When using the penalty method, you can specify that the boundaries in the contact pair
should stick to each other after coming into contact by adding an Adhesion node.
The adhesive layer is conceptually without thickness, but by specifying an offset in the
Contact node, you can to some extent include the dimensions of the adhesive layer.
The adhesive layer always has a finite stiffness. For a glue layer, this represents the true
stiffness. For a more conceptual joining of two boundaries, this stiffness should be
considered in the same way as the penalty stiffness in the contact formulation. The
stiffness can differ between tension and compression: In compression the stiffness is
always taken as the penalty stiffness, whereas you can change the tensile stiffness.
THE DECOHESION NODE
When adhesion is active, it is possible to break the bond between the source and
destination boundaries by adding a Decohesion subnode to Contact. To model
decohesion, it is required that an Adhesion node is present and active in the same parent
Contact node.
Decohesion defines a cohesive zone model (CZM) based on interface damage
mechanics on the adhesive layer. Damage is assumed to be a scalar variable that initiates
as 0 and grows to 1 during decohesion, and in principle degrades the stiffness of the
adhesive layer. Since damage is a scalar, both the normal and tangential stiffness
CONTACT MODELING
|
233
components degrade simultaneously, irrespective of whether the actual loading
direction. However, the penalty stiffness of the contact condition is not affected by
damage.
Two alternative CZM are available. The Displacement-based damage models defines
damage growth as a function of a mixed mode displacement quantity. It comes with
several traction separation laws that associate the onset of damage with the peak
strength of the interface. For some of them, it is possible to choose between different
mixed mode failure criteria. The Energy-based damage models define damage growth
as a function of the stored undamaged elastic energy density of the interface. It also
comes with several different traction separation laws. However, these are more general
and define the onset of damage at an arbitrary elastic energy density. In principle, you
can define the model so that damage initiates immediately during loading of the
adhesive layer, that is for zero energy density. The strength of the interface is then
determined by the critical energy release rate and the shape of the damage evolution
function. In this way, the energy-based damage models can be viewed as a
regularization of linear elastic fracture mechanics.
Decohesion is an inherently unstable process. The elastic energy in the strained
adhesive layer is released during decohesion. Numerically, the decreasing branch of the
traction-separation curve manifests itself as a local negative stiffness. Such problems are
only possible to solve as long as the surrounding material can absorb the released
energy. The numerical stability is, furthermore, closely coupled to the physical stability
of the structure. The following points can help to set up a model with decohesion and
to overcome problems with convergence.
• If the structure is in a load-controlled situation, there is no possibility to continue
the analysis when the peak external load has been exceeded. Physically, this
corresponds to a sudden collapse of the component, or in the case of decohesion, a
rapid breakage of the adhesive layer.
• If the structure is loaded by prescribed displacements, it is usually possible to
continue the analysis further. It may, however, happen that the stored elastic energy
in the structure is large enough to force a complete breakdown of the adhesive layer
once a certain external displacement is reached. If possible, use prescribed
displacements in a decohesion analysis, and evaluate the applied load from the
reaction forces.
• Sometimes it is not possible to use prescribed displacements, for example if the load
is distributed. You can then add a Global Equation to control the loading rate by
234 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
some other quantity that increases monotonically. This is the same technique as the
one used for postbuckling problems.
• To improve the robustness of the solver, it is sometimes beneficial to modify the
settings in the Method and Termination section of the Fully Coupled or Segregated
nodes in the solver sequence. For example, allow a larger number of iterations or try
a different nonlinear method. Often, the Constant (Newton) method can improve the
convergence of models with decohesion.
• The robustness of the solver can also be improved by modifying the parameter or
time stepping algorithm. For a stationary study, you can tune the step size in the
Parametric node, and for a time-dependent study, you can modify the time stepping
of the Time-Dependent Solver. A good idea is often to reduce the maximum allowed
step size of the solver and to allow for smaller step size than the default. Note that
if the maximum step size allowed is too large, the solver might bypass the
decohesion process altogether; in other words, even though a converged solution is
obtained, it might be invalid.
• The solution of the unstable failure due to decohesion is, to some degree, always
mesh dependent; see, for example, Ref. 1. It is therefore good practice to make sure
that the mesh of the interface and in its vicinity is fine enough to allow the energy
released during decohesion to properly redistribute in the structure. This can help
avoid solution jumps where several mesh elements are completely damaged in a
single step. Such solution jumps can be difficult for the solver to get pass, and even
if it does, the solution after the jump might be invalid.
• The true unstable failure of decohesion is a dynamic event. This can be analyzed
using a time-dependent solver, but the computational cost can be high. The inertial
forces will then balance the released energy, which is transformed to kinetic energy.
For time-dependent studies, it is possible regularize the CZM with a viscous delay by
selecting Delayed damage in the Regularization list. This option adds a delay to the
release of energy, which is controlled by the Characteristic time . Using this option can
help to suppress the instability of the solution when the step size or mesh size is too
large. If the viscous damage is used to stabilize a rate-independent decohesion
CONTACT MODELING
|
235
problem, the value of  must be chosen with care. As a rule of thumb,  should at least
be one or two orders of magnitude smaller than the expected time step.
For an example showing a decohesion analysis, including how to use a
global equation to control an unstable problem, see Mixed-Mode
Debonding of a Laminated Composite: Application Library path
Structural_Mechanics_Module/Contact_and_Friction/
cohesive_zone_debonding.
THE WEAR NODE
By adding a Wear subnode to a Contact node, it is possible to model adhesive or
abrasive wear of the material when the contacting boundaries are sliding along each
other. Since wear involves solving evolution equations, the Wear node only adds a
contribution for time-dependent studies. Moreover, wear is typically a slow process
where dynamic effects are of small significance. You should, therefore, usually set
Structural transient behavior to Quasistatic in the Structural Transient Behavior section
of the physics interface settings.
The most general technique to model the removal of material during the wear process
relies on the deformed geometry concept. When selecting the Deformed geometry
formulation, the wear feature adds a (hidden) Deforming Domain feature that controls
the material frame through an adaptive mesh smoothing. The wear, as computed in the
Wear node is fed as a (hidden) Prescribed Normal Mesh Displacement boundary
condition to the deforming domain, and thus describes the actual removal of material
from the geometry. When using this formulation, you must be aware that the adaptive
mesh means that state variables stored in Gauss points, for example plastic strains or
creep strains, will not represent the same material points all the time. Whether or not
this effect is acceptable must be judged on a case-by-case basis. Unless the amount of
material that is removed is large, or gradients are strong, this is mainly an issue close
to the boundary where material is removed by the wear process.
Alternatively, wear can be incorporated as an offset in the contact condition. This
formulation is computationally less expensive, and is suitable as long as only small
amounts of material are removed, and the wear does not change the orientation of the
normal to the boundary significantly.
The slip velocity used for the wear computation can be obtained from either a Friction
node or a Slip Velocity node, so one of these two nodes should be present and active
under the same Contact parent node. For the Generalized Archard wear model, this is a
236 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
requirement. In most cases, the orientation of the slip velocity is known a priori in a
wear analysis, in which case Slip Velocity provides the more efficient solution.
In general, modeling wear on the destination side is slightly more accurate, since it is
there that the contact pressure and slip velocity are originally computed. When
modeling wear on the source side, these quantities are mapped from the destination
boundary. Multiple Wear nodes under the same Contact node contributes with each
other, which means that it is possible to model wear on both source and destination
simultaneously. However, adding multiple wear contributions to either source or
destination may give unphysical results. On the source side it is possible to also use the
Rigid Material material model; this is not permitted on the destination due to general
restrictions of the Contact node.
• Documentation of the Contact, Friction, Slip Velocity, Adhesion,
Decohesion, and Wear nodes.
• Contact Analysis Theory in the Structural Mechanics Theory chapter.
Quasistatic Contact Analysis
When including contact in a stationary or quasistatic simulation, make sure that the
bodies are sufficiently constrained. If the bodies are not in contact in the initial
configuration, and there are no constraints on them, there will be possible rigid body
displacements. This will cause the solver to fail and must be avoided.
For a more detailed discussion about sufficient constraints, see
Constraints under Stationary Analysis.
Sometimes, as when simulating mounting processes, the structure is not fully
constrained until the contact is fully established. There are some strategies for how you
can deal with this problem.
• Create the geometry or set initial values for the displacement variables so that there
is a small penetration in the initial configuration.
• Use boundary conditions giving a prescribed displacement rather than a prescribed
force. When possible, this is usually the best way to stabilize problem. Note that you
can always obtain the force actually applied from the reaction forces.
• Add a Stabilization subnode.
CONTACT MODELING
|
237
• Add a temporary weak spring during the beginning of the simulation. Assuming
that a parameter p, ranging from 0 to 1, is used for applying the external load, you
can introduce a stabilizing spring with stiffness kx in the x direction as
k x = k  1 – p 2
–  p  10 
and similarly in any other direction that needs to be restrained. It is not important
whether the spring is applied to domains, boundaries, or edges, but it should not
create significant local forces. The value for the stiffness k should be chosen so that
the force generated by the spring balances the external load at a sufficiently small
displacement. A too weak spring will give a too large initial overclosure of the
contact boundaries. A too stiff spring might influence the solution too much.
Dynamic Contact Analysis
The contact formulations in COMSOL Multiphysics can be used in transient as well as
quasistatic analyses. In truly dynamic problems, where inertial effects are significant, a
contact formulation must conserve fundamental quantities, such as linear and angular
momentum and energy, across the contact pair. An important class of dynamic
problems, where these quantities must be conserved, is impact analysis.
To model dynamic contact events, two specialized contact methods are provided, the
Penalty, dynamic and the Augmented Lagrangian, dynamic methods. Both are based on
a viscous formulation that constrains the gap rate to be zero, ensuring that the normal
contact is dissipative and does not introduce any spurious energy contribution to the
system. Since the methods are dissipative, they are mainly intended for short duration
events, such as soft impact between two bodies. For prolonged interaction between
two bodies, energy dissipation can become significant, and overclosures can become
large, since the gap rate is only approximately zero. Both the dissipation and the
accuracy are controlled by a penalty factor that for these two methods conceptually
represents a dashpot, rather than a spring. It therefore has a characteristic time user
input that sets its magnitude. As a rule-of-thumb, it should be of the order of the
contact event duration, but the best choice must be decided on a case-by-case basis.
The Penalty, dynamic method also provides the possibility to combine the stiffness and
viscous based penalization of the normal contact. For impact analysis, it is often best
to use only the viscous formulation by setting the stiffness Penalty factor control to
Viscous only.
When modeling dynamic contact, the main interest is often the kinematics between the
contacting bodies. If you rely on the (default) adaptive time-stepping algorithm, the
238 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
solver typically also tries to resolve the wave propagation in the domains adjacent to
the contact pairs. This can cause unnecessarily small time steps and increase the
computation time. To avoid this, you can modify the solver to use a manual
time-stepping algorithm in the settings for the Time-Dependent Solver in the solver
sequence. Make sure to use time steps that are small enough to capture the contact
event, otherwise spurious energy contributions can result, and cause the problem to
“blow up”.
The time-dependent solvers in COMSOL Multiphysics introduce numerical damping
to stabilize the time stepping. This kind of stabilization is often necessary. However,
excessive numerical damping runs the risk of removing vital information from the
simulation. For this reason, the BDF solvers should be avoided for dynamic contact
analyses. The default solver suggests the generalized- solver when inertial terms are
included in the structural mechanics problem.
Regardless of the method that is used, and how the solver is set up, it is good practice
to do an a posteriori check of conservation of momentum and energy, to ensure that
the solution is acceptable.
For examples of dynamic contact problems, see
• Transient Rolling Contact: Application Library path
Structural_Mechanics_Module/Contact_and_Friction/
transient_rolling_contact.
• Impact Between Two Soft Rings: Application Library path
Structural_Mechanics_Module/Verification_Examples/ring_impact.
In both examples, an energy balance check is included. The latter model
also verifies the conservation of momentum.
Multiphysics Contact Analysis
Two different classes of multiphysics contact problems will be described in this section.
FLUXES THROUGH CONTACT SURFACES
In some contact problems, there is some kind of flux from one domain to another
through the contact zone. This can for example be a heat flux, an electric current, or
moisture transport. The common property here is that the other physics fields than the
displacements are present in domains where the solid mechanics problem is solved.
CONTACT MODELING
|
239
Typically, there will be a more or less perfect insulation as long as there is no contact,
but as soon as contact is established there will be a flux through the contact area.
This class of problems often exhibit a high degree of nonlinearity, which may lead to
convergence problems in the nonlinear solver. As an example, consider heat transfer
through the contact area, where initially only a small spot is in contact. The solution
for the temperature field is then extremely sensitive to the size of the contact area. If,
at the same time, the solid deforms due to thermal expansion, there may be large
changes in the contact area between iterations,
It is important to resolve the size of the contact area accurately, that is, to
use a very fine mesh in the contact area when modeling fully coupled
multiphysics problems.
If the contact area is larger, a fine mesh is not required because then the temperature
solution is not that sensitive to the size. If possible, start with an initial configuration
where the contact area is not very small.
You can use the contact variables (gap and contact pressure) in expressions for
quantities in other physics interfaces. As an example, a thermal resistance in the contact
region can depend on the contact pressure.
In many cases, the penalty method is preferred in multiphysics contact problems
because of its better stability and less restrictive requirements on solver selections. If
the contact conditions depend strongly on the contact pressure, use the augmented
Lagrangian method because if its higher accuracy.
FIELDS EXIST IN THE GAP
In this class of problems, a field exists between the domains controlled by solid
mechanics.
This is the case in, for example, Fluid–Structure interaction (FSI) problems. Here, the
equations in the fluid are solved on a domain with a moving mesh, so that the shape
of the fluid domain is controlled by the displacements of the solid. Another case of the
same type is when there is an electric field in an air gap.
If contact is established, the mesh in the original gap between the source and
destination boundaries will collapse. This must be avoided. The remedy is to add an
offset in the contact settings to either the source boundary, the destination boundary,
or both. If you do this, contact forces will be transmitted without the geometrical gap
being fully closed.
240 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
If, for example, this technique is used when modeling a valve, there will still be some
small flux even though the valve is closed, since there is a geometrical gap with the
width of the artificial offset. By choosing a suitably small offset, you can however make
that flux negligible.
Special Types of Contact Problems
INTERFERENCE FIT
Interference fits can be analyzed using contact modeling. This is necessary if you are
interested in checking the connection with respect to, for example, slipping or local
stresses.
There are two possible approaches for modeling interference fits, both equally valid:
• The actual geometry of the two parts before assembly is modeled. In this case, there
will be some overlap between the two domains.
• A nominal geometry in which the contacting boundaries have the same location is
created. In this case, the overlap is described as part of the contact modeling.
An imported CAD geometry can use either of these approaches, depending of the
strategy used during the geometry creation. Often, the geometrical parts are modeled
as nominal, and instead equipped by tolerance information that describe the amount
of interference.
True Geometry
With a true geometry, you can often immediately solve the contact problem.
Sometimes convergence problems may, however, appear, in particular if the material
model is nonlinear. The cause is often that the initial overlap is too far from the final
solution.
To deal with such a problem, add an offset in the settings for the Contact node. The
offset should be defined by a parameter, so that the boundaries of the two domains are
barely in contact in the initial state. Now, the offset can be reduced to zero
step-by-step, using an auxiliary sweep in the solver.
CONTACT MODELING
|
241
Nominal Geometry
When working with a nominal geometry, you always need to add an offset in the
Contact node. The offset equals the size of the interference. If needed for convergence
reasons, ramp up the offset using an auxiliary sweep in the solver.
Interference Fit Connection in a Mountain Bike Fork: Application
Library path Structural_Mechanics_Module/Contact_and_Friction/
mountain_bike_fork
SELF-CONTACT
To model self-contact, include the same boundaries in both the source and destination
selections of the Contact Pair definition. This will cause the boundaries to act as both
source and destination in the contact search and mapping. For mechanical contact, this
results in a unbiased (or symmetric) contact formulation, as the contact conditions are
formulated on both sides of the contact pair. Note that a source is not allowed to
partially intersect the destination when used for mechanical contact.
This technique to model self-contact means that some of the considerations discussed
in this chapter regarding contact modeling do not apply. For example, instead of the
recommendations in Meshing for Contact Analysis, it is recommended to use a
uniform mesh element size along the contacting boundaries. Self-contact is a case
where it might be necessary to increase the quadrature order used in the weak
equations, see Quadrature Settings.
For examples of self-contact problems, see
• Self-Contact of a Loaded Spring: Application Library path
Structural_Mechanics_Module/Contact_and_Friction/
loaded_spring_contact.
• Contact Analysis of a Rubber Boot Seal: Application Library path
Nonlinear_Structural_Materials_Module/Hyperelasticity/rubber_boot_seal.
Fallback Conditions to Contact Regions
In the Solid Mechanics, Shell, and Membrane interfaces, certain boundary conditions
may act as fallback conditions to a contact region, or any pair region, if their selection
overlaps with the source and destination boundaries. The Layered Shell interface does
242 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
not support any fallback conditions. When a boundary condition is considered as a
fallback, the condition is only active for regions that are not in contact.
In the Solid Mechanics interface, the following boundary conditions are by default
recognized as fallback conditions if their selection intersects any source and destination
boundary:
• Boundary Load
• Spring Foundation
• Added Mass
• Free
In the Shell and Membrane interfaces, the following boundary conditions can be
recognized as fallback conditions:
• Face Load
• Spring Foundation
• Added Mass
To enable the fallback condition in these nodes, change the Allowed region to Fallback
and nonpair regions in the Applicable Pair Regions section of settings window of the
node. To display the Applicable Pair Regions section, click the Show More Options
button (
) and select Advanced Physics Options in the Show More Options dialog box.
The most common case when a fallback condition is used is when there is a pressure
load acting on the part of the boundary that is currently not in contact. In this case
you would add a Boundary Load or Face Load with a selection that intersects with the
source and destination boundaries.
Solver Settings for Contact Analysis
This section provides useful tips for tuning solver settings for contact analysis in
general, and tips specific to different methods.
GENERAL SETTINGS
The following solver settings can help to successfully perform contact simulations in
general:
• In a contact analysis, you almost invariably use an incremental approach. It is
possible to solve a problem without friction in a single stationary load step, but such
an approach will often fail to converge. In a stationary analysis, you should instead
CONTACT MODELING
|
243
use the parametric continuation solver, and gradually increase the load or
displacement. Enable it by selecting Auxiliary sweep under Study Extensions in the
settings for the Stationary solver.
• Use a direct solver, rather than an iterative solver, as linear equation solver if the
problem size allows it. Direct solvers are less sensitive and can provide better
convergence.
• As a default, the double dogleg nonlinear solver is selected when a stationary study
is generated and Contact nodes are present in the model. For the majority of contact
problems this solver has more stable convergence properties than the Newton
solver, which is the default solver for most other problems. Using otherwise similar
settings, the double dogleg solver tends to be somewhat slower than the Newton
solver on problems where both solvers converge. It is, however, often possible to
take larger parameter steps when using the double dogleg solver. For some
problems, the Newton solver can still be the better choice, so if you experience
problems using the default settings, try to switch solvers.
• For contact problems, it is often necessary to let the parametric solver use a defensive
strategy when going from one parameter step to the next. This can be controlled by
setting the value of Predictor in the Parametric. By default, the parametric solver will
do so by setting the predictor to Constant when contact is present. However, it can
sometimes be more efficient to use a more aggressive strategy by setting it to Linear.
• Always solve contact problems that involve friction or decohesion incrementally,
using a parametric or time-dependent solver. The evolution of the friction forces is
history dependent. For contact problems without friction, an incremental strategy
is not necessary but often a good choice.
• If the model includes friction, try solving the problem without friction first if
possible. When the study runs absent friction, enable friction again.
• The convergence of many contact problems can be improved by modifying the
parameter or time step algorithm. For a stationary study, you can tune the step size
in the Parametric node, and for a time-dependent study, you can modify the time
stepping in the Time-Dependent Solver.
• For models that include decohesion, see the suggestions under The Decohesion
Node.
THE PENALTY METHOD
Since the penalty method only adds a weak contribution to the physics, there are no
special solver requirements, apart from the suggestions that apply to contact analysis
in general. If the simulation shows poor convergence, or even diverges, it is for the
244 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
penalty method often related to the choice of the penalty factor. A too high penalty
factor may cause the ill-conditioning, which can manifest itself either in poor
convergence of the Newton solver or large errors in the linear solver. If this is
encountered, consider using a smaller penalty factor. However, a too small penalty
factor will deteriorate the accuracy of the simulation, and contact might even be lost if
the overclosure becomes too large.
THE SEGREGATED AUGMENTED LAGRANGIAN METHOD
The segregated solution method for the augmented Lagrangian formulation
introduces extra contact degrees of freedom for the contact pressure and the friction
forces. It also relies on a special solver sequence to obtain the correct solution. Some
general considerations when using this method are:
• The convergence check relies on the scaling of the degrees of freedom, but since
contact pressures and friction forces often are zero over parts of the simulation, you
should not rely on automatic scaling. When the solver sequence is first created, both
contact pressure and friction forces are given a manual scaling which is relevant for
typical metal-to-metal contact. You should in most cases change this to values
appropriate for your application. The variable scaling is accessed under Dependent
Variables in the solver sequence. Set the scale for each variable to a value that is
representative for the expected result. Too large values may give a too early
convergence, while too small values may lead to an excessive number of iterations.
• The default solver sequence generates one lumped step in the segregated solver for
each Contact node. This split of variables into different lumped steps does not
influence the solution as such; you can equally well group the contact variables in a
single lumped step. Each lumped step will however generate an individual curve in
the convergence plot, making it easier to pinpoint the source of possible
convergence problems. You can also increase the granularity even more by changing
Solver log to Detailed in the Advanced node in the solver sequence. This will give a
separate convergence curve for each dependent variable.
The default solver generates a solver sequence that is stable and gives and accurate
solution for the majority of contact problems. However, if convergence is difficult
other settings can be tested:
• The Segregated solver is generated with a termination technique set to Tolerance.
This setting ensures the convergence of the contact degrees of freedom, that is, that
their value only changes within the specified tolerance during the latest segregated
iteration. If, however, convergence of the contact DOFs is of less importance, you
can accept the solution after n segregated iterations instead. To do this, set the
CONTACT MODELING
|
245
termination technique to Iterations or tolerance and specify the maximum number
of segregated iterations. The solver will then continue to the next step if the
tolerance criteria is fulfilled, or if the maximum number of iterations is reached.
Note that the solution of the segregated groups is still converged in each segregated
iteration.
• For efficiency purposes, the nonlinear solver in the Segregated Step that includes the
displacement field is by default set to accept the solution after seven iterations,
regardless of convergence or not. If you notice in the solver log that the solution is
far from convergence after these seven iterations it can be necessary to change this
setting. Updating the contact DOFs with a nonconverged solution can cause the
overall problem to diverge. By changing the termination technique to Tolerance, the
segregated solver will instead do a cutback if such a situation is encountered.
THE COUPLED AUGMENTED LAGRANGIAN METHOD
The coupled solution method for the augmented Lagrangian formulation introduces
special contact degrees of freedom for the contact pressure and the friction forces.
Otherwise it places no special restriction on the solver sequence. Some general
considerations when using this method are:
• The convergence check relies on the scaling of the degrees of freedom, but since
contact pressures and friction forces often are zero over parts of the simulation, you
should not rely on automatic scaling. When the solver sequence is first created, both
contact pressure and friction forces are given a manual scaling typical for
metal-to-metal contact. You should in most cases change this to values appropriate
for your application. The variable scaling is accessed under Dependent Variables in the
solver sequence.
• Since the solution to the augmented Lagrangian can be nonsmooth, the default
double dogleg nonlinear solver in stationary studies is sometimes too conservative.
The convergence can in such cases often be improved by using a Newton solver, for
example, the Constant (Newton) with a full Jacobian update.
• Although the penalty factor does not affect the accuracy of the solution, it can have
significant influence on the convergence properties of the model.
THE NITSCHE METHOD
Since the Nitsche method only adds a weak contribution to the physics, there are no
special solver requirements, apart from the suggestions that apply to contact analysis
in general. If the simulation shows poor convergence, or even diverges, it is often
related to the choice of the penalty factor. A too low value may cause the solution to
246 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
be unstable, while as for the penalty method, a too high value may cause
ill-conditioning.
DYNAMIC CONTACT
The dynamic contact methods in general inherit the properties and suggested solver
settings from the corresponding standard method. With regards to solver settings, the
main difference for the dynamic methods is how to set up the time-dependent solver,
where it is recommended to use manual time stepping, see Dynamic Contact Analysis.
Monitoring the Solution
It is often useful to monitor the solution during a contact analysis. This can be done
in different ways.
Using the Results while solving functionality in the study step is a good practice. You
can either use a stress plot, or a plot of the contact pressure. In most cases, the scale of
a deformed plot should be set to 1 when monitoring contact problems. If you select
Results while solving in the Segregated node, the plot is updated after each iteration,
thus allowing you to monitor the convergence in detail.
For each contact pair, two global variables that can be used in probe plots are available.
These are the maximum contact pressure (<phys>.Tnmax_<pair>) and the minimum
gap distance (<phys>.gapmin_<pair>).
Looking at the convergence plot will give valuable information about the convergence
properties. There will, as a default, be one graph per Contact node in the Model Tree,
which will help you pinpoint the source of a convergence problem. You can also
increase the granularity even more by changing Solver log to Detailed in the Advanced
node in the solver sequence. This will give a separate convergence curve for each
dependent variable.
You can also select to include information about the contact state in the solver log. To
do that, select the Add contact status to solver log check box in the Advanced section of
the settings for the Contact node. For each contact pair, messages like
69 points of 120 are now in contact.
33 points started to stick. 72 points are now sticking.
12 points started to slide. 47 points are now sliding.
will be generated for each time or parameter step. Only changes are reported.
CONTACT MODELING
|
247
Dependent Variables in Contact Analysis
The Contact and its subnodes will generate a number of degrees of freedom depending
on the settings and study type. You will see these degrees of freedom appear under
Dependent Variables in the solver sequence. There are two types of extra variables
created:
• Variables changed until convergence is reached during the iterations. These variables
appear in the Lumped Step nodes in the Segregated solver or in the Fully Coupled
node.
• Variables used to store the state, once the iterations have converged for a certain
time or parameter step, so called internal degrees of freedom. Such state variables
are not immediately visible in the solver sequence, but it you select the Displacement
Field node under Dependent Variables in the solver sequence, you will see them listed
as ‘Internal variables’.
If you change settings in the Contact or Friction nodes after the solver
sequence has been generated, dependent variables may be added or
removed. The second case is never a problem, but when new dependent
variables are created, they are not automatically added to the groups in the
segregated solver. You may then encounter the error message
“Segregated solver steps do not involve all components.” You
can then either regenerate the solver sequence, or manually insert the
missing variables into the Lumped Step node.
In Table 2-11 the dependent variables that can be created by the Contact and its
subnodes are summarized. To shorten the variable names, the full scope has been
removed. As an example, the contact pressure variable for pair p1 in component comp1,
generated in the Solid Mechanics interface solid, will have the full name similar to
comp1.solid.Tn_p1. In the table, it is shown as Tn.
TABLE 2-11: DEPENDENT VARIABLES OCCURRING IN CONTACT ANALYSIS.
VARIABLE NAME
DESCRIPTION
EXPLANATION
CREATED
SOLVER NODE
Tn
Contact pressure
The contact
pressure in the
normal direction
Contact:
Lumped
Step
Tt
248 |
Friction force
The friction force
vector
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Augmented
Lagrangian used
Friction:
Augmented
Lagrangian used
Lumped
Step
TABLE 2-11: DEPENDENT VARIABLES OCCURRING IN CONTACT ANALYSIS.
VARIABLE NAME
DESCRIPTION
EXPLANATION
CREATED
SOLVER NODE
gap_old
Previous gap
distance
Physical gap
variable from the
last converged
solution,
Contact: Penalty,
dynamic or
Internal
state
variable
Augmented
Lagrangian,
dynamic used
cm_old
Previous mapped
source
coordinates
The location on
the source where
this point was
located at last
converged
solution
Friction node
present
Internal
state
variable
sliptot_old
Previous
accumulated slip
Total slip in this
point at last
converged
solution
Friction or Slip
velocity: Store
Internal
state
variable
accumulated slip
selected
contact_old
Contact variable
in previous step
Nonzero if the
point was in
contact at last
converged
solution within
the friction
detection
tolerance
Friction node
present
Internal
state
variable
isContact_old
Contact status
variable in
previous step
Nonzero if the
point was in
contact at last
converged
solution
Contact: Add
Internal
state
variable
Nonzero if the
point was in a
sliding state at last
converged
solution
Contact: Add
Nonzero if the
point was in a
sticking state at
last converged
solution
Contact: Add
isSliding_old
isSticking_old
Sliding friction
status variable
previous step
Sticking friction
status variable
previous step
contact status to
solver log
selected
contact status to
solver log
Internal
state
variable
selected. Friction
node present.
contact status to
solver log
Internal
state
variable
selected. Friction
node present.
CONTACT MODELING
|
249
TABLE 2-11: DEPENDENT VARIABLES OCCURRING IN CONTACT ANALYSIS.
VARIABLE NAME
DESCRIPTION
EXPLANATION
CREATED
SOLVER NODE
Wfric
Frictional
dissipation density
Energy dissipated
by friction
Friction present
and Compute
Segregated
step
frictional
dissipation
selected.
Wfric_old
Previous frictional
dissipation density
Energy dissipated
by friction at the
last converged
solution
Slip velocity
present and
Compute
frictional
dissipation
Internal
state
variable
selected.
activation_old
Adhesion
condition at
previous step
Nonzero if the
adhesion
condition was
fulfilled at the last
converged
solution
Adhesion node
present
Internal
state
variable
cma_old
Previous adhesive
mapped source
coordinates
Position on the
source where this
point was located
when adhesion
was detected.
Adhesion node
present
Internal
state
variable
um_max_old
Maximum
displacement
jump at previous
step
Maximum norm
of displacement
jump vector
reached until
previous step.
Decohesion node
present and
Internal
state
variable
Ydm_max_old
250 |
Maximum damage
energy at
previous step
Maximum value of
the stored
undamaged elastic
energy at
previous step
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Displacementbased damage
selected
Decohesion node
present and
Energy-based
damage selected
Internal
state
variable
TABLE 2-11: DEPENDENT VARIABLES OCCURRING IN CONTACT ANALYSIS.
VARIABLE NAME
DESCRIPTION
EXPLANATION
CREATED
SOLVER NODE
vdmg_old
Viscous damage at
previous step
Value of the
viscous damage
variable at the
previous step
Decohesion node
present and
Internal
state
variable
These variables
are related to the
computation of
the energy
dissipated by
damage
Decohesion node
present and
Wdmg_old
Wsd_old
dmg_old
Delayed damage
selected
Compute damage
dissipation energy
Internal
state
variables
selected.
Important Contact Variables
In this section you will find a summary of variables created in the contact node that
can be useful in postprocessing. In Table 2-12 important field variables are listed. For
the Shell, Layered Shell and Membrane interfaces, these are appended with the suffix
‘_top’ or ‘_bot’, depending on which side of the boundary that is in contact. All
variables are also defined per contact node, for example <phys>.<contact_tag>.Tn
is the contact pressure from the contact node with the tag <contact_tag>. These
variables can be useful if the model includes multiple contact nodes. Table 2-13
presents global variables related to contact that can be useful for postprocessing.
TABLE 2-12: IMPORTANT CONTACT VARIABLES.
VARIABLE
DESCRIPTION
DEFINED IN
COMMENTS
<phys>.Tn
Contact pressure
Contact
Vector in global
coordinates also
available
<phys>.gap
Gap distance including
offsets
Contact
<phys>.Ttnorm
Friction force norm
Friction or Slip
Velocity
<phys>.Tt
Friction force
Friction or Slip
Velocity
<phys>.qfric
Friction dissipation
rate
Friction or Slip
Velocity
<phys>.fs
Adhesive stress
Adhesion
Vector
<phys>.us
Displacement jump
Adhesion
Vector
<phys>.adhesion
Adhesion condition
Adhesion
Vector
CONTACT MODELING
|
251
TABLE 2-12: IMPORTANT CONTACT VARIABLES.
VARIABLE
DESCRIPTION
DEFINED IN
<phys>.bdmg
Damage
Decohesion
COMMENTS
<phys>.um_max
Maximum
displacement jump
Decohesion
If displacementbased damage
<phys>.Ydm_max
Maximum damage
energy
Decohesion
If energy-based
damage
<phys>.Wcnt
Contact energy
density
Contact
<phys>.Wfric
Frictional dissipation
density
Friction or Slip
Velocity
<phys>.Wadhe
Adhesive elastic
energy
Adhesion
<phys>.Wdbmg
Damage dissipation
energy density
Decohesion
TABLE 2-13: GLOBAL CONTACT VARIABLES.
VARIABLE
DESCRIPTION
DEFINED IN
<phys>.gapmin_
Minimum gap
distance, contact pair
<pair_tag>
Contact
Maximum contact
pressure, contact pair
<pair_tag>
Contact
<pair_tag>
<phys>.T_tot
Total contact force
Contact
Vector
<phys>.Tn_tot
Total contact force,
pressure contribution
Contact
Vector
<phys>.Tt_tot
Total contact force,
friction contribution
Friction or Slip
Velocity
Vector
<phys>.Wcnt_tot
Total contact energy
Contact
Integration over
all contact
boundaries
<phys>
.Wfric_tot
Total frictional
dissipation
Friction or Slip
Velocity
Integration over
all contact
boundaries
<pair_tag>
<phys>.Tnmax_
252 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
COMMENTS
TABLE 2-13: GLOBAL CONTACT VARIABLES.
VARIABLE
DESCRIPTION
DEFINED IN
COMMENTS
<phys>
.Wadhe_tot
Total adhesive elastic
energy
Adhesion
Integration over
all contact
boundaries
<phys>.Wdmg_tot
Total damage
dissipation energy
Decohesion
Integration over
all contact
boundaries
References for Contact Modeling
1. J.L. Chaboche, F. Feyel, and Y. Monerie, “Interface debonding models: a viscous
regularization with limited rate dependency,” International Journal of Solids and
Structures, vol. 38, pp. 3127–3160, 2001.
CONTACT MODELING
|
253
Activating and Deactivating Material
In some applications, you may want to activate or deactivate material during an
analysis. An example is when you want to model the addition of material during
processes such as additive manufacturing or welding.
The information in this section is applicable if your license includes the
Structural Mechanics Module or the MEMS Module.
The Activation subnode can be used for this purpose. You enter an activation
expression to determine whether material is active or not. When this Boolean
expression is satisfied, the material is activated. Rather than truly adding or removing
material, the Activation subnode alters the stiffness and density of the material to
emulate this.
It is typically required that material is activated in a state of zero stress. Therefore,
Activation activates material in a stress-free state by removing all elastic strains present
at the point of activation.
ACTIVATION
Add an Activation subnode when you want to activate or deactivate one or several
domains selected in a Linear Elastic Material node. The Activation expression field is used
to define when material should be activated, and the Activation scale factor is used to
reduce the elastic stiffness and density of the material which is not active.
In Figure 2-17 a case is shown where the material in domains 1, 2, and 3 is to be
activated when an auxiliary sweep parameter para exceeds the value 1.5. The
activation scale factor has a default value of 10-5.
The activation condition can be any type of expression or function. A common case is
that it is a function of the temperature. The activation expression is evaluated in each
Gauss point. This means that an element can be partially activated. If you want to force
whole elements to be activated, you can for example put the activation expression
inside the centroid() operator.
254 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Figure 2-17: Settings for the Activation subnode.
VARIABLES
Two useful variables are created when you add the Activation subnode. The variable
isactive is set to ‘1’ when the activation condition is satisfied, and it is ‘0’ otherwise.
The variable wasactive is used to record if the material has been active at any previous
step in the analysis. This variable can be used to “lock” the state of activation, once it
has been reached. Suppose that you want the material in the previous example to
remain active even if para later becomes less than 1.5. The activation expression for an
interface with the name solid could then be expressed as:
(para > 1.5) || solid.wasactive
Similarly, the variable wasinactive is used to record if the material has been inactive
at any previous step in the analysis.
ACTIVATING AND DEACTIVATING MATERIAL
|
255
Domains that are not selected in any Activation subnode always have the isactive
variable set to ‘1’.
TABLE 2-14: VARIABLES DEFINED BY THE ACTIVATION SUBNODE.
VARIABLE
DESCRIPTION
<physics>.isactive
Current state of the material (1 or 0)
<physics>.wasactive
Variable set to 1 if isactive has been 1 previously
<physics>.wasinactive
Variable set to 1 if isactive has been 0 previously
RESULTS
If you have performed an analysis in which only part of the material is active, it is useful
to apply a Filter and only display the regions that actually are active; see Figure 2-18.
When an Activation subnode is added in a Solid Mechanics or Membrane interface,
such a Filter node is automatically added to the default stress plots.
Figure 2-18: Filter settings to only display active material.
256 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
S pr i ng s a nd Damp ers
The Spring Foundation and Thin Elastic Layer nodes supply elastic and damping
boundary conditions for domains, boundaries, edges, and points.
The features are completely analogous, with the difference that a Spring Foundation
connects the structural part on which it is acting to a fixed “ground,” while the Thin
Elastic Layer acts between two parts, either on an interior boundary or on a pair.
A Spring Foundation is most commonly used for simulating boundary conditions with
a certain flexibility, such as the soil surrounding a construction. Another important use
is for stabilizing parts that would otherwise have a rigid-body singularity. This is a
common problem in contact modeling before an assembly has actually settled. In this
case a Spring Foundation acting on the entire domain is useful because it avoids the
introduction of local forces.
A Thin Elastic Layer used as a pair condition can simulate thin layers with material
properties that differ significantly from the surrounding domains. Common
applications are gaskets and adhesives.
When a Thin Elastic Layer is applied on an interior boundary, it usually models a local
flexibility, such as a fracture zone in a geological model.
The following types of data are defined by these nodes:
• Spring Data
• Loss Factor Damping
• Viscous Damping
SPRING DATA
The elastic properties can be defined either by a spring stiffness or by a force as function
of displacement. The force as a function of displacement can be more convenient for
nonlinear springs. Each spring node has three displacement variables defined, which
can be used to describe the deformation dependency. These variables are named
<interface_name>.uspring1_<tag>, <interface_name>.uspring2_<tag>, and
<interface_name>.uspring3_<tag> for the three directions given by the local
coordinate system. In the variable names, <tag> represents the tag of the feature
defining the variable. The tag could, for example, be spf1 or tel1 for a Spring
Foundation or a Thin Elastic Layer, respectively. These variables measure the relative
extension of the spring after subtraction of any predeformation.
SPRINGS AND DAMPERS
|
257
In addition to explicitly supplying a spring stiffness, you can choose to enter elastic
material data and the layer thickness. The spring stiffness is then computed internally,
based on an assumption of plane strain conditions.
LOSS FACTOR DAMPING
The loss factor damping adds a loss factor to the spring data above, so that the total
force exerted by the spring with loss is
f sl =  1 + i f s
where fs is the elastic spring force, and  is the loss factor.
Loss factor damping is only applicable for eigenfrequency and frequency-domain
analysis. In time-dependent analysis the loss factor is ignored.
VISCOUS DAMPING
It is also possible to add viscous damping to the Spring Foundation and Thin Elastic
Layer features. The viscous damping adds a force proportional to the velocity (or in
the case of Thin Elastic Layer: the relative velocity between the two boundaries). The
viscosity constant of the feature can be made dependent on the velocity by using the
variables named <interface_name>.vdamper1_<tag>, <interface_name>
.vdamper2_<tag>, and <interface_name>.vdamper3_<tag>, which contain the
velocities in the three local directions.
Bracket — Spring Foundation Analysis: Application Library path
Structural_Mechanics_Module/Tutorials/bracket_spring
Spring Foundation and Thin Elastic Layer
258 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Defining Multiphysics Models
The following modeling tips are about how to define multiphysics models. A good
place to start reading is in Building a COMSOL Multiphysics Model in the COMSOL
Multiphysics Reference Manual.
In this section:
• Thermal-Structure Interaction
• Acoustic–Structure Interaction
• Thermal–Electric–Structural Interaction
Thermal-Structure Interaction
The Thermal Stress, Solid Interface included with this module has a predefined
one-way approach for thermal-structure interaction (thermal stress), which combines
a Solid Mechanics interface with a Heat Transfer interface from the Heat Transfer
Module or COMSOL Multiphysics.
There are also similar multiphysics interfaces available for thin structures, as described
in The Thermal Stress, Shell Interface, The Thermal Stress, Membrane Interface, and
The Thermal Stress, Layered Shell Interface. The latter requires the Composite
Materials Module.
By default, COMSOL Multiphysics takes advantage of the one-way dependence and
solves the problem sequentially using the segregated solver. The solution for the
temperature is separated from the stress-strain analysis, which then uses the computed
temperature field from the heat transfer equation.
Using a single iteration in the segregated solver does not produce a
correct result if there are thermal properties that depend on the
displacements. Examples are when a heat source causes mechanical losses
(damping) in the material or when thermal contact is present.
DEFINING MULTIPHYSICS MODELS
|
259
Acoustic–Structure Interaction
When the Structural Mechanics Module is used together with an acoustics physics
interface from the Acoustics Module, it is possible to model a wide range of Acoustic–
Structure interaction problems.
There are several physics interfaces available that are documented and
described in the Acoustic–Structure Interaction Interfaces chapter in the
Acoustic Module User’s Guide
• The Acoustic–Solid Interaction, Frequency Domain Interface
• The Acoustic–Solid Interaction, Transient Interface
• The Acoustic–Piezoelectric Interaction, Frequency Domain Interface
• The Acoustic–Piezoelectric Interaction, Transient Interface
• The Solid Mechanics (Elastic Waves) Interface
• The Elastic Waves, Time Explicit Interface
• The Poroelastic Waves Interface
• The Acoustic–Solid–Poroelastic Waves Interaction Interface
• The Acoustic–Poroelastic Waves Interaction Interface
• The Acoustic–Shell Interaction, Frequency Domain Interface
• The Acoustic–Shell Interaction, Transient Interface
• The Thermoviscous Acoustic–Solid Interaction, Frequency Domain
Interface
• The Thermoviscous Acoustic–Shell Interaction, Frequency Domain
Interface
Thermal–Electric–Structural Interaction
The Joule Heating and Thermal Expansion Interface enables thermal–electric–
structural interaction. This is a combination of three physics interfaces: Solid
Mechanics, Heat Transfer in Solids, and Electric Currents.
The thermal-electric coupling is bidirectional, with Joule heating and
temperature-dependent electrical properties, while the temperature coupling to the
Solid Mechanics interface is unidirectional.
260 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
By default, COMSOL Multiphysics takes advantage of the one-way dependence and
solves the problem sequentially using the segregated solver. Temperature and electric
potential are solved using a coupled approach and then the stress-strain analysis uses
the computed temperature field from the heat transfer equation.
Using a single iteration does not produce a correct result if there are
thermal properties or electrical that depend on the displacements, making
the thermal-structure part into a bidirectional coupling.
DEFINING MULTIPHYSICS MODELS
|
261
T he r m a lly C o u p l ed Prob l em s
A wide class of structural mechanics problems are related to effects of variations in
temperature. In this section various such effects are discussed.
Temperatures can either be computed using another physics interface, usually Heat
Transfer in Solids, or directly be prescribed in the input for the various physics nodes.
For information about the predefined coupling between the Solid
Mechanics and Heat Transfer in Solids interfaces, see The Thermal Stress,
Solid Interface.
In this section:
• Temperature-Dependent Material Data
• Thermal Expansion
• Constraints and Thermal Expansion
• Thermoelastic Damping
Temperature-Dependent Material Data
Many material properties, such as Young’s modulus, coefficient of thermal expansion,
and yield stress, can have a significant dependence on temperature. In many cases,
materials supplied in the material libraries and databases have such dependencies
incorporated.
Materials in the COMSOL Multiphysics Reference Manual
If a material property under the Materials branch has a temperature dependence, you
have to input the temperature to be used in the Model Input section in the settings
window for the node in the physics interface that references the property. It is possible
that not all aspects of a material are defined in the same node in the Model Builder tree.
For example, if a problem is run with thermal expansion and plasticity, then:
• Young’s modulus, Poisson’s ratio, and mass density are given in the Linear Elastic
Material node.
262 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
• Yield stress and hardening function are given in the Plasticity node.
• Coefficient of thermal expansion is given in the Thermal Expansion (for Materials)
subnode.
The Plasticity node is available as a subnode to the Linear Elastic Material
node when you have either the Nonlinear Structural Materials Module or
the Geomechanics Module.
For each of these nodes, there is a Model Input section in the Settings window. Some
of these sections may be empty if none of the properties given in that node have a
temperature dependence. In general, you have to supply the temperature in all the
Model Inputs sections.
As a default, the value of the temperature T is obtained from a Common model input.
You can also select User defined to enter a value or expression for the reference
temperature locally. This can be done either by explicitly giving a temperature or by
selecting a temperature variable from another physics interface.
USING COMMON MODEL INPUT
When the option Common model input is selected in a physics node, you can see or
). Doing that
modify the value actually used by clicking the Go To Source button (
will move you the node in the Model Builder that is defining the value of the property.
That location can be:
• The Default Model Inputs node under Global Definitions
• A Model Input node under Definitions->Shared Properties in the current component
If you want to create a model input value which is local to your current selection, click
. This will create a new Model Input node under
the Create Model Input button
Definitions->Shared Properties in the current component, having the same selection as
in the current node.
See also Default Model Inputs and Model Input in the COMSOL
Multiphysics Reference Manual.
MASS DENSITY AND VOLUME REFERENCE TEMPERATURE
All structural mechanics interfaces are formulated on the material frame. This means
that the equations of motion are written for a certain volume in its initial configuration.
THERMALLY COUPLED PROBLEMS
|
263
The preservation of mass requires that the mass density is constant. In a structural
mechanics problem this means that the mass density must not change. If you are using
a material in which the density has a temperature dependence, you must specify a
specific temperature at which the value is evaluated. This is the volume reference
temperature. Conceptually, you can consider this as the temperature at which the
domain has the size in which it is drawn. In practice, the choice of reference
temperature is seldom an issue, unless your application requires extreme precision. The
density of a solid material has a rather slow variation with temperature, so in most cases
it is sufficient to use room temperature as reference.
If any material in the model has a temperature-dependent mass density, the Volume
reference temperature list will appear in the Model Input section of the material settings.
As a default, the value of Tref is obtained from a Common model input. You can also
select User defined to enter a value or expression for the reference temperature locally.
All effects of volume change with temperature are incorporated through the thermal
expansion effects.
See also
• Using Common Model Input.
• Default Model Inputs and Model Input in the COMSOL Multiphysics
Reference Manual.
Thermal Expansion
As the temperature changes, most materials react by a change of volume. For a
constrained structure, the stresses that evolve even with moderate temperature changes
can be considerable. The volume change can be represented a thermal strain th,
which produces stress-free deformations. For a linear elastic material, the constitutive
law is
 = C    –  th 
264 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
In the computations, the thermal expansion appears as a load, even though it formally
is a part of the constitutive relations.
You can include thermal expansion in a model either by adding a Thermal
Expansion (for Materials) subnode to the chosen material, or by using the
Thermal Expansion.
TEMPERATURE DEPENDENCE OF THE THERMAL EXPANSION
COEFFICIENT
When performing an analysis over a larger range of temperatures, you often need to
consider the temperature dependence in the values of the thermal expansion
coefficient itself.
As long as you are using materials from the COMSOL Material Library, everything is
handled internally. When you want to enter data from your own measurements or from
the literature, you do, however, need to be aware of some details in the definitions
used.
Tangent or Secant Data
Thermal expansion coefficients can appear in two forms: tangent and secant.
The tangent form states that the increment in length is
dL
-------- =  t  T dT
L
(2-29)
where t is the tangential thermal expansion coefficient. This form, which is the
thermodynamic definition, is conceptually simple, because t is uniquely defined at
each temperature. It is, however, less convenient to use in practice because an
integration is required for determining the actual change in length for a finite
temperature difference.
The secant formulation, which is the default in COMSOL Multiphysics, is often used
in engineering:
L
-------- =   T T
L0
In the secant formulation, the actual values of  will however depend on the choice of
reference temperature, Tref, at which the material has the reference length L0:
THERMALLY COUPLED PROBLEMS
|
265
L
-------- =   T,T ref   T – T ref 
L0
Converting from Tangent Form to Secant Form
Equation 2-29 can be integrated, giving
T
L
ln  ------ =
L0
 t   d
(2-30)
T ref
Define
T
I  T,T ref  =
 t   d
T ref
Thus,
L
L – 1 = e I  T,T ref  – 1
-------- = -----L0
L0
giving the secant thermal expansion coefficient as
I  T,T ref 
e
– 1  T,T ref  = ------------------------------- T – T ref 
For most materials and temperature ranges I  T,T ref  « 1 , which makes it possible to
approximate with the simpler expression
I  T,T ref 
  T,T ref  = ------------------------ T – T ref 
(2-31)
If you have access to tangent data, you can choose between two different methods for
using them in COMSOL Multiphysics:
• In most of the physics interfaces, you can enter tangent data directly by selecting
Tangent coefficient of thermal expansion in the settings for Thermal Expansion. When
using this option, a numerical integration of Equation 2-30 will be performed each
266 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
time the thermal strain is used. This will have a negative impact on the performance,
when compared to using a secant coefficient of thermal expansion.
• Precompute the expression in Equation 2-29 externally for the intended range of
temperatures. This can for example be done in a spreadsheet program. Enter the
computed result as a function, which is then used as any other secant temperature
dependent thermal expansion coefficient.
When using Tangent coefficient of thermal expansion, the integrate
operator is used. It is called with the two integration limits being the
reference temperature <phys>.Tref and the current temperature <phys>
.T, where <phys> is the tag of the physics interface. If you define the
expression for the coefficient of thermal expansion yourself, you must
ensure that it depends on a ‘free’ variable, and not use the same
temperature variable as you use to prescribe the current temperature
<phys>.T.
Thermal Expansion Coefficient Dependence on Reference Temperature
Letm(T) be the temperature-dependent function that represents the measured values
of the secant thermal expansion coefficient. The change in length of a sample at a given
temperature T with respect to the sample’s original length at a temperature Tm is called
dilation.
Note that by definition, the dilation at T = Tm is zero, so Tm denotes the strain-free
state of the material as far as the measured values of m(T) is concerned. Denote the
length of the sample at a temperature T as L(T) and the strain-free length as
L0 = L(Tm). The dilation can be then expressed as LTL(Tm. Using the definition
of the secant coefficient of thermal expansion, L(T) can be written as:
L  T  =  1 +  m  T   T – T m  L  T m 
(2-32)
When using the measured data, it is possible that the strain-free state occurs at a
temperature Tref which differs from Tm. The dilation at any temperature T would then
be defined as LTL(Tref, where L(Tref) can be written as.
L  T ref  =  1 +  m  T ref   T ref – T m  L  T m 
(2-33)
As a result of this shift in the strain-free temperature, it is necessary to redefine the
thermal expansion coefficient so that L(T) and L(Tref) can be related using
Equation 2-32 but with Tm replaced by Tref.
THERMALLY COUPLED PROBLEMS
|
267
L  T  =  1 +  r  T   T – T ref  L  T ref 
(2-34)
Here r(T) is the redefined thermal expansion coefficient, based on Tref. It can be
derived from the relations above. Using Equation 2-32 and Equation 2-34 there are
two ways of writing the current length L(T), so that
 1 +  r  T   T – T ref  L  T ref  =  1 +  m  T   T – T m  L  T m 
(2-35)
Equation 2-33 makes it is possible to eliminate L(Tref) and L(Tm) from
Equation 2-35:
 1 +  r  T   T – T ref    1 +  m  T ref   T ref – T m   = 1 +  m  T   T – T m  (2-36)
It is now possible find r(T), expressed in known quantities. After some algebra, the
final expression is
 m  T  –  m  T ref 
 m  T  +  T ref – T m  ----------------------------------------------T – T ref
 r  T  = ----------------------------------------------------------------------------------------------------1 +  m  T ref   T ref – T m 
(2-37)
In order to arrive at this form of r(T), the numerator has been rewritten, using
 m  T   T – T m  –  m  T ref   T ref – T m  =
 m  T   T – T ref  +  m  T   T ref – T m  –  m  T ref   T ref – T m  =
(2-38)
 m  T   T – T ref  +  T ref – T m    m  T  –  m  T ref  
Representation in COMSOL Multiphysics
Most materials listed in the material libraries and databases available with COMSOL
Multiphysics and its add-on products contain a function for the measured
temperature-dependent thermal expansion coefficient curve. You can find this from
the Materials branch, as shown in Figure 2-19. The Piecewise function named
alpha_solid_1 is the measured thermal expansion coefficient m(T).
Using Functions in Materials in the COMSOL Multiphysics Reference
Manual
The Material Contents section in Figure 2-19 shows the material property alpha,
which is the redefined thermal expansion coefficient r(T). The complete expression
for alpha is as follows:
268 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
(alpha_solid_1(T[1/K])[1/K]+(Tempref-293[K])*
if(abs(T-Tempref)>1e-3,(alpha_solid_1(T[1/K])[1/K]
-alpha_solid_1(Tempref[1/K])[1/K])/(T-Tempref),
d(alpha_solid_1(T[1/K]),T)[1/K]))/
(1+alpha_solid_1(Tempref[1/K])[1/K]*(Tempref-293[K]))
This is essentially Equation 2-37, but with a small modification to avoid problems if
T=Tref.
m(T)
r(T)
Figure 2-19: An example in COMSOL Multiphysics showing the Materials branch and
where to find the temperature-dependent thermal expansion coefficient.
In the definition of alpha (to be more specific: <material_tag>.def.alpha) in
COMSOL Multiphysics, Tm is set as 293 K and Tref is obtained from the variable
Tempref, which typically fetches its value from the physics interface.
THERMALLY COUPLED PROBLEMS
|
269
Using Your Own Material Data
If you use our own material data in COMSOL Multiphysics (via an interpolation or
any other function), you can still copy-paste the built-in expression for alpha into your
New Material. You just need to:
• Replace the function name alpha_solid_1(T[1/K])[1/K], with the function
name that you have assigned to the temperature-dependent measured thermal
expansion coefficient and use the correct temperature units.
Take care when describing the units. Temperature unit conversions can be
the cause of subtle errors because of the shift in zero-point value. Use
kelvin (K) as the temperature unit to the largest possible extent. As an
alternative, you can use the other absolute temperature scale, Rankine
(R). Avoid using Fahrenheit and Celsius unless you are completely
familiar with how the temperature unit conversion works.
• Ensure that the value of Tm is changed from 293 K to the actual value of
temperature that was used as the strain-free temperature to compute m(T) in the
function that you created.
User-Defined Materials and Libraries in the COMSOL Multiphysics
Reference Manual
Constraints and Thermal Expansion
When a structure is undergoes thermal expansion, the fact that the motion is restricted
by constraints will in general cause stresses. There are three types of such effects:
• The global expansion is restricted by constraints at different locations, so that
internal forces are introduced throughout the structure.
• At a boundary that is constrained, local stresses can appear if the boundary is not
free to expand in the tangential direction.
• Internally, the same type of local constraint effects will be caused by rigid objects,
such as Rigid Material.
In many cases, not only the structure which actually is modeled deforms due to the
changes in temperature, but also the surroundings (which are approximated by
constraints) will deform. You can take this effect into account by adding a Thermal
270 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Expansion subnode to the constraints. The constraints will then provide an extra
displacement based on a given temperature field. For thermal strains, which have a
simple variation in space (for example, linear temperature variations), it is possible to
completely offset the constraint stresses using this method. For more general cases, the
stresses caused by the constraint can be significantly reduced.
The thermal expansions of the constraints are independent of that of the material in
the adjacent domain, so that the surrounding structure can be made from another
material, or have a different temperature distribution.
You can, however, also inherit temperature and thermal expansion coefficient from the
domain being constrained. This is useful for the common case that the temperature
and materials are the same over the modeled structure body and its surroundings.
The spatial variation of the temperature and coefficient of thermal
expansion must be explicit functions of the material frame coordinates. It
is not possible to use a computed temperature distribution for the thermal
expansion of the constraints.
• Thermal Expansion (for Constraints)
• Thermal Expansion of Constraints in the theory section.
For an example showing how to relive the stress at constraints in a heated
structure, see Thermal Expansion in a MEMS Device: Application
Library path Structural_Mechanics_Module/Thermal-Structure_Interaction/
thermal_expansion.
Thermoelastic Damping
In most engineering problems, the coupling between temperatures and structural
problems can be considered as unidirectional. Only the thermal expansion is
considered.
The opposite effect, where changes in stress cause heat generation, may be important
in small structures vibrating at high frequencies. The Thermoelasticity interface,
available with the MEMS Module, is designed for analyzing such problems.
THERMALLY COUPLED PROBLEMS
|
271
It is also possible to take this effect into account by adding the Thermoelastic Damping
node to the Heat Transfer in Solids interface. When you add a Thermal Expansion node
to a material in the Solid Mechanics interface, the heat source term is computed and
made available to the Heat Transfer in Solids interface.
When you add a Thermal Expansion node under the Multiphysics Couplings branch, it is
possible to select whether the thermoelastic damping effect should be taken into
account or not. The heat source contribution is then included automatically without
adding any data in the heat transfer interface.
In either case, the heat source term is only present when Structural Transient Behavior
is set to Include inertial terms.
See also
• Entropy and Thermoelasticity
• Thermal Expansion (for Materials)
• The Fluid–Solid Interaction Interface
272 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Fluid–Structure Interaction
Fluid–Structure interaction (FSI) involves several phenomena where a solid structure
and a fluid interact with each other. The interaction has three possible components,
which can be more or less important:
• The pressure and viscous forces in the fluid provides a load on the boundary of the
solid. Usually, the pressure is dominant.
• The deformation of the structure changes the geometry of the fluid domain.
• The fluid sees the structure as a moving wall, which imposes a velocity at the
interface.
You can model FSI with four different structural mechanics interfaces: Solid
Mechanics, Multibody Dynamics, Shell, and Membrane. The Fluid–flow can be
modeled with any domain-level physics interface from the Single-Phase Flow group and
the Two-Phase Flow groups under Multiphase Flow.
Deforming Fluid Domains
When a Fluid–Structure interaction multiphysics interface is added using the Model
Wizard, a Deforming Domain node can be added automatically in the Model Builder under
the Definitions node. This is the case for the following interfaces:
• Fluid–Solid Interaction
• Fluid–Shell Interaction
• Fluid–Membrane Interaction
• Fluid–Multibody Interaction
• Fluid–Multibody Interaction, Assembly
The Deforming Domain node is, however, not added for multiphysics interfaces denoted
‘Fixed Geometry’, which are intended for cases where the deformation of the fluid
domains is small everywhere.
A deforming domain represents domains and boundaries where the mesh can deform.
By default, the Deforming Domain node has an empty selection. You can then select any
fluid domain. However, this is only needed if the geometry of such a domain
experience significant changes due to the deformation or rotation of the adjacent solid
domains. Otherwise, the moving mesh computations could introduce unnecessary
FLUID–STRUCTURE INTERACTION
|
273
overhead and nonlinearity in the model (see Deformed Mesh Fundamentals).
Domains selected in the Solid Mechanics interface are not applicable. The
deformations of the solid parts are handled in the formulation of the Solid Mechanics
interface.
If no domains are selected in the Deforming Domain node, a fixed
geometry case is solved.
Under the Deforming Domain, you can also choose the Mesh smoothing type, by default
set to Hyperelastic. More information of the smoothing type can be found in
Deforming Domain chapter in the COMSOL Multiphysics Reference Manual
By default, the mesh is free at all external boundaries of the geometry, and it follows
the solid boundaries at the Solid–fluid interfaces. You can also add other types of
boundary conditions for the mesh motion; for details, see Deformed Geometry and
Moving Mesh in the COMSOL Multiphysics Reference Manual.
Union or Assembly
In most cases you model FSI problems so that the geometry sequence is set up to form
a union, and the same multiphysics coupling, Fluid–Structure Interaction, is used
irrespective of the type of structural mechanics interface. This coupling will
automatically find all boundaries that are shared between the structure and the fluid.
There are, however, cases where the assembly mode must be chosen, particularly when
having mechanisms, as is common in the Multibody Dynamics interface. In that case,
the interface between the solid and the fluid is no longer formed by a common
boundary. Rather, it consists of two boundaries, located at the same place in space.
These boundaries will in general slide with respect to each other. To model this, you
use the Fluid–Structure Interaction, Pair multiphysics coupling. You must create
appropriate pairs containing the boundaries from both types of physics under
Definitions, and manually select them in the Fluid–Structure Interaction, Pair node.
UNION — FLUID–STRUCTURE INTERACTION
When using Fluid–Structure Interaction, the spatial frame also deforms with a mesh
deformation that is equal to the displacements u_solid of the solid within the solid
domains. The mesh is free to move inside the fluid domains, and it adjusts to the
motion of the solid walls. This geometric change of the fluid domain is automatically
accounted for in COMSOL Multiphysics by the ALE method.
274 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
ASSEMBLY — FLUID–STRUCTURE INTERACTION, PAIR
The Fluid–Structure Interaction, Pair coupling does not automatically transfer the mesh
deformation at the interface from structural displacements.
For the moving mesh, you must specify the deformation of the mesh manually. Add a
Prescribed Mesh Displacement node under the Moving Mesh node, in which you give the
structural displacement as the mesh displacement expression. The variables for the
displacement in the structure is provided by the multiphysics coupling.
The variable names to use have the form <tag>.u_solid, <tag>
.v_solid, and <tag>.w_solid, where <tag> is the tag of the
multiphysics coupling, for example fsip1.
Contact and FSI
Sometimes the structural deformations are so large that objects may come into contact
with each other with the fluid being squeezed in between. Modeling contact together
with FSI requires some special considerations. The mesh in the fluid domain may
deform, but the topology remains the same — a fluid domain cannot be split into two.
If you are to model a valve or a similar structure, then the two solid parts cannot come
exactly into contact.
By adding an offset in the settings for the Contact node, you can force the two sides of
the solid to experience contact at some distance before they meet in the geometrical
sense. This approach only will, however, leave a thin channel through which the fluid
can pass. The reduction in flow may be sufficient, but you can block it even further by
increasing the viscosity in the channel when the gap is closed. To do that, you can, for
example, compute the minimum gap anywhere in the contact pair, and then make the
viscosity a function of it. Another option is to compute the wall distance in the fluid
from both sides of the contact pair and use that information to modify the viscosity.
Do not increase the viscosity more than a couple of orders of magnitude, to avoid
numerical problems.
In configurations where you more or less completely cut off the whole flow, you must
pay particular attention to your boundary conditions. A prescribed flux will cause an
extreme pressure build-up upstream of the valve and thus unrealistically large forces on
the structure.
FLUID–STRUCTURE INTERACTION
|
275
One-Way FSI
For some fixed geometry FSI problems, you can consider the coupling as being
unidirectional. One physics interface affects the other, but it is not reciprocal. Typical
examples are when the fluid slightly deforms the structure, or when small structural
vibrations modify the fluid flow. In this case, it is not necessary to compute the solution
with both physics interface solved together. It is more efficient to first solve for the
governing physics interface only, and then the other one with results from the first as
input. To solve such a problem sequentially, you need to create a study configuration
manually, with one study step for each physics interface. The governing physics
depends on the coupling type. For the case of fluid loading on a structure, the
governing physics is the fluid one. For the case of velocity transmission to a fluid, the
governing physics is the solid one.
Deformed geometry FSI, or fixed geometry fully coupled FSI, should not
be solved using a one-way approach.
Below are the steps to follow to compute a one-way FSI problem sequentially:
1 In the study step settings windows, under the Physics and Variables Selection section,
clear the physics that is solved in the second step, so that only the governing physics
is selected.
2 Add a second study step to the study and in the settings windows make sure you
have the governing physics cleared.
If the selected study steps are of stationary type, you can generate the default solver
configuration, edit it if necessary, and compute the solution. The mapping of the
solution from the first to the second study step is done automatically.
In case of a transient problem, continue with the steps below:
3 In the second study step settings window, expand the section Physics and Variables
Selection. Under Initial values of variables solved for make sure the settings are
defined as in the table below:
276 |
Settings
User controlled
Method
Solution
Study
<previous study step>
Selection
First
CHAPTER 2: STRUCTURAL MECHANICS MODELING
4 Under Values of variables not solved for define the settings as in the table below:
Settings
User controlled
Method
Solution
Study
<previous study step>
Selection
All
In the case of a fluid loading to structure coupling type, the structural mechanics
problem can be treated as quasistatic. This can be handled by running the structural
analysis as a parametric sweep over a number of static load cases, where time is used as
the parameter.
For an example of one-way FSI using a quasistatic structural analysis, see
Fluid-Structure Interaction in a Network of Blood Vessels: Application
Library path Structural_Mechanics_Module/Fluid-Structure_Interaction/
blood_vessel.
FLUID–STRUCTURE INTERACTION
|
277
Component Mode Synthesis
Introduction
Component mode synthesis (CMS) is a family of procedures in which one or more
parts of a finite element model are represented by a small reduced-order model
(ROM). There are several possible algorithms through which such a reduction can be
made. In COMSOL Multiphysics, the popular Craig–Bampton method is used for
model reduction with a dual assembly technique to ensure compatibility between
components.
The reduced component is sometimes called a dynamic substructure. Essentially, it
contains small mass, damping, and stiffness matrices, tuned so that it can represent the
static stiffness, as well as a set of important eigenmodes and the inertia of the original
component. An important assumption is that the reduced structure is linear.
The reduced component accounts for the constraints applied on the component. It can
also contain, for example, information about loads applied to the component prior to
model reduction.
Since the reduced components only have a small number of degrees of freedom (often
of the order of 10-100), they are computationally more efficient than the original full
FEM components. To create a reduced component, it is necessary to both perform an
eigenfrequency analysis and to solve for a number of static load cases. These studies
are, however, computed at the component level, and are thus usually computationally
much cheaper than analyzing the full model.
For general information on reduced-order modeling and model
reduction, see also
• Reduced-Order Modeling
• Model Reduction
in the COMSOL Multiphysics Reference Manual.
COMSOL Implementation
The Component Mode Synthesis (CMS) technique is currently implemented in the
Solid Mechanics, Shell, and Multibody Dynamics interfaces. You use the Reduced
278 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Flexible Components node in either of these interfaces to control the generation and use
of such reduced components.
Reduced components are connected to each other and to nonreduced parts of the
model through Attachment features. It means that all physics features that can access
an attachment can be used to connect the reduced components. The most common
option is to use joints, but there are other alternatives, such as Spring-Damper, or
bearing foundations in the rotordynamics interfaces.
The global model can consist of either a set of reduced components, or a mix of
ordinary FE discretized domains and reduced components. The reduced components
can be used as linear parts in an otherwise nonlinear model.
A requirement to be able to create a valid reduced component is that its underlying
physics is linear with regards to material models, the strain formulation, and other
possible contributions such as springs and loads
COMSOL Multiphysics always forces a geometrically linear formulation
on selections that intersect that of a Reduced Flexible Components node.
When using a reduced component in the global model, the connection to
nonreduced parts must be such that the deformation of the reduced
component is limited to small rotations and small strains.
You can compute all type of results and visualize reduced components just as if they
are ordinary domains in your model. One important property of the reduced
component is that only the results for the reduced set of degrees of freedom are stored.
It means that for time-dependent studies with many time steps, the file sizes can be
reduced by orders of magnitude.
Applications
Some examples of applications of the CMS reduction technique include:
• In multibody dynamics models, you usually have a number of physical components,
coupled by joints. The ultimate reduction is then to use rigid domains. When it is
necessary to take the flexibility of a component into account, using a reduced
flexible component is attractive.
COMPONENT MODE SYNTHESIS
|
279
• In rotordynamics, it is common that the foundation supporting the rotor must be
part of the analysis. Such a foundation will almost invariably have linear properties.
It is then well suited to be considered as a reduced flexible component. This can
greatly reduce the number of the degrees of freedom in the rotordynamic analysis,
which is often computationally heavy.
• In many situations, only a smaller part of a model is nonlinear. It is then possible to
reduce the linear parts once and for all, and then iterate on a much smaller nonlinear
system of equations. For this to be feasible, it must however be possible to dissect
the structure in a way that can be represented by attachments.
Working with CMS Models
CREATING REDUCED COMPONENTS
A reduced component can be created in an applicable physics interface by adding a
Reduced Flexible Components node, in which you select all domains that are to be
reduced, as shown in Figure 2-20. Subsequently, one Component Definition subnode
should be added for each set of domains for which a reduced-order model (ROM) is
to be generated. By default, this step is automated and the selected domains are
grouped into disconnected components as detected from the geometry. With this
setting, a number of Component Definition subnodes are created and their selections are
set automatically. However, by setting Component definition to User defined in the
Reduced Flexible Components node, you can take manual control of the geometric
definition of the components by adding, removing, or modifying Component Definition
nodes. In each such node, select a number of domains that defines a component. This
may be necessary if domains are not physically adjacent, but connected by other means,
for example, by springs.
By default, disconnected geometries connect by the Continuity and Thin Elastic Layer
pair features are merged when automatically generating Component Definition
subnodes. This also applies to Boundary to Boundary, Edge to Boundary, and Edge to
Edge connection features in the Shell interface. The automatic handling of such
connections can be disabled by clearing Include connections and pairs in component
definition in the Reduced Flexible Components node.
280 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Figure 2-20: A Reduced Flexible Components node with two automatically generated
Component Definition subnodes.
• If the components are geometrically disjoint, then Form Union should
be used in the geometry sequence. If not, Form Assembly is probably a
better choice, but then you may have to either create unions between
domains that are part of the same components, or edit the settings in
the Component Definition nodes manually.
• In the majority of cases, it is sufficient with one Reduced Flexible
Components node per physics interface. If you, however, do not want to
train all ROMs in one sweep, having a single Reduced Flexible
Components node per actual component can be useful. Another case is
if you decide to reduce one additional component after already having
reduced one or several other components. Then, adding an additional
Reduced Flexible Components node can be an alternative.
COMPONENT MODE SYNTHESIS
|
281
The Reduced Flexible Components node is only applicable on domains
where the material behavior is determined by a Linear Elastic Material node
or a Section Stiffness node in the Shell interface. You can, however, have
several such nodes with different properties and settings within one
reduced component.
A disconnected reduced component, as defined by a Component Definition subnode,
can only be connected to other parts of the geometry by attachment features. In fact,
to be able to create the ROM, each component must be connected to at least one
Attachment node. By using attachments, a reduced component can be connected to
any number of other parts, reduced or full, of the model assembly.
See also Attachments.
When working with CMS, the full static and dynamic behavior of a component is
represented by a number constraint modes and constrained eigenmodes that are
computed in the training phase. These are independent of each other and are used to
construct one ROM for each component. Each Attachment node connected to a
component will add a number of static load cases that describe the constraint modes:
six in 3D, and three in 2D. The number of eigenmodes to be used is controlled
manually. You can either define it for all components in the Reduced Flexible
Components node, or individually in each Component Definition subnode. To get an
accurate representation of the reduced component, always make sure to use a sufficient
number of eigenmodes to describe the dynamics of each component. During the
eigenfrequency training step, all attachments are treated as fixed constraints, hence, the
eigenmodes are always constrained.
Note that, from a computational point of view, each eigenmode is represented as a
degree of freedom when using the reduced component in a global analysis. For
computational efficiency, you should avoid using unnecessarily many eigenmodes.
To create the ROMs, a special study sequence needs to be set up for each Reduced
Flexible Components node. It should sweep over all Component Definition subnodes, and
for each component, compute the static load cases and the requested eigenmodes in
training study steps as outlined above. The results from these study steps are then used
)
in a Model reduction step to generate a ROM. By using the Configure CMS Study (
button in the Reduced Flexible Components node, the setup of this special study
282 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
sequence is automated. In the model tree, a generated ROM is represented as a node
with the label Reduced Component under Global Definitions as seen in Figure 2-21.
Figure 2-21: Nodes in the model tree that are added automatically when working with
CMS.
• When a Reduced Flexible Components node is added, a set of parameters
are also automatically added under the Global Definitions branch. These
are placed in the CMS Parameters node seen in Figure 2-21, which is
created by the first Reduced Flexible Components node in the model.
Additionally, each Reduced Flexible Components node creates an explicit
selection node with the label CMS Component (<tag>) in its model
component. The parameters and selection are used in the
corresponding CMS study and should therefore not be deleted or
modified. As a safeguard, they are regenerated if missing when the
Configure CMS Study (
) action is executed.
• If you change the number of Component Definition nodes or add new
features to the physics interface after setting up the CMS study and
want to run it again, the safest option is to reconfigure the study by
) action. Note that this will delete
using the Configure CMS Study (
any ROMs that have previously been generated. To save these in the
model, you can temporarily change the name of the existing Reduced
Component nodes under Global Definitions before reconfiguring the
CMS study.
COMPONENT MODE SYNTHESIS
|
283
APPLYING LOADS TO REDUCED COMPONENTS
Loads can be applied to a reduced component in two fundamentally different ways:
1 External to the ROM: In this case, the weak contribution of the load on the reduced
component is part of the assembly procedure for the global FE model. This is the
default choice and can handle any type of loads. It is, however, the computationally
more expensive of the two methods.
2 Internal to the ROM: The load can either be constant or a function of a global
reduced model input. In this case, the load is stored as part of the ROM.
Be careful not to mix up the two alternatives; doing so can lead to double load
contributions. For this reason, option 1 is usually recommended. When the Configure
CMS study (
) button is used, all load type features are disabled in the study steps of
the CMS study.
Figure 2-22: Loads are, by default, disabled in the model reduction study.
The advantage of option 2 is that it can be computationally cheaper in the global
analysis, since any evaluation of weak equations in domains of the reduced component
is avoided. To use this approach, enable the relevant load features in the reference
study step to the Model Reduction study step in the CMS study. The same load features
should then be disabled in all other studies. By selecting Include load contributions in
Reduced Components in the Reduced Flexible Components node, you can change the
284 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
default behavior of loads when the Configure CMS study (
) button is used. When
selected, all loads are enabled in the study steps of the generated CMS study.
You can find an example of both approaches for load application in this
tutorial model:
• Component Mode Synthesis Tutorial: Application Library path
Structural_Mechanics_Module/Tutorials/cms_tutorial
• Component Mode Synthesis Tutorial: Application Library path
Multibody_Dynamics_Module/Tutorials/cms_tutorial
• Component Mode Synthesis Tutorial: Application Library path
MEMS_Module/Dynamics_and_Vibration/cms_tutorial
While conceptually similar to other load features, Linearly Accelerated Frame, Rotating
Frame, Gravity, and Base Excitation are always considered as internal to the ROM and
part of the reduced component. They are, by default, enabled in the CMS Study when
) button. The reason is that they are considered to
using the Configure CMS study (
contribute to the acceleration of the frame. If necessary, use control inputs to
parameterize, for example, the gravity vector or rotation speed.
THE CMS STUDY
The CMS study is a parametric sweep over a set of components as defined by the
Component Definition subnodes of a Reduced Flexible Components node with the aim to
create one ROM for each component. The study is automatically generated by using
) button in a Reduced Flexible Components node. The
the Configure CMS Study (
auto-generated study and solver sequences have a number of built-in features and
settings that greatly simplifies the process of creating a reduced component; especially
when there are multiple components to be reduced. The study sequence is shown in
Figure 2-23 and consists of:
• A Parametric sweep over the components to be reduced
• A Stationary training study step to compute the constraint modes from the static
load cases
• An Eigenfrequency training study step to compute the constrained eigenmodes
• A Model Reduction study step to generate the ROM. This step can either use a Time
Dependent or Frequency Domain study step as a reference.
COMPONENT MODE SYNTHESIS
|
285
Figure 2-23: The automatically generated CMS study.
If the global model is to be used in a frequency domain analysis, use a
Frequency Domain study step as a reference during model reduction. If not,
use a Time Dependent study step. Both steps are added by the Configure CMS
study (
) action, and can be enabled or disabled depending on the use
case. By default, the Time Dependent study step is enabled.
Key to the CMS study is that all study steps are solved on a subset of the total model;
the selection of the component. This is controlled in the Compile Equations nodes of
the solver sequence. When using an auto-generated CMS study, the selections used are
automatically updated during the sweep over components.
Running a CMS study creates a number of datasets in the Results branch as well as
subnodes to the Reduced-Order Modeling node under Global Definitions.
• The Reduced Model Data datasets contains the solution that is used to create a ROM,
including the constraint modes and eigenmodes. It also contains the matrices of the
ROM, which can be inspected by using the System Matrix derived values node.
• Depending on the chosen reference study step during model reduction, Frequency
Domain, Modal Reduced-Order Model or Time Dependent, Modal Reduced-Order Model
nodes are created under Global Definitions. When created from a CMS Study, these
are always created with a default label Reduced Component and names that are related
to the generating study and physics. Moreover, the CMS study generates ROMs
with a stateful interface, which is a requirement for it to connect to other parts of
the model. You can use Model Control Inputs and other settings in the generated
ROMs to modify their behavior when used in a global analysis.
Once the ROMs have been created, you can in principle delete the CMS
study to clean up the model tree. In fact, you only need to keep the
Reduced Flexible Components node and the generated ROMs under Global
Definitions.
286 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Neither the names, nor the order of the list of ROMs in the Reduced-Order
Modeling node under Global Definitions should be changed, as this will
break the connection between the ROMs, the physics, and the reduced
component. The automatic naming convention has the structure <rom>
_n_<feat>_<phys>_<i>, where <rom> is a generic tag for the generating
ROM, <feat> is the tag of the Reduced Flexible Components node that
generated the CMS study, <phys> is the physics tag, and <i> is a number.
For example, the ROM of the first component in a Solid Mechanics
interface is typically named rom1_n_rfc1_solid_1.
SETTING UP THE GLOBAL MODEL
Using ROMs created from a Reduced Flexible Components node and a CMS Study in a
global model, in general, requires no further steps to be taken. The only requirement
is that the states of the ROMs are solved together with the other dependent variables
of the model. By default, the Solve for status of these ROMs are synchronized with the
Solve for status of the generating physics in non-CMS studies, which takes care of this
requirement.
If all the domains of the physics interface are reduced, it is possible to turn
off the synchronization of the Solve for status, since in such cases it is only
necessary to solve for the states of the ROMs. By not solving for the
dependent variables of the physics, it is made sure that no double
contributions are added by, for example, load features. Clear the
Synchronize ‘Solve for’ study setting for Reduced Components check box in
the Reduced Flexible Components node to make this possible.
One way to add more control over the behavior of a ROM is to add control inputs in
Global Reduced Model Inputs under Global Definitions. These should be added to the
model before solving the CMS study, and can be used in expressions in relevant physics
nodes. After running the CMS study, you can modify the input expression for each
COMPONENT MODE SYNTHESIS
|
287
added control input, either globally or individually in each of the generated Reduced
Component nodes.
If you include a load in a reduced component, and enter a value or a
parameter for its amplitude, then that load will have a constant value when
the component is reused. If you want to be able to, for example, make that
load time dependent, or to switch it off, then you define it using a control
input.
For a more detailed discussion on how to work with ROM control inputs
and their limitations, see Reduced-Order Model Inputs in the COMSOL
Multiphysics Reference Manual.
IMPORTANT CONSIDERATIONS
A number of important considerations to be aware of when working with CMS and
reduced components are listed below:
• Do not modify the content of automatically generated nodes in the model tree, such
as the CMS Parameters node, and the CMS Component selection.
• Only zero-valued constraints can be applied to a reduced component. While it is
fundamentally possible to apply constraints on a reduced component in a global
analysis, the correct way is to apply them when generating the ROMs in a CMS
study so that such constraints can be accounted for while computing constraint
modes and eigenmodes. Later, constraints can be removed in all other studies. This
is handled automatically for most such features including for example:
- Fixed Constraint
- Prescribed Displacement
- Roller
- Symmetry
No constraint equations are added for these features on selections that intersect that
of a Reduced Flexible Components node. For the Prescribed Displacement node and
similar features, any nonzero values set for the constraint are, moreover, ignored in
the CMS study.
• Attachment nodes can be used without a connection to other parts of the model to
define additional static modes of the reduced component. Note that attachments by
default induce a rigid boundary on its selection.
288 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
• Added Mass, Spring Foundation, and Thin Elastic Layer are special features that add
either mass or stiffness to the reduced component, and can therefore be considered
as part of its basic properties. By default, these are enabled in the CMS Study when
) button. No mass nor stiffness is added in a
using the Configure CMS study (
global study on selections intersecting with that of a Reduced Flexible Components
node.
• When working with CMS, the following subnodes to Linear Elastic Material and
Section Stiffness are supported when creating reduced components:
- Thermal Expansion
- Hygroscopic Swelling
- Initial Stress and Strain
- External Stress
- External Strain
- Damping
- Fiber
All other subnodes are, by default, disabled in the CMS Study when using the
Configure CMS study (
) button. Some options in the supported features may,
however, not be supported. For example, the External material option in External
Strain is not supported with CMS.
• In the Damping subnode to Linear Elastic Material or Section Stiffness, the following
Damping types are supported:
- Isotropic loss factor
- Anisotropic loss factor
- Loss factor
- Rayleigh damping
- Viscous damping
- Wave attenuation
When using the Configure CMS study (
) button, the Damping subnode is disabled
in the training steps to avoid complex eigenpairs, but active in the reference step to
the model reduction. Any contributions are removed on selections that intersects
with that of a Reduced Flexible Components node in a global study.
• Damping can also be added to reduced components by Spring Foundation, Thin
Elastic Layer, and Low-Reflecting Boundary nodes. For these features, damping
contributions are only added on selections intersecting with that of a Reduced
COMPONENT MODE SYNTHESIS
|
289
Flexible Components node in the reference step to the model reduction. No
contributions are added in the training steps for such selections to avoid complex
eigenpairs.
• Reduced components are by definition linear. Do not use any features that are
nonlinear such as Creep, Damage, or Plasticity on the same selection as a Reduced
Flexible Components node. Also, make sure not to induce nonlinearity by user
defined expressions in features that are to be reduced. This also applies to boundary,
edge, and point features adjacent to the domains selected in a Reduced Flexible
Components node.
• It is not possible to compute dissipated energy due to for example damping on
selections that intersect that of a Reduced Flexible Components node. The Calculate
dissipated energy setting is ignored for such selections.
• Certain features that add weak contributions on domain, boundary, edge, or point
level should be used with care if their selections intersect that of a Reduced Flexible
Components node. To get consistent results and avoid double contributions, it may
be necessary to manually disable some features in the model tree of the training
study step of a generated CMS study, or in the global study that uses a ROM.
Examples of such features, other than loads, include Weak Contribution. By default,
these are disabled in the CMS Study when using the Configure CMS study (
) button.
• Most features that add global dependent variables are not applicable together with
reduced components. The reason is that it is difficult to automatically determine to
which part of the model such variables belong. Hence, do not use features such as
Average Rotation, Rigid Body Contact, Rigid Connector, Prescribed Velocity, or Point
Load, Free when setting up reduced components. By default, all such features are
disabled in the CMS Study when using the Configure CMS study (
) button. The only
exception is the Attachment feature which is specially designed to work with reduced
components.
• Features and functionality that add dependent variables which are expected to have
a significantly different order of magnitude compared to the displacements should
be used with caution when creating reduced components. The reason is that such
DOFs can corrupt the scaling of the eigenvectors used to train the ROM during
290 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
model reduction, which in the end will result in an inaccurate ROM. Examples of
functionality that may cause this are:
- The Pressure mixed formulation in Linear Elastic Material
- The Flexible connection type in Attachment nodes
- The Lagrange multipliers added by weak constraints
If such functionality must be used, you can try to manually adjust the scaling of the
eigenvectors by changing the Maximum absolute value in the Eigenvalue Solver of the
CMS Study. Another alternative is the try setting Scaling of eigenvectors to Mass Matrix.
• Translating or rotating a ROM is not supported. Hence you cannot use a single
ROM to represent multiple reduced components.
• Import of ROMs created in another COMSOL Multiphysics model or any external
software is not supported for reduced components.
COMPONENT MODE SYNTHESIS
|
291
Computing Mass Properties
In structural mechanics analysis, especially when modeling dynamic problems, the
mass properties of a structure or its part can be an important aspect of the design. To
compute such mass properties, you can use Mass Properties node, which can be added
under Component>Definitions>Physics Utilities. There, you can select the geometry
domains to be included into the computations and select physics interfaces that will
define the mass properties. You can add and configure several mass property
contributions if needed.
292 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Volume, mass, center of mass, and moments of inertia will be computed. They will
become available as predefined variables, which you find in the Equation View node’s
settings window under the corresponding Mass Properties node.
Besides for postprocessing purposes, you can also use these variables in any
user-defined expressions, user inputs, and in optimization criteria.
Structural mechanics interfaces contribute to the mass properties in several ways:
• All material models, including Rigid Material, define mass density contributions.
• Added Mass nodes for all geometric entity levels can also contribute with added mass
density. It is possible to suppress the contribution from an Added Mass node by using
the Exclude contribution check box in the Frame Acceleration Forces section.
• Point Mass nodes contribute both with mass and with the specified mass moment of
inertia. It is possible to suppress the contribution from a Point Mass node by using
the Exclude contribution check box in the Frame Acceleration Forces section.
• The Hygroscopic Swelling nodes, which can be added to most material models for all
structural elements, can use the moisture content as an extra mass density
contribution.
COMPUTING MASS PROPERTIES
|
293
• Rigid Material and Rigid Connector can contribute directly to the total mass properties
via their Mass and Moment of Inertia subnodes.
• Structural elements like beams and shells take their true geometrical dimensions into
account when contributing to the mass properties. As an example, a beam
contributes to the rotational inertia around its axis, even though the geometrical
model is only an edge. The beam cross-section properties are used to compute the
data.
The mass properties can be computed on both initial geometry (material frame) and
deformed geometry (spatial frame). The results may differ considerably in case of large
deformations. To compute the results in the undeformed geometry, you do not have
to perform the whole analysis; it is sufficient to choose Get Initial Values under the Study
node. To obtain the mass properties in the deformed configuration, you need to the
full analysis, so that the displacement results are available.
In the COMSOL Multiphysics Reference Manual:
• Mass Properties
• Studies and Solvers
• Derived Values, Evaluation Groups, and Tables
294 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Effective Properties of Periodic
Structures
Sometimes you need to model on different scales. The heterogeneous properties of a
material in the microscopic scale are often unfeasible to use directly on a macroscopic
scale, in which a structure is typically analyzed. In such a case, you typically want to use
a homogeneous material model with appropriately averaged properties.
The Cell Periodicity feature facilitates the evaluation of such average properties. It is
based on the idea of a representative volume element (RVE). The RVE is a domain
that is representative for the material on a microscopic scale.
If the material is truly periodic, an RVE is typically identified as the smallest possible
unit cell. If the material has a random distribution of, for example, porosities, the RVE
should be large enough to be representative for the average properties of the material
on a macroscopic scale.
The only requirement on the shape of the RVE is that it should be possible to fill space
with a repetitive pattern of RVEs. This means that there are a set of matching boundary
pairs, each pair having the same geometry, but offset by a given distance.
Material Homogenization Using the Cell Periodicity Node
To model a periodic unit cell or a RVE (representative volume element), you add the
domain feature Cell Periodicity, and select the domains representing the cell. For each
pair of matching boundaries, add a Boundary Pair subnode, and select the
corresponding boundaries, typically on the opposite sides of the cell.
In principle, there is no limitation on the physics features you can use for modeling the
cell, as long as the basic assumptions about periodicity and homogeneity are valid. You
should, however, not add any displacement constraints since the possible rigid-body
motions are automatically constrained by the Cell Periodicity node.
MESHING
For periodic boundary conditions, the accuracy of the analysis is significantly better if
each pair of matching boundaries has the same mesh. This can be accomplished for
example using the Identical Mesh feature in the mesh sequence.
EFFECTIVE PROPERTIES OF PERIODIC STRUCTURES
|
295
When using nonmatching boundary meshes, the stress disturbances can be reduced by
using a weak constraint.
HOMOGENIZED MATERIAL PROPERTIES
Two different types of material properties can be automatically evaluated using the Cell
Periodicity node. With the Free Expansion periodic condition, you can calculate the
homogenized material properties related to the free expansion of the RVE when
exposed to a variation in temperature or moisture concentration — that is, the
averaged coefficient of thermal expansion and the averaged coefficient of hygroscopic
swelling. To set up an analysis for the evaluation of thermal properties, add a Thermal
Expansion subnode to each material model used in the RVE, and apply a one degree
increment in temperature. Similarly, for hygroscopic properties, add Hygroscopic
Swelling subnodes and apply a unit increment in concentration. Without adding these
subnodes to the material models of the RVE, no expansion is applied to the unit cell,
and consequently the results will be zero. The results will also be zero if no variation
in temperature or concentration is applied. If requested, the computed material
properties are by default presented in a separate evaluation group under Results.
With the Average strain or Average stress periodic conditions, you can calculate the
homogenized elastic properties of the RVE. Use Average strain to compute the
elasticity matrix, or Average stress to compute the compliance matrix. In order to
compute these properties, the deformation of the RVE needs to be evaluated for a
number of fundamental load cases. These correspond to the perturbations of the unit
cell with each component of the average strain or stress tensor, while keeping the other
components equal to zero. Setting up this analysis can be automated with the Create
Load Groups and Study option under the Study and Material Generation button. It creates
a load group for each tensor component, populates the average strain or stress tensor,
and creates a study with a load case for each load group. When the calculation of an
average material property is requested, the computed values are by default presented
in a separate evaluation group under Results. If no material property evaluation is
requested, or if it is not available, the results can be used to study the response of the
RVE to the applied load cases.
You can also create a global material using the Create Material option under the Study
and Material Generation button. This is available for the Average strain or Average stress
periodic conditions. This option creates a material that contains the homogenized
elasticity or compliance matrix, which can be accessed by other components in the
model. Note that if you want to use the computed material properties in another
model or store them in a user-defined material library, use the Create Material by Value
296 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
option. For the Create Material by Reference option, the automatically generated global
material contains variables linked to the Cell Periodicity node in the current model.
Micromechanical Model of a Fiber Composite: Application Library path
Structural_Mechanics_Module/Material_Models/
micromechanical_model_of_a_fiber_composite
EFFECTIVE PROPERTIES OF PERIODIC STRUCTURES
|
297
Modeling Pretensioned Bolts
The information about pretensioned bolts is applicable if your license
includes the Structural Mechanics Module.
Bolted joints are common in mechanical and civil engineering structures. If you are
interested in analyzing the details of a bolted joint, the prestress in the bolt must be
taken into account in order to correctly capture the behavior under service loads. The
Bolt Pretension functionality in COMSOL Multiphysics is designed to simplify such
analyses. You can model the bolts either using solid or beam elements.
During mounting, a bolt is tightened to a certain prestress. The mounting of the bolt
is, in general, accompanied by deformations of the surrounding structure. In the
subsequent service, the force in the bolt can then change due to external loads.
Sometimes the sequence in which the bolts are tightened is important. This will be the
case if significant nonlinearities are induced by the tightening process. Modeling such
a process is also fairly straightforward. This is, however, a less common case which adds
some extra complexity to the modeling, so it will be discussed separately below.
MODELING THE BOLTS
You must use a specific modeling technique in order to use a bolt in a prestress analysis.
Using Solid Elements
1 You can model bolts using solid elements in 3D or 2D axial symmetry. In 3D, it is
usually most efficient to add the predefined bolt geometries from the Part Libraries.
In 2D axial symmetry, the bolt is always assumed to be axially symmetric, and thus
having the Z-axis as its center of rotation.
2 Make sure that there is at least one interior boundary perpendicular to the bolt axis
somewhere in the shank. In the following, this boundary is referred to as the slit
boundary (Figure 2-24). The slit boundary can be composed of several adjacent
boundaries in the geometry.
3 If you are using bolts from the Part Libraries, a slit boundary is predefined, and has
the selection name Pretension cut. In order to make this boundary selection
visible from the physics interface, select its Keep check box in the Boundary Selections
section of the settings for the part instance (Figure 2-25).
4 If needed, add contact conditions between the bolt head and the component and
between different components clamped by the bolt. In many cases, it is sufficient
298 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
and more efficient to use a continuity condition between the bolt head and the
component.
5 Add a Bolt Pretension node, in which the pretension force or stress is prescribed for
a set of bolts sharing the same data.
6 For each bolt having the same essential data, add a Bolt Selection subnode where its
slit boundary is selected.
7 The label of the bolt, which is an input in the Bolt Label section, is used to identify
the bolts during result evaluation. A suggestion for the name is automatically
generated, based on the base name given in the parent node.
When a bolt is located in a symmetry plane (so that only half the bolt is
modeled), and Automatic symmetry detection is selected in the Bolt
Selection node, the given pretension force is interpreted as the force in the
whole bolt, and not as the force in the half-present bolt. This makes it
possible to use the same Bolt Pretension node for a set of similar bolts
where some of them are located in symmetry planes.
Figure 2-24: Example of a bolted joint with the bolt modeled as a solid.
MODELING PRETENSIONED BOLTS
|
299
Figure 2-25: Getting access to the slit boundary selection for a bolt from the Part Libraries.
Using Beam Elements
1 When modeling with beam elements, you will typically use a Polygon with three
points to model each bolt (Figure 2-26).
2 There must be at least one interior point somewhere in the shank. In the following,
this point will, in analogy with the solid, be referred to as the slit boundary.
300 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
3 Since there is no explicit bolt head when you model a bolt using beams, you need
to connect it to the solid component using some type of abstract coupling. There
are several options:
- You can connect the end of the beam to the edge of the bolt hole (the lower end
in Figure 2-26). Then, use the Solid–Beam Connection multiphysics coupling,
with Connection type set to Solid Edges to Beam Points. In this case, you select the
edge of the bolt hole.
- You can create a circular boundary having the diameter of the bolt head on the
surface of the component (the upper end in Figure 2-26). Then, use the Solid–
Beam Connection multiphysics coupling, with Connection type set to Solid
Boundaries to Beam Points. In this case, you select the annular solid boundary.
- Even without creating an extra boundary, you can use the Solid–Beam
Connection multiphysics coupling, with Connection type set to Solid Boundaries to
Beam Points, general. Then set Connected region to Distance (manual) and enter half
the head diameter as Connection radius. In this case, you select the entire
boundary on which the bolt head is residing. This method is convenient, but will
often give more spurious stresses around the bolt hole, since partial element faces
will be connected.
- You can use the two first approaches, but rather than using a multiphysics
coupling for the connection, you can add rigid connectors in both physics
interfaces, and then connect them. This approach is more expensive, since it adds
degrees of freedom in both the rigid connectors, plus the constraints to couple
them. It is however an approach that may be suitable for imported meshes, where
connection data in this form is available.
All these techniques are shown in the Structural Mechanics Module Application
Library example Modeling of Pretensioned Bolts.
4 Add a Bolt Pretension node, in which the pretension force or stress is prescribed for
a set of bolts with the same data.
5 For each bolt having the same essential data, add a Bolt Selection subnode where its
slit boundary is selected.
MODELING PRETENSIONED BOLTS
|
301
6 The label of the bolt, which is an input in the Bolt Label section, is used to identify
the bolts during result evaluation. A suggestion for the name is automatically
generated, based on the base name given in the parent node.
Figure 2-26: A bolt modeled using the Beam interface.
THE PREDEFORMATION DEGREE OF FREEDOM
Each bolt defined in the Bolt Selection node has a single global degree of freedom called
predeformation, d. At the slit boundary, the two sides of the bolt are disconnected so
that the displacements over it can be discontinuous. The discontinuity is represented
by:
u u = u d –  d – r n
Here the subscript u denotes the upside of the slit boundary, and d denotes the
downside. n is the normal pointing out from the downside. The sign has been selected
so that d gets a positive value when the bolt force is tensile. An optional relaxation r
can also be included.
The axial force in the bolt is thus caused by a small overlap between the two sides of
the slit boundary. It is computed as the reaction force belonging to the degree of
freedom d.
302 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
It is only meaningful to introduce the relaxation in a later study step. If it is present all
the time, then its only effect would be to increase the predeformation during the
pretension analysis by r. Thus, the value of r is usually a function of the load history,
which is initially zero.
SETTING UP THE STUDY STEPS
In an analysis of prestressed bolts, you have to use two or more separate study steps.
They can be part of a single study or be placed in different studies. The first study step,
in which the bolt prestress is prescribed, simulates the mounting process. If you would
only use a force to load the bolt (for example, as an initial stress), the resulting stress
in the bolt would be less than the intended, due to the compression of the material
around the bolt. The prestress step ensures that the bolts have the intended prestress,
irrespective of the flexibility of the surrounding structure and their interaction.
In the subsequent studies, the bolt force is allowed to change, while keeping the
extension of the bolt, as caused by the first study, fixed. The procedure to do this is as
follows:
1 Run the study step for the mounting simulation. The predefined study type Bolt
Pretension is designed for this. You may need to apply the pretension load in smaller
steps, if there are nonlinearities in the system. Then, you select Auxiliary sweep in the
Study Extensions section in the settings for the Bolt Pretension study step. Introduce
a load ramping parameter, which is used to multiply the pretension forces.
2 Add one or more studies or study steps to analyze the effects of the service loads.
3 Since the pretension degrees of freedom are not solved for in the service load study
steps, they must obtain their values from the pretension study step. If the study steps
are sequential within the same study, no special action is needed, since the default
then is to inherit values from the previous study step. For other cases, go to the
Values of Dependent Variables section of the study step, set Values of variables not
solved for to User controlled, and then select the pretension study step.
SEQUENTIAL TIGHTENING
If you need to take the order of the bolt tightening into account, then you must use
an auxiliary sweep where the sweep parameter is used to control the tightening history.
You need to perform the following steps:
1 In each Bolt Selection node representing a bolt that is not fully pretensioned from
the beginning of the study step, select the Sequential tightening check box.
MODELING PRETENSIONED BOLTS
|
303
2 A new text field, Pretensioning expression, is now shown. In this text field, you enter
a Boolean expression, which evaluates to a nonzero value at the parameter values
when the prestress is applied. It may happen more than once, if the bolt is not given
its full pretension force at once. An example of such an expression is
round(par)==3 || round(par)==11.
3 If you want the bolt prestress (when applied) to have a value that differs from the
value given in the parent Bolt Pretension node, change the setting of Pretension type
from From parent to another option. Extending the example above, the expression
for the pretension force could be 50[kN]*if(par>3.5, 1, 0.6). The only thing
that matters here is the value of the force at the parameter values when the
pretension force is set, in this example 3 and 11.
A sequential tightening precess may have a quite slow convergence rate until a certain
number of bolts have been loaded. The reason is that it is common that two mating
boundaries barely touch, so that many contact iterations are needed. It is advisable to
304 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
start by giving all bolts a small prestress, maybe 1% of the final value, in order to
stabilize the model.
It is important to make sure that you only solve for the bolt
predeformation degrees of freedom in the pretension study step, and not
when analyzing the service loads.
If you use the Bolt Pretension study type for the pretension study step, and
any other study type to analyze the service loads, the solvers are
automatically set up to handle this. The Bolt Pretension study type is
actually a special case of a Stationary study step, with the sole purpose of
activating the predeformation degrees of freedom. These degrees of
freedom are by default not solved for in any other study type.
If you, however, set up your studies manually, the information below is
useful. Also, in versions prior to 5.3, this automatic mechanism was not
available, so in older models the studies were always set up manually.
You enable or disable the solution of individual degrees of freedom under
the Dependent Variables node for a certain study step in the solver
sequence. If required, begin by clicking Show Default Solver in the study
node or in the Solver Configurations node of the study. Then move to the
Dependent Variables node, and in the General section, set Defined by study
step to User defined.
You can now go to the node for each predeformation degree of freedom
below Dependent Variables and adjust the state of the Solve for this state
check box.
For more information, see also Dependent Variables and Studies and
Solvers in the COMSOL Multiphysics Reference Manual.
RESULTS
The results in a bolt do not belong to any part of the geometry, but are global
variables. To access the result from a certain bolt, a full scope of the type <interface>
.<Bolt Pretension tag>.<Bolt Selection tag>.<variable> must be used. An
MODELING PRETENSIONED BOLTS
|
305
example could be solid.pblt1.sblt1.F_bolt. The bolt results are summarized in
the table below.
TABLE 2-15: BOLT VARIABLES.
VARIABLE
DESCRIPTION
d_pre
Predeformation
F_bolt
Axial force in the bolt
F_shear
Shear force in the bolt (3D only)
If you place a bolt in a symmetry plane, that only half of the bolt is modeled, this will
automatically be detected. The results are reported for the whole bolt, not for the
symmetric half.
When there are pretensioned bolts in a study, evaluation groups containing the bolt
forces will automatically be generated.
Studies and Solvers in the COMSOL Multiphysics Reference Manual
• Modeling of Pretensioned Bolts: Application Library path
Structural_Mechanics_Module/Tutorials/bolt_pretension_tutorial
• Prestressed Bolts in a Tube Connection: Application Library path
Structural_Mechanics_Module/Contact_and_Friction/tube_connection
306 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Simplified Modeling of Bolt Threads
When an internal and an external thread are engaging, there will be a complex local
stress state. When analyzing such geometries, you can approach the problem at three
levels:
• Make a full 3D model of the actual thread geometry and solve the contact problem.
This approach is only used in some rare cases, since such a model by necessity
becomes very large. Also, the actual stress state in the thread itself is seldom the
target of an analysis.
• Ignore the thread completely and just connect the two parts by a union operation
or through a Continuity pair. This approach will provide an accurate solution outside
a region with a size of a couple of bolt diameters from the bolt hole.
• Use the simplified Bolt Thread Contact condition. With this approach, the stresses
will be correct, except at distances where stress concentrations caused by the actual
thread geometry are significant. The important part of the solution that can be
captured by this simplified contact condition is that the contact pressure between
the threads will push the walls of the bolt hole outward. This will cause significant
tensile hoop stresses around the bolt hole.
When you use Bolt Thread Contact, you model the face of both the bolt and the bolt
hole as cylinders. The actual geometry of the thread is taken care of by the
mathematical formulation of the contact condition. The most important parameter is
the thread angle, since it determines the direction of the contact forces.
For each individual bolt, you need to add one Bolt Thread Contact node.
PENALTY FACTOR
The contact condition is enforced using a penalty formulation. In practice, this means
that a stiff spring is inserted between the two boundaries. In most contact problems,
you want to use a high penalty factor, in order to avoid excessive overclosure of the
contacting boundaries. In this case, however, there is a certain flexibility which has its
source in a slight bending of the threads in real life. This effect can to some extent be
accounted for by allowing a certain flexibility in the contact condition. For this reason,
the default penalty factor is rather low. You may need to adjust it to suit your
conditions.
A higher penalty factor also means that the force is transferred from the external thread
to the internal thread over a shorter distance along the bolt axis.
SIMPLIFIED MODELING OF BOLT THREADS
|
307
CONTACT ORIENTATION
In most cases, you know a priori which side of the thread that will be in contact. You
can reduce the size of the contact problem by a factor of two by selecting an
appropriate value for the Contact orientation. The default is to search in both
directions.
If a bolt is pretensioned, the contact orientation will be Up if the bolt orientation is such
that the Orientation vector points toward the bolt head. If the bolt geometry, including
orientation, is computed using the Automatic option, you will often have to use the
Direction adjustment option to have full control over the up and down directions.
MODELING HINTS
• You must create one Contact Pair for each bolt and mating bolt hole. The bolt
should be the destination side of the contact pair.
• In the Part Libraries, you will find predefined parameterized bolt geometries that
also contain a domain intended to be used as drill for the bolt hole.
• The cylindrical surfaces of the bolt and bolt hole should have the same diameter. If
you want to decrease the stiffness of the bolt because it is not solid all the way out
to the nominal diameter, a good suggestion is to decrease Young’s modulus by a
factor based on the stress area of the bolt.
• Since the contacting boundaries are cylindrical, there is a risk that the bolt, instead
of computing the gap to the nearest point on the bolt hole, will instead see a point
on the opposite side. A good practice is to select Manual from the Search distance list
in the settings for the Contact Pair. Half the diameter of the bolt is an appropriate
search distance.
• Since the relative displacements between the bolt and the hole are small, setting
Mapping method to Initial Configuration in the settings for the Contact Pair can
improve efficiency.
• In the initial state, the two objects being joined may possess rigid body modes, just
like in any other contact problem. If so, you can for example add weak springs to
maintain stability.
308 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Modeling Embedded Structures and
Reinforcements
Lower dimension structural elements such as trusses, beams, and membranes can be
embedded into a solid domain by adding an Embedded Reinforcement multiphysics
coupling. This modeling technique is intended for efficient modeling of thin structures
in solids, where it is unfeasible or not necessary to resolve the geometry of the thin
structure. Some typical use cases include:
• Reinforcement bars in concrete structures
• Piles or sheets in soil
• Fibers in composite materials
• Embedded sensors in a structure. Embedding sensors can either be used to model
a real sensor, or as a modeling technique to extract, for example strain in some
predefined location and direction in a solid domain.
The connection between the embedded structure and the solid can be set up using
different techniques; either a rigid connection by adding constraints between the
points in the respective interface, or by adding springs. When a spring type connection
is used, the connection can be linear or nonlinear. Using a nonlinear connection can
be important when modeling reinforcement in structures, especially when predicting
failure and postfailure behavior.
The multiphysics coupling is intended for situations where the volume of the
embedded structure is small compared to the solid domain. Hence, no compensation
is made for the mass of the small structure. If a detailed model of the connection and
composite structure is required, the geometry should include the interface between
the embedded structure and the solid. The connection should then be modeled using
MODELING EMBEDDED STRUCTURES AND REINFORCEMENTS
|
309
some other coupling technique as discussed in Coupling Different Element Types, or
using Contact Modeling.
When the Embedded structure is a Beam interface and a Rigid connection
type is used, the displacements are only constrained to the solid domain
at the mesh nodes of the beam elements. This means that higher-order
variations of the displacement field between mesh nodes is allowed. The
Spring connection will, however, constrain also the higher-order variations
of the displacement field.
The functionality provided by the Embedded Reinforcement multiphysics
coupling to some extent overlaps with other couplings available to
different structural mechanics interfaces. For example, both the Embedded
Reinforcement and the Solid–Thin Structure Connection can be used to
attach a membrane as a cladding on a solid domain. An important
difference is, however, that the Solid–Thin Structure Connection will add
constraints on the solid domain, while the Embedded Reinforcement will
add constraints on the membrane. Depending on the mesh, the results
may differ significantly.
The same difference applies when comparing the Embedded Reinforcement
to a Solid–Beam Connection on shared edges.
GEOMETRY AND MESHING
When modeling embedded structures, it is sometimes easier to form the geometries of
the coupled interfaces from an assembly. In the finalization step of the geometry
sequence, you should select Form an assembly in the Action list. This will also put less
restrictions on the mesh of the respective geometry. If Form Union is selected in the
Action list, the same mesh will be shared by both interfaces; which has to respect and
resolve the geometry of the embedded structure.
While there is no strict restriction on the mesh size when modeling embedded
structures in an assembly; a good practice is that the mesh used for the two coupled
interfaces is of approximately the same size, or that the mesh of the embedded
structure is slightly finer. Use the same shape order in both interfaces when modeling
embedded structures that share the geometry and mesh with the solid domain, that is,
when Form Union is selected in the Action list.
310 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
In some situations, the connection can be sensitive to mesh elements of the embedded
structure that are partially within the solid domain. This is especially sensitive for the
penalty connection, where the weak equations are evaluated at the integration points
of the embedded mesh element. A slight shift in the mesh can cause an integration
point to either be inside or outside the solid domain.
PENALTY FACTORS
When using the spring type connection, the accuracy of the connection is controlled
by the spring stiffness matrix. The components of this matrix are most naturally
represented in the local coordinate system of the embedded structure, for which only
the diagonal components are of interest. Mathematically, the spring stiffness can be
viewed as penalty factors that must be sufficiently high to accurately enforce the
regularized constraint, but if they are too high the overall stiffness matrix will be
ill-conditioned. This means that in most cases, the spring stiffness in only a numerical
parameter. However, there can be situations where the interface between the
embedded structure and the solid domain has a measurable stiffness, for example, if
the connection is used to idealize an interface with a finite, but small, thickness such
as a glue layer. In such cases the spring stiffness will have a real physical interpretation.
The default expression for the spring stiffness of the connection is derived from the
stiffness and cross-sectional properties of the mesh element of the embedded structure.
The available spring connection types and the corresponding default expressions for
the spring stiffness are summarized in Table 2-16. All spring stiffness components have
the same default expressions.
TABLE 2-16: DEFAULT EXPRESSION FOR SPRING STIFFNESS.
CONNECTION
TYPE
SPRING CONSTANT PER UNIT LENGTH
SPRING CONSTANT PER UNIT
SURFACE AREA
Truss
1e3*truss.Eequ*
truss.area/h^2
1e3*truss.Eequ*
truss.perimeter/h^2
Wire
1e3*wire.Eequ*beam.area/h^2
1e3*wire.Eequ*
wire.perimeter/h^2
Beam
1e3*beam.Eequ*beam.area/h^2
N/A
Membrane
N/A
1e5*mbrn.Eequ*
mbrn.d/h^2
LOCAL ORIENTATIONS
Many quantities used by the connection, such as the spring stiffness and constitutive
models, are most naturally represented in the local coordinate system of the embedded
structure. For beam and membranes, the multiphysics coupling picks up the local
MODELING EMBEDDED STRUCTURES AND REINFORCEMENTS
|
311
coordinate system defined by the physics interface. However in the Truss or Wire
interfaces, only the direction of the local edge tangent tle is defined. For the
multiphysics coupling, two transverse direction are also needed when using a spring
connection. Thus, the multiphysics coupling defines a local coordinate system by
assuming that tle is the normal to a plane. The actual directions of the two in-plane
tangents are not important, and it is assumed that the first tangent points in the global
z direction. Hence, the first transverse direction is
e z –  t le  e z t le
t 1 = --------------------------------------------e z –  t le  e z t le
and the second transverse direction is
t le  e z
t 2 = t le  t 1 = --------------------------------------------e z –  t le  e z t le
where ez is the base vector that points in the global z direction. Since no distinction is
made between t1 and t2, only a single transverse spring constant, kt, has to be entered
when defining the spring stiffness matrix.
BOND SLIP MODELS
It is possible to include a bond slip model of the interface when modeling the
embedded structure connection with a nonlinear spring. This nonlinear behavior
follows a plasticity model, where the relative displacement between the two coupled
interfaces is additively decomposed into an elastic displacement and a plastic
displacement, or slip. Modeling bond slip is limited to small sliding only, since the
mapping between the embedded structure and the solid domain is made in the
reference configuration.
The slip is defined using a local constitutive model. This local model adds a set of
internal degrees-of-freedom that are solved for and stored in the model at each Gauss
point of the embedded structure. Typically, these internal variables include the relevant
components of the slip vector ul,p, the accumulated slip upe, and the friction
dissipation density Wp. The last variable is only added if the Calculate dissipated energy
check box is selected in the Energy Dissipation section. The internal variables used by
the Embedded Reinforcement multiphysics coupling are shown as separate fields under
Dependent Variables node in the solver sequence.
The resistance to slide in the bond slip model is determined by the cohesion c, which
can be a function of any variable or field present in the model; by adding a generic
312 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
expression to the initial cohesion c0. A built-in hardening model with respect to upe
can be also be added, in which case c = c0+ch, where ch describes some hardening
function.
In many applications the bond slip behavior of the interface is described by a Coulomb
type friction. However, the bond slip model by default has no dependence on the
normal force acting on the interface since the connection has no formal direction of
the normal of the interface. A Coulomb type friction model can still be considered if a
good estimate of the normal force can be found by adding such a dependence to c0.
If, for example, the pressure in the solid domain can be considered as the normal
pressure acting on the interface, use an expression like 0.1*<tag>
.ExtCplOp(solid.p) to define c0 with a friction coefficient equal to 0.1. Here <tag>
is the tag of the multiphysics coupling and <tag>.ExtCplOp(expr) is the operator
that maps the expression from the solid domain to the embedded structure.
SOLVER SETTINGS
When adjusting the settings of the solver sequence for a model that includes an
Embedded Reinforcement multiphysics coupling, make sure that the dependent variables
of the coupled interfaces are solved in the same group. Also, note that the fields related
to the bond slip model should be included in the same solver group as well. This is only
a potential issue if a segregated solver is used, and it is handled automatically by the
default solver suggestion.
MODELING EMBEDDED STRUCTURES AND REINFORCEMENTS
|
313
Modeling Thin Layers
Sometimes, there are thin layers between larger components that cannot be ignored in
a structural analysis. The reasons are either because they have significant flexibility or
damping properties, or that they may fail. Examples of such layers are glue layers,
O-rings, and gaskets. Other cases can involve transition zones between particles or
fibers and the binder in a composite material.
When the layer is thin compared to other dimensions of the structure, it is difficult to
produce a mesh with acceptable quality without compromising the numerical
conditioning of the stiffness matrix. The Thin Layer boundary feature allows to
overcome this problem by making simplifications, so that there is no need for a mesh
in the through-thickness direction.
There are three different approximations available for modeling thin layers:
• Solid
• Membrane
• Spring
These approximations differ in the simplifications made for obtaining the deformation
gradient in the thin layer. For more details see Thin Layers.
The Thin Layer Node
The Thin Layer node is used to identify boundaries that have a thin layer attached to
them. These boundaries may either be exterior or interior boundaries to the domain
where the physics interface is active. The Thin Layer node also determines the thickness
of the thin layer, and how to approximate the deformation gradient on it. The first
choice is whether to use a Layered or a Nonlayered thin structure.
In the majority of cases, the Nonlayered approximation is sufficient to capture the
behavior of the thin layer. For this type of layer, two sets of degrees of freedom (DOFs)
are introduced at the boundary; one set corresponds to the upside, and one set to the
downside as illustrated in Figure 2-27. In COMSOL Multiphysics, this is referred as a
slit of the displacement field on the thin layer boundary.
Note that in Figure 2-27 no extra integration points are introduced in the
through-thickness direction, and that numerical integration is made on the
midsurface. Hence, dependent variables always have a linear variation in the thickness
314 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
direction; that is, their gradients are constant in the through-thickness direction. This
also applies to inelastic quantities such as plastic strains.
Upside
Midsurface
Downside
Figure 2-27: Illustration of a nonlayered thin stratum between two mesh elements using
quadratic serendipity shape functions. Circles indicate nodal points and squares
integration points.
The Layered type can be used when a more detailed description of the
through-thickness behavior is needed. For this type of thin layer, a slit of the
displacement field is made on the boundary, and additional DOFs are introduced
between the upside and downside as illustrated in Figure 2-28. These extra DOFs
facilitate a more detailed through-thickness representation of stresses and strains, and
they make it possible to, for example, model composites and laminate strata.
Continuity is enforced by constraints between the DOFs on the up- and downside, and
the extra DOFs. The through-thickness discretization is controlled by the attached
material. For more details about modeling layered structures, see Composite Materials
Modeling
Upside
Midsurface
Downside
Figure 2-28: Illustration of a discretized layered thin layer using a single mesh element in
the through-thickness direction. The thin layer is injected between two mesh elements using
quadratic serendipity shape functions. Circles indicate nodal points and squares
integration points.
MODELING THIN LAYERS
|
315
When the Nonlayered type is used, it is possible to choose different approximations of
the deformation measure in the thin layer:
• Solid
• Membrane
• Spring
The description in Figure 2-27 is representative of the solid and spring
approximations. The solid approximation is the most general and accounts for the full
normal and tangential deformations in the thin layer. The spring approximation is
similar but neglects the membrane deformation. This is useful for cases where the
behavior of the thin layer is given by force versus extension data, as is often the case
when modeling gaskets.
For the membrane approximation, no slit is introduced and the thin layer only
accounts for the membrane deformation. It thus only contributes with tangential
stress, while plane stress conditions apply in the through-thickness direction. This is
typically the case when the thin layer describes a cladding on an exterior boundary or
a reinforcement layer on an interior boundary.
The different thin layer approximations are compared in Thin Layer
Interfaces: Application Library path
Nonlinear_Structural_Materials_Module/Hyperelasticity/thin_layer_interfaces
Interior and Exterior Boundaries
A Thin Layer can be applied to either exterior or interior boundaries of the physics
interface. However, there are some noticeable differences between adding a thin layer
on an exterior or on an interior boundary.
On an interior boundary, the selected boundary is always considered to be the
midsurface of the thin layer. It is not possible to apply any loads or boundary
conditions on interior boundaries.
On an exterior boundary, the bottom of the thin layer is attached to the adjacent
domain. This means that the thickness of the thin layer extends outward from the
domain in the direction of the normal. For a nonlayered thin structure, an exterior
displacement field is introduced to create the slit, so it is possible to apply loads and
boundary conditions to this exterior field. For example, applying a fixed constraint on
an exterior thin layer makes it equivalent to a Spring Foundation. For a layered thin
316 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
structure, the top side of the layered material is always the exterior. Loads and
boundary conditions can be applied to the top side only.
When the thin layer boundary is part of a contact pair, the thickness of the exterior thin
layer is considered when modeling contact.
Material Models
A Thin Layer can be assigned different material models:
• Linear Elastic Material
• Nonlinear Elastic Material
• Hyperelastic Material
• Spring Material
The first three material models are equivalent to the corresponding domain material,
hence the discussion in Introduction to Material Models is valid also for thin layers.
The Spring Material is a special material model only available with the spring
approximation. As the name implies, data for this material model is given in terms of
spring constants, or as force as a function of extension. It can be useful for certain types
of modeling where data is given in this format, for instance, when normal force versus
closure curves are available.
It is also possible incorporate inelastic effects by adding one or several subnodes to
these material models.
Loads and Boundary Conditions
Several loads and boundary conditions can be applied to a thin layer. Exactly what
boundary conditions are available and how they are treated depends on the thin layer
approximation. Whether the thin layer is an exterior or interior boundary of the physics
interface also affects the available boundary conditions.
On exterior boundaries, loads and boundary conditions can be applied to the exterior
displacement field of the nonlayered stratum, or on the top side of a layered material
for a layered stratum. For example, applying a fixed constraint to a thin layer on an
exterior boundary makes is equivalent to a Spring Foundation. It is also possible to
apply loads and boundary conditions to edges and points of the thin layer. For a
nonlayered stratum, loads and other boundary conditions apply to the exterior
MODELING THIN LAYERS
|
317
displacement field. However, for a layered stratum, all extra DOFs attached to the edge
or point are constrained.
When a Roller is applied on a boundary perpendicular to a thin layer, a
Roller should in most cases also be added to the edge of the thin layer. This
is especially important if the roller represents a symmetry condition.
On interior boundaries, only loads and boundary conditions on edges and points are
available. Moreover, these are only relevant for a layered stratum. For a nonlayered
stratum, there are no free DOFs on which to apply the boundary conditions.
Result Evaluation and Visualization
For a nonlayered thin structure, many variables defined by the material models have
the same name for both the thin layer and the adjacent domain. For example, the von
Mises stress is always called solid.mises. Hence, the context in which the variable is
evaluated is important.
If solid.mises is evaluated using a surface plot in a 3D model, it will have the
following interpretation:
• On boundaries with no thin layer, it will show the von Mises stress of the adjacent
domain.
• On boundaries that intersect a nonlayered thin layer, it will show the von Mises
stress on the thin layer.
Use the mean() and side() operators to force the evaluation of variables in adjacent
domains. For example, using mean(solid.mises) for a surface plot will average the
stresses from the two adjacent domains, and it will not consider the stress in the thin
layer between these two.
Extra care must be taken when evaluating results on entities of lower dimensions, such
as points, to make sure that the expression is evaluated in the correct context. The
mean() or side() operators can then be applied multiple times. For example, using
mean(mean(mean(solid.mises)))in a point plot for a 3D model will ensure that the
von Mises stress in the domain material is evaluated. Similarly, a point plot with the
expression mean(side(1,solid.mises)) will evaluate the von Mises stress in the
thin layer on boundary 1.
318 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
When one or more thin layers are present in a model, a default plot is
added to show the stress in the thin layer.
See Results Evaluation in Composite Materials Modeling for a discussion
on how to evaluate and visualize results for layered thin layer.
MODELING THIN LAYERS
|
319
Modeling Cracks
A crack in a solid model can be represented in two fundamentally different ways:
• As an ideal crack — that is, by a single boundary. Across this boundary, the
displacement field is discontinuous. Using COMSOL Multiphysics nomenclature,
this is called a slit condition.
• By the crack geometry, in which case the two sides of the crack are two different
boundaries. In the true geometry, the two crack surfaces may coincide, or there may
be a distance between them.
Both cases have an analogous representation in a symmetry plane. The ideal crack is
just a boundary located in the symmetry plane, but without the symmetry conditions,
so that it can open. This can, however, just as well be considered as special case of a
geometrical crack, so in symmetry planes the distinction more or less disappears.
Fundamental for cracks is that the stress and strain states at the crack tip are singular,
so any mesh refinement will only produce even higher stresses. For a linear elastic
material, the stresses and strains in the vicinity of the crack vary as 1  r , where r is
the distance from the crack tip.
The Crack Node
The Crack node serves several purposes:
• In the case of an ideal crack on an internal boundary, the degrees of freedom are
split so that the displacements on the two crack surfaces are independent.
• In the case that a crack is located in a symmetry plane, all constraints that may be
applied (such as symmetry) are removed. It is then possible for the crack to open.
• If possible, a crack growth direction is computed. For some cases this is instead a
user input.
• A number of variables, such as an estimate of the crack length are created.
• A mesh suggestion is generated.
• By using the J-Integral subnode under Crack, you can compute J-integrals and stress
intensity factors.
320 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
• By using the Virtual Crack Extension subnode under Crack, you can compute
energy release rates and stress intensity factors.
• By using the Crack Closure subnode under Crack, you can add contact conditions
between the crack faces.
The selected boundaries can form branched cracks.
MESH
At a crack tip, there will be an automatic mesh refinement. In the mesh sequence, you
will find an extra Size node, with all crack tips selected. You may want to adjust the
mesh size in that node.
J-integrals
The J-integral is a path independent integral that can be used to characterize the
severity of the stress state at the crack tip, both for linear and some nonlinear materials.
You can compute J-integrals by adding one or more J-integral subnodes under Crack.
Originally, the J-integral concept was derived for 2D, in which case it was sufficient to
integrate certain functions of stress and strain along an arbitrary curve from one
boundary of the crack to the other.
m

face
y
x
Figure 2-29: Example of a J-integral path.
MODELING CRACKS
|
321
There are some important assumptions when computing the J-integral:
• The curve is completely inside the domain.
• The curve does not enclose any other singularities, such as crack tips.
• No volume forces act inside the curve.
• No thermal stresses or similar inelastic strain contributions act inside the curve.
• If there is a load on the crack faces, this requires an extra correction. This is taken
into account if the load is given using the Face Load subnode under Crack.
In cases where the J-integral is not applicable, you can instead use the Virtual Crack
Extension Method method.
You can specify the integration path as a circle with a given radius, in which case it cuts
the mesh elements at arbitrary locations. In 2D, you can also select a sequence of
internal or external boundaries describing the path. It is recommended that you
evaluate more than one path to assess the accuracy of the solution.
The importance of this method is that stresses and strains far from the singular fields
at the crack tip are used for the evaluation.
J-integrals can be computed also in 3D, but there are some complications. In the 3D
case, the value of J will vary along the crack front. The local value is computed by a
similar path integral, which then must be placed in the plane perpendicular to the crack
front. This is automatically handled by the J-integral node. The J-integral in 3D should
be considered as a continuous function along the crack front.
In 3D, there is also a surface integral contribution which needs to be computed for the
area that is enclosed by the curve. Unfortunately, this causes the singular field to enter
the integration, a fact that reduces accuracy. In addition, the computational effort
increases significantly. Evaluations of J-integrals in 3D can take a noticeable time.
Another problem, that exists only in 3D, occurs if the crack front terminates at a free
boundary. If the crack front is not perfectly perpendicular to the free boundary, the
integration path will not entirely remain inside the solid domain. This is manifested as
spurious results close to the free boundary.
PREDEFINED PLOTS
When J-integral nodes are present, they will generate predefined plots. These plots
reside in a Cracks plot group. The contents of the plots differ significantly between 2D
and 3D, as described below.
322 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
2D
The integration paths are plotted as magenta curves. An arrow shows the crack growth
direction. At the crack tips, the value from the last J-integral node is printed. An
example is shown in Figure 2-30.
Figure 2-30: Predefined plot for a 2D case with a crack in a symmetry plane. Three
integration paths are shown; 2 circular and one along boundaries.
3D
In 3D, the integration paths are shown as transparent gray boundaries. The actual
integration paths are located where this boundary is intersected by planes
perpendicular to the crack front.
A colored arrow plot shows the crack growth direction, as well as the local value of the
J-integral as computed in the last J-integral node. An example is shown in Figure 2-31.
MODELING CRACKS
|
323
Figure 2-31: Predefined plot for a case with a 3D crack in a symmetry plane. One
integration path is used.
DEFAULT EVALUATION GROUPS
In both 3D and 2D, a predefined evaluation group, named Fracture Mechanics Results,
is also generated. It contains a table with values of J-integrals and stress intensity factors
for all integration paths. In 3D, however, only the maximum value of J along the crack
front is reported.
Virtual Crack Extension Method
Similar to the J-integral method, the virtual crack extension method is used for
computing the energy release rate and stress intensity factors. These two methods
complement each other. The advantage with the virtual crack extension method is that
it contains less assumptions. It can be used, for example, in the presence of body loads
and thermal strains.
The virtual crack extension evaluation does, however rely on a significantly more
complicated setup of the model, so for cases when the J-integral method is applicable,
that should be the first choice.
324 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
USING THE VIRTUAL CRACK EXTENSION METHOD
The first step is to add a Virtual Crack Extension Method subnode under the Crack
node used to model the crack. You can only have one Virtual Crack Extension subnode
under each Crack node.
In most cases, the default settings in Virtual Crack Extension are sufficient. You may
want to adjust the size of the sensitivity region. Its significance is discussed in Virtual
Crack Extension Theory. If the crack geometry is such that there may be more than
one crack front, you also need make a selection in the Crack Front section.
) on the Sensitivity section toolbar and
Then, click the Automated Model Setup icon (
). This will initiate the following
select the Create Deformed Geometry and Study (
actions:
• A Deformed Geometry node with subnodes is added in the component. See
Deformed Geometry Features for more information.
• A Control Variable Field node is added under Definitions, having the crack front as
selection.
• A new study named Virtual Crack Extension Study is added. It contains a Sensitivity
study step with an appropriate objective function.
When the study has been run, the predefined evaluation group Fracture Mechanics
Results will contain the values of the energy release rate and stress intensity factors.
Stress Intensity Factors
Stress intensity factors are computed from J-Integral and Virtual Crack Extension. For
a linear elastic material, there is a relation between the J-integral (or energy release
rate) and the stress intensity factors. This relation is, however, only unique when the
stress intensity factors are known, and not when the value the J-integral is known:
2
1
2
2
1
J = G = ----------  K I + K II + ------------ K 

E eff
1 –  III
(2-39)
The split between KI, KII, and KIII is estimated using the displacement field on the
crack faces at some distance behind the crack tip.
In Equation 2-39, Eeff is an effective Young’s modulus, defined as
MODELING CRACKS
|
325
 E
 --------------E eff =  1 –  2

 E
if plane strain
if plane stress
This expression is actually only defined for 2D stress states. In 3D, the expression for
plane strain is used, since the stress state at the crack tip in a thick solid essentially
resembles plane strain.
FREE BOUNDARY IN 3D
At a free boundary, a state of plane stress prevails. Close to the boundary, there will be
a transition zone where neither plane stress nor plane strain is applicable. In this region,
the stress intensity factors, as computed from the J-integral, may be uncertain. It
should be noted, however, that for most metals, the variation in Eeff between plane
strain and plane stress is about 10%, leading to an error in the computed stress intensity
factor in the transition region that is no more than 5%.
UNITS FOR STRESS INTENSITY FACTORS
3/2
The SI unit for stress intensity factors is N/m . Other common units are MPa·m1/2,
psi·in1/2, and ksi·in1/2. The unit handling system in COMSOL Multiphysics only
operates with integer powers of the base units, and can thus not handle stress intensity
factors in a consistent manner.
Because of this, the expressions that define the stress intensity factors include a removal
of the units, and the stress intensity factors appear as a unitless quantities. The value of
a stress intensity factor should be interpreted as having an implicit unit, which is
composed from the base units in the current unit system, for example, N/m3/2.
Contact Between Crack Faces
When a crack is defined by an internal boundary, or is located on a symmetry
boundary, it is possible to consider contact between the crack faces by adding a Crack
closure subnode. When such a node is added, all boundaries selected in the Crack node
are applicable and selected in the Crack closure subnode as well, which means that
contact is added between all crack faces.
Contact between crack faces is implemented by the penalty method as described in
Contact Analysis Theory in the Structural Mechanics Theory chapter. By default,
frictionless contact is considered. However, if the crack is defined by internal
boundaries, you can also take friction into account.
326 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
The kinematics of the contact condition between crack faces differs from that used in
general contact analysis and the Contact node. It is fully defined by the displacement
discontinuity defined by the slit condition of the crack, and thus involves no contact
search algorithm. The gap gn is then given by
gn = n   uu – ud 
where n is the spatial normal to the internal boundary, and uu and ud are the
displacements on the “upside” and “downside”, respectively. Similarly, the tangential
deformation gt is given by
gt = –t   uu – ud 
where t is the spatial tangent to the internal boundary. In 3D, there are two
components of gt given by t1 and t2, respectively. Friction is based on an incremental
formulation, and the incremental slip is given by
g t = g t – g t,old
where gt,old is the tangential deformation at the previous converged increment. For a
symmetric crack uu  0 and ud  u. Note that no tangential deformation is computed
in such cases. Given that the gap and the slip are computed from the displacement
jump across an internal boundary, the contact formulation is only valid for small sliding
since the same nodal points are always connected even as the bodies deform.
MODELING CRACKS
|
327
Buckling Analysis
Linearized Buckling Analysis
A linearized buckling analysis can be used for estimating the critical load at which a
structure becomes unstable. This is a predefined study type that consists of two study
steps: An initial step in which a unit load is applied to the structure, and a second step
in which an eigenvalue problem is solved for the critical buckling load.
The idea behind this type of analysis can be described in the following way:
Consider the equation system to be solved for a stationary load f, in case of geometric
nonlinearity;
Ku =  K L + K NL u = f
Here the total stiffness matrix, K, depends in the solution, since the problem is
nonlinear. It has been split into a linear part, KL, and a nonlinear contribution, KNL.
In a first-order approximation, KNL is proportional to the stress in the structure and
thus to the external load. If the linear problem is solved first for an arbitrary initial load
level f0,
KL u0 = f0
(2-40)
then the nonlinear problem can be approximated as
 K L + K NL  u 0  u = f 0
where  is called the load multiplier.
An instability is reached when this system of equations becomes singular, so that the
displacements tend to infinity. The value of the load at which this instability occurs can
be determined by, in a second study step, solving an eigenvalue problem for the load
multiplier .
 K L + K NL  u 0  u = 0
COMSOL reports a critical load factor, which is the value of at which the structure
becomes unstable. The corresponding deformation is the shape of the structure in its
buckled state.
328 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
The level of the initial load used is immaterial since a linear problem is solved. If the
initial load actually was larger than the buckling load, then the critical value of  is
smaller than 1. It is also possible that the computed value of  is negative. This signifies
that a reversed load will give the critical case.
LIVE AND DEAD LOADS
In some situations, not all loads that act on the structure can vary, and you may want
to compute the critical load factor only with respect to the uncertain (‘live’) load. For
example, gravity is often treated as a ‘dead’ load. The dead loads do, however, affect
the stress distribution in the structure, so they cannot be completely ignored. Using
the same terminology as above,
d
Ku =  K L + K NL + K lNL u = f
Here, the superscripts ‘d’ and ‘l’, stands for live and dead loads, respectively. By solving
two problems, one with the live loads, and one with the dead loads, it is possible to
separate their effects:
l
l
d
d
KL u0 = f0
KL u0 = f0
Now, the following eigenvalue problem is solved to determine the critical load factor:
d
l
 K L + K NL  u 0  + K NL  u 0  u = 0
For any load feature, you can specify that is a dead load by selecting the Treat as dead
load check box in the Linear Buckling section.
To perform a buckling analysis including both live and dead loads, you need three
study steps: two stationary steps, and the linear buckling study step.
1 In the first study step, you solve for the dead loads only. Disable any live loads in the
solver.
2 In the second study step, you solve for all loads; the live loads with an arbitrary
scaling factor plus the dead loads.
BUCKLING ANALYSIS
|
329
3 Finally, in settings for the Linear Buckling study step, you need to point to these two
solutions as Values at linearization point and Live loads solution, respectively.
Figure 2-32: Selecting the solutions for a buckling analysis with live and dead loads.
GEOMETRIC NONLINEARITY
Sometimes, the preload case requires a geometrically nonlinear analysis in order to
produce the correct state. This means that it is no longer solved using the linear set of
equations given by Equation 2-40, but rather
 K L + K NL  u 0  u 0 = f 0
(2-41)
The assumption for the buckling analysis is still that KNL is proportional to the external
load, even though this may be disputable for a strongly nonlinear case. KNL is based
on the stresses, which must be computed in the same way for both cases, that is, under
the same assumption about geometric nonlinearity. The effect is that the stiffness
330 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
matrix at the linearization point includes the nonlinear part from Equation 2-41, and
the eigenvalue problem is reformulated as
  K L + K NL  u 0   +   – 1 K NL  u 0  u = 0
FOLLOWER LOADS
Loads that depend on the deformation are called follower loads. An example of this is
a pressure load, since the orientation of the load will depend on surface deformation.
Such loads contribute to the stiffness matrix, and can thus affect the buckling load. As
a default, all loads in the structural mechanics interfaces are multiplied by the load
factor in a linear buckling study step.
If the computation of the predeformation requires a geometrically
nonlinear analysis, then geometric nonlinearity must be used also in the
Linear Buckling study step.
In this case, it must be assumed that the critical load factor  is
significantly larger than 1.
• Be aware that for some structures, the true buckling load can be
significantly smaller than what is computed using a linearized analysis.
This phenomenon is sometimes called imperfection sensitivity. Small
deviations from the theoretical geometrical shape can then have a large
impact on the actual buckling load. This is especially important for
curved shells.
• For a structure that exhibits axial symmetry in the geometry,
constraints, and loads, the critical buckling mode shape can still be
nonaxisymmetric. A full 3D model should always be used when
computing buckling loads.
• It must always be checked that allowable stresses are not exceeded
before the buckling load is reached.
• Studies and Solvers and Linear Buckling in the COMSOL Multiphysics
Reference Manual
• Linear Buckling in the theory section of the Structural Mechanics
Module User’s Guide
BUCKLING ANALYSIS
|
331
• Bracket — Linear Buckling Analysis: Application Library path
Structural_Mechanics_Module/Tutorials/bracket_linear_buckling
• Buckling Analysis of a Truss Tower: Application Library path
Structural_Mechanics_Module/Buckling_and_Wrinkling/
truss_tower_buckling
Nonlinear Buckling Analysis
A linear buckling analysis gives an approximation to the critical load of a structure. To
gain more confidence in the results, a full nonlinear analysis where the load is slowly
increased can be performed. Such an analysis will, in general, not give a distinct value
of the buckling load. Rather, there will be an increasing level of deviation from the
linear response. The allowable load is given by some criterion of allowable deformation
or stress. In some cases, the nonlinear buckling analysis will stop because a singularity
is encountered. This can then be considered as the buckling load.
In a nonlinear buckling analysis, you use an auxiliary sweep, where a parameter for the
load is increased. This type of analysis requires significantly more computing time than
a linearized buckling analysis.
Modeling Imperfection in a Buckling Analysis
Real structures always contain some level of imperfections in the geometry. Beams are
not perfectly straight, plates are not perfectly flat, and so on. For some structures, the
real-life failure load is much smaller than the ideal buckling load that would be the
result of a linearized buckling study.
There are different ways in which you can take imperfections into account. If the actual
imperfections are known, they may even be part of the geometry. More common,
however, is that the analysis is based on the ideal geometry. In this case, using the
deformed geometry concept provides a convenient tool for introducing the
imperfection.
For more information about deformed geometries, see Deformed
Geometry and Moving Mesh and Deformed Geometry Features in the
COMSOL Multiphysics Reference Manual
332 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
If the imperfection is known from some external source, say a standard that stating that
a certain curvature must be assumed for a beam, then you can directly enter
expressions for such deviations. Do as follows:
1 On the Definitions tab, click Deformed Geometry, and select Prescribed Deformation.
Alternatively, you can right-click on the Component node and select
Deformed Geometry>Prescribed Deformation.
2 In the added Prescribed Deformation node, select the appropriate Geometric entity
level, and then select the part of the geometry to perturb.
3 Enter expressions for the Prescribed deformation in terms of the geometry frame
coordinates, for example, Xg, Yg, and Zg.
Another common approach for generating an initial imperfection is to first perform a
linearized buckling analysis, and then add one or more suitably scaled buckling modes
as initial imperfection. The rationale behind this is that it is reasonable to assume that
the structure is sensitive to an imperfection that resembles a buckling mode.
The procedure for entering buckling models as imperfections is also based on a
deformed geometry, but is more complicated. For this reason, a special tool is available
for setting up such an analysis, as described below.
1 Run a linear buckling analysis, in which you solve for one or more buckling modes.
2 On the Definitions tab, click Physics Utilities, and select Buckling Imperfection.
Alternatively, you can right-click on the Definitions node and select Physics Utilities>
Buckling Imperfection.
BUCKLING ANALYSIS
|
333
3 In the added Buckling Imperfection node, do the following
a From the Linear buckling study list, choose the study from which the imperfection
mode shapes are to be selected. Only studies containing a Linear Buckling study
step are shown in the list.
b Under Mode selection, add the buckling modes to include in the Mode column.
Also, specify a scale factor for each mode in the corresponding field under Scale
factor.
c To add a Deformed Geometry node with necessary subnodes in which the selected
sum of buckling modes are used as predeformation, click the Create button (
in the Deformed Geometry section header.
)
d From the Study list, choose the study that is the nonlinear buckling study. The
default, and most common case, is New, in which case the study does not already
exist. You can also select any existing Stationary study.
e From the Load parameter list, choose the parameter to use as a load parameter for
ramping up the load. The parameter must be defined under a Parameters node,
so you may have to move there to create it. Its purpose is to act as a multiplier to
the same load that was used in the linear buckling study.
f Click the Create button (
) in the Nonlinear Buckling Study section header to set
up the nonlinear study. If Study is set to New, a new study is created. If an existing
study is selected, its settings will be modified. In either case, geometrical
nonlinearity will be activated in the study, and a continuation solver will be set up
334 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
using the Load parameter as auxiliary sweep parameter. The range of the sweep is
based on the lowest buckling mode selected in the Mode selection table.
Figure 2-33: Settings in the Buckling Imperfection node.
4 Go back to the physics, and make sure that the loads are multiplied by the load
multiplier parameter.
BUCKLING ANALYSIS
|
335
5 Run the nonlinear buckling study.
• When the nonlinear study is generated, the default expression for the
auxiliary sweep parameter values is set to
<CritFactor>*log(range(1,1,20))/log(15)
Here, <CritFactor> is the critical load factor in the linearized
buckling analysis. This means that the load is increased in 20 decreasing
steps, from 0 to about 1.1 times the critical load factor.
• Under Definitions, a Deformed Geometry node with one or more
Prescribed Deformation subnodes is created. These subnodes contain
references to special variables containing the selected superposition of
buckling modes (Figure 2-34).
Figure 2-34: The automatically generated deformed geometry settings.
Buckling Analysis of a Truss Tower: Application Library path
Structural_Mechanics_Module/Buckling_and_Wrinkling/truss_tower_buckling
336 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Performing a Random Vibration
Ana ly s i s
INTRODUCTION
Sometimes, the loads on a structure are random in nature. An example is the wind load
on a tower. In addition to the average wind, there are gusts caused by the turbulence
in the flow. The gusts will give a time-dependent excitation, which can induce a
dynamically amplified response in the structure. The frequency and amplitude of these
gusts will be randomly distributed. If the structure is large, the peaks in the wind speed
may not even occur synchronously at locations far from each other.
If the pressure is measured, it is possible to give a statistical representation of the wind
load. The statistical representation of an input like a force to be used in a random
vibration analysis is the power spectral density (PSD), which is a function of the
frequency.
Similarly, the computed results quantities are represented by their PSD, from which it
is possible to derive a root-mean-square (RMS) value.
There are two main cases when a random vibration analysis is useful. In addition to the
scenario outlined above, it is common that design standards (in particular for
electronic components and devices) include requirements on random vibration
testing. To simulate such a test, a random vibration analysis can be performed. In this
case, the prescribed PSD of the excitation is a simplified envelope intended to cover a
multitude of loading conditions.
For a detailed theory, see Random Vibration Theory.
Correlation
When several loads act on a structure, they can have different degrees of
interdependency. This is described by a statistical measure of their correlation. There
are two important special cases of correlation, which significantly simplify the analysis.
If the loads are random in nature and completely independent of each other, they can
be described as being uncorrelated. This would be the case when, for example, two
separate drilling machines are used simultaneously at some distance from each other.
PERFORMING A RANDOM VIBRATION ANALYSIS
|
337
If several loads have the same source, they can be fully correlated. Vibration testing is
a common example. In such case, several points on the structure are attached to the
same shaker table. Thus, they will experience identical (but random) acceleration
histories. Another example could be when a certain load is decomposed into
components along different coordinate axes. Clearly, the X- and Y-components are just
scaled versions of the total load, and thus they are fully correlated.
In a general case, the correlation between two loads is a function of both the distance
between their positions and the frequency. The input to the analysis includes not only
the PSD of each load but also their cross-correlation.
Spatial Variation of Random Loads
The PSDs and cross-correlation matrices are assumed to be functions of frequency
only. It is not allowed to write expressions that are functions of the spatial coordinates.
The expression for the load inside the physics interface, however, can have such
dependencies as long as they appear as a pure multiplier to the spectrum.
In principle, however, the PSD and even the full cross-correlation functions could be
considered to vary continuously over a structure, and thus be functions of the spatial
coordinates. An example of this could be the wind pressure on a high tower.
If you want to model such situation, you need to split the loaded region into smaller
parts, each with its own constant spectrum definition. Note that the number of
off-diagonal cross-correlation functions increases quadratically with the subdivision.
SETTING UP A RANDOM VIBRATION ANALYSIS
Random vibration analysis is based on a modal representation of the structure. It
represents a type of mode superposition and relies on the reduced-order model (ROM)
concept.
In principle, you can perform random vibration analysis on any reduced-order model
that is of the Frequency Domain, Modal type. This requires a number of settings and
studies run in an appropriate order.
It is significantly more convenient to start by adding a Random Vibration (PSD) study,
either from the Add Study window or from the Select Study page in the Model Wizard.
The Random Vibration (PSD) study is not a study in itself; rather, it adds a number of
nodes to the Model Builder tree to facilitate a random vibration analysis. These nodes
serve the purpose of setting up the ROM and providing input data to the random
vibration analysis.
338 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Two studies are added:
• One study with an Eigenfrequency study step for computing the eigenfrequencies
and corresponding eigenmodes.
• One study with a Model Reduction study step, in which the ROM is created. It
references the eigenfrequency study, as well as an embedded Frequency Domain study
step. The latter can mainly be considered as a placeholder which is a mandatory
input to the model reduction. In case you have already computed the eigenmodes,
you can change the setting of the Training study in this node to point to the
corresponding existing eigenfrequency study, and then delete the newly generated
one.
The Model Reduction study step is set up to be suitable for a random
vibration analysis. In particular, it is required the Ensure reconstruction
capability is selected.
Under Global Definitions, a Reduced-Order Modeling node becomes available. It contains
three subnodes:
• A Global Reduced Model Inputs node, in which you define the control parameters for
the ROM. All loads that represents random excitations must have a value multiplied
by one of such parameters.
• A Frequency Domain, Modal Reduced-Order Model node. This is a placeholder for the
ROM to be created.
• A Random Vibration node. Here, you prescribe the PSD functions and the
cross-correlation functions, if needed. They can be function of frequency only (the
internal variable freq); it is not possible to prescribe a coordinate dependency.
WORKFLOW
Here, you find recommended steps to perform a random vibration analysis.
1 Add a Random Vibration (PSD) study.
2 In the Global Reduced Model Inputs node, add all required control parameters. The
values that you assign to the parameters are not important. Control parameters are
used in the same manner as ordinary parameters in expressions for the loads in the
physics interface. You need as many control parameters as you have different PSD
functions.
PERFORMING A RANDOM VIBRATION ANALYSIS
|
339
3 In the physics interface, create the loads that should have a random variation.
Typically, the value is just the name of a control parameter, even though it is possible
to also add a scalar multiplier to it.
• The reduced-order models on which the random vibration analysis is
based are not unit aware. Always use the base units from the current
unit system in the context of a random vibration analysis.
• Only ‘Neumann type’ loads like forces and pressures can be given a
random excitation. It is not possible to use ‘Dirichlet type’ loads like
prescribed displacements, velocities, or accelerations. This is similar to
other mode superposition methods.
For the common case that a number of support points have the same
acceleration PSD, the support acceleration can be replaced by a frame
acceleration load, using the Base Excitation feature. This is how
vibration testing is analyzed. See also Absolute Versus Relative
Accelerations.
4 If you want any scalar outputs, define them as Variables under Definitions in the
component. You can use, for example, probes or functions like at3() to create
scalar outputs. It is also possible to compute scalar results using, for example, Point
Evaluation during result presentation. Such evaluations will, however, require a
larger computational effort than scalar outputs that are part of the ROM definition.
5 In case you want to reuse a previously computed eigenfrequency study, go to the
Model Reduction study step. Change the settings for Training study in the Model
Reduction Settings section to point to the correct eigenfrequency study.
6 Run the study containing the Model Reduction study step. It will automatically create
a ROM that can be used for all further evaluations.
340 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
7 Define the PSD and cross-correlation functions required for representing the
loading as functions under Global Definitions. These functions should depend on
frequency only.
It is common that an input PSD is provided in terms of straight lines in a
log-log diagram of PSD value versus frequency, f. To mimic this behavior,
you can use an interpolation function (say int1) where you enter pairs of
log(f) and log(PSD) values. You then reference this function through an
expression like exp(int1(log(freq[1/Hz]))). This will provide a linear
interpolation in a log-log space.
8 Go to the Random Vibration node. Select the appropriate Correlation type.
9 For each control parameter, enter the corresponding spectrum function. The
argument to the function should be the built-in frequency variable freq.
10 If the correlation type is Cross-correlated, enter also the off-diagonal part of the
Correlation matrix.
11 To make these settings available for result evaluation, run Update Solution for the
model reduction study.
RESULT EVALUATION
For presentation of random vibration results, you can use the standard features under
Results, with the provision that the quantity you are studying is a linear function of the
displacements. You can use any linear expression, not only built-in variables.
In addition to linear variables, there is also a special case where the RMS of quadratic
forms can be computed.
The evaluation of random vibration results is done through special operators, listed in
Table 2-17, which are defined by the Random Vibration node (with a tag rvib1 in this
example).
TABLE 2-17: RANDOM VIBRATION OPERATORS.
OPERATOR
SYNTAX
EXPLANATION
psd
rvib1.psd(expr)
Evaluates the PSD of an expression for the
given frequency
cross
rvib1.cross(expr1, expr2)
Evaluates the cross-correlation between two
expressions for a given frequency,
PERFORMING A RANDOM VIBRATION ANALYSIS
|
341
TABLE 2-17: RANDOM VIBRATION OPERATORS.
OPERATOR
SYNTAX
EXPLANATION
rms
rvib1.rms(expr, f1, f2, N)
Evaluates the RMS value of an expression
within the frequency interval [f1, f2]. N
points are used for integrating over the
interval.
rms
rvib1.rms(expr)
Evaluates the RMS value of an expression.
The frequency interval, as well as the
integration settings are taken from settings
in the corresponding Random Vibration
node.
m
rvib1.m(K,expr, f1, f2, N)
Evaluates the K:th order moment of the
PSD. Thus, rvib1.rms(expr, f1, f2, N) =
sqrt(rvib1.m(0,expr, f1, f2, N)). The
maximum supported moment order is K=4.
m
rvib1.m(K,expr)
Evaluates the K:th order moment of the
PSD. The frequency interval, as well as the
integration settings are taken from settings
in the corresponding Random Vibration
node. The maximum supported moment
order is K=4.
q2
rvib1.q2(expr, f1, f2, N)
Evaluates the RMS of a quadratic form, for
example the square of an effective
displacement, or the square of the von Mises
equivalent stress. The expression must not
contain time derivatives like velocities or
accelerations. Rather than
rvib1.q2(utt^2,…), you can write
rvib1.q2(u^2*(2*pi*freq)^4,…).
The quadratic form itself must be
real-valued. This means that evaluation using
the von Mises stress can only be done if the
material properties are real-valued. In
particular, it should be noted that loss factor
damping implies a complex-valued stiffness.
q2
342 |
rvib1.q2(expr)
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Evaluates the RMS value of a quadratic form.
The frequency interval, as well as the
integration settings are taken from settings
in the corresponding Random Vibration
node.
TABLE 2-17: RANDOM VIBRATION OPERATORS.
OPERATOR
SYNTAX
EXPLANATION
q2sq
rvib1.q2sq(expr, f1, f2, N)
Evaluates the square root of the RMS of the
quadratic form. The norm of the quadratic
form is used as input. See q2 operator above
for more information. The relation between
these two operators is:
rvib1.q2sq(sqrt(expr),…) =
sqrt(rvib1.q2(expr,…))
q2sq
rvib1.q2sq(expr)
Evaluates the square root of the RMS of the
square root of a quadratic form. The
frequency interval, as well as the integration
settings are taken from settings in the
corresponding Random Vibration node.
The operator q2sq() is a convenience version of the q2() operator. Some important
quantities have special variables, intended for use in the q2sq() operator, see
Table 2-18.
TABLE 2-18: PREDEFINED VARIABLES FOR USE WITH THE Q2SQ OPERATOR.
VARIABLE
DESCRIPTION
<phys>.mises_rv
von Mises equivalent stress
<phys>.disp_rv
Norm of displacement
<phys>.vel_rv
Norm of velocity
<phys>.utt_rv
Norm of acceleration
<phys>.rot_rv
Norm of rotation
<phys>.rotvel_rv
Norm of rotational velocity
<phys>.rotacc_rv
Norm of rotational acceleration
You cannot use ordinary variables like <phys>.mises or <phys.disp> as
arguments to the q2sq() operator. The reason is that the argument must
never evaluate to zero.
It is convenient to plot the PSD of a result quantity computed, for example, at certain
point in the structure for a given frequency range. Such evaluation sweeps over the
frequency can be defined in a Global Evaluation Sweep node.
The RMS of a result quantity does not give direct information about its peak value.
Formally, probability theory says that for a long enough process, the peak value can be
PERFORMING A RANDOM VIBRATION ANALYSIS
|
343
arbitrarily large. In practice, it is common to assume that the peak value is three (or
sometimes four) times larger than the RMS value. There are good reasons for this
practice.
• The input signal is usually bounded for physical reasons. It is not a true Gaussian
distribution.
• For testing, the shaker table accelerations are limited, and this is even expected in
the requirements on the signal.
• The whole random vibration analysis assumes linearity. Nonlinear effects will
typically limit the response.
Absolute Versus Relative Accelerations
It is common that the input to a random vibration analysis is a PSD for a base
acceleration. Since it is not possible to directly prescribed nonzero displacements (or
accelerations) at constrained points, the standard approach is to replace the base
acceleration with an inertia load on the structure. This can be seen as a frame
transformation, where the analysis is made in a coordinate systems that is connected to
the fixture. This change of frame does not affect for example stress or strain results.
The computed accelerations, however, are measured relative to the support points, not
relative to a room fixed frame. In most cases, you are interested in the absolute
accelerations, that is what would be measured by an accelerometer. When the Base
Excitation feature is used to describe the acceleration, special variables containing the
absolute (room fixed) accelerations are also available.
• Bracket — Random Vibration Analysis: Application Library path
Structural_Mechanics_Module/Tutorials/bracket_random_vibration
• Random Vibration Analysis of a Deep Beam: Application Library
path Structural_Mechanics_Module/Verification_Examples/
random_vibration_deep_beam
344 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Performing a Response Spectrum
Ana ly s i s
INTRODUCTION
Response spectrum analysis is used to approximately determine the structural response
to short nondeterministic events like earthquakes and shocks. The idea is that the event
is characterized by the peak response that it would give a single degree of freedom
(SDOF) oscillator having a certain natural frequency and damping ratio. The response
value is provided as a function of the natural frequency of the oscillator.
If the dynamic structural response is viewed as a mode superposition, each eigenmode
within the given frequency range acts as an SDOF oscillator, with a peak amplitude that
is known from the spectrum. There is, however, no information about when each
mode reaches its peak value. The most conservative assumption is that all modes
should be combined using the individual peak values. Using such approach will in most
cases result into an extremely conservative design. For this reason, other summation
methods have been developed. When performing a response spectrum analysis, you
will have access to several such methods.
SETTING UP A RESPONSE SPECTRUM ANALYSIS
The response spectrum analysis is not a study type. The computations are performed
during result evaluation. You enter the methods and parameters in the settings for the
Response Spectrum 2D or Response Spectrum 3D datasets. These datasets require the
following:
• An eigenfrequency solution, where the eigenmodes to be included in the response
spectrum analysis have been computed. All computed eigenmodes are used. If you
want to filter out a particular set of modes, you can add a Combine Solutions study
step after the Eigenfrequency study step. Such a filter can for example be based on the
effective modal mass, so that only modes which contribute significantly to the mass
are included.
The time to evaluate a result when using a response spectrum dataset
varies almost quadratically with the number of eigenmodes you include.
PERFORMING A RESPONSE SPECTRUM ANALYSIS
|
345
• A corresponding set of modal participation factors. To generate them, add a
Response Spectrum node under Definitions in the component. If you have computed
the eigenfrequency prior to adding the Response Spectrum node, you need to
perform an Update Solution.
• In some response spectrum evaluation methods, you are required to compensate for
the mass that is not represented by the included eigenmodes. In order to do so, a
number of special stationary load cases must also be computed. You can set up all
nodes required in the model builder tree by clicking the Create missing mass
correction study (
) button on the Response Spectrum section header in the
Response Spectrum node settings.
Adding a Response Spectrum Study
In the Add Study dialog, there is a study type called Response Spectrum. When you select
it, two things happen:
• A study, containing a single Eigenfrequency study step is created.
• A Response Spectrum node is added under Definitions in the first component which
contains at least one structural mechanics physics interface. In this node, the
Eigenfrequency study list will be initialized to point to the Eigenfrequency study step
that was just created.
If you already have computed the eigenfrequencies of a structure, and then want to
perform a response spectrum evaluation, there is no need to add a new study. Just add
a Response Spectrum node under Definitions->Variable Utilities, and then do an Update
Solution to make the new variables available.
346 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Missing Mass Correction
You create a missing mass correction study from the Response Spectrum node by
clicking the Missing mass correction study: Create button.
It is not possible to undo this operation. To revert, you will have to
manually delete all the nodes which were created.
A number of items are then created in the model tree:
• A set of load group nodes are created under Global Definitions. There are two load
groups for each spatial direction. The load group nodes are placed under a common
group named Load Groups for Missing Mass Correction.
The Parameter name of the load group is reserved, and you should not modify it.
• A new study named Study: Missing Mass Load Cases is created. This study contains
three or four study steps, depending on the space dimension. First, there is one
Combine Solutions study step for each spatial direction. In these steps, a weighted
sum of the eigenmodes is computed. The weights are the modal participation factors
in each direction. This gives a measure of the mass that the eigenmodes represent.
These study steps must reference the eigenvalue solution, including any subsequent
filtering. If you change the study from which the eigenmodes are to be taken, you
must also change the choice in the Solution list in all of the Combine Solutions nodes.
PERFORMING A RESPONSE SPECTRUM ANALYSIS
|
347
The final study step in the study is a stationary study step, where each load group is
solved separately by adding one load case per load group.
If the physics interface has loads other than those automatically generated
for missing mass correction, you need to make sure that those loads are
not solved for in the Missing Mass Static Load Cases study step. There are
several ways of doing that. You can, for example:
• Disable the other load nodes temporarily in the model tree before
solving.
• Disable them in this study, by using Modify model configuration for study
step in the Physics and Variables section in the settings for the study
step. This is the preferred method.
• Assign the other loads to a new load group.
• In each structural mechanics physics interface in the component, a set of Gravity
nodes are added. There are two such nodes for each spatial direction. Each gravity
node is connected to a corresponding load group. Half of the loads are pure gravity
loads, used when only together with the Static ZPA method. The other set of loads,
which are used in the Missing mass method, are referencing the combined solutions
348 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
as the depend on the computed eigenmodes. The gravity nodes are placed under a
common group, named Loads for Missing Mass Correction.
SETTINGS FOR THE RESPONSE SPECTRUM DATASETS
Defining the Spectra
You input the spectra as functions under Global Definitions. Usually, either an
interpolation function, or an analytic function, or a piecewise function is used.
There are two common methods to describe the design response spectra: either as
function of frequency, or as function of period time. Use the Depends on setting to
control this.
The handling of units in the functions are nonstandard:
• The unit of the argument is ignored. The function is called with either frequency
(hertz) or period time (seconds) as defined by the setting in Depends on.
• The unit of the function is not checked. The function will, however, be scaled to
model units, so if you, for example, enter the unit mm/s^2 for an acceleration
spectrum, the function will (in an SI system) be scaled by 1/1000. You would get
the same effect if the entered unit is inconsistent (for example, mm).
PERFORMING A RESPONSE SPECTRUM ANALYSIS
|
349
The spectra you enter have the following correlation to the spatial directions:
• In 2D, you give two spectra: one horizontal and one vertical. The horizontal
spectrum acts along the global X-axis, and the vertical one acts along the Y-axis.
• In 3D, the vertical spectrum always acts along the global Z-axis.
• In 3D, you can supply two different horizontal spectra, called primary and
secondary horizontal spectrum. Those spectra act in two orthogonal directions,
which by default coincide with the global X and Y directions. By giving a nonzero
value to Primary axis rotation, you can make the primary spectrum act in an arbitrary
direction in the XY-plane.
• Some Spatial combination methods in 3D (CQC3 and SRSS3) assume that the two
horizontal spectra are equal except for an amplitude scale factor. In such case, you
only provide one spectrum together with a Secondary horizontal spectrum scale factor
(value between 0 and 1).
Mode Combination
The combination of the eigenmodes is the core of the response spectrum methods.
Most commonly the combination is done in two passes: first the response to the
excitation in each spatial direction is determined, and then a total response is computed
by combining the spatial responses. However, for certain methods the total response
is computed in one pass.
First, you select a Spatial combination method. If it is SRSS or Percent method, you also
select a Mode combination method.
The mode combination methods require different inputs. In particular, several of them
provides a possibility to choose whether the coupling terms between modes are to be
considered as always positive, or they may actually reduce the total response. This is
controlled by the Use absolute value for coupling terms check box. Its default value
differs between the methods, according to what is expected to be the most common
choice.
Periodic Modes and Rigid Modes
For frequencies higher than the highest frequency content of the excitation, the SDOF
system will respond as a rigid body. Some of the response spectrum evaluation methods
take this into account. The effect is that high-frequency (“rigid”) modes are assumed
to have a higher degree of correlation than low-frequency (“periodic”) modes. To take
this effect into account, you can select Rigid modes to be the Gupta method or the
Lindley-Yow method.
350 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Missing Mass Correction
In general, only a small fraction of the total number of eigenmodes are used in the
superposition. Therefore, some fraction of the total mass of the structure is not
accounted for. The ignored modes usually have high natural frequencies. Such modes
will not have a significant dynamic amplification. The mass in the corresponding
SDOF system will just follow the movement of the foundation. This means that if the
distribution of the missing mass is known, then it can be treated as an extra stationary
mass force, where the peak acceleration during the event replaces the acceleration of
gravity.
You can use two different methods for missing mass correction:
• In the Missing mass method, the difference between the true mass distribution and
the mass represented by the used eigenmodes will act as extra static load. Typically,
most of the missing mass is located close to support points, where the modal
amplitudes are low. This method can be used together with either the Gupta method
or the Lindley–Yow method.
• In the Static ZPA method, the total inertial force is used as static load. At the same
time, only the periodic part of the response is used in the mode summation. This
method can only be used together with the Lindley–Yow method because it is only
compatible with the assumptions about how the rigid modes are scaled.
RESULT INTERPRETATION
All results from a response spectrum analysis are positive; the evaluation methods
contain absolute values or RMS-like operations. This has important implications for
the interpretation of the results:
• If the sign of your result quantity is important for the conclusions, you need to
manually consider also the case of a negative value.
• It is not meaningful to evaluate a quantity that is not proportional to the mode
amplitude. This does, however, not mean that you are limited to linear quantities;
equivalent stresses like von Mises and Tresca are nonlinear, but they are still
proportional to the mode amplitude.
• It is not meaningful to show deformation or vector plots of response spectrum
results.
An underlying implicit assumption for response spectrum analysis is that it is
performed in a frame of reference that follows the foundations of the structure. Thus,
all displacements, velocities, and accelerations are relative to the foundation, which in
itself is accelerating. Thus, it is difficult to evaluate the absolute acceleration. The
PERFORMING A RESPONSE SPECTRUM ANALYSIS
|
351
conservative way of doing so is to add the peak acceleration of the underlying event to
the computed acceleration. This will usually be rather conservative since the peak of
the excitation seldom coincides in time with the peak of the response.
For displacements, the relative displacements between two objects within the same
moving frame is usually a more important result than the absolute displacement, so it
does seldom matter whether a constant value is added to all points or not.
• The theory is described in Response Spectrum Analysis Theory.
• The Response Spectrum node is described in the COMSOL
Multiphysics Reference Manual.
• Combine Solutions and Updating a Solution in the COMSOL
Multiphysics Reference Manual.
• The settings for the special datasets are described in Response
Spectrum 2D and Response Spectrum 3D in the COMSOL
Multiphysics Reference Manual.
• Earthquake Analysis of a Building: Application Library path
Structural_Mechanics_Module/Dynamics_and_Vibration/
building_response_spectrum
• Shock Response of a Motherboard: Application Library path
Structural_Mechanics_Module/Dynamics_and_Vibration/
motherboard_shock_response
352 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Stress Linearization
The information about stress linearization is applicable if your license
includes the Structural Mechanics Module.
Stress linearization is a procedure in which the stress distribution along a line through
the thickness in a solid is approximated with an equivalent linear stress distribution,
similar to what would be the result of an analysis using shell theory. The line is
commonly referred to a stress classification line, SCL. This type of evaluation is
common in the analysis of pressure vessels. It is also useful for the design of
reinforcements for concrete structures and for fatigue analysis of welds.
To perform a stress linearization, you add one Stress Linearization node for each SCL.
ORIENTATION OF STRESS COMPONENTS
The stresses along the SCL are represented in a local orthonormal coordinate system,
x1-x2-x3. The x1 direction is oriented along the SCL, so it is mainly the stresses in the
second and third directions that are of interest.
• In 3D, you must specify the x2 direction and thus implicitly the x3 direction. You
specify the orientation either by selecting a point in the x1-x2 plane or by defining
an orientation vector in an approximate x2 direction. In either case, the actual x2
direction is chosen so that it is perpendicular to the SCL and lies in the plane you
have specified. The x3 orientation is then taken as perpendicular to x1 and x2. As
long as you are only interested in a stress intensity, the choice of orientation is
arbitrary.
• In 2D, the x3 direction is the out-of-plane direction, and the x2 direction is
perpendicular to the SCL in the XY-plane.
• In 2D axial symmetry, the x3 direction is the azimuthal direction, and the x2
direction is perpendicular to the SCL in the RZ-plane.
CREATING THE STRESS CLASSIFICATION LINE
The most straightforward way to create an SCL is to include it in the geometry, and
then select it in a Stress Linearization node. This corresponds to using the Line
linearization type where the SCL is defined by Edge.
STRESS LINEARIZATION
|
353
Figure 2-35: Four stress classification lines in a transition region at a pressure vessel
nozzle.
There are, however, some situations where this direct approach is less convenient:
• When the introduction of the SCL in the geometry must be done after the analysis,
since the locations of critical regions were not obvious when setting up the initial
analysis. It is of course possible to add new edges and rerun the analysis, but this
may not be a good solution if the analysis time is long.
• When the introduction of the edges for the SCL makes the meshing more difficult.
It may, for example, not be possible to use swept meshes anymore, or the mesh
quality is reduced in critical regions.
In the two above cases an alternative is to define an SCL that is not included in the
geometry by connecting two arbitrary points with a straight line. This corresponds to
using the Line linearization type where the SCL is defined by Two points. The
introduction of the SCL will in this case not make it necessary to update the geometry
and rerun the analysis. Since the SCL is disconnected from the geometry and mesh,
this option will also make meshing easier. The downside is then the you cannot control
the mesh quality along the SCL.
354 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
In some cases it is difficult to a priori determine where to create the SCL or the critical
location may change depending on, for example, loading conditions or time. For such
cases, it is also possible to define it in a distributed manner such that an infinite number
of SCLs are created in a domain. The starting point of the SCLs are given by a
boundary selection, and they extend along the normals of the boundary through the
selected domains. This corresponds to using the Distributed linearization type.
STUDIES AND SOLUTIONS
Stress linearization is a pure postprocessing operation. The Stress Linearization node
will only create a number of variables, which can be evaluated under Results. It is thus
possible to add such nodes after the main analysis has been performed. In order to
make the new variables available for postprocessing, you must then run an Update
Solution.
RESULTS
When you have included one or more Stress Linearization nodes in a model, a number
of datasets and an extra predefined plot are generated.
One edge dataset is created for each SCL. These datasets are named Linearization
Line <n>, where n is an integer number.
Figure 2-36: Generated datasets in a model with five SCL.
The plot contains graphs for the 22 component of the actual stress, the membrane
stress, and the linearized stress. The first Linearization Line dataset is selected. By
STRESS LINEARIZATION
|
355
changing edge dataset in the plot group, you can easily move between the different
stress classification lines.
Figure 2-37: Plot along a stress classification line.
For the Distributed linearization type, the created Linearization Line dataset corresponds
to a single SCL in selected domain. The starting point is specified in the Postprocessing
section of the feature, and must lie on the selected boundaries. The endpoint is
computed internally such that the cut line extends through the selected domains along
the boundary normal of the point.
VARIABLE NAMES
Each Stress Linearization node adds a number of variables. Many of these variables exist
with two different scopes, physics scope and feature scope. The physics scope is the
name of the physics interface, having the default value ‘solid’. The feature scope
contains also the tag of the Stress Linearization node, for example, ‘sl1’.
As an example, the variable solid.Sm22 and the variable solid.sl1.Sm22 have the
same value. The variables with physics scope make it more convenient to create
expressions using postprocessing. You could, for example, make a line plot of
356 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
solid.sb22 and get all edges having a stress linearization colored by their individual
results.
TABLE 2-19: VARIABLES FOR STRESS LINEARIZATION.
VARIABLE
DESCRIPTION
VARIABLE IN
THEORY SECTION
COMMENT
SCOPE
Sllsij
Stress tensor in
local coordinate
system
ij
ij = 11, 12, 13, 22,
23, 33
Physics,
Feature
Smij
Membrane stress
m,ij
ij = 11, 12, 13, 22,
23, 33
Physics,
Feature
Sbmaxij
Maximum bending
stress
b(max),ij
ij = 11, 12, 13, 22,
23, 33
Feature
Sbij
Bending Stress
b,ij
ij = 11, 12, 13, 22,
23, 33
Physics,
Feature
Smbij
Membrane +
bending stress
mb,ij
ij = 11, 12, 13, 22,
23, 33
Physics,
Feature
Spsij
Peak stress,
starting point
p(start),ij
ij = 11, 12, 13, 22,
23, 33
Feature
Speij
Peak stress,
starting point
b(end),ij
ij = 11, 12, 13, 22,
23, 33
Feature
SIm
Stress intensity,
membrane
int
Physics,
Feature
SImbs
Stress intensity,
membrane +
bending, starting
point
int
Feature
SImbe
Stress intensity,
membrane +
bending, endpoint
int
Feature
SImb
Stress intensity,
membrane +
bending,
max(SImbs, SImbe) Physics,
Feature
mises_m
Equivalent von
Mises stress
(membrane)
Physics,
Feature
mises_b
Equivalent von
Mises stress
(membrane)
Physics,
Feature
STRESS LINEARIZATION
|
357
TABLE 2-19: VARIABLES FOR STRESS LINEARIZATION.
VARIABLE
DESCRIPTION
VARIABLE IN
THEORY SECTION
COMMENT
SCOPE
mises_mb
Equivalent von
Mises stress
(membrane plus
bending)
Physics,
Feature
tresca_m
Equivalent von
Tresca stress
(membrane)
Physics,
Feature
tresca_b
Equivalent von
Tresca stress
(membrane)
Physics,
Feature
tresca_mb
Equivalent von
Tresca stress
(membrane plus
bending)
Physics,
Feature
Nij
Local in-plane
force
Nij
ij = 22, 23, 33
Feature
Mij
Local bending
moment
Mij
ij = 22, 23, 33
Feature
Qi
Local out-of-plane
shear force
i = 2, 3
Feature
lengthtot
Length of SCL
L
Feature
arclength
Coordinate along
SCL
X1
Feature
Stress Linearization in the Structural Mechanics Theory chapter.
358 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Evaluating Stresses in Welds
Weld evaluation consists on the calculation of stresses and forces transmitted by the
weld. These are computed on the plane of the weld throat, and different criteria can
be used to compute equivalent stresses and safety indexes. It is currently possible to
perform weld verification in the Shell interface for double-sided and single-sided fillet
as well as butt joints. It is assumed that the 3D solid model can be approximated by
shells.
To perform a weld evaluation, you select the Weld verification check box in the Edge to
Edge feature in the Shell interface.
The weld evaluation is a postprocessing tool and it is performed during result
presentation. It is not necessary to recompute the solution if the welding type, the weld
size, or the allowable stresses are changed. It is enough to update the solution.
The evaluation is based on the shell section forces at the weld edge on the source side
of the connection. From these forces, available from the Shell interface, only the
components that are transmitted through the weld are kept. The forces are
transformed to the weld reference frame. The equivalent stress is computed as follows:
EVALUATING STRESSES IN WELDS
|
359
 eq =
2
2
2
 perp + 3   perp +  para 
where the contribution of the normal stress parallel to the weld throat is neglected
because it does not transfer any load through the weld.
For a single-sided fillet, the top and bottom options switch the sign of the eccentricity
used to compute the additional stresses due to bending.
Different safety indexes are available to evaluate the weld: failure index, damage index,
safety factor, and margin of safety.
SOURCE AND DESTINATION SELECTION
When interested in weld evaluation the source and destination in the Edge to Edge
feature needs to be selected in a proper way to obtain meaningful results for the
one-sided and double-sided fillet joints. The source has to be the edge belonging to
the plate that would have both top and bottom sides welded if a double-sided fillet was
to be used.
LIMITATIONS
The weld evaluation for the fillet welds assumes that the connecting shells are
perpendicular to each other and the angle between the shell and the throat plane is 45
degree.
360 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
When using a double-sided fillet weld, one side is more critical than the other. The
results will always show the safety factors on the most critical side, where usually the
shear stresses are greater. The single-sided fillet is treated in the same manner.
VARIABLE NAMES
When the weld evaluation check-box is selected, a set of new variables are defined. All
of them are item scoped and the most important are listed below.
TABLE 2-20: VARIABLES FOR WELD EVALUATION.
VARIABLE
DESCRIPTION
weld_di
Damage index
weld_ms
Margin of safety
weld_fi
Failure index
weld_sf
Safety factor
weld_seq
Equivalent stress along the edge
weld_tfwavgi
Traction vector average in the weld
reference system, i component
weld_tfeavgi
Traction vector average in the edge
reference system, i component
EVALUATING STRESSES IN WELDS
|
361
Solver Settings for Structural
Mechanics
COMSOL Multiphysics includes many solvers and solver settings. To make it easier to
use a suitable solver and its associated solver parameters, the physics interfaces have
different default settings based on the study type and features used. In some situations,
the default settings may need to be changed. This section helps you to select a solver
and its settings to solve structural mechanics and related multiphysics problems.
In this section:
• Symmetric Matrices
• Selecting Iterative Solvers
• Specifying Tolerances and Scaling for the Dependent Variables
Studies and Solvers in the COMSOL Multiphysics Reference Manual
If you make changes to the physics, this will not be reflected in the solver
settings unless you regenerate the solver sequence.
Symmetric Matrices
Use the Matrix symmetry list (see the General section in the Settings window for
Advanced for a solver node such as Stationary Solver). There you can explicitly state
whether the assembled matrices (stiffness matrix, mass matrix) resulting from the
compiled equations are symmetric or not.
Normally the matrices from a single-physics structural mechanics problem are
symmetric, but there are exceptions, including the following cases:
• Multiphysics models solving for several physics simultaneously (for example, heat
transfer and structural mechanics). Solving for several Structural Mechanics
interfaces, such as shells combined with beams, does not create unsymmetrical
matrices.
362 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
• Contact with friction.
• Elastoplastic analysis
Advanced and Stationary Solver in the COMSOL Multiphysics Reference
Manual
One of the benefits of using the symmetric solvers is that they use less memory and are
faster. The default option is Automatic, which means the solver automatically detects if
the system is symmetric or not. Some solvers do not support symmetric matrices and
always solve the full system regardless of symmetry.
Selecting the Symmetric option for a model with unsymmetric matrices
may lead to incorrect results. For a nonlinear problem that is only weakly
unsymmetric, it may still be useful, since the faster solution of the
symmetric problem may offset the lower convergence rate. This is, for
example, the case for contact problems with a low coefficient of friction.
Complex matrices can be unsymmetric, symmetric, or Hermitian. Hermitian matrices
do not appear in structural mechanics problems.
Selecting the Hermitian option for a model with complex-valued
symmetric matrices produces incorrect results.
Selecting Iterative Solvers
The default solver for structural mechanics is the MUMPS direct solver in 2D and the
PARDISO direct solver in 3D. For large 3D problems (several hundred thousands or
millions of degrees of freedom) it is beneficial to use iterative solvers when possible to
save time and memory. The drawback is that they are more sensitive and might not
converge if the mesh quality is low. The iterative solvers also have more options than
the direct solvers.
For Stationary and Time Dependent studies and Frequency Domain studies in 3D, a
GMRES iterative solver is preconfigured and available as an alternative solver
suggestion for solid mechanics models.
SOLVER SETTINGS FOR STRUCTURAL MECHANICS
|
363
If the model is set up using quadratic (default) or higher-order elements for the
displacement dependent variable, this GMRES solver will use geometric multigrid
(GMG) as the preconditioner.
For slender geometries, changing to SOR Line as presmoother and postsmoother can
give better results compared to SOR, which is the default for the GMG preconditioner.
For models using linear elements for the displacement dependent variable, the
preconditioner will be changed to smoothed aggregated algebraic multigrid (AMG).
This is to avoid remeshing when creating the discretization on the coarse level. Note
that you need to manually regenerate the solver sequence after you change the element
order if you want to make use of such change in the predefined iterative solver
configuration.
For eigenfrequency and eigenvalue studies, use the default direct solver
Specifying a shift frequency greater than the lowest eigenfrequency results
in indefinite matrices.
Studies and Solvers in the COMSOL Multiphysics Reference Manual
Solver Settings for Viscoelasticity, Creep, and Viscoplasticity
Viscoelasticity, creep, and viscoplasticity are time-dependent phenomena. The time
scale, however, is often such that inertial effects can be ignored. When that is the case,
you can modify the solver settings to improve the performance of the time-dependent
analysis.
PHYSICS INTERFACE SETTINGS
In the Model Builder, click the Solid Mechanics node. In the Settings window, under
Structural Transient Behavior, select Quasi static to treat the elastic behavior as
quasi static (with no mass effects; that is, no second-order time derivatives for the
displacement variables). Selecting this option gives a more efficient solution for
problems where the variation in time is slow when compared to the natural frequencies
of the system since no mass matrix will be created.
364 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
SOLVER SETTINGS
When Quasi static is selected on the physics interface Settings window, the automatic
solver suggestion changes the method for the Time Stepping from Generalized alpha to
BDF.
For a Fully Coupled node (or Segregated node for multiphysics problems), the default
Nonlinear method under Method and Termination is Automatic (Newton). To get a faster
computation time when the strain rate is low or moderate, select Constant (Newton) as
the Nonlinear method instead.
In the COMSOL Multiphysics Reference Manual:
• Studies and Solvers
• Fully Coupled and Segregated
Specifying Tolerances and Scaling for the Dependent Variables
The absolute tolerance parameters used for time-dependent studies are problem
specific. By default, the absolute tolerance is applied to scaled variables, with the
default value being 0.001 for all solution components.
The default scaling for the displacement components is based on the size of the
geometry in the model, and certain reasonable scales are used for the pressure and
contact force variables, if any. You are encouraged to change these scales as soon as
better values are known or can be guessed or estimated from the applied forces, yield
stress, reaction forces, maximum von Mises stress, or similar. The same suggestion
applies to the displacement scale, which can be estimated easily if the problem is
displacement controlled. This approach can significantly improve the robustness of the
solution. The variable scaling is accessed under Dependent Variables in the solver
sequence. The scales need to be entered using the main unit system in the model.
Solver Settings
In many situations, the default in COMSOL Multiphysics when having several physics
interfaces is to generate a solver sequence with a segregated solver. When several
structural mechanics interfaces are present, it can happen that the degrees of freedom
are placed in different segregated steps by the default solver generation. It is, however,
not possible to solve a model where the structural mechanics degrees of freedom are
SOLVER SETTINGS FOR STRUCTURAL MECHANICS
|
365
placed in different segregated groups, so in this case you must modify the solver
settings.
• If the model only consists of structural mechanics interfaces, the best option is
usually to replace the segregated solver with a fully coupled solver.
• If the model contains contact conditions where the augmented Lagrangian method
is used, there are two versions of the algorithm: one based on a special segregated
solver, and one based on a fully coupled solver. In the first case, a segregated solver
must be used. Place all structural mechanics degrees of freedom except the contact
variables in one segregated step. The contact variables should remain in the lumped
step, which should appear directly after the step with the other mechanical degrees
of freedom.
• If there are other types of physics interfaces than structural mechanics being solved
in the same study, then the segregated solver should usually be kept. Make sure that
all structural mechanics degrees of freedom except segregated contact variables are
solved in one segregated step.
In the COMSOL Multiphysics Reference Manual:
• Solution Operation Nodes and Solvers
• About the Stationary Solver
366 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Using Reduced Integration
Using reduced integration in structural mechanics often have two main justifications:
• Reduce the per mesh element computational effort for assembly of system matrices.
• Improve the accuracy of the finite element by, for example, alleviating locking and
an overly stiff behavior.
The reduced computational effort stems from the fewer quadrature points in which
expressions are evaluated during the assembly of the system matrices. This reduction
can be particularly beneficial for models where a comparably large time is spent in
assembly, as compared to the time needed to solve the system of equations. Typical
examples include structural dynamics where the many increments can lead to a
significant time spent on assembling, and nonlinear material models where each
assembly step can be expensive. Plasticity, for example, involves solving a system of
nonlinear equations at each quadrature point, thus reducing the number of quadrature
points can significantly speed up the assembly time.
Reduced integration can be used selectively for different material models within the
same physics interface.
DISPLACEMENT ORDER AND MESH ELEMENT TYPES
The accuracy and performance of finite elements derived using a reduced integration
scheme depends on both the shape order of the displacement field and on the mesh
element type. For some combinations, reduced integration will give “exact” results,
whereas other combinations may result in deformation modes that produce zero strain
energy — so-called spurious zero energy modes or hourglass modes. In the latter case,
stabilization is needed to suppress such unwanted modes of deformation.
Linear
Using a linear displacement shape order is typically not encouraged in structural
mechanics, since all mesh element types lead to a deficient formulation. The derived
finite elements can be considered overly stiff, especially when a coarse mesh is used.
This overly stiff behavior is commonly caused by shear-locking effects.
These deficiencies can be alleviated by using a reduced integration scheme, which for
linear shape order results in a quadrature order equal to zero. Having only a single
integration point per mesh element removes the shear locking for linear elements, and
it can significantly improve the accuracy in coarse meshes. However, the derived finite
elements exhibit severe hourglassing and require stabilization to be useful. An example
USING REDUCED INTEGRATION
|
367
of a two-dimensional bending problem is given in Figure 2-38, which shows the
performance of linear quadrilaterals using reduced integration with and without
stabilization. A so-called hourglass pattern emerges without stabilization making the
solution clearly not viable.
Figure 2-38: Two-dimensional bending example using a linear displacement field and
reduced integration with stabilization (left) and without it (right).
Using reduced integration for a linear displacement shape order can also remove
volumetric locking and improve the accuracy for incompressible materials, either with
or without a mixed formulation.
The derived finite elements are still sensitive to hourglassing even when stabilization is
used. It is therefore recommended to avoid singularities, since these can excite
hourglass modes and consequently be detrimental for features such as:
• Point and edge loads
• Point and edge constraints
Linear triangular and tetrahedral mesh elements exhibit poor accuracy when using
reduced integration, and are generally not recommended for such scheme.
For quadrilateral and brick mesh elements, the accuracy of the finite element and the
efficiency of the hourglass stabilization is best for mesh element with a good aspect
ratio and quality. The same applies to pyramid and wedge mesh elements.
Quadratic Serendipity
Finite elements derived using quadratic serendipity shape functions and reduced
integration in general have a less stiff behavior than their fully integrated counterparts.
The coarse mesh accuracy in terms of displacements can therefore be improved by
using reduced integration.
If the displacement field uses quadratic serendipity shape functions, any mesh element
leads to a finite element that has no hourglass modes, and therefore no stabilization is
368 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
needed when using reduced integration. For this reason, using quadratic serendipity
shape functions together with reduced integration can be a very efficient formulation.
In theory, there could appear hourglass modes, but these are suppressed when the
finite elements are assembled.
If Automatic hourglass stabilization is selected, no stabilization is added
when serendipity shape functions are used for the displacement field.
Quadratic Lagrange
Finite elements derived using quadratic Lagrange shape functions and reduced
integration in general have a less stiff behavior than their fully integrated counterpart.
The coarse mesh accuracy in terms of displacements can therefore be improved by
using reduced integration.
However, when using reduced integration some mesh element types may lead to finite
elements that exhibit hourglass modes, this is the case for quadrilaterals and bricks.
Although these finite elements are not as sensitive as their linear counterpart, they
require stabilization to be viable. Stabilization is also encouraged for mesh elements
that have deformation modes with a very small stiffness, such as pyramids and wedges.
Higher-Order Shape Functions
Higher-order shape functions share many characteristics with the corresponding
quadratic shape orders. That is, there is no need for stabilization when using
serendipity shape functions, whereas finite elements derived from Lagrange shape
functions will have hourglass modes that require stabilization.
Triangular and Tetrahedral Mesh Elements
Triangular and tetrahedral mesh elements are special cases for which the reduced
integration scheme is exact given that the corresponding mesh element is not
distorted. These mesh element types do not exhibit hourglass modes when using
reduced integration, and therefore stabilization is not needed. If the current mesh only
consists of such mesh element types, turning off the hourglass stabilization may
improve the performance of your model. The accuracy is not affected by enabling or
disabling stabilization, since the stabilization terms would evaluate to zero.
However, it is not recommended to use triangular or tetrahedral mesh elements in
combination with a linear displacement shape order.
USING REDUCED INTEGRATION
|
369
HOURGLASS STABILIZATION
A number of energy quantities are added that can be used to evaluate the amount of
hourglass stabilization energy introduced, and also to portrait parts of the model that
are prone to hourglassing. These include:
• <phys>.Wstb, a field showing the stabilization energy density. Note that values are
extrapolated from the true quadrature points.
• <phys>.Wstbavg, a mesh-element average of the variable <phys>.Wstb. This
variable is not available for layered shell features.
• <phys>.Wstb_tot, the total amount of stabilization energy in the model.
As a crude rule-of-thumb, the total stabilization energy should not be more than 5%
of the total strain energy in the model. If this is not the case, revise the model or use
full integration.
Always make sure that the obtained solution does not exhibit hourglassing when using
reduced integration with formulations prone to it. This is especially the case when the
displacement field is linear, since such finite elements can be particularly sensitive to
hourglassing.
370 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Result Presentation
In this section, some special postprocessing techniques that are particularly useful for
structural mechanics models are presented.
In this section:
• Local Orientations
• How an Expression Is Evaluated
• Quality Settings
• Gauss Point Evaluation
• Postprocessing of Eigenmodes
• Plotting Applied Loads
General principles for result presentation and how to work with the
features under Results in the Model Builder are provided in Results
Analysis and Plots in the COMSOL Multiphysics Reference Manual.
Local Orientations
Many stress and strain tensor components are available both in local and global
directions. Some examples are:
• solid.sxy — Cauchy stress with respect to the global spatial coordinate system
• solid.sl12 — Cauchy stress with respect to the local coordinate system of the
material.
• solid.SXY — Second Piola–Kirchhoff stress with respect to the global material
coordinate system
• solid.Sl12 — Second Piola–Kirchhoff stress with respect to the local coordinate
system of the material
• solid.eXY — Strain with respect to the global material coordinate system
• solid.el12 — the local coordinate system of the material
As can be seen, tensor component indices containing the names of a coordinate
directions has orientations along those axes. Components in local directions contain
the letter ‘l’ and numerical indices.
RESULT PRESENTATION
|
371
The local directions are defined by the coordinate system attached to a material model.
For most material models, you can select a local coordinate system in the Coordinate
System Selection section of its settings. The purpose of this selection is twofold:
• It provides the orientations along which orthotropic and anisotropic material data
are interpreted.
• It acts as the coordinate system in which the local stress and strain tensor
components are presented.
When the material is isotropic, you can utilize the local coordinate system just for the
second purpose. In this case, the results of the analysis itself are independent of the
selected coordinate system. It just provides a transformation to be utilized during
result evaluation. If you want to change the orientations for the local components of
the tensors, you do not have to solve the study again. Instead, you select the new
) for
coordinate system in the material model node, and then run Update Solution (
the study or studies where you want the new definition to be applied.
Updating a Solution in the COMSOL Multiphysics Reference Manual.
ADDING YOUR OWN TRANSFORMATIONS
If there are no suitable local coordinate system variables defined from the physics
interface itself, you can create your own transformations.
The easiest way of doing that is to use the Local System Results node, available in some
of the structural mechanics interfaces. Here, the input is just a local coordinate system.
A more general approach is to add a Vector Transform or Matrix Transform under
Definitions>Variable Utilities, depending on the type of object you are going to
transform.
These nodes provide a large degree of flexibility in defining various types of transforms,
but for a pure rotation into a new coordinate system, the settings are straightforward.
Do the following:
1 Add the local coordinate system in which the results are to be presented under
Definitions.
372 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
2 In the Input section, enter the components of the vector or tensor to be
transformed. In most cases, you can pick it using Replace Expression (
).
Some tensors within the structural mechanics interfaces do not contain an
intrinsic information about the associated coordinate system. This is in
particular true for those tensors labeled as ‘local’. When using them in the
Matrix Transform node, you must then manually select the coordinate
system for the input tensor.
3 In the Vector Transform or Matrix Transform node, select the local coordinate system
in the Output section. In the latter node, select it twice.
4 Select the domain where you want this transformation to be valid.
5 Often, you want to enter your own name for the transformed object in the Name
text field.
Figure 2-39: Example of settings for transforming the displacement vector to a cylindrical
coordinate system.
RESULT PRESENTATION
|
373
If you define the transformation after the study was solved, you will need to run Update
Solution (
) for the study or studies where you want to access the transformed
variables.
You can now access the new transformed quantities for various type of result
presentation. They are accessible under Definitions in the Replace Expression dialog.
Figure 2-40: Picking a transformed result in the Replace Expression dialog.
Vector Transform and Matrix Transform in the COMSOL Multiphysics
Reference Manual.
How an Expression Is Evaluated
In order to get optimal quality in the result presentation, it is necessary to have some
understanding about how expressions are evaluated.
In structural engineering, the maybe most commonly evaluated result quantities are
stresses and strains. Stress expressions can, however, be sensitive to specific settings
during result presentation, and are for this reason used as an example in the discussion
below.
374 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Consider a linear elastic material with thermal expansion and creep. The stress tensor
 is then computed as
 =  ex + C  el =  ex + C    –  inel 
where C is the 4th-order elasticity tensor, “:” stands for the double-dot tensor product
(double contraction). The elastic strain el is the difference between the total strain 
and all inelastic strains inel. In this example, the inelastic strain tensor has two
contributions, creep strain cr and thermal strain th. There may also be an extra stress
term ex with contributions from initial stress and external stress.
When a stress tensor component is to be evaluated, the following happens:
• A position x in an element is identified, where the value is to be computed.
• The total strain is computed from the derivatives of the shape functions at x. The
strain depends on the values of the displacement degrees of freedom at the nodes
and on the shape functions in the element.
• The expression giving the thermal strain th is evaluated at x. This expression will
depend on a temperature, which may be prescribed or computed in another physics
interface.
• The creep strain cr is a state variable, which is stored at the Gauss points in the
element. The value is picked from the Gauss point closest to x.
• The inelastic strain inel (in this example, the creep strains is now subtracted from
the total strains, to form the elastic strain el.
• The elastic strain el is multiplied by the elasticity tensor C , evaluated at x, to give
the stress . The material properties may depend on the location, either explicitly,
or for example by a temperature dependency.
• Any extra stress ex, evaluated at x, is added to the stress tensor.
The subtraction between total and inelastic strains is however a sensitive operation. It
is not uncommon that these two terms are close to each other in value, so that the
resulting elastic strain is a small number obtained by subtraction of two larger
numbers. Since the three types of strain in this example have different types of
distribution through the element, there is a risk that this difference will exhibit artificial
variations inside the element.
As an example, let’s assume that the temperature has a quadratic variation through the
element, and that standard quadratic shape functions are used in Solid Mechanics. The
total strain is a linear function within each element, since it contains derivatives of the
shape functions. The computed elastic strain is the difference between the linear total
RESULT PRESENTATION
|
375
strain and the quadratic thermal strain. If there also are creep strains present, they will
be piecewise constant, since they are taken from the nearest integration point.
It must, moreover, be realized that the total strain is ‘correct’ only in an average sense.
It provides a kind of best fit given by the finite element formulation.
Quality Settings
In many features under Results, such as surface plots and line graphs, there is a section
named Quality, through which details of how the results are computed can be specified.
In some situations, you need to modify these settings to obtain optimal accuracy or
visually attractive presentations.
First, it can be noticed that stresses, strains, and any other variables that are based on
derivatives of the shape functions are not continuous over element borders. The
Smoothing control is used for improving plots by applying an averaging between
neighboring elements. The default when you add a result feature is to use smoothing,
and this will in general improve the results. It does however also hide any jumps in the
solution, which could indicate a too low resolution in the mesh. As soon as you are
investigating the quality of the solution, it is a recommended to avoid smoothing. In
the default stress plots that are generated by the structural mechanics interfaces, an
intermediate path is taken: the Smoothing threshold is set to Manual, with the Threshold
value set to 0.2. This means that as long as the values from adjacent elements do not
differ by more than 20%, smoothing is applied. If, however, there are significant jumps
in the solution, they will be clearly visible.
The Resolution setting determines at how many points in the element the result
quantity is evaluated. Essentially, a local finer mesh is used within the element for the
visualization. Using a high resolution can be problematic and lead to local overshoots
and artificial ‘waviness’ of the solution. For smooth expressions, like a stress in the
absence of inelastic strains or a displacement, this is not a problem. If, however, the
function has sudden variations within the element, a high resolution will give results
having artificial variations.
The default resolution depends on several factors, but will generally result in that a
result quantity is evaluated in a rather large number of points in the element. In
addition to affecting plot quality, having a high resolution can make the plotting
significantly slower.
Using a low resolution will remove the sudden variations, but may still not be an
optimal choice. If you set the quality to No refinement, the expression is evaluated only
376 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
at the corners of the element. This is, for example, rather far from the Gauss points
where many types of inelastic strains are stored. Also, a thermal strain with a quadratic
distribution will be rather far from its best linear approximation at the element corners.
The most robust solution if you encounter this type of problems it to create a
low-order field that approximates the “wavy” expression over the element, as described
in the next section.
Entering Quality Settings for Plot Settings Windows in the COMSOL
Multiphysics Reference Manual.
Gauss Point Evaluation
You can create a smooth field within each element for any expression by using the
gpeval() operator. In its most basic version, this operator has the following syntax:
gpeval(integration_order, expression).
For a general description of the gpeval() operator, see gpeval in the
COMSOL Multiphysics Reference Manual.
The gpeval() operator evaluates an expression at a given set of Gauss points and
creates an approximate smooth field using the least squares fit. It is important to use
the correct integration order to accurately evaluate state variables stored at Gauss
points, as in the case with many nonlinear material models. For example, when
quadratic shape functions are used with full integration, the first argument to the
gpeval() operator should be 4.
The physics interfaces define built-in variables with Gauss point evaluation for many
variables, including stress and strain. As an example, the built-in variable solid.sGpxx
is equivalent to using the expression gpeval(4,solid.sxx). Another example is
solid.misesGp. However, similarly using gpeval(4,solid.mises) can lead to
unphysical negative values caused by the extrapolation done by the operator. Hence,
for a variable that is strictly positive, one should use
RESULT PRESENTATION
|
377
max(0,gpeval(4,solid.mises)) or similar expressions; this is done for all relevant
built-in variables with Gauss point evaluation.
When adding predefined quantities (Add/Insert/Replace Expression or
Ctrl+Space) to an expression field, some variables including stress and
strain are presented with different definitions depending on where in the
model tree you are working.
• When modeling in the physics interfaces, or generally under Definitions,
the standard definition of variables is presented.
• When working under Results, the Gauss point evaluation definition of
variables is presented.
The variables that are visible in a certain context can be controlled using
) dialog.
the Show All Variables check boxes in the Show More Options (
When working with surface plots in a 3D geometry, or with line graphs in 2D and 3D,
there is a subtle difference between the built-in variables and the operator syntax. The
built-in variables are defined in the domain, and the field is projected from the domain
to be evaluated on boundaries and edges. If, however, you type in the operator syntax
as an expression in a line graph, the field is created only on that line, using only Gauss
points on the element edges. In order to avoid this, create domain variables under
Definitions>Variables using the operator syntax, and then use them on boundaries or
edges. Another alternative is to use the mean() operator, which evaluates any
expression in adjacent entities of higher order. For example, to evaluate a domain
variable in different plots in 3D, use the following syntax:
• Surface plot: mean(gpeval(integration_order, expr))
• Line graph: mean(mean(gpeval(integration_order, expr)))
• Point graph: mean(mean(mean(gpeval(integration_order, expr))))
There are also built-in operators that can be used specifically for evaluating domain
variables in any type of plot. Their syntax is summarized in Table 2-21. These operators
also automatically set the integration order to be consistent with its parent physics
378 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
interface <phys>, as opposed to the corresponding general operators. Also, for
example, reduced integration is taken into account.
TABLE 2-21: SUMMARY OF OPERATORS FOR EVALUATION EXPRESSION IN GAUSS POINTS OF DOMAIN MESH
ELEMENTS.
OPERATOR SYNTAX
EXPLANATION
<phys>.elemavg(expr)
Elementwise average in domain mesh
elements
<phys>.elemgpmax(expr)
Elementwise maximum over Gauss points in
domain mesh elements
<phys>.elemgpmin(expr)
Elementwise minimum over Gauss points in
domain mesh elements
<phys>.elemint(expr)
Elementwise integration in domain mesh
elements
<phys>.gpeval(expr)
Elementwise Gauss point evaluation in
domain mesh elements
Postprocessing of Eigenmodes
EIGENMODE SCALING
The eigenmodes that form the solution to eigenvalue problems, like eigenfrequency
and linear buckling, have some special properties that require attention. The most
important property is that an eigenmode is only defined up to an arbitrary
multiplicative factor. Thus, the actual values of the modal displacements have no
physical significance. In order to emphasize this, the default eigenmode plots have no
color legend.
The underlying theory does, however, assume that the mode shape is an infinitesimal
perturbation to the geometric shape.
If the eigenmodes have an unfortunate scaling, confusing effects can appear during
postprocessing:
• Any variable or expression used during postprocessing of an eigenvalue solution will
be evaluated using the setting of the Include geometric nonlinearity check box of the
eigenfrequency study step. If the values of the modal displacements are large and the
study step is geometrically nonlinear, then the nonlinear parts of the strain tensor
may become large. This is not consistent with the assumption of a small
perturbation.
RESULT PRESENTATION
|
379
• If the study step is geometrically linear, there can be other types if inconsistencies if
the modal displacements are large. Many variables are then defined under the
assumption that angles are small. As an example, the normal vectors to a shell can
appear to no longer have unit length.
• Rotational degrees of freedom scale the same way as the displacements. Computed
rotations can potentially get values of more than a full revolution.
In most cases, you only have to be aware of these phenomena. But if you really need
to access quantitative values (for example, as modal stresses), you need to use some
caution.
In a response spectrum analysis, all result quantities are computed by
scaling the modal results. In this case, it is necessary that all eigenmodes
are scaled so that the assumptions of geometric linearity are fulfilled.
The scaling of eigenmodes can be controlled in the Output section in the settings for
the Eigenvalue Solver node. By setting Scaling of Eigenvectors to Maximum and using a
small value for the Maximum absolute value, you can force the eigenmodes to be small.
All structural mechanics interfaces override the default value and set it to 10-6 times
the size of the bounding box of the geometry in order to keep the eigenmode
displacements small.
DEFORMATION PLOT ARTIFACTS
The automatic scaling of a deformation plot can give strange impressions, in particular
when the main deformation shape is a rotation. The geometry then seems to become
380 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
wider, since the displacements are directed in the infinitesimal tangential direction
rather than along a circular path.
Figure 2-41: A torsional eigenmode in a box beam.
EIGENMODES IN A DEFORMED STRUCTURE
When you perform a prestressed eigenvalue analysis, it is possible that the prestress
load case causes a significant deformation to the structure. The default eigenmode plot
will still show the mode relative to the original undeformed structure. Sometimes this
does not give a good enough representation of actual mode shape.
To improve the visualization, do the following:
1 Go to the settings for the 2D or 3D plot group containing the mode shape plot.
Under Plot dataset edges, set Frame to Spatial. This will make the outline to be given
by the deformed shape from the prestress load case.
2 In the dataset for the eigenvalue solution, set Frame to Spatial. The mode shapes are
now plotted relative to the deformed shape.
Plotting Applied Loads
When solving, predefined plots containing the applied loads are generated. You can
add them from the Add Predefined Plots window. Figure 2-42 shows an example of such
RESULT PRESENTATION
|
381
a plot. In this section, it is described in detail how you can work with these plots to
fine-tune the visualization.
Figure 2-42: Example of an automatically generated plot to visualize the boundary loads
applied to a bracket.
STRUCTURE OF DEFAULT LOAD PLOTS
For each structural mechanics physics interface and dataset, a node group is generated
under Results. Its name is Applied Loads (<interfaceTag>). Within this node group, one
plot group per type of load is created. The possible plot group names are listed in
Table 2-22.
TABLE 2-22: PLOT GROUP NAMES AND PLOT TYPES.
382 |
LOAD GROUP NAME
PLOT TYPE
DESCRIPTION
Volume Loads
Arrow Volume,
Arrow Surface,
Arrow Line,
Arrow Point
Generated from Body Load, Gravity, Linearly
Accelerated Frame, and Rotating Frame. The
plot type depends on the geometrical
dimension of the physics interface.
Boundary Loads
Arrow Surface
Generated from Boundary Load. Also, from
Added Mass on a boundary combined with
Gravity or Rotating Frame.
Face Loads
Arrow Surface
Generated from Face Load in Shell, Plate, and
Membrane interfaces.
Face Moments
Arrow Surface
Generated from Face Load in Shell, Plate, and
Membrane interfaces of nonzero moments are
present.
CHAPTER 2: STRUCTURAL MECHANICS MODELING
TABLE 2-22: PLOT GROUP NAMES AND PLOT TYPES.
LOAD GROUP NAME
PLOT TYPE
DESCRIPTION
Edge Loads
Arrow Line
Generated from Edge Load. Also, from Added
Mass on an edge combined with Gravity or
Rotating Frame.
Edge Moments
Arrow Line
Generated from Edge Load in Shell, Plate, and
Beam interfaces if nonzero moments are
present.
Point Loads
Arrow Point
Generated from Point Load.
Point Moments
Arrow Point
Generated from Point Load in Shell, Plate, and
Beam interfaces if nonzero moments are
present.
Global Loads,
Global Moments
Point
Trajectories
Generated from global features like Rigid
Connector and Rigid Material, which have
subnodes as Applied Load and Applied Moment.
Such loads are a type of point load, but they are
applied at a certain location in space, rather
than at a point in the geometry.
Fluid Loads
(Pressure)
Line
Generated from Fluid Load in Pipe Mechanics
interface.
Fluid Loads
(Drag Force)
Arrow Line
Generated from Fluid Load in Pipe Mechanics
interface.
In general, load groups are generated as soon as there is load of a certain type,
irrespective of whether the value of the load is nonzero or not. Load features in which
it is possible to enter both a force and a moment contribution, such as Edge Load in the
Beam interface, have a special behavior:
• A plot group for forces is always generated.
• A plot group for moments is only generated if there is a nonzero value in at least
one of the components of the moment vector.
Within a load group, there is one plot per load feature. In most cases, the plot has the
same label as the generating load feature, for example Boundary Load 2.
MODIFYING THE VISUALIZATION
The default appearance of the load plots provides a good overall visualization of the
loads applied to the model. However, for complex models or for creating plots for
export, you might want to modify the default setting. Most default settings are
presented in the following together with some prepared alternative settings and
suggestions that you can make use of. While the plots are automatically generated, you
RESULT PRESENTATION
|
383
can modify them in any way you want to improve the visualization for your specific
model; the plots are not reset each time you compute the study.
Style Inheritance
Within a load group, the style of each load plot is inherited from the previous plot. The
inheritance can be modified in the Inherit Style section. For example, clear the Color
check box to enable different color schemes for different loads and the Color and data
range to allow different ranges of the color legends.
Filled Surfaces
In order not to hide any load arrows, the default is to use a transparent representation
of the geometry. This is obtained through the extra surface plot Gray Surfaces together
with a Transparency subnode. This plot adds a uniform gray surface on each boundary
of the geometry. The effect is shown in Figure 2-42. If you disable the Gray Surfaces
plot, the structure will have a wireframe outline only. You can modify the transparency
level in the Transparency subnode, or delete the node completely. You can,
furthermore, add a Selection subnode to the Gray Surfaces node to modify on which
boundaries to plot the gray surface.
The Gray Surfaces plot is only generated for physics that use a 2D or 3D representation
of the geometry.
Arrow Heads
You can change the attachment of the arrow by changing the setting of Arrow base in
the Coloring and Style section. The default is in most cases to place the tail on the
geometry. One exception is, for example, a pressure boundary load for which the head
of the arrow is placed at the geometry.
Number of Arrows
For distributed fields, the default is to place one arrow at the center of each element,
element face, or element edge. If the density of arrows is not appropriate, you can
modify the settings in the Arrow Positioning section. For example, change Placement to
Mesh nodes to place an arrow in each point of the linear mesh, or set it to Uniform to
specify an arbitrary number of arrows to be plotted.
Color Scheme
The color scheme of the arrow plots is controlled in a Color Expression subnode. The
default color table is a Gradient going from red to black. You can change this in the
Coloring list. By selecting Color table, the color table is automatically set to Spectrum.
This color table can be useful for a clear visualization of the applied loads, when, for
example, the magnitude varies significantly between load features.
384 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
Deformation
By default, the load plots are presented in the initial configuration of the model.
However, when applicable, a Deformation subnode is added to each plot, but with the
Scale factor set to zero. Modify the scale factor to view the loads in a deformed state.
Note that when multiple load plots exist in a plot group, the scale factor is by default
inherited from the first plot. The exception is the Gray Surfaces plot, where the scale
factor is set independently of the other plots.
When the analysis includes geometric nonlinearities, the Scale factor is by default set to
one. Hence, the loads are presented in the deformed configuration for such cases.
• Under geometric nonlinearity, the size of the boundary load arrows
will scale with the local area deformation. Thus, a constant pressure
may appear as nonconstant.
• Load plots that make use of a Point Trajectories node include the
displacements explicitly in order to visualize the current position of the
load.
USING LOAD PLOTS DURING PREPROCESSING
The automatically generated plots of the applied loads can be useful during
preprocessing, for example to verify that loads are applied on the correct boundary and
in the intended direction. To generate the load plots before computing the study,
right-click the Study node, and select Get Initial Value, see Computing the Initial
Values. Doing so will generate all default and predefined plots requested by the
currently active features in all physics interfaces active in the study. You can then insert
the plot from the Add Plot window.
Note that plots are only generated the first time a dataset is created, which means that
the settings will not be updated for subsequent computation of the solution.
Moreover, load plots will not be generated for load features that are added after the
creation of the dataset. To generate new plots when new load features have been
added, delete the current load plots. Then compute the solution or do the Get Initial
Value, and insert the new load plots from the Add Plot window.
RESULT PRESENTATION
|
385
Part Libraries
The Part Libraries can be used to store and access a set of standard geometric entities.
It is possible to create custom user-defined geometry libraries or to use built-in
collections of geometric entities that are available with many add-on modules for
COMSOL Multiphysics.
A dedicated part library for the Structural Mechanics Module is included. The library
consists of two main parts:
• Bolts, nuts, and washers. These are parts intended for quick modeling of fasteners.
The bolts geometries are prepared for use with the Modeling Pretensioned Bolts
functionality. Some of the bolt geometries are also augmented with an extra domain
intended for use as a “drill” when building the geometry.
Figure 2-43: Example of a bolt part.
• Beam cross sections. These are 2D geometries, primarily intended for use in The
Beam Cross Section Interface. The library includes geometries for all standard beam
386 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
cross sections according to European and US standards, as well as generic beam
geometries.
Figure 2-44: Example of a standard beam cross section.
Figure 2-45: Example of a generic beam cross section.
PART LIBRARIES
|
387
All entities in the built-in the Part Libraries are fully parameterized, making them easy
to use as parts in large-scale industrial models.
Part Libraries in the COMSOL Multiphysics Reference Manual.
388 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
P a r a m e te r E s t i mat i on
Hyperelastic components like seals, insulators, soft sensors, and actuators frequently
exhibit a nonlinear stress-strain response. Viscoelastic models for rubber and soft
biological tissues display strain-rate sensitivity and hysteresis during cyclic loading.
Likewise, metals and alloys demonstrate ratcheting and nonlinear responses under
cyclic loading. To ensure precise predictions of these components’ behavior, it is
imperative to calibrate nonlinear material models using an extensive dataset of
experimental results.
With the Nonlinear Structural Materials Module, you can calibrate the model
parameters of any built-in and user-defined material model to experimental data using
nonlinear least-squares Parameter Estimation techniques. The Parameter Estimation
functionality is available in COMSOL Multiphysics in the context menu of a
Component or under Optimization in the Physics toolbar. Each Global Least-Squares
Objective subnode adds an objective function Q to the model, which is of the form
N
1
Q = --2
1
ˆ
 ----s2-  P  pi q  – Pi 
2
(2-42)
i=1 i
Herein, pi represents an experimental parameter (for example, applied stretch or time),
ˆ is the corresponding experimental value (for example, measured stress), and P(p ,
P
i
i
q) is the corresponding model prediction. The quantity si is a scale that weighs the
terms in the objective function and ensures that Q is dimensionless.
The model expression P normally depends implicitly on the model parameters q
through the solution of the forward problem. To solve the inverse problem, the
forward model and the objectives need to be combined with a study containing a
Parameter Estimation study step. When multiple objectives are selected in the study
step, the total objective function that is minimized is the sum of all the objective
functions selected. During the parameter estimation study, the forward problem will
be solved multiple times for different values of the model parameters, so it is good
practice to first set up and test the forward model before running a parameter
estimation study.
Three optimization solvers are available with the Nonlinear Structural Materials
Module in the Parameter Estimation study step: the derivative-free BOBYQA solver, and
the gradient-based IPOPT and Levenberg–Marquardt solvers. To avoid finding
PARAMETER ESTIMATION
|
389
unphysical regions in the parameter space, it is possible to specify bounds on the
parameters. For most least-squares problems, the default Levenberg–Marquardt
algorithm with a finite difference approximation of the Jacobian is a robust and
efficient choice of optimization solver.
By default, the Levenberg–Marquardt solver is set to terminate if either the increment
of the (scaled) parameters or the maximum angle between the error vector and the
Jacobian is smaller than a given optimality tolerance (default to 1e-3). In the settings
of the Optimization Solver, it is possible to include an additional termination criterion
based on the relative change of the objective function by selecting the Terminate also
for defect reduction check box, which can be useful if the solver reaches a relatively flat
local minimum in the parameter space. The default termination criteria are normally
more robust, however.
To monitor the progress of the optimization visually, is it possible to set up a plot while
solving that compares the current model prediction with the experimental data.
For further information about the Parameter Estimation functionality and
the optimization solvers, see
• Parameter Estimation and Global Least-Squares Objective in the
Optimization Module User’s Guide.
• The Parameter Estimation Study in the Optimization Module User’s
Guide.
• The Levenberg–Marquardt Solver in the Optimization Module User’s
Guide.
For examples showing how to set up a parameter estimation study, see
• Parameter Estimation of Hyperelastic Materials: Application Library
path Nonlinear_Structural_Materials_Module/Hyperelasticity/
parameter_estimation_hyperelasticity.
• Parameter Estimation of Elastoplastic Materials: Application Library
path Nonlinear_Structural_Materials_Module/Plasticity/
parameter_estimation_plasticity.
• Parameter Estimation of Viscoplastic Polymers: Application Library
path Nonlinear_Structural_Materials_Module/Viscoplasticity/
parameter_estimation_polymer_viscoplasticity.
390 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
PARAMETER ESTIMATION
|
391
392 |
CHAPTER 2: STRUCTURAL MECHANICS MODELING
3
Structural Mechanics Theory
This chapter contains the theory behind the implementation of the structural
mechanics functionality in COMSOL Multiphysics.
In this chapter:
• Solid Mechanics Theory
• Frames and Coordinate Systems
• Analysis of Deformation
• Stresses
• Equation of Motion
• Material Models
• Formulation of the Equilibrium Equations
• Study Types
• Damping
• Loads and Constraints
• Contact Analysis Theory
• Bolt Modeling Theory
• Stress Linearization
393
• J-Integral Theory
• Embedded Elements
• Thin Layers
• Enclosed Fluids
• Reduced Integration and Hourglass Stabilization
• Average Rotation
• Warpage
• Energy Quantities
394 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
S o li d M e c ha ni cs Th eory
Introduction
In the following, the theory for the Solid Mechanics interface is described. To a large
extent, this theory covers other structural mechanics physics interfaces, such as Shell
and Beam, which are included with the Structural Mechanics Module. For these other
interfaces, only the details which are specific to the interface are described in its
additional documentation.
• Theory for the Shell and Plate Interfaces
• Theory for the Membrane Interface
• Theory for the Beam Interface
• Theory for the Beam Cross Section Interface
• Theory for the Truss Interface
TENSOR NOTATION
Some of the theory is developed using tensor notation. In most cases, explicit index
notation is avoided. This means that the order of a tensor usually must be understood
from the context. As an example, Hooke’s law for linear elasticity is usually written like
 = C :
Here, the stress tensor  and the strain tensor  are second-order tensors, while the
constitutive tensor C is a fourth-order tensor. The ‘:’ symbol means a contraction over
two indices. In a notation where the indices are shown, the same equation would read
 ij = C ijkl  kl
where the Einstein summation convention has been used as a shorthand for
3
 ij =
3
  Cijkl kl
k = 1l = 1
In a few cases, nonorthonormal coordinate systems must be considered. It is then
necessary to keep track of the covariance and contravariance properties of tensors. In
such a case, Hooke’s law is written
SOLID MECHANICS THEORY
|
395

ij
= C
ijkl
 kl
The stress and constitutive tensors have contravariant components, while the strain
tensor has covariant components.
396 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
Frames and Coordinate Systems
In this section:
• Material and Spatial Coordinates
• Coordinate Systems
Material and Spatial Coordinates
The Solid Mechanics interface, through its equations, describes the motion and
deformation of solid objects in a 1-, 2-, or 3-dimensional space. In COMSOL
Multiphysics terminology, this physical space is known as the spatial frame, and
positions in the physical space are identified by lowercase spatial coordinate variables
x, y, and z (or r, , and z in axisymmetric components).
Continuum mechanics theory also makes use of a second set of coordinates, known as
material (or reference) coordinates. These are normally denoted by uppercase
variables X, Y, and Z (or R, , and Z) and are used to label material particles. Any
material particle is uniquely identified by its position in some given initial or reference
configuration. As long as the solid stays in this configuration, material and spatial
coordinates of every particle coincide and displacements are zero by definition.
More information can be found in About Frames chapter in the COMSOL
Multiphysics Reference Manual.
When the solid object deforms due to external or internal forces and constraints, each
material particle keeps its material coordinates X (bold font is used to denote
coordinate vectors), while its spatial coordinates change with time and applied forces
such that it follows a path
x = x  X t  = X + u  X t 
(3-1)
in space. Because the material coordinates are constant, the current spatial position is
uniquely determined by the displacement vector u, pointing from the reference
position to the current position. The global Cartesian components of this displacement
vector in the spatial frame, by default called u, v, and w, are the primary dependent
variables in the Solid Mechanics interface.
By default, the Solid Mechanics interface uses the calculated displacement and
Equation 3-1 to define the difference between spatial coordinates x and material
FRAMES AND COORDINATE SYSTEMS
|
397
coordinates X. This means the material coordinates relate to the original geometry,
while the spatial coordinates are solution dependent.
Material coordinate variables X, Y, and Z must be used in coordinate-dependent
expressions that refer to positions in the original geometry, for example, for material
properties that are supposed to follow the material during deformation. On the other
hand, quantities that have a coordinate dependence in physical space — for example, a
spatially varying electromagnetic field acting as a force on the solid — must be
described using spatial coordinate variables x, y, and z.
In a geometrically linear analysis, no difference is made between the two
coordinate systems. For this case, the material and spatial coordinates
coincide. This may seem inconsistent with equation Equation 3-1 but
ensures linearity for problems that are expected to be linear. It is then, for
example, equivalent to choose a coordinate system related to the material
frame or one related to the spatial frame. In a geometrically nonlinear
analysis, however, any use of a spatial coordinate in an expression will
introduce a nonlinear contribution because it will be deformation
dependent.
Coordinate Systems
Force vectors, stress and strain tensors, as well as various material tensors are
represented by their components in a specified coordinate system. By default, material
properties use the canonical system in the material frame. This is the system whose
basis vectors coincide with the X, Y, and Z axes. When the solid deforms, these vectors
rotate with the material.
Loads and constraints, on the other hand, are applied in spatial directions, by default
in the canonical spatial coordinate system. This system has basis vectors in the x, y, and
z directions, which are forever fixed in space. Both the material and spatial default
coordinate system are referred to as the global coordinate system in the physics
interface.
398 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
Vector and tensor quantities defined in the global coordinate system on either frame
use the frame’s coordinate variable names as indices in the tensor component variable
names.
For example, solid.SXY is the material frame XY-plane shear stress, also
known as a second Piola–Kirchhoff stress, while solid.sxy is the
corresponding spatial frame stress, or Cauchy stress. There are also a few
mixed tensors, most notably the deformation gradient solid.FdxY,
which has one spatial and one material index because it is used in
converting quantities between the material and spatial frames.
It is possible to define any number of user coordinate systems on the material and
spatial frames. Most types of coordinate systems are specified only as a rotation of the
basis with respect to the canonical basis in the underlying frame. This means that they
can be used both in contexts requiring a material system and in contexts requiring a
spatial one. A coordinate system defined on the spatial frame will in general introduce
nonlinearities in the problem, since its directions are deformation dependent in case of
a geometrically nonlinear analysis.
The coordinate system can be selected separately for each added material model, load,
and constraint. This is convenient when for example, an anisotropic material with
different orientation in different domains is required. The currently selected
coordinate system is called the local coordinate system.
Coordinate systems used for describing a material must be defined on the material
frame.
Boundary System
Many quantities for shells, membranes, and thin layers can best be interpreted in a local
coordinate system aligned to the surface. Material data, initial stresses and stress results
are always represented in this local coordinate system. The local system for stress
output coincides with the orientations defined for the material input.
When a Boundary System is selected, the orientation of the local system is fully defined
by the boundary system.
When using a boundary system, it also possible to control the orientation of the
normal by selecting the Reverse normal direction check box.
FRAMES AND COORDINATE SYSTEMS
|
399
Analysis of Deformation
The analysis of deformation aims at deriving descriptions of the local deformation in a
material suitable for use in a constitutive relation. Often, but not always, this amounts
to deriving a strain tensor.
This section starts by a general description of finite deformation in solids. At the end,
the specialization to engineering strains used in geometrically linear analysis, is made.
In this section:
• Lagrangian Formulation
• Deformation Measures
• Invariants of Strain
• Inelastic Strain Contributions
• Deformed Geometry
• Axial Symmetry
• Plane Strain
• Generalized Plane Strain
Lagrangian Formulation
The formulation used for structural analysis in COMSOL Multiphysics for both small
and finite deformations is a total Lagrangian formulation. This means that the
computed stress and deformation state is always referred to the material configuration
rather than to current position in space.
Likewise, material properties are always given for material particles and with tensor
components referring to a coordinate system based on the material frame. This has the
obvious advantage that spatially varying material properties can be evaluated just once
for the initial material configuration, and they do not change as the solid deforms and
rotates.
Consider a certain physical particle, initially located at the coordinate X. During
deformation, this particle follows a path
x = x  X t 
Here, x is the spatial coordinate and X is the material coordinate.
400 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
For simplicity, assume that undeformed and deformed positions are measured in the
same coordinate system. Using the displacement u it is then possible to write
x = X + u  X t 
The displacement is considered as a function of the material coordinates (X, Y, Z), but
it is not explicitly a function of the spatial coordinates (x, y, z). It is thus only possible
to compute derivatives with respect to the material coordinates.
In the following, the gradient operator is assumed to be a gradient with respect to the
material coordinates, unless something else is explicitly stated.

= X
=
  
X Y Z
The gradient of the displacement, which occurs frequently in the following theory, is
always computed with respect to material coordinates. In 3D:
u u u
X Y Z
u = v v v
X Y Z
w w w
X Y Z
The deformation gradient tensor, F, shows how an infinitesimal line element, dX, is
mapped to the corresponding deformed line element dx by
ANALYSIS OF DEFORMATION
|
401
x
dx = ------- dX = F dX
X
The deformation gradient F contains the complete information about the local
straining and rotation of the material. It is a two-point tensor (or a double vector),
which transforms as a vector with respect to each of its indices. It involves both the
reference and present configurations.
In terms of the displacement gradient, F can be written as
x- = u + I
F = -----X
The deformation of the material (stretching) will in general cause changes in the
material density. The ratio between current and initial volume (or mass density) is
given by
dV = 
-----0- = det  F  = J
---------
dV 0
Here, 0 is the initial density and  is the current density after deformation. The
determinant of the deformation gradient tensor F is related to volumetric changes with
respect to the initial state. A pure rigid body displacement implies J  1. Also, an
incompressible material is represented by J  1. These are called isochoric processes.
The determinant of the deformation gradient tensor is always positive (since a negative
mass density is unphysical). The relation   0/J implies that for J  1 there is
compression, and for J  1 there is expansion. Since J  0, the deformation gradient
F is invertible.
In the material formulations used within the structural mechanics interfaces, the mass
density should in general be constant because the equations are formulated for fixed
material particles. Thus, do not use temperature-dependent material data for the mass
density. The changes in volume caused by temperature changes are incorporated using
the coefficient of thermal expansion when adding Thermal Expansion (for Materials)
to the material model.
The variable solid.rho represents a “reference” or “initial” density 0,
and not the “current” density . If you are interested in finding the
density of the deformed material (the density in the spatial frame), you
can compute it using the expression solid.rho/solid.J.
402 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
Deformation Measures
Since the deformation tensor F is a two-point tensor, it combines both spatial and
material frames. It is not symmetric. Applying a singular value decomposition on the
deformation gradient tensor gives an insight into how much stretch and rotation a unit
volume of material has been subjected to. The right polar decomposition is defined as
F = RU
where U is the right stretch tensor given in the material frame, and R is a proper
orthogonal tensor such that det(R) = 1 and R-1 = RT. The rotation tensor R describes
the rigid rotation, and all information about the deformation of the material is
contained in the symmetric tensor U.
• The internal variables for the deformation gradient tensor with respect
to global material coordinates are named solid.FdxX, solid.FdxY,
and so on.
• The internal variables for the deformation gradient tensor with respect
to local material coordinates are named solid.Fdx1, solid.Fdx2,
and so on.
• The rotation tensor components are named solid.RotxX,
solid.RotxY, and so on.
• The right stretch tensor components are named solid.UstchXX,
solid.UstchXY, and so on.
An uppercase index refers to the material frame, and a lowercase index
refers to the spatial frame.
The stretch tensor contains physically important information about the deformation
state. The eigenvalues of the U tensor are the principal stretches, 1, 2, and 3. The
stretch of a line element with initial length L0 and current length L is
L = 1+
 = -----eng
L0
where eng is the engineering strain. The three principal stretches act along three
orthogonal directions. In the coordinate system defined by these principal directions,
the U tensor will be diagonal:
ANALYSIS OF DEFORMATION
|
403
1 0 0
U =
0 2 0
0 0 3
The right Cauchy–Green deformation tensor C defined by
T
C = F F = U2
It is a symmetric and positive definite tensor, which accounts for the strain but not for
the rotation. The eigenvalues of the C tensor are the squared principal stretches, thus
providing a more efficient way to compute the principal stretches than by using the
stretch tensor U directly.
The Green–Lagrange strain tensor is a symmetric tensor defined as
1
1 T
 = ---  C – I  = ---  F F – I 
2
2
Since C is independent of rigid body rotations, this applies also to the Green–Lagrange
strain tensor.
Using the displacement components and Cartesian coordinates, the Green–Lagrange
strain tensor can be written on component form as
1  u u u k u k
 ij = ---  --------i + --------j + ---------  --------- .
2  X j X i X i X j 
(3-2)
The rotation independence of the Green–Lagrange strain tensor,
together with the fact that it for small strain approaches the engineering
strain tensor explains why it is a common choice in constitutive models
for small strain- finite rotation. As an opposite, a pure rigid rotation causes
strains when engineering strains are used.
The Green–Lagrange is the natural strain representation in a Lagrangian
description. Since it is a tensor in the material frame, its values should be
interpreted in along the undeformed axis orientations.
404 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
• The internal variables for the Green–Lagrange strains are named
solid.eX, solid.eXY, and so on.
• The internal variables for the Green–Lagrange strain tensor in local
coordinates are named solid.el11, solid.el12, and so on.
• In a geometrically linear analysis, the strain variables
solid.eX,solid.el11, and so on, will instead represent engineering
strain.
• The right Cauchy–Green deformation tensor in local coordinate
system are named solid.Cl11, solid.Cl12, and so on.
Some textbooks prefer to use the left Cauchy–Green deformation tensor
B  FFT, which is also symmetric and positive definite but it is defined in
the spatial frame.
ENGINEERING STRAIN
Under the assumption of small displacements and rotations, the normal strain
components and the shear strain components are related to the deformation as follows:
 y = v
y
 xy 1  u v
 xy = ------ = ---  + 
2 y x
2
 yz 1  v w
 yz = ------ = ---  + 
2 z y
2
 z = w
z
 xz 1  u w
+
- = -- xz = -----2 z x 
2
x =
u
x
(3-3)
In COMSOL Multiphysics, the tensor form of strain representation (xy, yz, xz) is
used.
In the documentation, the symbol is used to denote the strain tensor in
general. In a geometrically nonlinear analysis, strains should be
interpreted as a Green–Lagrange strains. In a geometrically linear analysis,
the engineering strain is used.
The symmetric strain tensor  consists of both normal and shear strain components:
ANALYSIS OF DEFORMATION
|
405
 x  xy  xz
 =  xy  y  yz
 xz  yz  z
The strain-displacement relationships for the axial symmetry case for small
displacements are
r =
u
,
r
u
  = --- ,
r
z =
w
, and
z
 rz = u + w
z r
A special problem occurs at the axis of rotation, where both u and r are zero. To avoid
dividing by zero, the circumferential strain is for very small values of r redefined to
 =
u
r
The alternative expression is obtained by applying L’Hôpital’s rule.
A general description of the axially symmetric case is given in Axial Symmetry.
LOGARITHMIC STRAIN
The logarithmic strain, also called true strain, or Hencky strain, is a popular strain
measure for large strain, in particular when representing data from tensile tests. For a
uniaxial case, it is defined on the incremental form
dL
d = -------L
where L is the current length of the specimen. If this relation is integrated, the total
strain can be written as
L
 = log  ------ = log 
L0
Here L0 is the initial length and  is the stretch.
In order to generalize the logarithmic strain to a strain tensor, it is necessary to first
compute the three principal stretches and their orientation. Then, a logarithmic strain
tensor in the local principal stretch system is defined as
406 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
 lp =
log  1
0
0
0
log  2
0
0
0
log  3
This tensor is then transformed to the global coordinate system in order to give the
logarithmic strain tensor.
Invariants of Strain
PRINCIPAL STRAINS
The principal strains are the eigenvalues of the strain tensor (), computed from the
eigenvalue equation
  –  p I v p = 0
The three principal strains are sorted so that
 p1   p2   p3
This sorting is true also for the 2D and 1D cases. The corresponding vectors in the
principal directions, vpi, are orthonormal.
• The internal variables for the principal strains are named solid.ep1,
solid.ep2, and solid.ep3.
• The internal variables for the components of the directions of the first
principal strains are named solid.ep1X, solid.ep1Y, and
solid.ep1Z. The direction vectors for the other two principal strains
are named analogously.
The Green–Lagrange strain tensor is used in a geometrically nonlinear
analysis. The orientations of the principal directions will thus be with
respect to the material directions. If you plot the principal strains as
arrows, you should thus use an undeformed plot.
PRINCIPAL STRETCHES
The principal stretches are the eigenvalues of the stretch tensor U, and are also sorted
by size:
ANALYSIS OF DEFORMATION
|
407
 p1   p2   p3
The internal variables for the principal stretches are named
solid.stchp1, solid.stchp2, and solid.stchp3. The elastic
principal stretches are named solid.stchelp1, solid.stchelp2, and
solid.stchelp3.
The different invariants of the strain tensor form are useful for constitutive modeling
and result interpretation. The three fundamental invariants for any tensor are
I 1    = trace   
1
2
2
I 2    = ---  trace    – trace    
2
I 3    = det   
The invariants of the strain deviator tensor are also useful:
1
dev    =  – --- trace   I
3
J 1    = trace  dev     = 0
2
1
1
J 2    = --- dev   :dev    = --- I 1    – I 2   
2
3
2
3 1
J 3    = det  dev     = ------ I 1    – --- I 1   I 2    + I 3   
27
3
As defined above J2  0. I1 represents the relative change in volume for infinitesimal
strains and J2 represents the magnitude of shear strain.
In tensor component notation, the invariants can be written as
trace    =  kk
 kk
dev    ij =  ij – --------  ij
3
1
I 2    = ---   ii  jj –  ij  ji 
2
1
J 2    = --- dev    ij dev    ji
2
The volumetric strain is defined as
408 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
 vol = trace   
and the equivalent deviatoric strain as
2
--- dev    ij dev    ji =
3
 deve =
4
--- J 2   
3
The internal variable for the volumetric strain is solid.evol. The
internal variables for the components of the deviatoric strain tensor in the
local coordinate system are solid.eldev11, and so on. The internal
variable for the equivalent deviatoric strain is solid.edeve.
In terms of the principal strains, the strain invariants can be written as
I 1    =  p1 +  p2 +  p3
I 2    =  p1  p2 +  p2  p3 +  p1  p3
I 3    =  p1  p2  p3
The principal strains are the roots of the characteristic equation (Cayley–Hamilton
theorem)
3
2
p – I1 p + I2 p – I3 = 0
STRAIN RATE AND SPIN
The spatial velocity gradient is defined in components as
L kl =
 v
 x t 
 xl k
where vk(x,t) is the spatial velocity field. It can be shown that L can be computed in
terms of the deformation gradient as
L =
dF – 1
F
dt
where the material time derivative is used.
The velocity gradient can be decomposed into symmetric and skew-symmetric parts
L = Ld + Lw
ANALYSIS OF DEFORMATION
|
409
where
1
T
L d = ---  L + L 
2
is called the rate of strain tensor, and
1
T
L w = ---  L – L 
2
is called the spin tensor. Both tensors are defined on the spatial frame.
It can be shown that the material time derivative of the Green–Lagrange strain tensor
can be related to the rate of strain tensor as
T
d
------ = F L d F
dt
The spin tensor Lw(x,t) accounts for an instantaneous local rigid-body rotation about
an axis passing through the point x.
Components of both Ld and Lw are available as results and analysis
variables under the Solid Mechanics interface.
• The components of the rate of strain tensor are named solid.Ldx,
solid.Ldxy, and so on.
• The components of the spin tensor are named solid.Lwx,
solid.Lwxy, and so on.
Inelastic Strain Contributions
Many of the material models in COMSOL Multiphysics will compute a stress based on
an elastic strain. The elastic strain tensor is obtained after removing any inelastic
deformation contribution from the total deformation from the displacements. There
are several possible inelastic strain contributions:
• Initial strain, 0
• External strain, ex
• Thermal strain, th
• Hygroscopic strain, hs
• Plastic strain, pl
410 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
• Creep strain, cr
• Viscoplastic strain, vp
• Viscoelastic strain, ve
ADDITIVE DECOMPOSITION
In a geometrically linear analysis, the elastic strain is computed by a straightforward
subtraction of the inelastic strain:
 e =  –  inel
where
 inel =  0 +  ex +  th +  hs +  pl +  cr +  vp +  ve
Additive decomposition of strains can also be used in a geometrically nonlinear
analysis. In this case, it can however only be justified as long as the strains are small. In
the case of large deformations, the different strain contributions may not even be
commutative.
Choose to use additive decomposition also for geometric nonlinearity by selecting the
Additive strain decomposition check box in the settings for Linear Elastic Material or
Nonlinear Elastic Material.
MULTIPLICATIVE DECOMPOSITION
In the finite deformation case, the inelastic strain is instead removed using a
multiplicative decomposition of the deformation gradient tensor. The elastic
deformation gradient tensor is the basis for all strain energy formulations in
hyperelastic materials, and also for the elastic strain in linear and nonlinear elasticity. It
is derived by removing the inelastic deformation from the total deformation gradient
tensor.
The total deformation gradient tensor is defined as the result of two successive
operations, an inelastic deformation followed by an elastic deformation:
ANALYSIS OF DEFORMATION
|
411
F = F el F inel
(3-4)
The order is important here, multiplication from the left makes the elastic
deformation act on the inelastically deformed state.
Since a deformation gradient tensor describes a mapping from one frame
to another, there are actually three frames involved in this operation. The
F tensor is defined by the displacements as usual and describes the
mapping from the material frame to the spatial frame. The Finel tensor,
however, describes a mapping from the material frame to an intermediate
frame, and the Fel tensor describes a mapping from the intermediate
frame to the spatial frame.
When the inelastic deformation gradient tensor is known, the elastic deformation
gradient tensor is computed as
–1
F el = FF inel
(3-5)
so the inelastic deformations are removed from the total deformation gradient tensor.
The inelastic deformation tensor Finel is derived from inelastic processes, such as
thermal expansion or plasticity. When there are several inelastic contributions, they are
applied sequentially to obtain the total inelastic deformation tensor Finel:
F inel = F 1 F 2 F 3 F 4 ...
where Fi is the inelastic strain contribution from subnode i under a Linear Elastic
Material, Nonlinear Elastic Material, or Hyperelastic Material.
• The order is important when deformations are finite. The
contributions are applied in the same order as the subnodes appear in
the model tree. If a Thermal Expansion node appears before a Plasticity
node, then the physical process can be viewed as a thermal expansion
followed by a plastic deformation.
• When a certain inelastic strain contribution is small, the order is not
significant.
• If the inelastic strain is a pure isotropic volume change, as is often the
case for thermal expansion and hygroscopic swelling, the order is not
significant.
412 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
The right Cauchy–Green deformation tensor C is computed from the deformation
gradient F, as well as the Green–Lagrange strain tensor 
T
1
C = F F and  = ---  C – I 
2
The elastic right Cauchy–Green deformation tensor is then computed from Fel
T
C el = F el F el
and the elastic Green–Lagrange strain tensor is computed as
1
 el = ---  C el – I 
2
The internal variables for the elastic right Cauchy–Green deformation
tensor in the local coordinate system are named solid.Cel11,
solid.Cel12, and so on; and for the elastic Green–Lagrange tensor in
local coordinates solid.eel11, solid.eel12, and so on.
The elastic, inelastic, and total volume ratios are related as
det  F  = det  F el det  F inel  or J = J el J inel
The internal variables for the elastic, inelastic, and total volume ratio are
named solid.Jel, solid.Ji, and solid.J.
After Equation 3-5, the elastic Green–Lagrange strain depends on the inelastic
deformation as
–1
–T
–1
1
1 –T
 el = ---  C el – I  = --- F inel  C – C inel F inel = F inel   –  inel F inel
2
2
(3-6)
where the inelastic Green–Lagrange strain reads
1 T
1
 inel = ---  C inel – I  = ---  F inel F inel – I 
2
2
When using multiplicative decomposition of deformation gradients, Hooke’s law for a
Linear Elastic Material produces a second Piola–Kirchhoff stress tensor which is
linearly related to the elastic Green–Lagrange strain
ANALYSIS OF DEFORMATION
|
413
S el = C  el
This is however, a stress tensor defined in the intermediate configuration. Introducing
a pull-back operation of this tensor, Hooke’s law for the multiplicative decomposition
of elastic and inelastic strains reads
–T
–1
S = J inel F inel C    –  inel F inel
Large Strain Plasticity
In case of large strain plasticity, the plastic strains are primarily not represented as
strains, but as the plastic deformation gradient tensor, Fpl.
The plastic Green–Lagrange strain tensor is computed from the plastic deformation
gradient tensor as
1 T
 pl = ---  F pl F pl – I 
2
As opposed to the small strain formulation, the total, plastic, and elastic Green–
Lagrange strain tensors are related through Equation 3-6 as follows:
–T
–1
 el = F pl   –  pl F pl
Deformed Geometry
The equations solved by the Solid Mechanics interface are formulated in the material
frame. The Deformed Geometry functionality in COMSOL Multiphysics allows one
to make the material frame differ from the geometry frame, which implies that the
geometry of the structure on the material frame can differ from that originally drawn.
This is useful for analyzing the behavior of different shapes of an original object, for
example as part of shape optimization.
In the COMSOL Multiphysics Reference Manual:
Deformed Geometry and Moving Mesh
By default, the material does not follow a change in shape. Deformation of the
geometric boundaries therefore corresponds to addition or removal of material.
The deformed geometry functionality can be also used to set up an incremental
deformation of a structure. This can be achieved by using the Elastic Predeformation
414 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
node in the Solid Mechanics interface. This can significantly speed up computations is
case of large deformations.
ELASTIC PREDEFORMATION
The total displacement field of the solid is represented as
u tot = u pd + u
and the corresponding deformation gradient is multiplicatively decomposed as
F tot = FF pd
One can use upd to define the displacement of the material frame with respect to the
geometry frame, and take u as an update solution of the equations solved by the Solid
Mechanics interface on the material frame. (The corresponding deformation gradient
F connects the material and spatial frames.) Note that the virtual work on such a
displacement update is done by the total stress, and to get the correct stress, one can
use as Fpd the deformation gradient connecting the geometry and material frames, and
then set the elastic deformation gradient to
F el = F tot
(3-7)
This is used in the stress calculation during the update step. Thus, the transformation
from geometry to material frame is assumed to be a result of elastic deformation.
The process can be repeated in a parametric sweep, for example, by gradually ramping
up the load, so that the displacement update on each step is small. During each step,
the previous value of the total displacement is used in the material frame definition
u pd = u tot, old
Alternatively, a time-dependent study can be used. In this situation, the above formula
will be applied during each time step to recompute upd before the step, using the
stored previous solution, while u will represent a displacement increment computed
during the time step. In addition, the density is updated as 0/Jpd where
J pd = det  F pd 
Again, Fpd is the deformation gradient connecting the geometry and material frames,
and it will be updated before each time step or parameter sweep value.
The approach can be combined with large strain plasticity. In this case,
ANALYSIS OF DEFORMATION
|
415
F tot = F el F pl
which together with Equation 3-7 gives
–1
F el = FF pd F pl
Note that both Fel and Fpl represent the total deformations of their corresponding
types, while Fpd is the total (elastic and plastic) deformation gradient from the previous
update.
Axial Symmetry
The 2D axisymmetric implementation in COMSOL Multiphysics by default assumes
independence of the azimuthal component of the displacement. Therefore, the
physical components of the radial and axial displacement, u and w, are used by default
as dependent variables for the axially symmetric geometry. It is also possible to include
the dependent variable v for the out-of-plane displacement, or an azimuthal mode
extension in time-harmonic studies. See Circumferential Displacement and
Circumferential Modes.
STRAINS
The displacement gradient with respect to the cylindrical coordinates of the
undeformed geometry reads
u --1- u v u
– ---R R  R Z
1- v u v
u = v --+ ---R R  R Z
w
R
1- w
--R 
w
Z
The assumption of axial symmetry neglect gradients in the azimuthal direction, so the
displacement vector is considered independent on the azimuthal angle, u = u(R, Z),
and
u   = v   = w   = 0 .
The displacement gradient after this assumption reads
416 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
u v u
– ---R R Z
u- v
u = v --R R Z
w
w
0
Z
R
and the Green–Lagrange strain tensor is
T
T
1
 = ---  u + u + u u 
2
Assuming that there is no torsion around the axis of symmetry, so there is no
out-of-plane displacement, v = 0, the deformation gradient can be further simplified
to read
u
u
0
Z
R
u
u = 0 ---- 0
R
w
w
0
R
Z
For geometrically linear analysis, the nonlinear terms in the Green–Lagrange strain
tensor are dropped
u
R
1 u w
+
0 --- 
2   Z  R
0
u--R
0
1
---  u + w 0
2   Z  R
w
Z
T
1
 = ---  u + u  =
2
and the volumetric strain is computed from
u- + w
 vol = I 1    = u + --R R Z
For the 1D axisymmetric representation, only the radial component of the
displacement field is computed, and only gradients with respect to the radial direction
are considered, this is, u = u(R), and u  uZ  0.
ANALYSIS OF DEFORMATION
|
417
CIRCUMFERENTIAL DISPLACEMENT
When the out-of-plane displacement is considered in a 2D axisymmetric model,
torsion is allowed with respect to the symmetry axis. In this case, the displacement
gradient reads
u v u
– ---R R Z
u- v
u = v --R R Z
w
w
0
Z
R
and the Green–Lagrange strain tensor is
T
T
1
 = ---  u + u + u u 
2
For geometrically linear analysis, the nonlinear terms in the Green–Lagrange strain
tensor are dropped
u
R
T
1
 = ---  u + u  =
2
1  v v  1  u w
--– ---- --+
2   R R 2   Z  R
1
v-
---  v – --2   R R
u--R
1
--- v
2 Z
1
---  u + w
2   Z  R
1
--- v
2Z
w
Z
and the volumetric strain is computed from
u- + w
 vol = I 1    = u + --R R Z
CIRCUMFERENTIAL MODES
A standard 2D axisymmetric representation of the structure assumes the independence
of the solution with respect to the azimuthal angle . The following 3D solution
represents an extension of this assumption:
u  R  Z t  = u 0  R Z  + u 1  R Z  exp  it – im 
418 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
where m is a circumferential mode number (or azimuthal mode number) that can
only have integer values to obey the axially symmetric nature of the corresponding 3D
problem, that is, there is an azimuthal symmetry  =  + 2. Thus,
u  R  + 2 Z t  = u  R  Z t 
The static prestress solution u0 can be obtained using a standard static analysis in 2D
axially symmetric geometry; and the circumferential wave number km  m/R can be
introduced to describe the circumferential modes.
The displacement vector u1 can have nonzero values in all three components, which
are functions of the radial and axial positions. For a given circumferential mode
number m, the displacement vector u1 can be found using an eigenfrequency analysis
in a 2D axisymmetric geometry. Hence,
 = 2f
f = f  m u 0 
and the perturbation solution becomes
u 1 = u 1  R Z  exp  2if  m u 0 t – im 
The solution u = u0 + u1 represents eigenmodes in the corresponding 3D structure,
which can be computed assuming certain constraints on the axis and possible static
prestress and independent of the position along the axis.
Plane Strain
For two-dimensional problems, there are tree possible approximations: plane strain,
Generalized Plane Strain, and Plane Stress. The selection is made in the settings for the
Solid Mechanics node.
For plane strain, the deformation occurs in the xy-plane and it is fully characterized by
the in-plane displacement components u(X,Y) and v(X,Y). There is no out-of-plane
displacement, w = 0, and there are only in-plane strains. In this case, the displacement
gradient reads
ANALYSIS OF DEFORMATION
|
419
u u
u =  X  Y
v v
X Y
and the strain tensor ij  ij X Y only has in-plane components:
 =
 x  xy
 xy  y
For the 1D plane strain representation, only the x-component of the displacement field
is computed, and only gradients with respect to the x direction are considered, this is,
u = u(X), uY  uZ  0, and xy  y  0.
Generalized Plane Strain
One possible extension of the Plane Strain formulation is to assume that the
displacement field depends on the out-of-plane coordinate Z, but in-plane strains are
independent of it.
The above assumption have the following 3D solution for the displacement field:
a 2
u = u 0  X Y  – --- Z
2
b
2
v = v 0  X Y  – --- Z
2
w =  aX + bY + c Z
here, u0(X,Y) and v0(X,Y) are the in-plane displacement components; and a, b, and c
are constants independent of the X, Y, and Z coordinates. The gradient of the
displacement field then reads:
u 0 u 0
X Y
– aZ
u = v v
0
0
– bZ
X Y
aZ bZ aX + bY + c
420 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
At the cross section Z = 0, the in-plane deformation is fully characterized by the
in-plane displacement components u0(X,Y) and v0(X,Y). The displacement gradient
then simplifies to
u 0 u 0
X Y
0
u = v v
0
0
0
X Y
0 0 aX + bY + c
The out-of-plane shear strains are zero, xz  yz  0, and under the assumption of
small displacements and rotations the normal strain reads
 z = ax + by + c
(3-8)
The above conditions differ from the Plane Strain formulation only by the fact that the
out-of-plane strain component z can vary linearly throughout the cross section.
The generalized plane strain approximation is good when the structure is free to
expand in the out-of-plane direction, and the possible bending curvature is small with
respect to the extents of the structure in the xy-plane. In the case where there is no
out-of-plane bending, the out-of-plane strain component simplifies to z  c.
In COMSOL Multiphysics, the coefficients a, b, and c in Equation 3-8 are modeled
as extra degrees of freedom that are constant throughout the model (global variables).
For the 1D representation, only the x-component of the displacement field is
considered, and only gradients with respect to this direction are computed, this is,
u = u(X), uY  uZ  0, and xy  y  0. It is possible to apply the generalized
plane strain assumption to either the xy-plane, the xz-plane, or to both planes, in which
case the strain components are augmented to y  b and z  c.
For the 1D axisymmetric representation, only the radial component of the
displacement field is considered, and only gradients with respect to this direction are
computed, this is, u  u(R), and u  uZ  0. It is possible to apply the
generalized plane strain assumption to the r-plane, so the strain is augmented to
z  c.
GEOMETRIC NONLINEARITY
In case of geometric nonlinearity, the strains are represented by the Green–Lagrange
strain tensor:
ANALYSIS OF DEFORMATION
|
421
1
 = ---  u T + u + u T u 
2
Consider the following displacement field expressed in terms of the material
coordinates:
a 2
u  X Y  – --- Z
2
u=
2
b
v  X Y  – --- Z
2
 a  X + u  + b  Y + v  + c Z
Coefficients a, b, and c are assumed to be small. Then, using the above displacement
field in the displacement gradient evaluated in the plane Z = 0 simplifies to
u u
X Y
0
u = v v
0
X Y
0 0 aX + u  + bY + v + c
We obtain the strain components by dropping quadratic and higher order terms in the
coefficients a, b, and c:
2
1 2
 XX = u X + ---  u X + v X 
2
2
1 2
 YY = v Y + ---  u Y + v Y 
2
1
 XY = ---  u Y + v X + u X u Y + v X v Y 
2
 XZ =  YZ = 0
 ZZ = a  X + u  + b  Y + v  + c
Thus, in the leading order approximation, the strains become independent of the
out-of-plane coordinate Z.
OUT-OF-PLANE WAVES
When a 2D plane strain model represents a cross-section of the structure that has a
significant uniform extension in the out-of-plane Z direction, the following 3D
solution can be sought in form of the amplitude expansion:
422 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
u  X Y Z t  = u 0  X Y  + u 1  X Y  exp  it – ik Z Z 
The first term, u0, represents a static in-plane prestress deformation:
u 0  X Y 
u 0 = v  X Y 
0
0
This can be obtained by a standard static analysis using a 2D geometry for the cross
section with the corresponding boundary conditions.
The second part of the solution, u1, presents a time-harmonic linear perturbation with
an amplitude that can be a function of the in-plane coordinates X and Y. Such a
perturbation can be seen as an out-of-plane wave, with a small amplitude that
propagates in the Z direction, a wavelength L, and phase velocity c:
k Z = 2  L
c =   kZ
2i
u 1 = u 1  X Y  exp ---------  ct – Z 
L
Note that in contrast to the prestress solution u0, the perturbation amplitude u1 can
have nonzero values in all the displacement components:
u 1  X Y 
u1 =
v 1  X Y 
w 1  X Y 
There are two alternative approaches. The wavelength L, and thus the wave number
kZ, can be considered as a parameter. Then,  can be computed by an eigenfrequency
analysis for the 2D cross section with all three displacement components taken as
dependent variables. As a result, one obtains
 = 2f
f = f  L u 0 
c   u 0  = Lf  L u 0 
ANALYSIS OF DEFORMATION
|
423
Thus, the wave speed for the out-of-plane wave is computed as a function of the
wavelength L and possible prestress u0 in the material. The dependence of the wave
speed on the wavelength is often called dispersion.
Alternatively, the frequency f (and thus can be taken as a parameter. Then, the
solution can be computed via eigenvalue analysis with respect to the wave number kZ
using the 2D cross section geometry. Hence,
k Z = 2  L
L = L  f u 0 
c  f u 0  = fL  f u 0 
which determine the wavelength L and phase velocity c for the wave that propagates
out-of-plane for a given frequency f under given in-plane prestress deformation u0.
Such interpretation of the perturbation solution is sometimes called a signaling
problem.
424 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
Stresses
In this section:
• Defining Stress
• Invariants of the Stress Tensor
• Plane Stress
• Initial Stresses and Strains
• Axial Symmetry and Stresses
Defining Stress
This section summarizes the definition of different stress measures, stress invariants,
and other important definitions.
Three different stress measures are used in COMSOL Multiphysics:
• Cauchy stress defined as force/deformed area in fixed spatial directions not
following the body. This is a symmetric tensor.
• First Piola–Kirchhoff stress P. The forces in the spatial directions are related to the
area in the original (material) frame. This is an unsymmetric two-point tensor.
• Second Piola–Kirchhoff stress S. Both force and area are represented in the material
configuration. For small strains the values are the same as Cauchy stress tensor but
the directions are rotating with the body. This is a symmetric tensor.
The stresses relate to each other as
–1
S = F P
–1
 = J PF
T
–1
= J FSF
T
In a geometrically linear analysis, the distinction between the stress measures disappear,
and they all converge to the same values.
In the documentation, the symbol is used to denote not only Cauchy
stress, but stress in general. The symbols P and S are used whenever it is
necessary to make a distinction. In geometrically nonlinear analysis, the
stress should in general be interpreted as second Piola–Kirchhoff stress.
STRESSES
|
425
• The internal variables for the Cauchy stresses are named solid.sx,
solid.sxy, and so on.
• The internal variables for the first Piola–Kirchhoff stresses are named
solid.PxX, solid.PxY, and so on.
• The internal variables for the second Piola–Kirchhoff stresses are
named solid.SX, solid.SXY, and so on.
SIGN CONVENTIONS
A positive normal stress in COMSOL Multiphysics acts in tension. This is the most
widely used definition in general physics and engineering.
Within the field of geomechanics it is however common to let compressive stresses be
positive, since compression is almost always dominant in that field of science. When
working with the material models intended for soils and rocks, you must be aware of
that the “positive in tension” convention is used also there in order to maintain
consistency within the software.
Specifically, the ordering of Principal Stresses is such that p1  p2  p3 (including
signs). In geotechnical applications the dominant principal stresses will usually be
compressive, so the third principal stress will the be the one which you may consider
as “largest”.
The convention used in Ref. 1 refers to the hydrostatic pressure (trace of the stress
Cauchy tensor) with a positive sign. The use of the first invariant of Cauchy stress
tensor I1() is preferred in this document where there is a risk of confusion. The
pressure in COMSOL Multiphysics is always defined as positive under compression, or
equivalently, it has the opposite sign of the Cauchy stress tensor’s trace.
Invariants of the Stress Tensor
The different invariants of the stress tensor form an important basis for constitutive
models and also for interpretation of stress results. The three fundamental invariants
for any tensor are
I 1    = trace   
2
2
1
I 2    = ---  trace    – trace    
2
I 3    = det   
426 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
(3-9)
In many cases, the invariants of the deviatoric stress tensor are also useful.
1
dev    =  – --- trace   I
3
J 1    = trace  dev     = 0
2
1
1
J 2    = --- dev   :dev    = --- I 1    – I 2   
2
3
2
3 1
J 3    = det  dev     = ------ I 1    – --- I 1   I 2    + I 3   
27
3
(3-10)
As defined above J2  0. In many material models, the most relevant invariants are I1,
J2, and J3. I1 represents the effect of mean stress, J2 represents the magnitude of shear
stress, and J3 contains information about the direction of the shear stress.
In tensor component notation, the invariants can be written as
trace    =  kk
 kk
dev    ij =  ij – ---------  ij
3
1
I 2    = ---   ii  jj –  ij  ji 
2
1
J 2    = --- dev    ij dev    ji
2
The pressure is defined as
I1   
trace   - = –---------------p = –----------------------3
3
and is thus positive in compression.
• The internal variables for the invariants I1, I2, and I3 are named
solid.I1s, solid.I2s, and solid.I3s, respectively.
• The internal variables for the invariants J2 and J3 are named
solid.II2s and solid.II3s, respectively.
• The internal variable for the pressure is solid.pm.
PRINCIPAL STRESSES
The principal stresses are the eigenvalues of the stress tensor, computed from the
eigenvalue equation.
STRESSES
|
427
  –  p I v p = 0
The three principal stresses are ordered so that
 p1   p2   p3
This ordering is true also for the 2D cases. The corresponding principal directions vpi
are orthonormal.
• The internal variables for the principal stresses are named solid.sp1,
solid.sp2, and solid.sp3.
• The internal variables for the components of the directions of the first
principal stress are named solid.sp1x, solid.sp1y, and
solid.sp1z. The direction vectors for the other two principal stresses
are named analogously.
In terms of the principal stresses, the stress invariants can be written as
I 1    =  p1 +  p2 +  p3
I 2    =  p1  p2 +  p2  p3 +  p1  p3
I 3    =  p1  p2  p3
The principal stresses are the roots of the characteristic equation (Cayley–Hamilton
theorem)
3
2
p – I1 p + I2 p – I3 = 0
OTHER STRESS INVARIANTS
It is possible to define other invariants in terms of the primary invariants. One common
auxiliary invariant is the Lode angle 
3 3 J3 cos 3 = -----------  ----------2 J3  2
2
(3-11)
The Lode angle is bounded to 0    3 when the principal stresses are sorted as
p1  p2  p3 (Ref. 1).
Following this convention,  = corresponds to the tensile meridian, and  = 3
corresponds to the compressive meridian. The Lode angle is part of a cylindrical
428 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
coordinate system (the Haigh–Westergaard coordinates) with height (hydrostatic
axis)  = I 1 / 3 and radius r = 2J 2 .
The Lode angle is undefined at the hydrostatic axis, where all three
principal stresses are equal (p1 = p2 = p3 = I1/3) and J2 = 0. To avoid
division by zero, the Lode angle is actually computed from the inverse
tangent function atan2, instead of the inverse cosine, as stated in
Equation 3-11.
The Lode angle and the equivalent (von Mises) stress can be called in user
defined yield criteria by referencing the variables solid.thetaL and
solid.mises, where solid is the name of the physics interface node.
The octahedral plane (also called -plane) is defined perpendicular to the hydrostatic
axis in the Haigh–Westergaard coordinate system. The stress normal to this plane is
oct = I1/3, and the shear stress on that plane is defined by
 oct =
2/3J 2
The functions described in Equation 3-9 and Equation 3-10 enter into expressions
that define various kind of yield and failure surfaces. A yield surface is a surface in the
3D space of principal stresses that circumscribe an elastic state of stress.
The principal stresses p1, p2, and p3) can, when sorted as p1  p2  p3, be
written by using the invariants I1 and J2 and the Lode angle (Ref. 1):
4J
1
 p1 = --- I 1 + ---------2- cos 
3
3
4J
1
 p2 = --- I 1 + ---------2- cos   – 2
------

3
3
3
4J
1
2
 p3 = --- I 1 + ---------2- cos   + -----
3
3
3
Plane Stress
For two-dimensional problems, there are tree possible approximations: Plane Strain,
Generalized Plane Strain, and plane stress. The selection is made in the settings for the
Solid Mechanics node.
STRESSES
|
429
In the plane stress formulation in COMSOL Multiphysics, the plane stress conditions
 zz =  xz =  yz = 0
(3-12)
are not enforced through a modified constitutive relation, as is common in many
textbooks. Instead, an extra set of degrees of freedom for the out-of-plane strains are
introduced, and Equation 3-12 is enforced by solving for the strains.
For a general anisotropic linear elastic material in case of plane stress, COMSOL
Multiphysics solves three equations. For isotropy and orthotropy, only one extra
degree of freedom is needed since the out-of-plane shear components of the stress
tensor are zero.
• For isotropic and orthotropic materials, the extra degree of freedom is
named wZ, and represents w  Z .
• For anisotropic materials in 3D or 2D, two more degrees of freedom
area added, uZ and vZ. They represent u  Z and v  Z .
Initial Stresses and Strains
Initial stresses and strains refer to a stress and strain state that would exist even without
the external loads. Initial stresses and strains are not initial values in the mathematical
sense. They apply all through the solution, and may even vary with time or solution
parameters. They should rather be considered as an offset to the stress and strain state
in the constitutive relation.
The initial strain is subtracted from the total strain, before the constitutive law is
applied for computing the stresses. The initial stress is added to the stress computed by
using the constitutive law. As an example, linear elasticity including both an initial
strain 0 and an initial stress s0 can be written as
s = s 0 + C    –  0 
It can also be noted that the effect of the initial strain is analogous to, for example, a
thermal strain or other inelastic strain contributions.
Use either the initial strain or the initial stress (but not both) when you have results
from another analysis or another physics interface, which you want to incorporate into
the stress-strain relation.
430 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
Both the initial stress and strain are tensor variables defined via components in the local
coordinate system for each domain.
In case of nearly incompressible material (mixed formulation), the components of the
total initial stress (that is, without volumetric-deviatoric split) are still input. The initial
pressure in the equation for the pressure help variable pw is computed as
1
p 0 = – --- I 1  s 0 
3
In the case of geometric nonlinearity, the initial stress represents the second Piola–
Kirchhoff stress, not the Cauchy stress. The initial strain is interpreted as a Green–
Lagrange strain.
OTHER POSSIBLE USES OF INITIAL STRAINS AND STRESSES
Many inelastic effects in solids mechanics (for example creep, plasticity, damping,
viscoelasticity, poroelasticity, and so on) are represented by additive contributions to
either the total strain or total stress. Then the initial value input fields can be used for
coupling the elastic equations (solid mechanics) to the constitutive equations (usually
General Form PDEs) modeling such extra effects. When adding stress contributions,
you may however find it more convenient to use the External Stress concept.
The Initial Stress and Strain node can be added to Linear Elastic Material, Nonlinear
Elastic Materials, Piezoelectricity, Elastoplastic Soil Models, Magnetostriction and
Piezomagnetism, or Shape Memory Alloy materials.
External Stress
The external stress represents an additional stress contribution which has a source
other than the constitutive relation. It is similar to the initial stress described in Initial
Stresses and Strains, and the two features can be used interchangeably. As an example,
linear elasticity including an external stress ext can be written as
 =  ext + C 
(3-13)
This additive contribution is the default option when adding external stresses to either
the material representation (second Piola–Kirchhoff stress) or spatial representation
(Cauchy stress).
It is also possible to prescribe a stress contribution that only acts as a load on the
structure, but that is not added into the stress tensor definition as described in
Equation 3-13. The typical case is when there is a pore pressure in a porous material,
STRESSES
|
431
a common case in geotechnical engineering. The stress carried by the solid material
excluding the pore pressure is often called the effective stress. The load from the pore
pressure helps to balance the external loads, while not contributing to the stress tensor
of the solid. The contribution to the virtual work of the external stress (load) is then
W =
V – ext dv
(3-14)
With the External Stress feature it is also possible to model residual stresses due to, for
instance, manufacturing processes. The Residual stress option augments the stress
tensor as defined in Equation 3-13, and it also removes the deformation created from
it by applying an external load with opposite sign, as described in Equation 3-14. In
this way there is no induced deformation in the solid, but the definition of the stress
tensor and its invariants are augmented, which has an impact in plasticity, creep, or
viscoplasticity.
When External Stress (Nominal) is selected, the external stress tensor does not have to
by symmetric, thus the contribution of the external stress acts as an external load, to
the virtual work is
W =
V –u Pext dv
IN SITU STRESS
The in situ stress is a common residual stress used in geotechnical engineering. The
vertical stress, v, also called overburden pressure, lithostatic pressure, or confining
pressure, represents the stress in a point given by the weight of the overlaying material.
 v = gD
The elevation D is the distance of a point in the soil to the top boundary, is the
density and g the acceleration of gravity. This analytical expression for the vertical stress
is derived for a slab of soil of infinite lateral extension.
The lateral or horizontal stress h is normally given as a factor or the vertical stress
h = k0 v
The factor k0, called the coefficient of lateral earth pressure, is normally computed
from the angle of internal friction, from the Poisson’s ratio, or more complex formulas.
When the z-axis represents the vertical coordinate, the in situ stress tensor is written as
432 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
h
 ins =
h
v
The External Stress subnode can be added to Linear Elastic Material, Nonlinear Elastic
Materials, Elastoplastic Soil Models, Shape Memory Alloy, or Hyperelastic Materials.
External Strain
The external strain represents an inelastic strain contribution which has a source other
than the elastic deformation. It is similar to the initial strain described in Initial Stresses
and Strains, and the two features can be used interchangeably. As an example, linear
elasticity including an external strain ext can be written as
 = C  el with  el =  –  ext
(3-15)
This Additive Decomposition of strains,  =  el +  ext , is the default option when
adding external strains to represent either the second Piola–Kirchhoff stress or the
Cauchy stress.
It is possible to prescribe a large external strain contribution that follows a
Multiplicative Decomposition of the deformation gradient tensor. In this case, the
elastic deformation gradient reads
–1
F el = FF ext
(3-16)
Enter the external deformation gradient, F ext , the external stretches in the local
–1
coordinate system,  ext , or the inverse deformation gradient, F ext . The external
strain can also be computed by Using External Materials.
The External Strain subnode can be added to Linear Elastic Material, Nonlinear Elastic
Materials, Shape Memory Alloy, or Hyperelastic Materials.
See also
• Using External Materials
• External Material and Working with External Materials in the
COMSOL Multiphysics Reference Manual.
STRESSES
|
433
Axial Symmetry and Stresses
The physical stress components are defined on the global coordinate system:
r = 
11
2 22
 = r 
z = 
33
 rz = 
13
The first invariant of the stress tensor is
I1    =
   gij  = r +  + z
ij
i j
434 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
E qua ti o n o f M ot i on
The first Piola–Kirchhoff stress P is calculated from the second Piola–Kirchhoff stress
as P  FS. The first Piola–Kirchhoff stress relates forces in the present configuration
with areas in the reference configuration, and it is sometimes called the nominal stress.
Using the first Piola–Kirchhoff stress tensor, the equation of motion can be written in
the following form:
2
0
 u
t
2
T
= X  P + FV
(3-17)
where the density corresponds to the material density in the initial undeformed state,
the volume force vector FV has components in the actual configuration but given with
respect to the undeformed volume, and the tensor divergence operator is computed
with respect to the coordinates on the material frame. Equation 3-17 is the strong
form that corresponds to the weak form equations within the Solid Mechanics
interface (and many related multiphysics interfaces) in COMSOL Multiphysics. Using
vector and tensor components, the equation can be written as
2
0
 ux
t
2
2
0
 uy
t
2
2
0
 uz
t
2
= 
P xX P xY P xZ
+
+
+ F Vx
X
Y
Z 
P
P
P
=  yX + yY + yZ + F Vy
X
Y
Z 
P
P
P
=  zX + zY + zZ + F Vz
X
Y
Z 
The components of the first Piola–Kirchhoff stress tensor are nonsymmetric in the
general case, thus
P iJ  P Ij
because the component indices correspond to different frames.
The boundary load vector FA in case of geometric nonlinearity can be related to the
first Piola–Kirchhoff stress tensor via the following formula:
EQUATION OF MOTION
|
435
F A = Pn 0
where the normal n0 corresponds to the undeformed surface element. This force
vector is often referred to as the nominal traction. In components, it can be written as
F Ax = P xX n X + P xY n Y + P xZ n Z
F Ay = P yX n X + P yY n Y + P yZ n Z
F Az = P zX n X + P zY n Y + P zZ n Z
The Cauchy stress, ,can be calculated as
–1
 = J PF
T
–1
= J FSF
T
The Cauchy stress is a true stress that relates forces in the present configuration (spatial
frame) to areas in the present configuration, and it is a symmetric tensor.
Equation 3-17 can be rewritten in terms of the Cauchy stress as
2

 u
t
2
= x   + fV
where the density corresponds to the density in the actual deformed state, the volume
force vector fV has components in the actual configuration (spatial frame) given with
respect to the deformed volume, and the divergence operator is computed with respect
to the spatial coordinates.
The pressure is computed as
p = –1
--- trace   
3
which corresponds to the volumetric part of the Cauchy stress, and it is positive in
compression. The deviatoric part is defined as
 d =  + pI
The second invariant of the deviatoric stress
1
J 2    = ---  d : d
2
is used for the computation of von Mises (equivalent) stress
436 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
 mises =
3J 2   
EQUATION OF MOTION
|
437
Material Models
There are many material models available for structural analysis in COMSOL
Multiphysics. In this section, the theory for all material models is presented. The
material models available, and also some detailed aspects of them, depend on which
licenses you have. The material models, grouped by families, are as follows:
• Linear Elastic Material
• Nonlinear Elastic Materials
- Ramberg–Osgood
- Power Law
- Bilinear Elastic
- Uniaxial Data
- Shear Data
- Hyperbolic Law
- Hardin–Drnevich
- Duncan–Chang
- Duncan–Selig
- Small Strain Overlay
- User Defined
• Linear Viscoelasticity
- The Maxwell Model
- The Generalized Maxwell Model
- The Kelvin–Voigt Model
- The Generalized Kelvin–Voigt Model
- Standard Linear Solid Model
- The Burgers Model
- Generalized Maxwell Model with Fractional Derivatives
- Generalized Kelvin–Voigt Model with Fractional Derivatives
- Standard Linear Solid Model with Fractional Derivatives
- Burgers Model with Fractional Derivatives
- User Defined
438 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
• Hyperelastic Materials
- Neo-Hookean
- St Venant–Kirchhoff
- Mooney–Rivlin, Two Parameters
- Mooney–Rivlin, Five Parameters
- Mooney–Rivlin, Nine Parameters
- Yeoh
- Ogden
- Storakers
- Varga
- Arruda–Boyce
- Gent
- van der Waals
- Blatz–Ko
- Gao
- Murnaghan
- Delfino
- Fung
- Extended Tube
- User Defined
- Mullins Effect
• Distributed Fiber Models
• Elastoplastic Materials
- The von Mises Criterion
- The Tresca Criterion
- Orthotropic Plasticity
MATERIAL MODELS
|
439
• Porous Plasticity
- The Shima–Oyane Criterion
- The Gurson Criterion
- The Gurson–Tvergaard–Needleman Criterion
- The Fleck–Kuhn–McMeeking Criterion
- The FKM–GTN Criterion
- Capped Drucker–Prager
• Soil Plasticity
- The Mohr–Coulomb Criterion
- The Drucker–Prager Criterion
- The Matsuoka–Nakai Criterion
- The Lade–Duncan Criterion
• Failure Criteria for Concrete and Rocks
- The Bresler–Pister Yield Criterion
- The Willam–Warnke Criterion
- The Ottosen Criterion
- The Original Hoek–Brown Criterion
- The Generalized Hoek–Brown Criterion
• Damage Models
• Coupled Damage–Plasticity
• Elastoplastic Soil Models
- The Modified Cam-Clay Soil Model
- The Modified Structured Cam-Clay Soil Model
- The Extended Barcelona Basic Soil Model
- The Hardening Soil Model
- The Hardening Soil Small Strain Model
• Creep and Viscoplasticity
- Creep
- Viscoplasticity
- Creep and Viscoplasticity for Large Strains
440 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
• Inelastic Strain Rate
• Shape Memory Alloy
• Piezoelectricity
• Magnetomechanics
• Magnetostriction and Piezomagnetism
• Electrostriction
• Ferroelectroelasticity
• Rigid Material
• Safety Factor Evaluation
You can also add a material model which you have coded yourself and made available
as a binary library file using an External Stress-Strain Relation.
In the COMSOL Multiphysics Reference Manual:
• Working with External Materials
• External Material
Linear Elastic Material
For a linear elastic material, Hooke’s law relates the stress tensor to the elastic strain
tensor:
 =  ex + C  el =  ex + C    –  inel 
(3-18)
where C is the 4th order elasticity tensor, “:” stands for the double-dot tensor product
(or double contraction). The elastic strain el is the difference between the total strain
 and all inelastic strains inel. There may also be an extra stress contribution ex with
contributions from initial stresses and viscoelastic stresses. In case of geometric
nonlinearity, the second Piola–Kirchhoff stress tensor and the Green–Lagrange strain
tensor are used.
The elastic strain energy density is
1
1
W s = ---  el   C  el + 2 0  = ---  el    +  0 
2
2
(3-19)
MATERIAL MODELS
|
441
This expression assumes that the initial stress contribution is constant during the
straining of the material.
TENSOR VS. MATRIX FORMULATIONS
Because of the symmetry, the strain tensor can be written as the following matrix:
 x  xy  xz
 xy  y  yz
 xz  yz  z
A similar representation applies to the stress tensor:
 x  xy  xz
 xy  y  yz
 xz  yz  z
Due to the symmetry, the elasticity tensor can be completely represented by a
symmetric 6-by-6 matrix as:
D =
D 11 D 12 D 13 D 14 D 15 D 16
C
D 12 D 22 D 23 D 24 D 25 D 26
C
D 13 D 23 D 33 D 34 D 35 D 36
= C
D 14 D 24 D 34 D 44 D 45 D 46
C
D 15 D 25 D 35 D 45 D 55 D 56
C
D 16 D 26 D 36 D 46 D 56 D 66
C
1111
1122
1133
1112
1123
1113
C
C
C
C
C
C
1122
2222
2233
2212
2223
2213
which is the elasticity matrix.
ISOTROPIC MATERIAL AND ELASTIC MODULI
In this case, the elasticity matrix becomes
442 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
C
C
C
C
C
C
1133
2233
3333
3312
3323
3313
C
C
C
C
C
C
1112
2212
3312
1212
1223
1213
C
C
C
C
C
C
1123
2223
3323
1223
2323
2313
C
C
C
C
C
C
1113
2213
3313
1213
2313
1313
1– 

 1– 

 1–
E
D = -------------------------------------- 1 +    1 – 2 
0
0
0
1 – 2--------------2
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
1 – 2--------------2
0
0
0
0
0
0
1
– 2--------------2
(3-20)
Different pairs of elastic moduli can be used, and as long as two moduli are defined,
the others can be computed according to Table 3-1.
TABLE 3-1: EXPRESSIONS FOR THE ELASTIC MODULI.
DESCRIPTION
VARIABLE
DE
DEG
DKG
D
Young’s
modulus
E=
E
E
9KG -----------------3K + G
3 + 2
 -------------------+
Poisson’s
ratio
=

E- – 1
------2G
1
3K – 2G--- --------------------2 3K + G
 -------------------2 + 
Bulk
modulus
K=
E ----------------------3  1 – 2 
EG -------------------------3  3G – E 
K
 + 2
------3
Shear
modulus
G=
E -------------------21 + 
G
G

Lamé
parameter 
=
E
-------------------------------------- 1 +    1 – 2 
G  E – 2G 
---------------------------3G – E
2G
K – -------3
Lamé
parameter 
=
E -------------------21 + 
G
G
Pressurewave speed
cp =
E  1 –   - --------------------------G  4G – E ----------------------------------------  1 +    1 – 2    3G – E 
Shear-wave
speed
cs =
E -----------------------2  1 +  
G


K
+ 4G  3------------------------
 + 2
---------------
G

According to Table 3-1, the elasticity matrix D for isotropic materials is written in
terms of Lamé parameters  and ,
MATERIAL MODELS
|
443
 + 2


0 0 0

 + 2

0 0 0



+
2
0 0 0
D =
0
0
0
 0 0
0
0
0
0  0
0
0
0
0 0 
(3-21)
or in terms of the bulk modulus K and shear modulus G:
K + 4G
-------- K – 2G
-------- K – 2G
-------- 0 0 0
3
3
3
2G
4G
2G
K – -------- K + -------- K – -------- 0 0 0
3
3
3
D =
2G
2G
4G
K – -------- K – -------- K + -------- 0 0 0
3
3
3
0
0
0
G 0 0
0
0
0
0 G 0
0
0
0
0 0 G
(3-22)
ORTHOTROPIC AND ANISOTROPIC MATERIALS
There are two different ways to represent orthotropic or anisotropic data. The
Standard (11, 22, 33, 12, 23, 13) material data ordering converts the indices as:
11
1
x
22
2
y
33  3  z
12 21
4
xy
23 32
5
yz
13 31
6
xz
thus, Hooke’s law is presented in the form involving the elasticity matrix D and the
following vectors:
444 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
x
x
y
y
z
 xy
=
z
 xy
 yz
 yz
 xz
 xz
ex
 x
x

 y
y

 z
z
–
+ D
 2 xy
2 xy

2
2 yz

yz

2 xz
 2 xz











inel
COMSOL Multiphysics uses the complete tensor representation internally to perform
the coordinate system transformations correctly.
Beside the Standard (11, 22, 33, 12, 23, 13) Material data ordering, the elasticity
coefficients can be entered following the Voigt notation. In the Voigt (11, 22, 33, 23,
13, 12) Material data ordering, the sorting of indices is:
11
1
x
2
y
22
33  3  z
4
yz
23 32
13 31
5
xz
12 21
6
xy
The last three rows and columns in the elasticity matrix D are thus swapped.
Orthotropic Material
The elasticity matrix for orthotropic materials in the Standard (11, 22, 33, 12, 23, 13)
Material data ordering has the following structure:
D =
D 11 D 12 D 13 0
0
0
D 12 D 22 D 23 0
0
0
D 13 D 23 D 33 0
0
0
0 D 44 0
0
0
0
0
0
0
0 D 55 0
0
0
0
0
(3-23)
0 D 66
where the components are as follows:
2
2
E x  E z  yz – E y 
D 11 = ---------------------------------------- ,
D denom
E x E y  E z  yz  xz + E y  xy 
D 12 = – ---------------------------------------------------------------D denom
MATERIAL MODELS
|
445
2
2
E x E y E z   xy  yz +  xz 
D 13 = – ---------------------------------------------------------- ,
D denom
E y  E z  xz – E x 
D 22 = --------------------------------------D denom
E y E z  E y  xy  xz + E x  yz 
D 23 = – ----------------------------------------------------------------- ,
D denom
E y E z  E y  xy – E x 
D 33 = ---------------------------------------------D denom
D 44 = G xy ,
2
D 55 = G yz , and D 66 = G xz
where
2
2
2 2
D denom = E y E z  xz – E x E y + 2 xy  yz  xz E y E z + E x E z  yz + E y  xy
The values of Ex, Ey, Ez, xy, yz, xz, Gxy, Gyz, and Gxz are supplied in designated
fields in the physics interface. COMSOL Multiphysics deduces the remaining
components —yx, zx, and zy — using the fact that the matrices D and D1 are
symmetric. The compliance matrix has the following form:
D
–1
 yx  zx
1
-----– ------- – -------- 0
Ex Ey Ez
0
0
 xy 1
 zy
– ------- ------ – ------- 0
Ex Ey Ez
0
0
0
0
0
 xz  yz 1
– ------- – -------- -----Ex Ey Ez
=
0
0
0
0
1
--------- 0
G xy
0
0
0
1
0 --------- 0
G yz
0
0
0
0
1
0 --------G xz
The values of xy and yx are different for an orthotropic material. For a
certain set of given material data, you must make sure that the definition
of the indices is consistent with the definition used in COMSOL
Multiphysics.
The elasticity matrix in the Voigt (11, 22, 33, 23, 13, 12) Material data ordering changes
the sorting of the last three elements in the elasticity matrix:
446 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
D 44 = G yz ,
D 55 = G xz , and D 66 = G xy
If a pair of elastic moduli is present in the material definition, the values of Ex, Ey, Ez,
xy, yz, xz, Gxy, Gyz, and Gxz are computed automatically. Note that the resulting
elasticity matrix will be isotropic. Depending on which pair of elastic moduli that is
available, the expressions in Table 3-1 are used to find the above values.
Transversely Isotropic Material
Transversely isotropic material is a subclass of orthotropic materials, for which one
principal direction in the material is different from the other two that are equivalent.
This special direction is assumed to be the first axis of the selected coordinate system.
Because of the symmetry, the following relations hold:
E3 = E2
 13 =  12
E2
G 23 = -------------------------2  1 +  23 
G 12 = G 13
Thus, only five elasticity parameters are needed to characterize the material.
Anisotropic Material
In the general case of fully anisotropic material, you provide explicitly all 21
components of the symmetric elasticity matrix D, in either Standard (11, 22, 33, 12, 23,
13) or Voigt (11, 22, 33, 23, 13, 12) Material data ordering.
If a pair of elastic moduli is present in the material definition, the components of the
symmetric elasticity matrix D are computed using one of Equation 3-20 to
Equation 3-22. Depending on which pair of elastic moduli that is available, the
expressions in Table 3-1 are used to compute the necessary values. In case the
orthotropic properties Ei, ij, and Gij are present in the material definition, the
components of the symmetric elasticity matrix D are computed using Equation 3-23.
Note that the resulting elasticity matrix will not be fully anisotropic in either case.
Crystal Symmetry
Here, the components of the elasticity matrix in Voigt notation (denoted by cij) are
referred to as elasticity constants. Because of the material symmetry, only certain
MATERIAL MODELS
|
447
components need to be specified. The following Crystal systems are available in
COMSOL Multiphysics:
Cubic (3 constants) c11, c12, c44
c 11 c 12 c 12 0
0
0
c 12 c 11 c 12 0
0
0
c 12 c 12 c 11 0
0
0
0
0
0 c 44 0
0
0
0
0
0 c 44 0
0
0
0
0
0 c 44
This crystal system includes the following crystal classes: 23 m3 432 43m m3m .
Hexagonal (5 constants) c11, c12, c13, c33, c44
c 11 c 12 c 13 0
0
0
c 12 c 11 c 13 0
0
0
c 13 c 13 c 33 0
0
0
0
0
0
0 c 44 0
0
0
0
0 c 44 0
0
0
0
0
0 c 66
where c 66 = 0.5  c 11 – c 12  .
This crystal system includes the following crystal classes:
6 6 6  m 622 6mm 62m 6  mmm , and it is equivalent to a Transversely Isotropic
Material.
Trigonal (6 constants) c11, c12, c13, c14, c33, c44
c 11 c 12 c 13 c 14
448 |
0
0
c 12 c 11 c 13 – c 14 0
0
c 13 c 13 c 33
0
0
0
c 14 – c 14 0
c 44
0
0
0
0
0
0
c 44 c 14
0
0
0
0
c 14 c 66
CHAPTER 3: STRUCTURAL MECHANICS THEORY
where c 66 = 0.5  c 11 – c 12  .
This crystal system includes the following crystal classes: 32 3m 3m .
Trigonal (7 constants) c11, c12, c13, c14, c25, c33, c44
c 11 c 12 c 13 c 14 – c 25 0
c 12 c 11 c 13 – c 14 c 25
0
c 13 c 13 c 33
0
0
0
c 14 – c 14 0
c 44
0
c 25
c 44 c 14
– c 25 c 25
0
0
0
0
c 25 c 14 c 66
0
where c 66 = 0.5  c 11 – c 12  .
This crystal system includes the following crystal classes: 3 3 .
Tetragonal (6 constants) c11, c12, c13, c33, c44, c66
c 11 c 12 c 13 0
0
0
c 12 c 11 c 13 0
0
0
c 13 c 13 c 33 0
0
0
0
0
0
0 c 44 0
0
0
0
0 c 44 0
0
0
0
0
0 c 66
This crystal system includes the following crystal classes: 422 4mm 43m 4  mmm .
Tetragonal (7 constants) c11, c12, c13, c16, c33, c44, c66
c 11 c 12 c 13 0
0
c 12 c 11 c 13 0
0 – c 16
c 13 c 13 c 33 0
0
0
0
0
0
0 c 44 0
0
0
0
c 16 – c 16 0
c 16
0 c 44
0
0
c 66
0
This crystal system includes the following crystal classes: 4 4 4  m .
Orthorhombic (9 constants) c11, c12, c13, c22, c23, c33, c44, c55, c66
MATERIAL MODELS
|
449
c 11 c 12 c 13 0
0
0
c 12 c 22 c 23 0
0
0
c 13 c 23 c 33 0
0
0
0
0
0
0 c 44 0
0
0
0
0 c 55 0
0
0
0
0
0 c 66
This crystal system includes the following crystal classes: 222 mm2 mmm . This type
of crystal symmetry is equivalent to an Orthotropic Material.
AXIAL SYMMETRY
For the linear elastic material, the stress components in coordinate system are

ij
ij
=  ex + C
ijkl
  kl –  inel kl 
For anisotropic and orthotropic materials, the 4th-order elasticity tensor is defined
from the D matrix according to:
r
 r

r


 



=
+ D  –

 z

z
z


 rz
2 rz
 2 rz

ex
inel
r

z
 rz
The user input D matrix always contains the physical components of the elasticity
tensor
phys
C ijkl
and the corresponding tensor components are computed internally according to:
C
ijkl
C
phys
ijkl
= ---------------------------------------------g ii g jj g kk g ll
For an isotropic material:
C
450 |
ijkl
ij kl
= g g
CHAPTER 3: STRUCTURAL MECHANICS THEORY
ik jl
il jk
+ g g + g g 
where and  are the first and second Lamé elastic parameters and g is the metric
tensor.
For a hyperelastic material, the second Piola–Kirchhoff stress tensor is computed as
S = 2
W s
C
which is computed as the contravariant components of the stress in the local
coordinate system:
S
ij
= 2
W s
 C ij
The energy variation is computed as
Stest    =
 S test  ij 
ij
i j
which can be also written as
S r test   r  + S  test     + S z test   z  + 2S rz test   rz 
ENTROPY AND THERMOELASTICITY
The free energy for the linear thermoelastic material can be written as
F = f 0  T  + W s   T 
where the strain energy density Ws T is given by Equation 3-19. Hence, the stress
can be found as
F
W
 =   =   = C    –  inel 
  T
  T
and the entropy per unit volume can be calculated as
F
–   = C p log  T  T 0  + S elast
  T 
where T0 is a reference temperature, the volumetric heat capacity Cp can be assumed
to be independent of the temperature (Dulong–Petit law), and the elastic entropy is
MATERIAL MODELS
|
451
S elast = 
where  is the thermal expansion coefficient tensor. For an isotropic material, it
simplifies into
S elast =    x +  y +  z 
The heat balance equation can be written as
C p

T
+ T S elast =    k T  + Q h
t
t
where k is the thermal conductivity matrix, and the heat source caused by the
dissipation is
ꞏ
Q h = 
where ꞏ is the strain-rate tensor and the tensor  represents all possible inelastic stresses
(for example, a viscous stress).
Using the tensor components, the heat balance can be rewritten as:
C p
T
+
t

 Tmn  t mn =    k T  + Qh
(3-24)
m n
In many cases, the second term can be neglected in the left-hand side of Equation 3-24
because all Tmn are small. The resulting approximation is often called uncoupled
thermoelasticity.
WAVE SPEED COMPUTATION
In case of geometric linearity, the governing equations for a linear elastic medium of
any anisotropy can be written in terms of the structural displacement vector u as:
2

 u
t
2
=    C u 
where C is the elasticity tensor.
Since the equations are linear, they possess the following time-harmonic wave
solutions:
452 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
u = un e
it – i k  r
where k  kn is the wave number vector, and n is the direction vector that defines the
wavefront propagation direction. The wavefront is an imaginary line connecting solid
particles of the same phase. The velocity of such wavefront in the direction normal to
it is given by the phase velocity c  k.
Using such a wave solution form leads to Christoffel’s equation:
2
(3-25)
c u n =  n  u n
where the Christoffel’s tensor is defined as
n = n  C  n .
The Christoffel’s equation can be considered as an eigenvalue problem. Thus, to have
a nontrivial solution un, the phase velocity must satisfy
2
det   n   – c I  = 0
which is often called the dispersion relation. In a general case, this is a cubic polynomial
with three roots c2  cj2(n). Thus, for an arbitrary anisotropic medium, three waves
with different phase velocities can propagate in each given direction.
If the wave propagation is initiated by a small perturbation that is initially localized in
space, the solution can be found using the Fourier and Laplace transforms, and it will
represent a so-called wave packet. The wave packet will propagate with the group
velocity given by:
 j
1 
= -----------  u n j   n  u n j 
2c j  n
k
j = 1 2 3
where un,j is the wave polarization vector that is the eigenvector corresponding to the
eigenvalue solution cj2(n) of Christoffel’s equation.
COMSOL Multiphysics provides predefined variables for the phase and group
velocities for waves of different types propagating in any chosen direction. These
MATERIAL MODELS
|
453
variables do not affect the solution as such, but are available during result presentation
if the Wave Speeds node has been added to the material.
The wave speed variables can be found in the Wave speeds folder under
Solid Mechanics in the Replace Expression tree.
Mixed Formulation
Nearly incompressible materials can cause numerical problems if only displacements
are used in the interpolating functions. Small errors in the evaluation of the volumetric
strain, due to the finite resolution of the discrete model, are exaggerated by the high
bulk modulus (or low bulk modulus to shear modulus ratios). This leads to an unstable
representation of stresses, and in general, to an underestimation of the deformation, as
spurious volumetric stresses might balance applied shear and bending loads.
When the Pressure formulation is selected in the Use mixed formulation list, the
volumetric stress pw is used as an additional dependent variable. The resulting mixed
formulation is also known as a u-p formulation. This formulation removes the effect
of the volumetric strain from the original stress tensor, and replaces it with an
interpolated pressure, pw. A separate equation constrains the auxiliary pressure variable
to make it equal (in an average sense) to the original pressure which is calculated from
the strains and material model.
When the Strain formulation is selected in the Use mixed formulation list, the volumetric
strain w is instead used as the additional dependent variable.
The mixed formulation is beneficial when the material data is such that the
deformation is close to being incompressible. For an isotropic elastic material, this
happens when the Poisson’s ratio approaches 0.5.
The mixed formulation is useful not only for linear elastic materials but
also for nonlinear elastic materials, elastoplastic materials, hyperelastic
materials, and viscoelastic materials.
The order of the shape function for the auxiliary variable (pw or w)
should be of lower order than that of the displacement field. Note that
some iterative solvers do not work well together with mixed formulation
because the stiffness matrix becomes indefinite.
454 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
When the Pressure formulation is selected for isotropic linear elastic materials, the stress
tensor s, computed directly from the strains, is replaced by a modified version:
s̃ = s +  p – p w I
where I is the unit tensor. The pressure p is calculated from the stress tensor as
1
p = – --- trace  s 
3
This is equivalent to define
s̃ = dev  s  – p w I
The auxiliary dependent variable pw is set equal to p using the equation
pw – p
--------------- = 0
K
(3-26)
where K is the bulk modulus. Scaling by the bulk modulus is necessary, since typical
values for the auxiliary pressure pw are in the order of 106 to 109 Pa, while typical
values for the displacement degrees of freedom are orders of magnitude smaller.
The modified stress tensor s̃ is then used then in calculations of the energy variation.
When the Strain formulation is selected for isotropic linear elastic materials, the
auxiliary volumetric strain w is used instead of the auxiliary pressure pw, and it is the
set equal to the volumetric strain vol using the equation
– K   w –  vol  = 0
(3-27)
The modified stress tensor then reads
s̃ = s + K   w –  vol I = dev  s  + K w I
The advantage of using the Strain formulation is that the values for the auxiliary strain
w often are of a similar order of magnitude as the displacement degree of freedom.
For orthotropic and anisotropic materials, the auxiliary pressure equation is scaled to
make the stiffness matrix symmetric. Note, however, that the stiffness matrix in this
formulation is not positive definite and even contains a zero block on the diagonal in
MATERIAL MODELS
|
455
the incompressible limit. This limits the possible choices of direct and iterative linear
solver.
In case of linear elastic materials with geometric nonlinearity (and also for
hyperelastic materials), the stress tensor s in the above equations is
replaced by the second Piola–Kirchhoff stress tensor S, see Nearly
Incompressible Hyperelastic Materials.
For Plane Stress problems (in 2D solid mechanics, shell, or membrane), it is also
possible to use an implicit incompressibility formulation. Based on the plane stress
equation (the normal stress is equal to zero), the pressure is analytically found and the
incompressibility constraint is enforced using the auxiliary transverse strain degree of
freedom.
Nonlinear Elastic Materials
As opposed to hyperelastic materials, where the stress-strain relationship becomes
significantly nonlinear at moderate to large strains, nonlinear elastic materials present
nonlinear stress-strain relationships even at infinitesimal strains.
Here, nonlinear effects on the strain tensor are not as relevant as the nonlinearity of
the elastic properties. Important materials of this class are Ramberg–Osgood for
modeling metal and other ductile materials, and the Duncan–Chang soil model.
The nonlinear elastic materials as such do not include strain-rate nor stress-rate in the
constitutive equations. It is however possible to add linear viscoelasticity to these
materials.
For a nonlinear material to be “energetically sound” it should be possible to take any
path in stress-strain space and return to the undeformed state without producing or
dissipating any net energy. A requirement is then that the bulk modulus depends only
on the volumetric strain, and the shear modulus depends only on the shear strains.
The splitting into volumetric and deviatoric components of the stress tensor helps
ensuring the “path independent” restriction for isotropic nonlinear elastic materials.
For isotropic linear elastic materials, the stress tensor follows Hooke’s law:
 =  ex + C  el =  ex + C    –  inel 
For a more detailed discussion, see Equation 3-18.
456 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
It is possible to split the stress and elastic strain tensors into the deviatoric and
volumetric contributions
1
 = dev    + --- trace   I
3
and
1
 el = dev   el  + --- trace   el I
3
Assuming only elastic stresses in linear isotropic elastic medium, Hooke’s law simplifies
to
1
 = dev    + --- trace   I = 2Gdev   el  + Ktrace   el I
3
where K is the bulk modulus and G is the shear modulus. By using the convention that
the pressure is the mean stress defined as positive in compression,
p = –1
--- trace   
3
The volumetric strain (positive in tension) is
 el,vol = trace   el 
The linear relation between pressure and volumetric elastic strain is thus
p = – K el,vol
The deviatoric stress and deviatoric elastic strain tensors are related by the shear
modulus
dev    = 2Gdev   el 
By using the contraction of the deviatoric stress and strain tensors, the invariants of
these tensors can alternatively be related through
1
2
J 2    = --- dev   :dev    =  2G  J 2   el 
2
For a body subject to pure torsion on the plane 12, the stress tensor components are
zero except the shear stress 12  21  , and also the elastic strain tensor has zero
components beside the shear strains on that plane 12  21  el/2.
MATERIAL MODELS
|
457
Then
1
2
J 2    = --- dev   :dev    = 
2
and
1
1 2
J 2   el  = --- dev   el :dev   el  = ---  el
2
4
The shear stress on the plane  = J 2    is then related to the elastic shear strain
 el = 2 12 = 2 J 2   el  by the shear modulus
 = G el
Nonlinear Moduli
For nonlinear elastic materials, there is a nonlinear relation between shear stress and
shear strain and/or a nonlinear relation between pressure and volumetric strain.
For the purpose of this discussion,  =
alternatively as variables.
J 2    and  el = 2 J 2   el  are used
In the most general case:
p = p   el,vol  and  =    el 
Tangent and Secant Moduli
The tangent shear modulus Gtel and the secant shear modulus Gsel in the most
general case depend nonlinearly on the shear strain, and are defined as
- and G = ----G t = -------s
 el
 el
Note that the secant modulus is sometimes called the chord modulus between zero and
current strain level.
The tangent bulk modulus Ktel,vol and the secant bulk modulus Ksel,vol depend
on the elastic volumetric strain, and are defined as
p and K = – -----------p K t = – ---------------s
 el,vol
 el,vol
For linear elastic materials, it is clear that Gt  Gs  G and Kt  Ks  K, but this is not
the case for nonlinear elastic materials.
458 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
At zero strain, the secant and shear moduli are equal to each other Gs0  Gt 0 and
Ks0  Kt 0.
The nonlinear elastic materials described in the next sections are represented by
introducing nonlinear secant shear and/or bulk moduli.
Geometric Nonlinearity
The nonlinear elastic material models are primarily intended for small strain analysis.
When used in a geometrically nonlinear study step, the strains will be interpreted as
Green–Lagrange strains and the stresses will be interpreted as second Piola–Kirchhoff
stresses. This is relevant for a situation with large rotations but small strains. If the
strains become larger than a few percent, then you must be careful when interpreting
input parameters and results since the strain and stress tensors also have a nonlinear
dependence on the displacements.
RAMBERG–OSGOOD
The Ramberg–Osgood material model (Ref. 1) is a nonlinear elastic material
commonly used to model plastic deformation in metals, but it also often used in soil
engineering. As it is an elastic model, it can only represent plasticity during pure
on-loading conditions.
For uniaxial extension, the stress-strain curve is defined by the expression
 - n
- +   ------- = --ref   
E
ref
Here, E means the initial Young’s modulus, and ref is the strain at a reference stress
ref. The parameter n is the stress exponent. It is common to use ref  0.002, so ref
is the stress at 0.2% strain, typically denoted by the symbol 0.2. This parameter has
several names depending on the literature: 0.2% offset yield strength, 0.2% proof stress,
0.2% proof strength, or 0.2% yield stress. Typical values for stainless steel are
E  200 GPa, 0.2  600 MPa, and n  4.8.
The linear strain is given by
 el = --E
and the nonlinear strain by
 n
 nl =  ref  ---------
  ref
MATERIAL MODELS
|
459
The total strain is the sum of linear and nonlinear strains
 - n
- +   ------- =  el +  nl = --ref   
E
ref
In order to avoid a circular dependence of internal variables, the nonlinear strain nl is
defined with an auxiliary degree of freedom, so the stress reads   Enl.
Ramberg–Osgood Material in Soil Engineering
In soil engineering, it is common to write the Ramberg–Osgood material with the
stress-strain expression
 ref    n
- +  -------- -------- = --E   ref
E
(3-28)
so at the reference stress ref, the strain is   ref/E. It is common to use
  3/7, so ref represents the stress level at which the secant Young’s modulus has
been reduced to 70% its initial value: E0.7  E/  0.7E. At this reference stress
the strain is   ref/E0.7.
POWER LAW
For this type of material, the shear stress is related to the elastic shear strain  by the
strain exponent n and a reference shear strain ref (Ref. 2)
 n
 = G 0  ref  -------
  ref
The secant shear modulus is given by the power law relation
 n–1
G s = G 0  -------
 ref
The strain exponent controls the nonlinear deformation:
• For n1 the material behaves as a dilatant (shear-thickening) solid
• For n1 the material is linear elastic
• For 0nthe material behaves as pseudoplastic (shear-thinning) solid
• For n the material is perfectly plastic
BILINEAR ELASTIC
The most commonly mentioned model of “bilinear elastic” material is defined with
two different bulk moduli for either tension and compression. Commonly, brittle
460 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
materials like graphite and ceramics exhibit this behavior. The secant bulk modulus
reads
K = K t for el,vol  
and
K = K c for el,vol  
whereel,vol is the volumetric strain, Kc is the bulk modulus for compression, and Kt
the bulk modulus for tension.
UNIAXIAL DATA
Many nonlinear stress-strain curves are measured in a tensile test, for which a nonlinear
curve of force vs displacement is obtained.
If only the uniaxial behavior is measured, the measurements do not fully define the
material behavior. An extra assumption is needed. The Uniaxial data material model
allows you to assume either a constant Poisson’s ratio, or a constant bulk modulus.
Also, if only uniaxial extension data is available, further assumptions are needed for
covering the uniaxial compressive behavior of the material.
For the uniaxial tensile test, the axial stress corresponds to the principal stresses
ax  1  mises, and the other two principal stresses are equal to zero, 2  3  0.
The principal (axial) strain is positive in tension, ax  1, and the other two
(transverse) strains are negative and related by the Poisson’s ratio 2  3  1.
For uniaxial compression, the axial strain is negative, and when the principal strains are
sorted as 1  2  3 it corresponds to the third principal strain, ax  3. The other
two (transverse) strains are positive and related by the Poisson’s ratio 1  2  3.
Also, the axial stress is negative in compression, and it corresponds to the third
principal stress ax  3  mises. The other two transverse stresses are zero
1  2  0.
Other strain measures that can be obtained from the elastic strain tensor or its principal
values, are the elastic volumetric strain
 vol,el = trace   el 
and the elastic shear strain,
 el = 2 J 2   el  =
2dev   el :dev   el  .
MATERIAL MODELS
|
461
These are used to define the elastic axial strain variable for multiaxial loading.
The uniaxial test defines the relation between the axial stress and elastic axial strain as
 ax = E s  ax
Here, Es is the secant Young’s modulus, and the axial stress ax is considered as a
function of the elastic axial strain ax. Thus
 ax
E s = ------- ax
At zero strain, the secant Young’s modulus is defined as
d ax
E s = -----------d ax
 ax = 0
Assuming a constant Poisson’s ratio, the secant shear modulus is defined as
Es
G s = -------------------21 + 
and the secant bulk modulus as
Es
K s = ----------------------3  1 – 2 
Furthermore, if only tensile stress-strain data is available, the elastic axial strain for
multiaxial loading is computed from the elastic shear strain  and Poisson’s ratio as
3  ax = -------------------21 + 
When nonsymmetric stress-strain data is available, the elastic axial strain for multiaxial
loading is computed from the elastic volumetric strain and Poisson’s ratio
 vol
 ax = --------------1 – 2
as this expression captures the change of sign in the elastic axial strain when changing
from a tensile to a compressive state.
When using a constant bulk modulus assumption, only the symmetric part from the
stress-strain data is considered. The secant shear modulus is instead defined as
462 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
3KE s
G s = -------------------9K – E s
and the elastic axial strain is defined from both volumetric and shear elastic strains
 vol
 - + ---------- ax = -----3
3
It is possible to use any uniaxial data function to define the axial stress as a function of
elastic axial strain
 ax =  ax   ax 
provided that
 ax = 0 when  ax = 0
The elastic axial strain ax can be called in user defined uniaxial stress
functions by referencing the variables solid.eax, where solid is the
name of the physics interface node. See also the description of the
Uniaxial Data material model in the Solid Mechanics interface
documentation.
SHEAR DATA
Many nonlinear stress-strain curves are measured in a shear test, for which a nonlinear
curve of force vs displacement is obtained.
If only the shear behavior is measured, the measurements do not fully define the
material behavior and therefore an extra assumption is needed. The Shear data
material model assumes a constant bulk modulus.
Other strain measures that can be obtained from the strain tensor or its principal
values, are the elastic volumetric strain
 vol,el = trace   el 
and the elastic shear strain,
 = 2 J 2   el  =
2dev   el :dev   el  .
These are used to define the nonlinear stress-strain relation for multiaxial loading.
MATERIAL MODELS
|
463
From the shear test one could define the relation between the shear stress  and the
elastic shear strain  as
 = Gs 
Here, the secant shear modulus Gs is constant for Linear Elastic materials, but in
general one could use a nonlinear relation. It is possible to use shear data to define the
shear stress as a function of elastic shear strain as follows:
 = 
provided that
 = 0 when  = 0
in which case, the secant shear modulus is computed from
  G s = --------
With the help of the secant shear modulus Gs computed from shear data, Hooke’s law
simplifies to
 = 2G s dev   el  + Ktrace   el I
where K is the bulk modulus.
The elastic shear strain can be called in user defined shear stress functions
by referencing the variables solid.esh, where solid is the name of the
physics interface node. See also the description of the Shear Data material
model in the Solid Mechanics interface documentation.
HYPERBOLIC LAW
A hyperbolic relation between shear stress and shear strain is obtained by setting the
secant shear modulus
1
G s = G -------------------------n
1 +  -------
  ref
where the strain exponent n and a reference shear strain ref control the shape of the
hyperbola.
464 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
For hyperbolic material models, the maximum shear modulus occurs at zero shear
strain, so practitioners might call G the “maximum shear modulus” and use the
notation Gmax. Sometimes it is also called “small strain shear modulus”.
HARDIN–DRNEVICH
The Hardin–Drnevich model (Ref. 3) is a hyperbolic soil model (with n  ) defined
by two input parameters: the initial shear modulus G and a reference shear strain ref:
1
G s = G ----------------
1 + ------ ref
This nonlinear soil model is commonly used for modeling soil dynamics in earthquake
engineering problems.
Since   Gs, the shear stress is bounded by max  Gref as the shear strain increases.
The hyperbolic Hardin–Drnevich model is normally used for quantifying stiffness
reduction curves in soils. Commonly, the reference shear strainref is replaced by the
reference shear strain at which the secant shear modulus has been decreased to 70% of
its initial value. Calling this shear strain value 0.7, the reference strain is written as
7
 ref = ---  0.7
3
and the secant shear modulus as
1
G s = G ----------------------3 
1 + --- --------7  0.7
so that when   0.7 the secant shear modulus is Gs .7G.
DUNCAN–CHANG
The original model was originated by Kondner to fit triaxial test data for undrained
soils. Duncan and Chang (Ref. 4) and other coworkers (Ref. 5) developed this
hyperbolic model to its current state. The material model is written in terms of the axial
and radial stresses 1 and 3 and the axial strain , and it describes the stress-strain
curve by fitting the hyperbola
  1 –  3 = --------------a + b
MATERIAL MODELS
|
465
here a and b are material parameters obtained by curve fitting data from the triaxial
test. The parameter a is related to the initial Young’s modulus E
1a = --E
and the parameter b defines the asymptote of the hyperbola, which is related to the
ultimate value of 13 denoted qult
1
--- =   1 –  3  ult = q ult
b
The ultimate value qult is related to the strength of the soil.
For the triaxial test, the axial strain is related to the shear strain  by the Poisson’s
ratio as
3
 = --------------------- 
21 + 
and the axial and radial stresses are related to the shear stress as  1 –  3 =
3 .
It is possible then to write the relation between shear stress and shear strain as
1 -------------------
2

1
+ 
 = -------------------------------------------1
3 1- ----------------------------+

E q ult 2  1 +  
Since the initial shear modulus is related to the initial Young’s modulus as
G  E2(1  ), this stress-strain relation can alternatively be written as

 = --------------------1
3
---- + --------G q ult
which is an hyperbolic law with a secant shear modulus of
G
G s = ---------------------------G
1 + -------- 3
q ult
466 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
DUNCAN–SELIG
The Duncan–Selig model is a combination of the Duncan’s hyperbolic material model
(Ref. 4, Ref. 5) and Selig’s model to describe nonlinear bulk modulus behavior. Selig
(Ref. 6) further developed the model of Duncan and others in order to include a
nonlinear volumetric response in soils.
The model defines the nonlinear volumetric response for the pressure as
 el,vol
p = – K ---------------------- el,vol
1 – ----------- ult
where el,vol is the volumetric strain, and ult is the asymptote of the hyperbola, the
maximum value for the volumetric compression. Note that K represents the bulk
modulus at zero strain.
The secant (nonlinear) bulk modulus is defined for this material model as
1
K s = K ---------------------- el,vol
1 – ------------ ult
SMALL STRAIN OVERLAY
The majority of soils exhibit a nonlinear stiffness behavior at small strains, coupled with
a hysteresis effect. This phenomenon is characterized by an exceptionally high shear
modulus at low strains, commonly referred to as small-strain stiffness. This
small-strain stiffness nonlinearly decays as the strain level increases.
The small strain overlay model (Ref. 26, Ref. 27) incorporates both the nonlinear
stiffness and hysteresis effects by utilizing a nonlinear shear modulus derived from the
shear strain history observed over multiple loading–unloading cycles.
The stress–strain relationship is defined by
 = 2Gdev   el,dev –  r,dev  + K   el,vol –  r,vol I +  r
where el,dev and el,vol are the deviatoric and volumetric elastic strains, and r,dev,
r,vol, and r are the deviatoric and volumetric elastic strains and stress at the last load
reversal point.
The secant shear modulus is defined from an Hyperbolic Law, in a similar way as done
for the Hardin–Drnevich model. The secant shear modulus for primary loading is
MATERIAL MODELS
|
467
defined by two input parameters, the initial shear modulus G0 and a reference shear
strain ref, as
1
G pl = G 0 ------------------ hist
1 + -------- ref
Here, hist is a measure of the shear strain history. In Ref. 26, the reference shear strain
is defined from  ref =  0.7  a , where a = 0.385 is a tuning parameter that fits
experimental data and 0.7 is the shear strain at which the secant shear modulus has
been decreased to 70% of its initial value.
The secant shear modulus for unloading and reloading is defined as
1
G ur = G 0 -------------------- hist
1 + ---------2 ref
which is higher than Gpl.
The load path is considered as primary loading if the soil has not reached any load
reversal stage, in which case Gpl is used. When a load reversal happens, the soil is
assumed to be on the unloading–reloading path, and Gur, is instead used.
USER DEFINED
This option allows you to write explicitly how the pressure depends on the elastic
volumetric strain. This could be an analytic function or data interpolated from a table.
The elastic volumetric strain vol,el can be called in user defined
expressions by referencing the variables solid.eelvol, where solid is
the name of the physics interface node.
Linear Viscoelasticity
Viscoelastic materials have a time-dependent response even if the loading is constant
in time. Many polymers and biological tissues exhibit this behavior. Linear
viscoelasticity is a commonly used approximation, where the stress depends linearly on
the strain and its time derivatives (strain rate). Also, linear viscoelasticity deals with the
additive decomposition of stresses and strains. It is usually assumed that the viscous
part of the deformation is incompressible so that the volumetric deformation is purely
elastic, but it is also possible to account for volumetric viscoelasticity.
468 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
For isotropic linear elastic materials in the absence of inelastic stresses, Hooke’s law in
Equation 3-18 reduces to
 = C  el
where the elastic strain tensor el    inel represents the difference between the total
strain and inelastic strains, such as thermal strains.
The stress tensor can be decomposed into a pressure and a deviatoric stress:
 = – pI +  dev
The pressure (mean stress or volumetric stress) is given with a positive sign in
compression
p = –1
--- trace   
3
and the deviatoric stress is computed from the total stress minus the volumetric
contribution
1
 dev = dev    =  – --- trace    =  + pI
3
The elastic strain tensor el can in the same way be decomposed into volumetric and
deviatoric components
1
 el = ---  el,vol I +  el,dev
3
with the volumetric elastic strain defined as
 el,vol = trace   el 
and the deviatoric contribution
 el,dev = dev   el 
For isotropic linear elastic materials, the pressure is then related to the volumetric
elastic deformation by the bulk modulus K
p = –1
--- trace    = – Ktrace   el  = – K el,vol
3
MATERIAL MODELS
|
469
and the deviatoric stress tensor is linearly related to the deviatoric elastic strain tensor
by the shear modulus G
 dev = dev    = 2Gdev   el  = 2G el,dev
The total stress in Equation 3-18 is then
 = K el,vol I + 2G el,dev
In case of geometric nonlinearity,  represents the second Piola–Kirchhoff stress tensor
and el the elastic Green–Lagrange strain tensor.
THE GENERALIZED MAXWELL MODEL
For deviatoric viscoelastic materials, the deviatoric stress d is not linearly related to the
deviatoric strain d but it also depends on the strain history. It is normally defined by
the hereditary integral:
t
 d
 d = 2   t – t'  -------- dt'
t'

0
The function (t) is called the relaxation shear modulus function (or just relaxation
function) and it can be found by measuring the stress evolution in time when the
material is held at a constant strain.
The relaxation function is often approximated by a Prony series:
N
t = G +
 Gm exp  – ------m-
t
m=1
470 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
A physical interpretation of this approach, often called the generalized Maxwell
model, is shown in Figure 3-1
d
d
G
G1
G2
1
2
1
2
Gm
.....
m
d
qm
m
m
m
Figure 3-1: Generalized Maxwell model.
Hence, G is the stiffness of the main elastic branch, Gm represents the stiffness of the
spring in branch m, and m is the relaxation time constant of the spring-dashpot pair
in branch m.
The relaxation times m are normally measured in the frequency domain, so the
viscosity of the dashpot is not a physical quantity but instead it is derived from stiffness
and relaxation time measurements. The viscosity of each branch can be expressed in
terms of the shear modulus and relaxation time as
m = Gm m
The auxiliary strain variable qm is introduced to represent the extension of the
corresponding abstract spring, and the auxiliary variables m  d  qm represent the
extensions in the dashpots.
The shear modulus of the elastic branch G is normally called the long-term shear
modulus, or steady-state stiffness, and it is often denoted with the symbol G. The
instantaneous shear modulus G0is then defined as the long-term shear modulus plus
the sum of the stiffnesses of all the viscoelastic branches
N
G0 = G +
 Gm
m=1
This is the equivalent stiffness when an external load is applied much faster than the
shortest relaxation time of any viscoelastic branch.
MATERIAL MODELS
|
471
Sometimes, the relaxation function (t) is expressed in terms of the instantaneous
stiffness and relative weights, so that the Prony series is given as
N


t - 

  t  = G0  w +
w m exp  – ----- m 


m=1

In this case, the long-term shear modulus is related to the instantaneous shear modulus
by the weight w  
G = w G0
and the shear moduli in each branch are defined by the weights wm
Gm = wm G0
It must be assumed then that the weights fulfill the constraint
N
w +
 wm = 1
m=1
The long-term shear modulus G is given in the parent material model (for
example, Linear Elastic Material). If your material data consists of the
instantaneous shear modulus G0 and the weights wm, you can convert the
data using the formulas above.
If your data consists of Young’s modulus and relaxation time per branch,
you can convert it to the equivalent shear moduli. As the strain tensors in
the dashpots are isochoric (volume preserving) it means that Gm  Em
In the parent Linear Elastic Material, you can enter the long-term elastic
data in any form, for example in terms of Young’s modulus, E, and
Poisson’s ratio, . It will then be converted to the corresponding shear
modulus G internally.
The stress per branch can be written either in terms of the strain in the spring, qm, or
the strain in the dashpot, m
ꞏ
 m = 2G m q m = 2 m  m = 2G m   d –  m 
The sum of the stresses in the viscoelastic branches is then computed from
472 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
N
N
q =

m =
 2Gm  d – m 
m=1
m=1
The total stress in Hooke’s law (Equation 3-18) is then augmented by the viscoelastic
stress q
 =  0 + C  el +  q
(3-29)
The same derivation is valid for a volumetric viscoelastic response, see Volumetric
Response.
In the case of mixed volumetric and deviatoric viscoelasticity, it is assumed that the
relaxation times per branch are the same for the deviatoric and volumetric
deformation.
Computing the Stress in Each Branch
For deviatoric viscoelasticity, the auxiliary variable m is a symmetric isochoric (volume
preserving) strain tensor, which has as many components as the number of strain
components of the problem class. Since the stress per branch is written as
ꞏ
 m = 2G m q m = 2 m  m = 2G m   d –  m 
the auxiliary variables m can be computed by solving the ODE
ꞏ
m m = Gm  d – m 
(3-30)
The relation between viscosity and relaxation time is
m = Gm m
so that Equation 3-30 can equivalently be written as
ꞏ
m m + m = d
(3-31)
The viscoelastic strain variables m are called for instance
solid.lemm1.vis1.ev1_11, where solid is the tag of the physics
interface, lemm1 is the tag of the linear elastic material, and vis1 is the tag
of the viscoelasticity node. The trailing numbers indicate the branch
number and the strain tensor indices.
MATERIAL MODELS
|
473
Volumetric Response
It is usually assumed that the viscous part of the deformation is incompressible so that
the volumetric deformation is purely elastic, but this does not have to be the case, and
the same derivation as stated in previous sections can be applied to the volumetric
response.
For volumetric viscoelasticity, the bulk modulus of the elastic branch K is normally
called the long-term bulk modulus, or steady-state stiffness, and it is often denoted
with the symbol K. The instantaneous bulk modulus K0is then defined as the
long-term bulk modulus plus the sum of the bulk moduli of all the viscoelastic
branches.
The scalar equation for the volumetric deformation per branch, em, is
 m eꞏ m + e m =  el,vol
(3-32)
where m is the relaxation time per branch and el,vol is the elastic volumetric strain.
The sum of the stresses in the viscoelastic branches is then computed from
N
N
q =

m=1
m =
 Km  el,vol – em I
m=1
where Km is the bulk modulus of branch m.
The volumetric viscoelastic strain variables em are called, for example,
solid.lemm1.vis1.evvol1, where solid is the tag of the physics
interface, lemm1 is the tag of the linear elastic material node, and vis1 is
the tag of the viscoelasticity node. The trailing number represents the
branch number (that is, the first branch in this case).
Equation 3-31 and Equation 3-32 are solved using a Local Time
Integration algorithm. Alternatively, the viscoelastic strain variables, m
and em, can be treated as additional degrees of freedom (DOFs), in which
case is it possible to select Gauss point data or Discontinuous Lagrange
shape functions (see Shape Functions and Element Types for details).
474 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
Using a Suitable Number of Branches
Only branches that have a relaxation time which is of the same order of magnitude as
the temporal variation of the loading are important for the viscoelastic response. The
cost in terms of memory consumption and computational speed increase significantly
if the model contains many branches, particularly in time domain and for
eigenfrequency analyses. In these cases many auxiliary equations of the form
Equation 3-31 have to be solved for.
However, if a viscoelastic branch relaxes much faster or much slower than the time
scale of the excitation period of external loads, the corresponding dashpot may be
considered to be either fully relaxed or rigid, depending on the relaxation time of the
branch relative to the excitation frequency. These fully relaxed or rigid branches can
then be removed and grouped into equivalent branches, thus reducing the
computational cost.
When the frequency band of interest is bounded by two cutoff frequencies, flower and
fupper, it is possible to prune viscoelastic branches that have relaxation times such as
11
---------  m  --------f high
f low
Branches with short relaxation times k represent the response of the viscoelastic
material to high frequency excitations. When the external loads represent excitations
bounded by an upper frequency fupper, it is possible to prune branches with relaxation
times that fulfill the relation k fupper  1. These branches are grouped into an
equivalent branch, with relaxation time and stiffness such as
 Gk k2
1
k
 high = -------------------- and G high = ----------- G k  k
 high
Gk k
k


k
Viscoelastic branches with relaxation times k such that 1  k flow are grouped into an
equivalent branch forming the low frequency cutoff. The stiffness and relaxation time
for the equivalent branch are computed from
1
1 - = ------------------G low
 low
Gk
- and G low =  G k
 -----k
k
k
MATERIAL MODELS
|
475
Frequency Domain
In frequency domain, the relaxation function becomes complex-valued. The complex
shear modulus for the generalized Maxwell model is then defined as the sum of the
shear modulus in the pure elastic branch plus the complex shear moduli in the
viscoelastic branches
N
G GM = G +
j m
 Gm ---------------------1 + j m
m=1
The storage and loss moduli are then computed as the real and imaginary parts of the
complex shear modulus
N

G' = real  G GM  = G +
m=1
2
  m 
G m ----------------------------2
1 +   m 
and
N
G'' = imag  G GM  =
 m
 Gm ---------------------------2
1 +   
m=1
m
Energy Dissipation
The dissipated energy density rate (SI unit: W/m3) in each dashpot m is
ꞏ
ꞏ
W m =  m : m
The rate of total dissipated energy density in the Generalized Maxwell material is then
N
ꞏ
Wv =
ꞏ
 Wm
m=1
ꞏ
In order to compute the dissipated energy density, the variable W v is integrated over
time. For frequency domain studies, the dissipation of viscous forces averaged over a
time period 2 is computed from the shear loss modulus G'' as
W v = G''˜d conj  ˜d 
476 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
THE MAXWELL MODEL
The Maxwell model (or Maxwell element) consists of a spring and a dashpot arranged
in series. Maxwell elements are the building blocks used in The Generalized Maxwell
Model.
d
d
G
q



d
Figure 3-2: Maxwell model.
In frequency domain, the compliance of the Maxwell model is defined as the sum of
the compliance modulus of the elastic part plus the compliance in the damper
1- + ------------1 J M = --G jG
The complex shear modulus then reads
j 1 - = -----------------G M = ------G
1 + j
JM
The storage and loss moduli are defined as the real and imaginary parts of the complex
shear modulus
2
  
G' = real  G M  = -----------------------2- G
1 +   
and

G'' = imag  G M  = -----------------------2- G
1 +   
THE GENERALIZED KELVIN–VOIGT MODEL
The generalized Kelvin–Voigt model is used to simulate the viscoelastic deformation
in a wide range of materials such as concrete, biological tissues, and glassy polymers.
MATERIAL MODELS
|
477
Just as for the generalized Maxwell model, the deviatoric strain d is not linearly related
to the deviatoric stress d, but it also depends on the strain history. It is normally
defined by the hereditary integral:
t
d =
 d
dt'
   t – t'  2--------t'
0
The function (t) is called the compliance function (also called creep compliance or
creep function) and it can be found by measuring the strain evolution in time when
the material is held at a constant stress.
The compliance function is often approximated by a Prony series:
N
t = J +
 Jm  1 – exp  – ------m- 
t
m=1
A physical interpretation of this rheological model consists of an elastic branch plus a
number of Kelvin–Voigt elements arranged in series, this approach is shown in
Figure 3-3.

d
1
2
N
1
2
N
G1
G2
GN
G
d
Figure 3-3: The generalized Kelvin–Voigt model.
Here, G is the stiffness of the main elastic branch, Gm represents the stiffness of the
spring in element m, and m is the relaxation time constant of the spring-dashpot pair
in branch m. The compliance J in the pure elastic branch is related to the shear
modulus by
1J = --G
and the compliances per branch are related to the shear moduli as
478 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
1J m = -------Gm
The relaxations time m is normally measured in the frequency domain, so the viscosity
of the dashpot is not a physical quantity but instead it is derived from stiffness and
relaxation time measurements. The viscosity in each branch can be expressed in terms
of the stiffness or compliance modulus and relaxation time as
m = Gm m = m  Jm
The auxiliary strain variables m are introduced to represent the extension of the
corresponding Kelvin–Voigt element. Since the elements are arranged in series, the
total viscoelastic strain is given as the sum of the auxiliary strains
 =
 m
(3-33)
m
The deviatoric stress d in the pure elastic branch is the same as in all the Kelvin–Voigt
elements
ꞏ
 d = 2Gdev   el  = 2G m  m + 2 m  m
(3-34)
Here, the deviatoric elastic strain is defined by the difference between the total and
inelastic strains.
Computing the Strain in Each Branch
The auxiliary strain variables m represent a symmetric isochoric (volume preserving)
strain tensor, which has as many components as the number of strain components of
the problem class.
The stress in each element m is given by the sum of the stresses in the spring and
dashpot arranged in parallel
ꞏ
ꞏ
 d = 2G m  m + 2 m  m = 2G m   m +  m  m 
Here, m is the strain in the element m, and m  mGm is the viscosity. The auxiliary
variables m are computed by solving the ODE
1
ꞏ
 m +  m  m = ------------  d
2G m
(3-35)
MATERIAL MODELS
|
479
The compliance of the elastic branch, J  1/G, is normally called the instantaneous
compliance, and it is often denoted with the symbol J0. This gives the equivalent
stiffness when the material is loaded by an abrupt load much faster than the shortest
relaxation time of any branch.
The long-term compliance J is defined as the instantaneous compliance plus the sum
of the compliances of the viscoelastic branches
N
N
J = J +

1- +
J m = --G
1
 -------Gm
m=1
m=1
The long-term shear modulus then reads G  1/J.
Sometimes, the compliance function (t) is expressed in terms of the instantaneous
compliance J and relative weights wm, so that the Prony series reads
N


t -  
t  = J1 +
w m  1 – exp  – -----

  
m 

m=1

In this case, the compliance and shear modulus in each branch are
J m = w m J and G m = G  w m
and the long-term shear compliance and long-term shear modulus read
N
N







J = J  1 +
w m and G  = G   1 +
w m




m=1
m=1


Frequency Domain
In frequency domain, the compliance function becomes complex valued. The complex
compliance for the generalized Kelvin–Voigt model is then defined as the sum of the
compliance in the pure elastic element (parent material) plus the complex compliances
in the viscoelastic elements.
N
1- +
J GVK = --G
1
1
- ---------------------- -------G m 1 + j m
m=1
The storage and loss compliances are then computed as the real and imaginary parts of
the complex compliance function
480 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
N
1- +
J' = real  J GVK  = --G
N


wm
1 ---------------------------1
1


---- 1 +
-----------------------------------=
2
G m 1 +    2
G
1
+




m
m 
m=1
m=1


and
N
J'' = imag  J GVK  =

m=1
– m
1
1
--------- ---------------------------= ---G m 1 +    2
G
m
N
– w m  m
 ---------------------------2
1 +   
m=1
m
Energy Dissipation
The dissipated energy density rate (SI unit: W/m3) in each branch m is given by the
dissipation in the dashpot
ꞏ
ꞏ ꞏ
W m = 2 m  m : m
The rate of total dissipated energy density in the generalized Kelvin–Voigt material is
then
N
ꞏ
Wv =
ꞏ
 Wm
m=1
ꞏ
In order to compute the dissipated energy density, the variable W v is integrated over
time. For frequency domain studies, the dissipation of viscous forces averaged over a
time period 2 is computed from the shear loss modulus G'' as
W v = G''˜d conj  ˜d 
MATERIAL MODELS
|
481
THE KELVIN–VOIGT MODEL
The Kelvin–Voigt viscoelastic model is represented by a spring connected in parallel
with a dashpot:
d
d
G

q
d
Figure 3-4: The Kelvin–Voigt model.
The stress tensor in the viscous branch is computed from the elastic strain rate
ꞏ
ꞏ
 q = 2 d = 2G d
(3-36)
so there is no need to add the extra DOFs to compute the auxiliary strain tensor .
The relaxation time relates the viscosity and shear modulus by   G. The equivalent
shear modulus is used in case of an anisotropic linear elastic material.
The dissipated energy density rate of the Kelvin–Voigt model is then computed from
its rate
ꞏ
ꞏ
W v =  q : d
The Kelvin–Voigt model is equivalent to viscous damping, see Viscous
Damping.
482 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
STANDARD LINEAR SOLID MODEL
The standard linear solid model, also called SLS model, Zener model, or
three-parameter model, is a simplification of the generalized Maxwell model with only
one spring-dashpot branch:
d
d G
G1
q1
1
1
q
1
d
Figure 3-5: Standard linear solid (SLS) model.
The stress in the viscoelastic branch is computed as
ꞏ
 q = 2G 1 q 1 = 2 1  1 = 2G 1   d –  1 
where the relaxation time is related to the stiffness and relaxation time as 1  1G1.
The auxiliary strain tensor 1 is computed by solving by the ODE
ꞏ
1 1 + 1 = d
and the dissipated energy density rate of the single branch is calculated from
ꞏ
ꞏ
W v =  q : 1
The long-term shear modulus G  G is given in the parent Linear Elastic Material,
and the instantaneous stiffness is given by the sum G  G  G.
The Standard linear solid model is equivalent to damping, see Maximum
Loss Factor.
MATERIAL MODELS
|
483
THE BURGERS MODEL
The Burgers model consists of a Maxwell (spring-dashpot) branch in series with a
Kelvin–Voigt branch. The rheological representation of this material model is shown
in Figure 3-6:
d
G
d
1
1
d

G2
2
2
d
Figure 3-6: The Burgers model.
The strain in the first dashpot follows the ODE
ꞏ
dev    = 2G   d –   = 2 1  1
where the shear modulus G is taken from the parent Linear Elastic material.
The strain in the second dashpot follows the ODE
ꞏ
2 2  2 = dev    – 2G 2  2
The total strain in the dashpots is computed from
 = 1 + 2
Combining these equations, it is possible to recover a second-order ODE for the strain
tensor :
G2
ꞏꞏ
1 - + --------1 - dev  ꞏ  – G
------2- ꞏ + ---------------dev   
 2 =  --------2
2 1  2
2 1 2 2
484 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
Note that the Burgers material has two relaxation times related to the stiffness and
viscosity in the springs and dashpots. The relaxation times 1 and2 are related to the
stiffness and viscosities as 1  1/G and 2  2/G2.
The instantaneous stiffness G  G is given in the parent Linear Elastic Material.
GENERALIZED MAXWELL MODEL WITH FRACTIONAL DERIVATIVES
Typically, the rheology of viscoelasticity models consists of springs and dashpots
arranged in series and in parallel. Using the framework of fractional calculus, the
constitutive equations of linear viscoelasticity can be generalized with a new type of
element, named spring-pot (Ref. 50). In some cases, viscoelasticity models with
fractional derivatives have shown to better match experimental data.
p, 
Figure 3-7: Spring-pot element.
The basic stress-strain relation of the spring-pot element is given by a proportionality
factor p and a fractional time derivative of order 
 = p
d
dt



 = pD 
The fractional order  takes a value between     . For   , the parameter p plays
the role of a stiffness in a spring, and for    the parameter plays the role of the
viscosity in a dashpot. The SI unit for such material parameter would be Pa·s.
For a pair of one spring and one spring-pot element connected in series, a so-called
Maxwell element with a fractional time derivative, the deviatoric stress strain relation
is given by

dev    = 2pD  = 2G   d –  
MATERIAL MODELS
|
485
The rheological representation of this arrangement is shown in Figure 3-8
d
d
G
q
p, 


d
Figure 3-8: A spring-pot element connected in series with a spring.
In frequency domain, the fractional time derivative operator is substituted by

D   j 

The fractional derivative models are available for frequency domain
analyses only.
Thus, the stress-strain relationship reads

Gp  j 
dev    = 2 ---------------------------- 
G + p  j 
For a standard spring-dashpot branch, the relaxation time is given by the ratio of
viscosity and stiffness,   G. Equivalently, the relaxation time  for a branch with a
spring and a spring-pot element in series is derived from

p = --G
Thus, p  G, and the stress-strain relationship in the spring-spring-pot system reads

G  j 
dev    = 2 --------------------------  d
1 +  j 
The complex-valued shear modulus for this Maxwell element reads

 j 
G M = -------------------------- G
1 +  j 
486 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
Storage and loss moduli are defined as the real and imaginary part of the complex shear
modulus
G' = real  G M  and G'' = imag  G M 
The loss factor is computed from
G'' = -------------------------------------------sin    2
 M = -----
G'
   + cos   2
For The Generalized Maxwell Model with fractional derivatives, all dashpots are
replaced with spring-pot elements. The rheological representation of this material
model is shown in Figure 3-9
d
d
G
G1
G2
1
2
1
2
qm
Gm
.....
m
d
m
m
m
Figure 3-9: The generalized Maxwell model with fractional derivatives.
The complex-valued shear modulus for the generalized Maxwell model with fractional
derivatives reads

G GM = G +
 j m  m
-------------------------------- Gm

1 +  j m  m
m

where Gm, m, and m are the shear modulus, relaxation time, and fractional order of
branch m, respectively. Storage and loss moduli are defined as the real and imaginary
part of the complex shear modulus.
G' = real  G GM  and G'' = imag  G GM 
GENERALIZED KELVIN–VOIGT MODEL WITH FRACTIONAL DERIVATIVES
The Kelvin–Voigt viscoelastic model with fractional time derivative consists of a spring
connected in parallel with a spring-pot element. The stress strain relation for such
arrangement reads
MATERIAL MODELS
|
487

dev    = 2pD  d + 2G d
The rheological representation of this arrangement is shown in Figure 3-10
d
d
, 
G
d
Figure 3-10: Spring spring-pot elements connected in parallel.
In frequency domain, substitute the fractional time derivative operator by

D   j 

The stress-strain relationship for this Kelvin element then reads

dev    = 2  p  j  + G  d
The relaxation time  for a spring and a spring-pot element in parallel is derived from

p = --G
so p  G, and the stress-strain relationship in the Kelvin–Voigt element reads

dev    = 2G   j  + 1  d
The complex-valued shear modulus in a spring-spring-pot arrangement reads

G KV =  1 +  j  G
Storage and loss moduli are defined as the real and imaginary part of the complex shear
modulus.

G' = real  G KV  =  1 +    cos   2 G
and
488 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY

G'' = imag  G KV  =    sin    2  G
The loss factor is computed from

G'' = ----------------------------------------------   sin    2  KV = -----
G'
1 +    cos   2
The complex-valued compliance of the Kelvin–Voigt element with fractional time
derivative reads
1- ------------------------1
1 - = --J KV = ---------G 1 +  j  
G KV
For The Generalized Kelvin–Voigt Model with fractional derivatives, all dashpots are
replaced with spring-pot elements.
The rheological representation of this material model is shown in Figure 3-11.

d
1
2
N
11
22
NN
G1
G2
GN
G
d
Figure 3-11: The generalized Kelvin–Voigt model with fractional derivatives.
The complex-valued compliance reads
1- +
J GKV = --G
1
1
- -------- -------------------------------
1 +  j  G m
m
m
m
where Gm, m, and m are the shear modulus, relaxation time, and fractional order of
element m, respectively. Storage and loss moduli are defined as the real and imaginary
part of the complex shear modulus
1 G GKV = ------------J GKV
MATERIAL MODELS
|
489
G' = real  G GKV  and G'' = imag  G GKV 
STANDARD LINEAR SOLID MODEL WITH FRACTIONAL DERIVATIVES
In the rheological representation of the Standard Linear Solid Model with fractional
derivatives, the dashpot is replaced with a spring-pot element.
d
d
G
G1
q1
1
1
q
d
Figure 3-12: Standard linear solid (SLS) model with fractional derivatives.
The deviatoric stress in the spring-spring-pot branch is computed as

 q = 2G 1   d –  1  = 2pD  1
here, 1 is the strain in the spring-pot element. In the frequency domain this equation
translates to
G1


 q = 2p  j   1 = ------------------------------- 2p  j   d
G 1 + p  j 
Using the relaxation time   (p/G1), this reads
G1

 q = 2 --------------------------  j   d = 2G q  d
1 +  j 
where Gq  G1(j)/(1+(j)) is the complex shear modulus of the spring-pot
branch.
Subsequently, the shear modulus is for the SLS model with fractional derivatives reads

 j 
G SLS = G + G q = G + -------------------------- G 1
1 +  j 
490 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
The storage and loss moduli are defined as the real and imaginary parts of the shear
modulus GSLS, respectively
G' = real  G SLS  and G'' = imag  G SLS 
BURGERS MODEL WITH FRACTIONAL DERIVATIVES
In the rheological representation of The Burgers Model with fractional derivatives, the
dashpots are replaced with a spring-pot elements. The rheological representation of
this material model is shown in Figure 3-13:
d
G
d
11
1
d

G2
22
2
d
Figure 3-13: The Burgers model with fractional derivatives.
The deviatoric stress in the main branch is computed as

 d = 2G   d –   = 2p 1 D 1  1
here, 1 is the strain in the spring-pot element. In frequency domain, and using the
relaxation times 1  (p1/G), this equation translates to
d

------- =  d –  =  j 1  1  1
2G
The stress in the second spring-pot follows

2p 2 D 2  2 =  d – 2G 2  2
MATERIAL MODELS
|
491
here, 2 is the strain in the second spring-pot element. In frequency domain, and using
the relaxation time 2  (p2/G2), this equation reads
d

 j 2  2  2 = ----------–
2G 2 2
The total strain in the spring-pots is computed from
 = 1 + 2
which combined with the relations for the strains in the spring-pots
1
1
- d
-  and  2 = --------------------------------------------- 1 = ----------------------------1 d

2G  j 1 
2G 2  1 +  j 2  2 
gives the stress and strain relation for Burgers model with fractional derivatives
 1

1
1
-  d =  d
- + --------------------------------------------- -------- + ----------------------------

1
2
2G

2G  j 
2G  1 +  j  
1
2
2
Subsequently, the compliance for the Burgers model with fractional derivatives reads
1
1- + ------------------------1
- + ------------------------------------------J B = --G  j   1 G  1 +  j  2 G
1
2
2
The storage and loss moduli are defined as the real and imaginary parts of the shear
modulus GB  1/JB, respectively
G' = real  G B  and G'' = imag  G B 
USER DEFINED
With the user-defined viscoelastic material model it is possible to directly enter
complex-valued expressions for the bulk and shear moduli or compliances, or for the
loss factor. The complex-valued bulk and shear moduli are entered in terms of storage
and loss moduli or compliances, respectively. The expressions can be functions taken
directly from interpolated data, or can be analytical expressions of the frequency
variable .
When the viscoelastic strain is deviatoric, the stress is computed from the shear storage
modulus and shear loss modulus as
 d = 2  G'    + jG''     d
492 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
or from the storage and loss compliances as
1
 d = 2 -------------------------------------  d
J'    + jJ''   
When the viscoelastic strain is volumetric, the pressure is computed from the bulk
storage modulus and bulk loss modulus
p = –  K'    + jK''      vol
or from the storage and loss compliances as
1
p = – --------------------------------------
Q'    + jQ''    vol
When loss factor damping is selected, the stress-strain relation is augmented by a
complex constitutive matrix
c
D =  1 + j v    D
where D is the constitutive matrix computed from the parent material, and Dc is the
complex constitutive matrix used to compute the viscoelastic stresses.
The User defined viscoelastic models are available for frequency domain
and eigenfrequency analyses only.
The internal variables for the frequencyf and angular frequency  are
named phys.freq and phys.omega. Here, phys is the name of the
physics interface, for instance solid.
TEMPERATURE EFFECTS
For many polymers, the viscoelastic properties have a strong dependence on the
temperature. A common assumption is that the material is thermorheologically simple
(TRS). In a material of this class, a change in the temperature can be transformed
directly into a change in the time scale. The reduced time is defined as
t
tr =
dt'
 -----------------------T  T  t'  
0
where T(T) is a temperature-dependent shift function.
MATERIAL MODELS
|
493
The implication is that the problem can be solved using the original material data,
provided that the time variable is transformed into the reduced time.
Think of the shift function T(T) as a multiplier to the viscosity in the dashpot in the
Generalized Maxwell model. This multiplier shifts the relaxation time, so
Equation 3-31 for a TRS material is modified to
ꞏ
 T  T  m  m +  m =  d
for all branches.
For the SLS model, the shift applies to the single relaxation time
ꞏ
 T  T  1  1 +  1 =  d
and for the Kelvin–Voigt model, the shift multiplies the right hand side in
Equation 3-36. In general, the shift function T will multiply all the relaxation times
or viscosities in a given viscoelasticity model.
Williams–Landel–Ferry Shift
One commonly used shift function is defined by the WLF (Williams–Landel–Ferry)
equation:
– C 1  T – T ref 
log   T  = ------------------------------------C 2 +  T – T ref 
where a base-10 logarithm is used. This shift is only valid over a certain temperature
range, typically around the glass transition temperature.
The first step to compute the shift function T(T) consists of building a master curve
based on experimental data. To do this, the curves of the viscoelastic properties (shear
modulus, Young’s modulus, and so forth) versus time or frequency are measured at a
reference temperature Tref. Then, the same properties are measured at different
temperatures.
494 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
The shift value of each curve, with respect to the master curve obtained at the
temperature Tref, defines the shift factor T(T). The constants C1 and C2 are material
dependent and are calculated after plotting log(T) versus T  Tref.
The shift factor at the reference temperature equals T(Tref) = 1, so that
Tref is the temperature at which the master curve is given. If the
temperature T drops below Tref  C2, the WLF equation is no longer
valid.
Since the master curve is measured at an arbitrary reference temperature Tref, the shift
function T(T) can be derived with respect to any temperature, and it is commonly
taken as the shift with respect to the glass transition temperature. The values C1 = 17.4
and C2 = 51.6 K are reasonable approximations for many polymers at this reference
temperature.
Arrhenius Shift
Below the Vicat softening temperature, the shift factor in polymers is normally
assumed to follow an Arrhenius law. In this case, the shift factor is given by the
equation
Q 1
1 -
log   T  = ----  --- – -------R T T ref
here, a base-e logarithm is used, Q is the activation energy (SI unit: J/mol), and R is
the universal gas constant.
Tool–Narayanaswamy–Moynihan Shift
Structural relaxation in glass can be modeled using the so-called Tool–
Narayanaswamy–Moynihan shift factor which is given as
Q  1–
1 -
log   T  = ----  --- + ------------ – -------RT
T
T 
f
ref
here, a base-e logarithm is used, Q is the activation energy (SI unit: J/mol), R is the
universal gas constant, T is the current temperature, Tref is a reference temperature, 
is a dimensionless activation energy fraction, and Tf is the so-called fictive
temperature. The fictive temperature is given as the weighted average of partial fictive
temperatures.
MATERIAL MODELS
|
495
 wi Tfi with  wi = 1
Tf =
i
i
Here, wi are the weights and Tfi are the partial fictive temperatures. The partial fictive
temperatures are determined from a system of coupled ordinary differential equations
(ODEs) which follow Tool’s equation
T – T fi
d
T = ----------------d t fi  T 
0i
here, 0i is a structural relaxation time.
STATIONARY ANALYSIS
For stationary analysis it is possible to select either the long-term stiffness, in which
case the stiffness of the viscoelastic branches is neglected, or the instantaneous stiffness,
in which case the contribution from all branches is used.
The instantaneous shear modulus G0 is defined as the sum of the stiffness of all the
branches
N
G0 = G +
 Gm
m=1
FREQUENCY DOMAIN ANALYSIS AND DAMPING
For Frequency-Domain Studies, Equation 3-29 and Equation 3-31 are simplified to
 d = 2  G' + jG''  d
where the shear storage modulus G' and the shear loss modulus G'' are user defined
expressions or are defined for the generalized Maxwell model as
N
G' = G +

m=1
2
  m 
G m ----------------------------2 and G'' =
1 +   m 
N
 m
 Gm ---------------------------2
1 +   
m=1
for the SLS model as
2
  1 
 1
G' = G + G 1 --------------------------2- and G'' = G 1 --------------------------21 +   1 
1 +   1 
496 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
m
for the Kelvin–Voigt model as
G' = G and G'' =  = G
The loss tangent is then computed from the ratio between the loss and storage moduli
G''
tan  = -----G'
where  is the phase angle between deviatoric stress and strain.
The internal work of viscous forces averaged over a time period 2 is computed as
Q h = G'' d conj   d 
EIGENFREQUENCY ANALYSIS
The direct use of frequency-dependent shear or bulk moduli, as described in
Frequency Domain Analysis and Damping, leads to a nonlinear eigenvalue problem.
COMSOL Multiphysics solves such nonlinear problems by expanding all nonlinear
expressions with quadratic polynomials around a frequency linearization point which
you can specify in the Eigenvalue Solver node. The linearized eigenvalue problem then
reads
2
 K   L  –  M u = 0
where L is the angular frequency at the linearization point. Thus, the solution of the
linearized system of equations depends on the choice of the linearization frequency L.
Selecting the linearization frequency closer to one of the eigenfrequencies will produce
a better result for that particular frequency, but not for all eigenfrequencies in the
study. Hence, the eigenfrequencies need to be computed one by one using a certain
iterative process that updates the linearization frequency L. This iterative procedure
is needed when fractional derivatives are used, and also for the User Defined
viscoelasticity model.
In order to avoid solving a nonlinear eigenvalue problem for the built-in viscoelasticity
models, the same procedure as for time-dependent analysis is used; that is, each
viscoelastic branch is represented by additional variables. For instance, for the The
Generalized Maxwell Model in an eigenfrequency analysis, Equation 3-31 reads
j m  m +  m = 
MATERIAL MODELS
|
497
The viscoelastic strain variables, m, are treated as additional degrees of freedom
(DOFs), and contribute to the damping and stiffness matrices of the coupled system
of equations.
This procedure results in a damped linear eigenvalue problem that can be solved using
the default eigenfrequency solver in a single run, for any specified number of
eigenfrequencies.
For more information see the Eigenfrequency section in the Studies and
Solvers chapter in the COMSOL Multiphysics Reference Manual.
An example of a nonlinear eigenvalue problem is shown in Eigenmodes of
a Viscoelastic Structural Damper: Application Library path
Structural_Mechanics_Module/Dynamics_and_Vibration/
viscoelastic_damper_eigenmodes
LOCAL TIME INTEGRATION
For the The Generalized Maxwell Model and the Standard Linear Solid Model it is
possible to use a local time integration algorithm for time-dependent analysis. By using
this algorithm, the degrees-of-freedom related to viscoelasticity are treated as internal
state variables, which makes the overall solution more efficient and also leaner in terms
of memory usage. The implemented algorithm is based on the method suggested in
Ref. 28, and it is schematically described in the following.
Consider the time evolution of a viscoelastic branch in the Generalized Maxwell model
characterized by an ODE of the type
ꞏ
m m + m =   t 
(3-37)
where m represents the viscoelastic strain in the m branch. The exact solution to
Equation 3-37 is then
t
n+1
m
1
t-  n + -----= exp  – -----   m m
m
n+1
 t n + 1 – s
-   s  ds
 exp  – -------------------m 
t
(3-38)
n
By assuming that the strain (t) varies linearly within time increments, the integral in
Equation 3-38 can be computed analytically, so the viscoelastic strain at increment
n  1 reads
498 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
t-
1 – exp  – -----  
n+1
n+1
n+1
n
m
t-   n –  n  – ----------------------------------m
= 
– exp  – -----
– 
m
  

t
m
------m
(3-39)
All variables in Equation 3-39 are evaluated at the increment n and are stored as
internal state variables. Equation 3-39 is solved for each branch in the Generalized
Maxwell model, or for the single branch in the Standard Linear Solid model.
See also the description of Viscoelasticity in the Solid Mechanics interface
documentation.
Large Strain Viscoelasticity
The implementation for large strain viscoelasticity follows the derivation by Holzapfel
(Ref. 1).
The generalized Maxwell model is based on the splitting of the strain energy density
into volumetric, isochoric, and the contribution from the viscoelastic branches
N
 m
W s = W iso + W vol +
m=1
The strain energy in the main hyperelastic branch is normally denoted with the
superscript  to denote the long-term equilibrium (as t  ).
The second Piola–Kirchhoff stress is computed from
S = 2
W s
= S iso + S vol +
C
N
 Qm
m=1
where the auxiliary second Piola–Kirchhoff stress tensors Qm are defined as
Qm = 2
 m
C
The time evolution of the auxiliary stress tensor Qm in each viscoelastic branch is given
by the rate
MATERIAL MODELS
|
499
1
ꞏ
ꞏ
Q m + ------- Q m = S iso,m
m
here, Siso,m is the isochoric second Piola–Kirchhoff stress tensor in the branch m.
These tensors are derived from the strain energy density in the main hyperelastic
branch and the energy factors m as
S iso m = 2
W iso m
W iso
= 2 m
=  m S iso
C
C
so the time evolution of the auxiliary stress tensor Qm is given by
1
ꞏ
ꞏ
Q m + ------- Q m =  m S iso
m
This equation is not well suited for modeling prestressed bodies. Applying the change
of variables
q m =  m S iso – Q m
the time evolution of the auxiliary stress tensor qm reads
 m qꞏ m + q m =  m S iso
For the The Generalized Maxwell Model, it is possible to write the Prony series in
terms of weights wm with respect to the instantaneous stiffness G0
N


t - 
  t  = G0  w +
w m exp  – -----
  
m 

m=1

Here, w is the ratio between the long term and instantaneous stiffness, w  GG0,
and the weight wm relates the branch stiffness to the instantaneous stiffness through
wm  GmG0. The weights are bounded by
N
w +
 wm = 1
m=1
Use this expression to relate the instantaneous stiffness in the small strain regime to the
large strain formulation. The instantaneous response for the second Piola–Kirchhoff
stress is computed from
500 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
N
S = S iso + S vol +
 m Siso
m=1
In this expression, the isochoric response represents the long term stiffness, and the
sum of the energy factors the contribution to the overall stiffness from the Maxwell
branches.
The weights in the Generalized Maxwell model for the small strain formulation are
related to the energy factors in the large strain formulation by
G0
Gm
 m = w m -------- = -------G
G
equivalently, the energy factors represent the ratio between the branch stiffness and the
long term stiffness in the main branch.
The volumetric contribution from the auxiliary stress tensor qm is
removed before adding these to the viscoelastic stresses per branch
Qm  mSiso  qm, so the stresses Qm are isochoric.
TEMPERATURE EFFECTS
The same options for defining Temperature Effects as described for Linear
Viscoelasticity are available for large strain viscoelasticity.
Hyperelastic Materials
A hyperelastic material is defined by its elastic strain energy density Ws, which is a
function of the elastic strain state. It is often referred to as the energy density. The
hyperelastic formulation normally gives a nonlinear relation between stress and strain,
as opposed to Hooke’s law in linear elasticity.
Most of the time, the right Cauchy–Green deformation tensor C is used to describe
the current state of strain (although one could use the left Cauchy–Green tensor B,
the deformation gradient tensor F, and so forth), so the strain energy density is written
as Ws(C).
For isotropic hyperelastic materials, any state of strain can be described in terms of
three independent variables — common choices are the invariants of the right
MATERIAL MODELS
|
501
Cauchy–Green tensor C, the invariants of the Green–Lagrange strain tensor, or the
principal stretches.
Once the strain energy density is defined, the second Piola–Kirchhoff stress is
computed as
S = 2
W s
C
In the general case, the expression for the energy Ws is symbolically evaluated down to
the components of C using the invariants definitions prior to the calculations of the
components of the second Piola–Kirchhoff stress tensor. The differentiation is
performed in components on the local coordinate system.
In Equation View, the definitions of the stress components are shown as
solid.Sl11 = 2*d(solid.Ws,solid.Cl11),
solid.Sl12 = d(solid.Ws,solid.Cl12), and so on. The factor 2 in
front of the differentiation operator for the shear stresses is omitted, since
the symmetry in the Cauchy–Green tensor will cause two equal
contributions.
Modeling Geometric Nonlinearity
For hyperelastic materials, the decomposition between elastic and inelastic
deformation is made using a multiplicative decomposition of the deformation gradient
–1
F el = FF in
Here, the inelastic deformation tensor Fin depends on the inelastic process, such as
thermal expansion, hygroscopic swelling, or plasticity.
In this case, the strain energy density depends on the elastic deformation only, Ws(Cel),
and the second Piola–Kirchoff stress can be written in terms of its elastic counterpart
–1
–T
S = J in F in S el F in
where Jin  det(Fin) and
502 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
S el = 2
W s
 C el
THERMAL EXPANSION AND THERMOELASTIC DAMPING
If thermal expansion is present, a stress-free volume change occurs. This is a pure
volumetric change, so the multiplicative decomposition of the deformation gradient
tensor in Equation 3-4 implies
det  F  = -------J
J el = --------------------det  F th 
J th
Here, the thermal volume ratio, Jth, depends on the thermal stretch th, which for
linear thermal expansion in isotropic materials can be written in terms of the isotropic
coefficient of thermal expansion, iso, and the absolute change in temperature
3 and 
J th =  th
th = 1 +  iso  T – T ref 
Here, the term isoT  Trefis the thermal strain. The isotropic thermal gradient is
therefore a diagonal tensor defined as
F th =  th I
The internal variables for the thermal stretch and the thermal volume
ratio are named solid.stchth and solid.Jth.
When the coefficient of thermal expansion  is anisotropic, the thermal strain is
computed from
 th =   T – T ref 
and the anisotropic thermal gradient is defined as
F th = I +  th
The tangent coefficient of thermal expansion can be computed then as
– 1 F th
 t = F th ----------T
On the opposite, when the tangent coefficient of thermal expansion is specified as a
function of temperature, the thermal strain can be found as
MATERIAL MODELS
|
503
 th = exp  H th  – I
where a matrix exponent is assumed, and the Hencky thermal strain tensor is defined as
T
H th =
Tref t    d
When the thermoelastic damping effect needs to be taken into account, the heat source
term can be computed as
M
Q ted = – T --------  t
t
where the Mandel stress tensor is introduced as M = CS .
HYGROSCOPIC SWELLING
Hygroscopic swelling is an internal strain caused by changes in moisture content. This
strain depends linearly on the moisture content
 hs =  h  c mo – c mo,ref 
where h is the coefficient of hygroscopic swelling, cmo is the moisture concentration,
and cmo,ref is the strain-free reference concentration. The coefficient of hygroscopic
swelling can represent isotropic or anisotropic swelling. The anisotropic hygroscopic
gradient is defined as
F hs = I +  hs
HYPERELASTICITY WITH PLASTICITY
It is possible to combine the hyperelastic material models with plasticity, viscoplasticity,
and creep. Since these models are primarily used for large strain applications, only the
large strain formulation is available. The decomposition between elastic and plastic
deformation is made using a multiplicative decomposition of the deformation gradient
tensor,
–1
F el = FF pl
504 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
Here, the plastic deformation tensor Fpl depends on the plastic flow rule, yield
function, and plastic potential.
• Multiplicative Decomposition
• Plastic Flow for Multiplicative Decomposition
• Creep and Viscoplasticity for Large Strains
ISOCHORIC ELASTIC DEFORMATION
For some classes of hyperelastic materials it is convenient to split the strain energy
density into volumetric (also called dilatational) and isochoric (also called
distortional or volume-preserving) contributions. The elastic deformation tensor is
then multiplicatively decomposed into the volumetric and isochoric components
F el = F el,vol F el
with Fel,vol as the volumetric elastic deformation (a diagonal tensor) and F el the
isochoric elastic deformation gradient. Isochoric deformation means that the volume
ratio is kept constant during deformation, so the isochoric elastic deformation is
computed by scaling it by the elastic volume ratio. The elastic volume ratio is defined
by
J el = det  F el  = det  F el,vol 
and the volumetric deformation as
1  3I
F el,vol = J el
By using Jel it is possible to define the isochoric-elastic deformation gradient
– 1/3
F el = J el
F el
the isochoric-elastic right Cauchy–Green tensor
T
– 2/3
C el = F el F el = J el
C el
and the isochoric-elastic Green–Lagrange strain tensor
1
 el = ---  C el – I 
2
MATERIAL MODELS
|
505
This scaling changes the eigenvalues of the tensor, but not its principal directions, so
the original and isochoric tensors remain coaxial to each other.
Some authors call F el and C el the modified tensors. Note that
det  F el  = det  C el  = 1
The internal variables for the isochoric-elastic Cauchy–Green
deformation tensor in local coordinate system are named solid.CIel11,
solid.CIel12, and so on.
The other two invariants normally used together with Jel are the first and second
invariant of the isochoric-elastic right Cauchy–Green deformation tensor
I 1  C el  and I 2  C el 
In these equations:
– 2/3
I 1  C el  = trace  C el  = J el
I 1  C el 
2
– 4/3
1 2
I 2  C el  = ---  I 1  C el  – trace  C el   = J el I 2  C el 
2
Since I 3  C el  = det  C el  = 1 , the third invariant is never explicitly used.
The internal variables for the invariants Jel, I 1  C el  , and I 2  C el  are
named solid.Jel, solid.I1CIel, and solid.I2CIel.
The invariants of the isochoric (modified) elastic Green–Lagrange strain tensor are
related to the invariants of the isochoric-elastic right Cauchy–Green deformation
tensor
1
I 1   el  = trace   el  = ---  I 1  C el  – 3 
2
1 2
1
I 2   el  = ---  I 1   el  – trace   el 2   = ---  I 2  C el  – 2I 1  C el  + 3 
2
4
506 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
1
I 3   el  = det   el  = ---  I 1  C el  – I 2  C el  
8
The internal variables for the invariants of the isochoric elastic Green–
Lagrange strain tensor are named solid.I1eIel, solid.I2eIel, and
solid.I3eIel.
COUPLED AND UNCOUPLED RESPONSES
The isochoric and volumetric responses of most materials are coupled (Ref. 12), in this
case, the strain energy density is written as a function of the elastic deformation
W s = W s  C el 
however, in many situations it is possible to assume that the pressure and deviatoric
stress are uncoupled, and therefore for numerous hyperelastic materials it is possible to
define the strain energy density as the sum of isochoric and volumetric counterparts
W s = W iso  C el  + W vol  J el 
here, C el is the isochoric elastic right Cauchy–Green deformation tensor, and Jel is
the elastic volume ratio.
VOLUMETRIC RESPONSE
The volumetric strain energy density, Wvol, is defined as an expression of the elastic
volumetric deformation Jel and the bulk modulus .
The Quadratic volumetric strain energy density is defined as:

2
W vol  J el  = ---  J el – 1 
2
(3-40)
The Logarithmic volumetric strain energy density (Ref. 12) is defined as:
2

W vol  J el  = ---  ln J el 
2
(3-41)
The Hartmann–Neff volumetric strain energy density (Ref. 13) is defined as:
–5
 5
W vol  J el  = ------  J el + J el – 2 
50
(3-42)
The Miehe volumetric strain energy density (Ref. 15) is defined as:
MATERIAL MODELS
|
507
W vol  J el  =   J el – ln J el – 1 
(3-43)
and the Simo–Taylor volumetric strain energy density (Ref. 16) is defined as:
 2
W vol  J el  = ---  J el – 2 ln J el – 1 
4
(3-44)
For a given volumetric strain energy density, the volumetric stress (pressure) is
calculated as
W vol
p m = – ------------J el
(3-45)
When the quadratic expression in Equation 3-40 is used, the pressure becomes linearly
related to the volume change:
p m = –   J el – 1 
but for other volumetric representations the pressure becomes a nonlinear function of
the volume change. For instance, if the expression in Equation 3-42 is used instead of
the quadratic function, the pressure reads
4
–6
1
p m = – ------   J el – J el 
10
THE LOCKING PROBLEM
A numerical scheme is said to exhibit locking if the accuracy of the approximation
deteriorates as a parameter tends to a limiting value (Ref. 17). Finite elements in solid
mechanics are said to “lock” when exhibiting an unphysical response to deformation
(Ref. 18). Locking can occur for many different reasons. For linear elastic materials,
this typically happens as Poisson’s ratio tends to 0.5, or the bulk modulus is much
larger than the shear modulus. Numerical errors arise because the shape functions are
unable to properly describe the volume preserving deformation.
To avoid the locking problem in computations, the mixed formulation replaces pm in
Equation 3-45 with a corresponding interpolated pressure help variable pw, which
adds an extra degree of freedom to the ones defined by the displacement vector u.
The general procedure is the same as described in Mixed Formulation for Linear
Elastic materials.
508 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
INCOMPRESSIBLE HYPERELASTIC MATERIALS
For incompressible hyperelastic materials, the volumetric strain energy density Wvol is
not defined at all, and the strain energy density Ws consists only of the isochoric
contribution and the incompressibility constraint
W s  u p w  = W iso –  J el – 1  p w
Instead of deriving the pressure from the volumetric strain energy, a weak constraint is
added to account for the incompressibility condition
J el = 1
The auxiliary pressure variable, pw, acts as Lagrange multiplier to enforce the
constraint Jel  1. This variable, positive in compression, is then used as the pressure
when computing stresses.
The contribution to the virtual work is
W = –
V S: dv + V   Jel – 1 pw dv
The second Piola–Kirchhoff stress is then given by
W iso
–1
S = 2 -------------- – p w JC
C
(3-46)
and the Cauchy stress tensor by
W iso
 = J – 1 FSF T = 2J –1 F -------------- F T – p w I
C
(3-47)
NEARLY INCOMPRESSIBLE HYPERELASTIC MATERIALS
For nearly incompressible hyperelastic materials, the strain energy density Ws is
decoupled into isochoric and volumetric counterparts:
W s = W iso + W vol
here, Wiso is the isochoric strain energy density and Wvol is the volumetric strain energy
density.
MATERIAL MODELS
|
509
The isochoric strain energy density depends on the material model, and it can be an
expression involving the following:
• Components of the isochoric elastic right Cauchy–Green tensor C el in the local
coordinate system.
• Principal invariants of the isochoric elastic right Cauchy–Green tensor C el .
• Principal invariants of the isochoric elastic Green–Lagrange strain  el .
• For User Defined hyperelastic materials, it is also possible to define the strain energy
density in terms of components of the isochoric elastic deformation gradient F el .
The volumetric strain energy density can be any of the expression described in
Volumetric Response. The default value for the bulk modulus is set to 100 times the
equivalent shear modulus at infinitesimal deformation, which gives an initial Poisson’s
ratio of approximately   0.495.
An auxiliary variable, pw, is added to map the pressure pm derived from the volumetric
strain energy density as described in Equation 3-45.
Then the variational problem is computed by the so-called perturbed Lagrangian
method (Ref. 19), so the contribution to the virtual work reads
W = –
1
V S: dv + V  ---  pw – pm pw dv
The second Piola–Kirchhoff stress is then defined as
W iso
–1
S = 2 -------------- – p w JC
C
(3-48)
where the extra pressure variable satisfies the weak constraint
W vol
p w = p m where p m = – ------------J el
the Cauchy stress tensor then reads
W iso
 = J – 1 FSF T = 2J –1 F -------------- F T – p w I
C
Using the Quadratic volumetric strain energy density results in the only
mixed formulation that returns a symmetric coupled stiffness matrix.
510 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
PREDEFINED HYPERELASTIC MATERIAL MODELS
Different hyperelastic material models are constructed by specifying different elastic
strain energy expressions. There are several predefined material models, as well as the
option to enter user defined expressions for the isochoric and volumetric strain energy
densities.
NEO-HOOKEAN
The strain energy density for the Compressible, coupled version of the Neo-Hookean
material is written in terms of the elastic volume ratio Jel and the first invariant of the
elastic right Cauchy–Green deformation tensor I1Cel (Ref. 11, 14)
1
2
1
W s = ---   I 1 – 3  –  ln  J el  + ---  ln  J el 
2
2
Here,  and  are the Lamé parameters (SI unit: Pa).
In Ref. 8 the coupled strain energy density is defined from Lamé parameters
 –
1
2 W s = ---   I 1 – 3  – ---  J el
– 1  with  = --- = --------------
2

1 – 2
The Compressible, uncoupled and Nearly incompressible versions use the isochoric
invariant I 1  C el  to define the isochoric strain energy density
1
W s = W iso + W vol = ---   I 1 – 3  + W vol
2
where the volumetric strain energy Wvol can use any of the expressions described in
Volumetric Response. See Nearly Incompressible Hyperelastic Materials for details.
The Incompressible option uses the same isochoric strain energy, but an extra variable
is added to enforce the incompressibility condition Jel  1, see Incompressible
Hyperelastic Materials.
It is possible to define the isotropic hyperelastic material from other pair
of elastic moduli, see the conversion from one set of elastic moduli to
Lamé parameters in Table 3-1.
See also the description of the Neo-Hookean material model in the Solid
Mechanics interface documentation.
MATERIAL MODELS
|
511
ST VENANT–KIRCHHOFF
One of the simplest hyperelastic material models is the St Venant–Kirchhoff material,
which is an extension of a linear elastic material into the hyperelastic regime.
For the Compressible, coupled response, the elastic strain energy density is written with
two parameters and two invariants of the elastic Green–Lagrange strain tensor, I1el
and I2el
1
W s = ---   + 2 I 12 – 2I 2
2
Here,  and  are Lamé parameters (SI unit: Pa). The bulk modulus  is calculated
from     23
The Compressible, uncoupled and the Nearly incompressible versions use the isochoric
invariants I 1   el  and I 2   el  to define the isochoric strain energy density
1
W iso = ---   + 2 I 1 2 – 2I 2
2
The elastic volume ratio Jel and the bulk modulus  are used to define the volumetric
strain energy density Wvol, see Volumetric Response and Nearly Incompressible
Hyperelastic Materials.
It is possible to define the isotropic hyperelastic material from other pair
of elastic moduli, see the conversion from one set of elastic moduli to
Lamé parameters in Table 3-1.
See also the description of the St Venant–Kirchhoff material model in the
Solid Mechanics interface documentation.
MOONEY–RIVLIN, TWO PARAMETERS
For the Compressible, uncoupled and Nearly incompressible versions, the isochoric strain
energy density is written in terms of the two isochoric invariants of the elastic right
Cauchy–Green deformation tensors I 1  C el  and I 2  C el 
W iso = C 10  I 1 – 3  + C 01  I 2 – 3 
The material parameters C10 and C01 (SI unit: Pa) are related to the Lamé parameter
(shear modulus)   C10  C01
512 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
The elastic volume ratio Jel and the bulk modulus are used to define the volumetric
strain energy density Wvol, see Volumetric Response and Nearly Incompressible
Hyperelastic Materials.
The Incompressible option uses the same isochoric strain energy, but an extra variable
is added to enforce the incompressibility condition Jel  1, see Incompressible
Hyperelastic Materials
See also the description of the Mooney–Rivlin, Two Parameters material
model in the Solid Mechanics interface documentation.
MOONEY–RIVLIN, FIVE PARAMETERS
Rivlin and Saunders (Ref. 2) proposed a phenomenological model for small
deformations in rubber-based materials on a polynomial expansion of the first two
invariants of the elastic right Cauchy–Green deformation, so the strain energy density
is written as an infinite series

Ws =

  Cmn  I1 – 3 m  I2 – 3  n
m = 0n = 0
with C00  . This material model is sometimes also called polynomial hyperelastic
material.
In the first-order approximation, the material model recovers the Mooney–Rivlin
strain energy density
W s = C 10  I 1 – 3  + C 01  I 2 – 3 
while the second-order approximation incorporates second-order terms
W s = C 10  I 1 – 3  + C 01  I 2 – 3  + C 20  I 1 – 3  2 + C 02  I 2 – 3  2 + C 11  I 1 – 3   I 2 – 3 
The Compressible, uncoupled and the Nearly incompressible versions use the isochoric
invariants of the elastic right Cauchy–Green deformation tensors I 1  C el  and I 2  C el 
to define the isochoric strain energy density
2
W iso =
2
  Cmn  I1 – 3   I2 – 3 
m
n
m = 0n = 0
MATERIAL MODELS
|
513
The elastic volume ratio Jel and the bulk modulus are used to define the volumetric
strain energy density Wvol, see Volumetric Response and Nearly Incompressible
Hyperelastic Materials.
The incompressible option uses the same isochoric strain energy, but an extra variable
is added to enforce the incompressibility condition Jel  1, see Incompressible
Hyperelastic Materials.
See also the description of the Mooney–Rivlin, Five Parameters material
model in the Solid Mechanics interface documentation.
MOONEY–RIVLIN, NINE PARAMETERS
The Mooney–Rivlin, nine parameters material model is an extension of the polynomial
expression to third order terms and the strain energy density is written as
3
W iso =
3
  Cmn  I1 – 3   I2 – 3 
m
n
m = 0n = 0
where I 1  C el  and I 2  C el  are the isochoric invariants of the elastic right Cauchy–
Green deformation tensors.
The elastic volume ratio Jel and the bulk modulus  are used to define the volumetric
strain energy density Wvol, see Volumetric Response and Nearly Incompressible
Hyperelastic Materials.
The Incompressible option uses the same isochoric strain energy, but an extra variable
is added to enforce the incompressibility condition Jel  , see Volumetric Response
and Incompressible Hyperelastic Materials.
See also the description of the Mooney–Rivlin, Nine Parameters material
model in the Solid Mechanics interface documentation.
YEOH
Yeoh proposed (Ref. 1) a phenomenological model in order to fit experimental data of
filled rubbers, where Mooney–Rivlin and Neo-Hookean models were to simple to
describe the stiffening effect in the large strain regime. The strain energy was fitted to
experimental data by means of three parameters (SI unit: Pa), and the first invariant of
the elastic right Cauchy–Green deformation tensors I1Cel
514 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
Ws = c1  I1 – 3  + c2  I1 – 3  2 + c3  I1 – 3  3
The shear modulus depends on the deformation, and it is calculated as
 W s W s
 = 2
+
 = 2c 1 + 4c 2  I 1 – 3  + 6c 3  I 1 – 3  2
  I1  I2 
This imposes a restriction on the coefficients c1, c2, c3, since   0.
The Compressible, uncoupled and the Nearly incompressible versions use the isochoric
invariant of the elastic right Cauchy–Green deformation tensor I 1  C el  to define the
isochoric strain energy density
W iso = c 1  I 1 – 3  + c 2  I 1 – 3  2 + c 3  I 1 – 3  3
The elastic volume ratio Jel and the bulk modulus are used to define the volumetric
strain energy density Wvol, see Volumetric Response and Nearly Incompressible
Hyperelastic Materials.
The Incompressible option uses the same isochoric strain energy, but an extra variable
is added to enforce the incompressibility condition Jel  1, see Incompressible
Hyperelastic Materials.
See also the description of the Yeoh material model in the Solid
Mechanics interface documentation.
OGDEN
The Neo-Hookean material model usually fits well to experimental data at moderate
strains but fails to model hyperelastic deformations at high strains. In order to model
rubber-like materials at high strains, Ogden adapted (Ref. 1) the energy of a
Neo-Hookean material to
N
Ws =
p
p
p
p
-   +  el2 +  el3 – 3 
 ---- p el1
p=1
Here p (SI unit: Pa) and p (dimensionless) are material parameters, and el1, el2,
and el3 are the principal elastic stretches such as Jel  el1el2el3.
MATERIAL MODELS
|
515
The Ogden model is empirical, in the sense that it does not relate the material
parameters p and p to physical phenomena. The parameters p and p are obtained
by curve-fitting measured data, which can be difficult for N  2. The most common
implementation of Ogden material is with N  2, so four parameters are needed.
The Compressible, uncoupled and the Nearly incompressible versions use the isochoric
elastic stretches
13
 eli =  eli  J el
so the isochoric strain energy density is defined as
N
W iso =
p
p
p
p
-   +  el2 +  el3 – 3 
 ---- p el1
p=1
The isochoric elastic stretches define a volume preserving deformation, since
 el1  el2  el3 =  el1  el2  el3  J el = 1
The shear modulus at infinitesimal deformation is then defined from
N
1
 = --2
 p p
p=1
The elastic volume ratio Jel and the bulk modulus are used to define the volumetric
strain energy density Wvol, see Volumetric Response and Nearly Incompressible
Hyperelastic Materials.
The Incompressible option uses the same isochoric strain energy, but an extra variable
is added to enforce the incompressibility condition Jel  , see Incompressible
Hyperelastic Materials.
Sometimes a slightly different definition of the strain energy function for
the Ogden material is used. If you have given material data for an Ogden
material, be careful that the definitions used are the same. If not, you will
need to rescale the p coefficients.
516 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
See also the description of the Ogden material model in the Solid
Mechanics interface documentation.
STORAKERS
The Storakers material (Ref. 18 and Ref. 25) is used to model highly compressible
foams. The strain energy density is written in a similar fashion as in Ogden material:
N
Ws =
2 k
k
k
k
– k k
-   +  el2 +  el3 – 3 + -----  J el
 -------2  el1
k

k=1
1
– 1 

k
The initial shear and bulk moduli are computed from the parameters k (SI unit: Pa)
and k (dimensionless) as
N
N
 =

 k and  =
 2k  k + --3-
1
k=1
k=1
for constantparameters k  , the initial bulk modulus becomes   2  1/3, so a
stable material requires    and   1/3. In this case, the Poisson’s ratio is given by
  2  2/3, which means that for a Poisson’s ratio larger than  2/9 is
needed.
See also the description of the Storakers material model in the Solid
Mechanics interface documentation.
VARGA
The Varga material model (Ref. 1) describes the strain energy in terms of the elastic
stretches as
W s = c 1   el1 +  el2 +  el3 – 3  + c 2   el1  el2 +  el2  el3 +  el1  el3 – 3 
The Compressible, uncoupled and Nearly incompressible versions use the isochoric elastic
stretches defined as
13
 eli =  eli  J el
to define the isochoric strain energy density:
MATERIAL MODELS
|
517
W iso = c 1   el1 +  el2 +  el3 – 3  + c 2   el1  el2 +  el2  el3 +  el1  el3 – 3 
The simplest Varga model is obtained by setting c1   and c2  
W iso =    el1 +  el2 +  el3 – 3 
The elastic volume ratio Jel and the bulk modulus are used to define the volumetric
strain energy density Wvol, see Volumetric Response and Nearly Incompressible
Hyperelastic Materials.
The Incompressible option uses the same isochoric strain energy, but an extra variable
is added to enforce the incompressibility condition Jel  1, see Incompressible
Hyperelastic Materials.
See also the description of the Varga material model in the Solid
Mechanics interface documentation.
ARRUDA–BOYCE
The other hyperelastic materials described are phenomenological models in the sense
that they do not relate the different material parameters (normally obtained by
curve-fitting experimental data) to physical phenomena.
Arruda and Boyce (Ref. 3) derived a material model based on Langevin statistics of
polymer chains.
The strain energy density is defined by
 chain

W s = nk B TN  --------------  + ln  --------------------- 
  lock
 sinh    
here, n is the chain density, kB is Boltzmann constant, T is the absolute temperature,
and  is computed from the inverse Langevin function   L1chainlock.
The number of segments in the polymeric chain, N, is used to derive the locking
stretch of the chain,  lock = N , and the equivalent chain stretch chain is computed
from the first invariant of the elastic right Cauchy–Green deformation tensor I1Cel,
 chain = I 1  3 .
The macroscopic shear modulus is defined as 0  nkBT. This material model is
sometimes also called the eight-chain model.
518 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
In Ref. 3, a series expansion of the inverse Langevin function is used to simplify the
expression for the strain energy density. In this case, the strain energy density reads

Ws = 0
cp
-I – 3 
 -------------p–1 1
N
p
p
p=1
Here, 0 is the initial macroscopic shear modulus, I1Cel is the first invariant of the
elastic right Cauchy–Green deformation tensor, and the coefficients cp are obtained by
series expansion of the inverse Langevin function.
Arruda and Boyce truncated the series and used only the first five terms. The
coefficients cp (dimensionless) are listed in Table 3-2:
TABLE 3-2: FIRST FIVE COEFFICIENTS OF ARRUDA–BOYCE MATERIAL MODEL.
C1
C2
C3
C4
C5
1/2
1/20
11/1050
19/7000
519/673750
Other authors (Ref. 1) use only the first three terms of the series.
The Compressible, uncoupled and Nearly incompressible versions use the isochoric
invariant I 1 = I 1  C el  to define the isochoric strain energy density, so when using the
inverse Langevin function the chain stretch is defined as  chain = I 1  3 , and in the
five terms approximation the isochoric strain energy is defined as
5
W iso =  0
cp
p
-I – 3 
 -------------p–1 1
N
p
p=1
Then, the elastic volume ratio Jel and the bulk modulus are used to define the
volumetric strain energy density Wvol, see Volumetric Response and Nearly
Incompressible Hyperelastic Materials.
The Incompressible option uses the same isochoric strain energy, but an extra variable
is added to enforce the incompressibility condition Jel  , see Incompressible
Hyperelastic Materials.
See also the description of the Arruda–Boyce material model in the Solid
Mechanics interface documentation.
MATERIAL MODELS
|
519
GENT
Many hyperelastic material models are difficult to fit to experimental data. The Gent
material (Ref. 20 and Ref. 21) is a simple phenomenological constitutive model based
on only two parameters,  and jm, which defines the strain energy density as

I 1 – 3
Ws = – 
--- j m log  1 – -------------
2
jm 

Here,  (SI unit: Pa) is the shear modulus and jm (dimensionless) is a limiting value
for I1  3, which takes care of the limiting polymeric chain extensibility of the material.
Since the strain energy density does not depend on the second invariant I2, the Gent
model is often classified as a generalized Neo-Hookean material. The strain energy
density tends to be the one of incompressible Neo-Hookean material as jm  . The
Gent material is the simplest model of the limiting chain extensibility family.
The Compressible, uncoupled and Nearly incompressible formulations use the isochoric
invariants I 1  C el  to define the isochoric strain energy density

I 1 – 3
W iso = – 
--- j m log  1 – -------------
jm 
2

The elastic volume ratio Jel and the bulk modulus are used to define the volumetric
strain energy density Wvol, see Volumetric Response and Nearly Incompressible
Hyperelastic Materials.
The Incompressible option uses the same isochoric strain energy, but an extra variable
is added to enforce the incompressibility condition Jel  , see Incompressible
Hyperelastic Materials.
See also the description of the Gent material model in the Solid
Mechanics interface documentation.
VAN DER WAALS
Kilian and co-workers formulated a van der Waals equation of state for real networks
of polymer chains from the analogy of an ideal gas (Ref. 22–24). The constitutive
model is based on four parameters which define the averaged invariant
I = I 1 +  1 –  I 2
520 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
the variable 
 =
I–3
---------------2
m – 3
and the function
f    = – log  1 –   – 
in order to define the isochoric strain energy density
3
---

2
2 I – 3 2
W iso =     m – 3 f    – -------  ----------- 
3
2


Here,  (SI unit: Pa) is the shear modulus. The maximum chain stretch m
(dimensionless) represents a limiting value for the averaged invariant I , which
accounts for the maximum chain extensibility in networks with finite chain lengths.
The dimensionless parameter  phenomenologically averages the two isochoric
invariants I 1 and I 2 , and the parameter  (dimensionless) represents the global
interaction between polymer chains.
The Compressible, uncoupled and Nearly incompressible formulations use the elastic
volume ratio Jel and the bulk modulus to define the volumetric strain energy density
Wvol, see Volumetric Response and Nearly Incompressible Hyperelastic Materials.
The Incompressible option uses the same isochoric strain energy, but an extra variable
is added to enforce the incompressibility condition Jel  ; see Incompressible
Hyperelastic Materials
See also the description of the van der Waals material model in the Solid
Mechanics interface documentation.
BLATZ–KO
The Blatz–Ko material model was developed for foamed elastomers and polyurethane
rubbers, and it is used to model compressible isotropic hyperelastic materials (Ref. 1,
26).
The elastic strain energy density is written with three parameters and the three
invariants of the elastic right Cauchy–Green deformation tensor, I1Cel, I2Cel, and
I3Cel  Jel2
MATERIAL MODELS
|
521

1 –
 I
1 
W s =  ---   I 1 – 3  + ---  I 3 – 1  +  1 –   ---   ----2- – 3 + ---  I 3 – 1 

 

2

2 I
3
Here,  is an interpolation parameter bounded to 0    1, the parameter  (SI unit:
Pa) is the shear modulus, and  is an expression of Poisson’s ratio,   1  2, or
Lamé parameters,   /2.
When the parameter   , or equivalently, Poisson’s ratio tends to 0.5; the strain
energy simplifies to a similar form of the Mooney–Rivlin, Two Parameters model

 I
W s =  ---  I 1 – 3  +  1 –   ---  ----2- – 3

2
2I
3
In the special case of   1, the strain energy reduces to a compressible Neo-Hookean
model (use 2    2/(1  2),
 – 2

W s = ---  I 1 – 3  + ------  J
– 1
2
2
This expression is also equivalent to the compressible Storakers model consisting in
one term, and the material parameter defined as 1  2
See also the description of the Blatz–Ko material model in the Solid
Mechanics interface documentation.
GAO
Gao proposed (Ref. 27) a simple compressible hyperelastic material where the strain
energy density is defined by two parameters, a (SI unit: Pa) and n, and two invariants
of the elastic right Cauchy–Green deformation tensors Cel:
n
n
Ws = a  I1 + I –1 
Here, the invariant I1Celis calculated as in the Blatz–Ko model:
I 2  C el 
–1
I –1 = trace  C el  = -----------------I 3  C el 
Gao proposed that the material is unconditionally stable when the parameters are
bounded to 1  n  3 and 0  a, and related these parameters under small strain to the
Young’s modulus and Poisson’s ratio by
522 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
n 2
3 n 8a- and  = ---------------n – 1E = ------------------2n + 1
2n + 1
Since n  1  1  2 and it is bounded to 1  n  3, this material is stable for an
initial Poisson’s ratio in the range of 0    27
See also the description of the Gao material model in the Solid Mechanics
interface documentation.
MURNAGHAN
The Murnaghan strain energy density is used in nonlinear acoustoelasticity. Most
conveniently, it is expressed in terms of the three invariants of the elastic Green–
Lagrange strain tensor, I1el, I2el, and I3el:
1
1
W s = ---   + 2 I 12 – 2I 2 + ---  l + 2m I 13 – 2mI 1 I 2 + nI 3
3
2
Here, l, m, and n (SI unit: Pa) are the Murnaghan third-order elastic moduli, which
can be found experimentally for many commonly encountered materials such as steel
and aluminum, and  and  are the Lamé parameters. Setting the Murnaghan moduli
to zero, l  m  n  , recovers a compressible St Venant–Kirchhoff material.
See also the description of the Murnaghan material model in the Solid
Mechanics interface documentation.
DELFINO
Delfino proposed a simple hyperelastic material for modeling carotid arteries (Ref. 29).
The strain energy density is defined by two parameters, a (SI unit: Pa) and b
(dimensionless), and the first invariant of the isochoric elastic right Cauchy–Green
deformation tensors I 1  C el  :
b
---  I – 3 

a 2 1
W iso = ---  e
– 1
b

The parameter a plays the role of shear modulus at the small strain limit.
MATERIAL MODELS
|
523
The Compressible, uncoupled and Nearly incompressible formulations use the elastic
volume ratio Jel and the bulk modulus to define the volumetric strain energy density
Wvol, see Volumetric Response and Nearly Incompressible Hyperelastic Materials.
The Incompressible option uses the isochoric strain energy, and an extra variable is
added to enforce the incompressibility condition Jel  1, see Incompressible
Hyperelastic Materials.
FUNG
Fung (Ref. 29) proposed one of the most popular strain energy functions to describe
the deformation in soft biological tissues and arteries. For this compressible
hyperelastic material, the strain energy density reads
c Q
W s = ---  e – 1 
2
the parameter c (SI unit: Pa) scales the global stiffness, and the quadratic form Q
(dimensionless) depends on the Green–Lagrange strain
T
Q = E AE
here, A is a 6-by-6 symmetric matrix (dimensionless), and E is a vector which contains
the elements of the elastic Green–Lagrange strain tensor sorted in either standard or
Voigt order, see Orthotropic and Anisotropic Materials.
For modeling the deformation in arteries, Fung proposed that the principal directions
of the strain tensor coincide with the radial, circumferential, and axial directions of the
artery, so the coefficient matrix A is described by nine independent parameters
(Ref. 29), see Orthotropic Material to see the structure of such matrix.
The Compressible, uncoupled and Nearly incompressible formulations use the
components of the isochoric elastic Green–Lagrange strain E el to define the isochoric
strain energy density
c Q
W iso = ---  e – 1 
2
where
T
Q = E AE
524 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
also, these formulations use the elastic volume ratio Jel and the bulk modulus to
define the volumetric strain energy density Wvol, see Volumetric Response and Nearly
Incompressible Hyperelastic Materials.
The Incompressible option uses the same isochoric strain energy, but an extra variable
is added to enforce the incompressibility condition Jel  , see Incompressible
Hyperelastic Materials.
EXTENDED TUBE
The extended tube model is a micromechanics-inspired material model that considers
the network constraints from molecular chains and the limited chain extensibility
(Ref. 33–35). The isochoric strain energy density of the model consists of two terms
W iso = W c + W e
The term Wc represents the energy from the cross-linking of the network, and We
represents the energy from confining tube constrains. These are written as
Gc   1 –    I1 – 3 

W c = ------  ------------------------------------+ log  1 –   I 1 – 3  
2  1 – I – 3

1
and
2G e – 
–
–
-   el1 +  el2 +  el3 – 3 
W e = --------2

Here, Gc and Ge are material parameters (SI unit: Pa), I 1 = I 1  C el  is the first
invariant of the elastic right Cauchy–Green deformation tensor,  el are the isochoric
principal stretches, and and  are dimensionless coefficients.
The parameters Gc and Ge plays the role of shear modulus at the small strain limit,
G0  Gc  Ge. The parameter  corresponds to the maximum finite chain extensibility,
as the strain energy Wc is singular for stretch values such as I 1 – 3 = 1   .
The Compressible, uncoupled and Nearly incompressible formulations use the elastic
volume ratio Jel and the bulk modulus to define the volumetric strain energy density
Wvol, see Volumetric Response and Nearly Incompressible Hyperelastic Materials.
The Incompressible option uses the isochoric strain energy, and it adds an extra variable
to enforce the incompressibility condition Jel  , see Incompressible Hyperelastic
Materials.
MATERIAL MODELS
|
525
Note that the material might be unstable for certain combinations of material
parameters, see Ref. 33-34 for a valid range of parameter values.
USER DEFINED
It is possible to define the strain energy density for compressible, nearly incompressible
or incompressible hyperelastic materials when selecting the user defined option.
For Compressible hyperelastic materials, enter an expression for the elastic strain energy
Ws, which can include any expressions involving the following:
• Components of Cel, the elastic right Cauchy–Green deformation tensor in the local
material coordinate system.
• Principal invariants of Cel
I 1  C el  = trace  C el 
2
1 2
I 2  C el  = ---  I 1  C el  – trace  C el  
2
I 3  C el  = det  C el 
The internal variables for these invariants are named solid.I1Cel,
solid.I2Cel, and solid.I3Cel.
• Components of the elastic Green–Lagrange strain tensor elin the local coordinate
system.
• Principal elastic stretches el1, el2, and el3, which are the square-root of the
eigenvalues of the elastic right Cauchy–Green deformation tensor Cel.
The internal variables for the principal elastic stretches are named
solid.stchelp1, solid.stchelp2, and solid.stchelp3.
• Invariants of the elastic Green–Lagrange strain tensor. Since
1
 el = ---  C el – I 
2
the invariants of el are written in terms of the invariants of Cel:
1
I 1   el  = trace   el  = ---  I 1  C el  – 3 
2
526 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
2
1 2
1
I 2   el  = ---  I 1   el  – trace   el   = ---  I 2  C el  – 2I 1  C el  + 3 
2
4
1
I 3   el  = det   el  = ---  I 3  C el  – I 2  C el  + I 1  C el  – 1 
8
The internal variables for these invariants are named solid.I1eel,
solid.I2eel, and solid.I3eel.
When the Nearly incompressible option is selected, the elastic strain energy is decoupled
into the volumetric and isochoric components:
• The volumetric strain energy Wvol, which can be an expression involving the elastic
volume ratio J  detFel
• The isochoric strain energy, Wiso, as an expression involving the invariants of the
isochoric elastic right Cauchy–Green tensor I 1  C el  and I 2  C el  ; the invariants of
the isochoric elastic Green–Lagrange strain I 1   el  , I 2   el  , and I 3   el  ; or the
13.
principal isochoric elastic stretches defined as  eli =  eli  J el
When the Nearly incompressible option is selected, an extra variable is added to map the
pressure, see The Locking Problem and Nearly Incompressible Hyperelastic Materials
for details.
The internal variables for Jel, I 1  C el  , and I 2  C el  are named
solid.Jel, solid.I1CIel, and solid.I2CIel.
The internal variables for I 1   el  , I 2   el  , and I 3   el  are named
solid.I1eIel, solid.I2eIel, and solid.I3eIel.
When the Incompressible option is selected, enter an expression for the isochoric elastic
strain energy Wiso, as is done for the Nearly incompressible option. An extra variable is
MATERIAL MODELS
|
527
added to enforce the incompressibility condition Jel  , see Incompressible
Hyperelastic Materials and Mixed Formulation.
The strain energy density must not contain any other expressions
involving displacement or their derivatives. Examples of such expressions
are components of the displacement gradient u and deformation
gradient F  u  I tensors, their transpose, inversions, as well as the
global material system components of C and . If they occur, such
variables are treated as constants during symbolic differentiations.
Select the Use elastic deformation gradient check box to define the elastic
strain energy density Ws, the isochoric strain energy density, Wiso, and the
volumetric strain energy, Wvol, in terms of the components the elastic
deformation gradient Fel.
Then, the second Piola–Kirchhoff stress is defined from
– 1 W s
S = F ---------- .
F
See also the description of the User Defined material model in the Solid
Mechanics interface documentation.
MULLINS EFFECT
Some nonlinear effects observed in rubbers, such as hysteresis in stress-stretch curves,
residual strains, and stress softening effects, are not accounted in the formulation of
common hyperelastic materials. The Mullins effect (Ref. 43-45) describes the
stress-softening phenomenon observed under cyclic loading in elastomers and
biological materials.
Ogden and Roxburgh (Ref. 46) used an additional state variable to model the Mullins
effect. The state variable is introduced to memorize the microstructural damage on
reinforced rubber after repeated loading-unloading cycles. The modified isochoric
strain energy density reads
W iso = W iso +    
528 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
here, Wiso is the isochoric strain energy of the undamaged material, and is referred
as the damage function. The choice of the damage function is completely
arbitrary as long as some constrains are fulfilled. The authors (Ref. 46) proposed a state
function based on the error function, which defined how the state variable  varies as
a function of the isochoric strain energy
W max – W iso
1
 = 1 – --- erf  --------------------------------

r 
m
here, erfis the error function, r and m are positive parameters, and Wmax is the
maximum attained value of the isochoric strain energy density on the loading path.
The associated microstructural damage is computed from
W max – W iso
1
d = 1 –  = --- erf  --------------------------------
m
r
and the isochoric strain energy modified by the Mullins effect reads
W iso =  1 – d W iso
Over the years others authors (Ref. 47-48) have proposed different flavors of Ogden–
Roxburgh model, the version implemented in COMSOL Multiphysics uses by default
the hyperbolic tangent function, and a parameter to define the maximum allowed
damage d  1r. The microstructural damage is then computed from
W max – W iso
d = d  tanh  -------------------------------------
W sat + W max
Here, d, , and Wsat are positive parameters. It is also possible to use the error
function as in the original formulation (Ref. 46), in which case the microstructural
damage is computed from
W max – W iso
d = d  erf  -------------------------------------
 W sat + W max
Miehe (Ref. 49) proposed an exponential expression for the damage variable in order
to model the Mullins effect
d = d  1 – e
– W max  W sat

where Wsat and d are positive parameters.
MATERIAL MODELS
|
529
Distributed Fiber Models
Composite materials are made out of an isotropic matrix reinforced with fibers. In
these reinforced materials, the fibers act as the main load carrier, while the surrounding
matrix supports the fibers and transfers loads to them. These materials are either
manufactured or have a natural origin such as biological tissue, leafs, or wood.
In COMSOL Multiphysics it is possible to add fibers to Linear Elastic or Nonlinear
Elastic materials, as well as to any of the built-in Hyperelastic material models. The
fibers are arranged in a specified orientation inside the matrix material. By subsequently
adding Fiber nodes as needed, it is possible to include fibers in many directions, thus
recreating complex anisotropic structures.
FIBERS FOR LINEAR AND NONLINEAR ELASTIC MATERIALS
For a matrix material described by a Linear Elastic or Nonlinear Elastic materials, a
Fiber described by a Linear Elastic material adds a contribution to the stress tensor of
the type
 fib = v fib  E fib – E  a a  a
Here, Efib E is the difference between the stiffness of the isotropic matrix E and the
fibers’ stiffness Efib, vfib is the fiber volume fraction, a is the direction vector for the
fiber orientation in the undeformed geometry, and a  a · el · a is the elastic strain
in the fiber direction a.
For a Linear Elastic Material, Hooke’s law (Equation 3-18) is augmented as
 =  ex + C  el +  fib
For Nonlinear Elastic Materials, the same contribution to the stress tensor is added,
although the stress-strain relation in the isotropic matrix could be nonlinear.
When the fiber stiffness is described by a Uniaxial stress function, the added stiffness
reads
 fib = v fib   a   a  – E a a  a
where aa is a function of the elastic strain in the fiber direction, a  a · el · a. A
linear elastic fiber can be described by
 a   a  = E fib  a
but in general, aa could be a nonlinear expression of the fiber strain a.
530 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
FIBERS FOR HYPERELASTIC MATERIALS
For Hyperelastic Materials, the Holzapfel–Gasser–Ogden model is available beside the
Linear elastic and Uniaxial data models for fibers. In this case, the fibers are represented
by additional contributions to the strain energy density (Ref. 29 and Ref. 30).
The Holzapfel–Gasser–Ogden constitutive model captures the anisotropic mechanical
response observed in arteries. The model combines a nearly incompressible material
for the isotropic matrix, with additional terms for two fiber families
W ani = W iso + W fib,1 + W fib,2
Here, Wiso is the strain energy density of the isotropic hyperelastic material. In Ref. 29
Wiso is represented by a nearly incompressible Neo-Hookean material; in COMSOL
Multiphysics it is possible to select any of the built-in hyperelastic material models.
The second and third terms, Wfib,1 and Wfib,2 are anisotropic additions that describe
the mechanical contribution of collagen fiber networks. These terms contribute with a
strain energy density of the type
k1 Q
2
W fib = ---------  e – 1  where Q = k 2  k 3  I 1 – 3  +  1 – 3k 3   I a – 1  
2k 2
where the parameter k1 represents the fiber stiffness (SI unit: Pa), k2 is a dimensionless
tuning parameter, and k3 is the fiber dispersion (dimensionless). A value of k3  0
recovers the formulation in Ref. 29, where all the fibers are perfectly oriented in the a
direction. Setting k3  1/3 means that the fibers are completely dispersed, thus
recovering a similar formulation as given in the Delfino material model.
The formulation in Ref. 29 and Ref. 30 is based on the Isochoric Elastic Deformation,
where the invariants are defined as
I 1 = trace  C el 
I a = a  C el  a
2
The invariant I a =  a represents the squared value of the isochoric elastic stretch in
the fiber direction a. A common modeling assumption for biological tissues is that
fibers cannot sustain compression, so the fiber stiffness is added only for tensile
stretches such as  a  1 .
In general, the anisotropic strain energy density for a hyperelastic material containing
N fiber families reads
MATERIAL MODELS
|
531
N
W ani = W iso +
 Wfib m
m=1
The second Piola–Kirchhoff stress tensor is then computed from
N
S = S iso +
 Sfib m
m=1
where the stress contribution from each fiber family is given by
W fib m
S fib m = 2 -------------------C
COMPRESSIBLE FIBERS
The hyperelastic formulation in the Holzapfel–Gasser–Ogden constitutive model
(Ref. 29 and Ref. 30) based on the isochoric elastic Cauchy–Green tensor can be
problematic when the matrix material is made of a compressible or nearly
incompressible material (Ref. 31 and Ref. 32).
The solution to this problem (Ref. 32) is to relax the isochoric restriction for the fiber
deformation, and use the total strain invariant in the fiber direction instead. The
contribution to the strain energy density then reads
k1 Q
2
W fib = ---------  e – 1  where Q = k 2  k 3  I 1 – 3  +  1 – 3k 3   I a – 1  
2k 2
where the invariants are defined as
I 1 = trace  C el 
I a = a  C el  a
USER DEFINED
The anisotropic strain energy density for the fiber family Wfib can also be specified as
a user-defined expression of the strain invariants Ia, Ib, Ic, Iab, Iac, and Ibc, where
I b = b  C el  b , I c = c  C el  c
I ab = a  C el  b , I ac = a  C el  c , and I bc = b  C el  c
532 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
or the isochoric version of these invariants I a , I b , I c , I ab , I ac , and I bc , where
I b = b  C el  b , I c = c  C el  c
I ab = a  C el  b , I ac = a  C el  c , and I bc = b  C el  c
here, b and c are orthogonal directions to the main fiber direction a.
The internal variables Ia, Ib, Ic, Iab, Iac, Ibc, I a , I b , I c , I ab , I ac , and
I bc are named item.IaCe, item.IbCe, item.IcCe, item.IabCe,
item.IacCe, item.IbcCe, item.IaCIe, item.IbCIe, item.IcCIe,
item.IabCIe, item.IacCIe, and item.IbcCIe, respectively. Here,
item is the name of the Fiber node (for instance, solid.hmm1.fib1).
THERMAL EXPANSION IN FIBERS
Not only the stiffness in the fibers might differ by orders of magnitude to the matrix
stiffness, but also the thermal properties, so it is possible to model thermal expansion
in fibers independently from the thermal expansion in the surrounding material. The
two basic assumptions are that the volume occupied by the fibers is small as compared
to the base material and that thermal expansion (or contraction) occurs in the fiber
direction only (there is zero transverse thermal expansion in the fibers).
For Linear Elastic and Nonlinear Elastic materials, fibers described by a Linear Elastic
material add a contribution to the stress tensor of the type
 fib = v fib  E fib – E  a a  a
where Efib  E is the difference between the stiffness of the isotropic matrix E and the
fibers’ stiffness Efib, vfib is the fiber volume fraction, a is the direction vector for the
fiber orientation in the undeformed geometry, and a  a  el  a is the elastic strain in
the fiber direction a.
When considering thermal expansion in the fibers, the stress reads
 fib = v fib  E fib   a –  th,fib  – E a a  a
where th,fib is the thermal strain in the fibers. When the fiber stiffness is described by
a Uniaxial stress function, the added stiffness reads
 fib = v fib   a   a  – E a a  a
MATERIAL MODELS
|
533
where aa is a function of the elastic strain in the fiber direction, where
 a = a    a –  th,fib .
For a Linear Elastic Material, Hooke’s law (Equation 3-18) is then augmented as
 =  ex + C  el +  fib
For Nonlinear Elastic Materials, the same contribution to the stress tensor is added,
although the stress-strain relation in the isotropic matrix could be nonlinear.
For Hyperelastic Materials containing one fiber family, the anisotropic strain energy
density reads:
W ani = W iso + W fib
The second Piola–Kirchhoff stress tensor is then computed from
W fib
S = S iso + 2 ------------C
When Thermal Expansion is added to fibers described by the Holzapfel–Gasser–Ogden
material model, the fiber contribution Wfib to the strain energy density is computed
from the invariants of the elastic Cauchy-Green tensor:
– T CF – 1
C el = F th
th
where the inelastic deformation gradient of the fibers is
F th = I +  th,fib a  a .
Thermal Strain in Fibers
The thermal strain in the fibers, th,fib, can be specified by different means. When the
secant coefficient of thermal expansion is used, it reads
 th,fib =  s  T fib – T ref 
Here, the secant coefficient of thermal expansion s can be temperature-dependent.
The reference temperature Tref is the temperature at which there are no thermal strains
in the fibers, and Tfib is the current fiber temperature.
When the tangent coefficient of thermal expansion is used, t, the thermal strain is
given by
534 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
 T fib

 th,fib = exp 
 t    d – 1
 T ref


It is also possible to explicitly enter the thermal strain, dL, as a function of the fiber’s
temperature
 th,fib = dL  T fib 
The coefficient of the thermal expansion or the thermal strain are considered in the
fiber direction a, since thermal expansion is assumed to occur in the fiber direction
only.
See also the description of the Fiber node in the Solid Mechanics chapter.
An example of an isotropic hyperelastic material reinforced with fibers is
shown in Arterial Wall Mechanics: Application Library path
Nonlinear_Structural_Materials_Module/Hyperelasticity/
arterial_wall_mechanics
Elastoplastic Materials
In this section:
• Plasticity
• Defining the Yield Criterion
• Plastic Flow
• Isotropic Plasticity
• Yield Function
• Orthotropic Plasticity
• Isotropic Hardening
• Kinematic Hardening
• Soil Plasticity
• Porous Plasticity
• Numerical Solution of the Elastoplastic Conditions
MATERIAL MODELS
|
535
• Energy Dissipation
• Nonlocal Plasticity
PLASTICITY
Many materials have a distinct elastic regime, in which the deformations are
recoverable and path independent. When the stresses exceed a certain level, the yield
limit, permanent plastic strains will appear.
The elastic part of the constitutive relation can be described by a Linear Elastic Material
Nonlinear Elastic Materials, or Hyperelastic Materials.
Elastoplastic material models are common, both when modeling metals and soils.
In geotechnical applications it is common to define compressive stresses as having
positive signs. In COMSOL Multiphysics, the convention is, however, to always use
positive signs for tensile stresses.
See also Sign Conventions.
DEFINING THE YIELD CRITERION
A yield criterion serves to define the stress condition under which plastic deformation
occurs. Stress paths inside the yield surface result in purely recoverable deformations
(elastic behavior), while paths intersecting the yield surface produces both recoverable
and permanent deformations (plastic strains).
In general, the yield surface can be described as
F = f    – fc = 0
where fc can be a constant value (for perfectly plastic materials), or a variable for
strain-hardening materials. The yield surface F is a surface in the space of principal
stresses, in which the elastic regime (F  0) is enclosed.
For brittle materials, the yield surface represents a failure surface, which is a stress
level at which the material collapses instead of deforms plastically.
Some authors define the yield criterion as f () = fc, while the yield
surface is an isosurface in the space of principal stresses F = 0, which can
2
2
be chosen for numerical purposes as F = f    – f c = 0 .
536 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
PLASTIC FLOW
The evolution of plastic deformation is typically referred as plastic flow. There are two
main implementations for plastic flow available in COMSOL Multiphysics depending
on what strain decomposition is selected. An additive decomposition of strains, is the
most suitable approach in the case of small strains, and a multiplicative decomposition
of the deformation gradient is more suitable when strains and/or rotations are
expected to be large. The additive and multiplicative decomposition of strains is
described in Inelastic Strain Contributions.
When an additive decomposition is used while the elastic or plastic strains are large, it
might produce incorrect results. As an example, the volume preservation, which is an
important assumption in metal plasticity, will no longer be respected. The additive
decomposition of strains is however widely used both for metal and soil plasticity
The type of strain decomposition used can be controlled in the Geometric
Nonlinearity section of the material model.
• An additive decomposition is always used for a geometrically linear
formulation.
• If the Include geometric nonlinearity check box is selected in Settings
window of the study, the default is to use a multiplicative
decomposition.
• Hyperelastic materials always use a multiplicative decomposition.
Plastic Flow for Additive Decomposition
The flow rule defines the relationship between the increment of the plastic strain
tensor ꞏ p and the current state of stress, for a yielded material subject to further
loading. The direction of the plastic flow is defined by
Q p
ꞏ
 p =  ---------
MATERIAL MODELS
|
537
Here,  is a positive multiplier (also called the consistency parameter or plastic
multiplier), which depends on the current state of stress and the load history, and Qp
is the plastic potential.
The “dot” (for ꞏ p ) means the rate at which the plastic strain tensor
changes with respect to Qp. It does not represent a true time
derivative. Some authors call this formulation rate independent
plasticity.
The direction of the plastic strain increment ꞏ p is perpendicular to the surface (in the
hyperspace spanned by the stress tensor components) defined by the plastic potential
Qp.
The plastic multiplier  is determined by the complementarity or Kuhn–Tucker
conditions
  0 , F y  0 and F y = 0
(3-49)
where Fy is the yield function. The yield surface encloses the elastic region defined by
Fy < 0. Plastic flow occurs when Fy = 0.
If the plastic potential and the yield surface coincide with each other Qp = Fy, the
flow rule is called associated, and the rate in Equation 3-50 is solved together with the
conditions in Equation 3-49.
F y
ꞏ
 p =  --------
(3-50)
For a nonassociated flow rule, the yield function does not coincide with the plastic
potential, and together with the conditions in Equation 3-49, the rate in
Equation 3-51 is solved using the plastic potential Qp (often, a smoothed version of
Fy).
538 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
Q p
ꞏ
 p =  ---------
(3-51)
When additive plasticity is used and the Include geometric nonlinearity
check box is selected on the study Settings window, the Cauchy stress
tensor is used to evaluate the yield function and plastic potential. Plastic
flow is, however, assumed in the direction the second Piola–Kirchhoff
stress tensor, and the computed plastic strain tensor can be interpreted as
a Green–Lagrange strain.
Plastic Flow for Multiplicative Decomposition
For a large strain formulation with multiplicative decomposition of deformation
(Ref. 3, Ref. 4, and Ref. 5), the plastic flow rule can be written as the Lie derivative
of the elastic left Cauchy–Green deformation tensor Bel:
Q p
–1
--- L  B el  =  ---------- B el

2
(3-52)
The plastic multiplier  and the plastic potential Qp (written in terms of the Cauchy
stress tensor ) satisfy the Kuhn–Tucker condition, as done for infinitesimal strain
plasticity
  0 , F y  0 and F y = 0
The yield function Fyin Ref. 3 and Ref. 4 was written in terms of
Kirchhoff stress and not Cauchy stress because the authors defined the
plastic dissipation with the conjugate energy pair  and d, where d is the
rate of strain tensor.
The Lie derivative of Bel is then written in terms of the plastic right Cauchy–Green rate
ꞏ
L  B el  = FC p– 1 F T
(3-53)
By using Equation 3-52 and Equation 3-53the plastic flow rule is written as (Ref. 4)
ꞏ
Q p
–1
--- FC p– 1 F T =  ---------- B el

2
(3-54)
MATERIAL MODELS
|
539
For the associated flow rule, the plastic potential and the yield surface coincide with
each other (Qp = Fy), and for the nonassociated case, the yield function does not
coincide with the plastic potential.
In COMSOL Multiphysics, the elastic left Cauchy–Green tensor is written in terms of
the deformation gradient F and the plastic right Cauchy–Green tensor Cp, so
Bel = FCp1FT. The flow rule then reads
ꞏ
Q p
C p– 1 = – 2 F – 1 ---------- FC p– 1

(3-55)
The plastic flow rule is then solved at Gauss points to find the inverse of the plastic
deformation gradient Fp1, by replacing the variables in Equation 3-55 with
ꞏ
ꞏ
ꞏ
C p– 1 = F p– 1 F p– T , C p– 1 = F p– 1 F p– T + F p– 1 F p–T , and B el = FF p–1 F p– T F T
After integrating the flow rule in Equation 3-55, the plastic Green–Lagrange strain
tensor is computed from the plastic deformation tensor
1 T
 p = ---  F p F p – I 
2
and the elastic Green–Lagrange strain tensor is computed from the elastic deformation
gradient tensor Fel = FFp1
1 T
 el = ---  F el F el – I 
2
The equivalent plastic strain variable is computed as the true equivalent
plastic strain (also called Hencky or logarithmic plastic strain) when a
multiplicative decomposition is used.
ISOTROPIC PLASTICITY
For isotropic plasticity, the plastic potential Qp is written in terms of at most three
invariants of Cauchy’s stress tensor
Q p    = Q p  I 1    J 2    J 3    
where the invariants of the stress tensor are
540 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
I 1    = trace   
1
J 2    = --- dev   :dev   
2
J 3    = det  dev    
so that the increment of the plastic strain tensor ꞏ p can be decomposed into
Q p I 1 Q p J 2 Q p J 3
Q p
ꞏ
 p =  ---------- =   ---------- -------- + ---------- --------- + ---------- ---------


I 1  J 2  J 3  
The increment in the plastic strain tensor ꞏ p includes in a general case both deviatoric
and volumetric parts. The tensor ꞏ p is symmetric given the following properties
I 1
-------- = I

J 2
--------- = dev   

J 3
2
--------- = dev   dev    – --- J 2 I
3

(3-56)
The trace of the incremental plastic strain tensor, which is called the volumetric plastic
strain rate ꞏ pvol , is only a result of dependence of the plastic potential on the first
invariant I1(), sinceJ2/ and J3/ are deviatoric tensors
Q p
Q p
ꞏ
ꞏ
 pvol = trace   p  =  trace  ---------- = 3 ---------
I 1
For metal plasticity under the von Mises or Tresca criteria, the volumetric plastic strain
rate ꞏ pvol is always zero because the plastic potential is independent of the invariant
I1. This is known as J2 plasticity.
A common measure of inelastic deformation is the equivalent plastic strain rate, (or
equivalent von Mises strain rate) which is defined from the plastic shear components
ꞏ
 pe =
2
--- dev  ꞏ p :dev  ꞏ p 
3
(3-57)
Some authors define the equivalent plastic strain rate directly from the yield surface and
the yield stress ys
MATERIAL MODELS
|
541
F
ꞏ
 pe = –  ---------- ys
(3-58)
and it is also possible to define it from a user defined expression hp
ꞏ
 pe = h p
(3-59)
Incompressible plastic deformation is experimentally observed in metals, but this is not
the case for most materials used in geotechnical applications. For instance, a nonzero
increment in volumetric plastic strain, ꞏ pvol , is explicitly used in Porous Plasticity and
Elastoplastic Soil Models.
• The equivalent plastic strain and the volumetric plastic strain are
available in the variables solid.epe and solid.epvol.
• In a time-dependent analysis, rates of plastic strains can be computed
with expressions like d(solid.epe,TIME).
YIELD FUNCTION
When an associated flow rule is applied, the yield function must be smooth, that is,
continuously differentiable with respect to the stress. In COMSOL Multiphysics, the
following form is used:
F y =  e    –  ys
where ys is the yield stress. The scalar function  e    is called equivalent stress. The
default form of the equivalent stress is the von Mises stress, which is often used in metal
plasticity:
 mises =
3J 2    =
3
--- dev   :dev   
2
Other expressions can be defined, such as Tresca stress, Hill equivalent stress, or a user
defined expression.
The Tresca equivalent stress is calculated from the difference between the largest and
the smallest principal stress
 tresca =  p1 –  p2
542 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
A user defined yield function can by expressed in terms of invariants of the stress tensor
such as the pressure (volumetric stress), p  I1, the equivalent von Mises stress
mises, or other invariants, principal stresses, or stress tensor components.
The von Mises Criterion
The von Mises criterion suggests that the yielding of the material begins when the
second deviatoric stress invariant J2 reaches a critical value. This criterion can be
written in terms of the elements of Cauchy’s stress tensor (Ref. 1)
1
2
2
2
2
2
2
J 2 = ---    11 –  22  +   22 –  33  +   33 –  11   +  12 +  23 +  13 = k 2
6
The von Mises criterion is implemented with the yield surface
Fy =
3J 2 –  ys = 0
where ys is the yield stress level (yield stress in uniaxial tension) and
is the equivalent von Mises stress.
3J 2 =  mises
The equivalent von Mises stress mises is available in the variable
solid.mises, where solid is the name of the physics interface node.
The Tresca Criterion
The Tresca yield surface is normally expressed in terms of the principal stress
components
1
--- max   1 –  2   1 –  3   2 –  3  = k
2
The Tresca criterion is a hexagonal prism with its axis equally inclined to the three
principal stress axes. When the principal stresses are sorted as 1  2  3, this
criterion is written as
1
---   1 –  3  = k
2
By using the representation of principal stresses in term of the invariants J2 and the
Lode angle 0    3, the Tresca criterion can alternatively be written as
4J
1
--- ---------2-  cos    – cos   + 2
------  =

2 3 
3
J 2 sin   + 
--- = k
3
MATERIAL MODELS
|
543
or equivalently
J 2 cos   – --- = k
6
The maximum shear stress is reached at the meridians ( = 0 or  = ). The Tresca
criterion can be circumscribed by setting the Lode angle  = 0, or equivalently, by a
von Mises criterion
 mises =
3J 2 = 2k
The minimum shear is reached at = , so the Tresca criterion can be inscribed by
setting a von Mises criterion
J2 = k
When dealing with soils, the parameter k is also called undrained shear strength.
The Tresca criterion can be used with either an associated or nonassociated flow rule,
in which case von Mises stress is applied in order to get better numerical performance.
The Tresca equivalent stress, tresca = 1  3 is implemented in the
variable solid.tresca, where solid is the name of the physics interface
node.
544 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY

upper limit
lower limit

Tresca criterion
Figure 3-14: The upper and lower limits of the Tresca criterion.
Figure 3-15: Classical yield criteria for metals. The Tresca criterion (left) and the
von Mises criterion (right).
The von Mises and Tresca criteria are independent of the first stress invariant I1 and
are mainly used for the analysis of plastic deformation in metals and ductile materials,
though some researchers also use these criteria for describing fully saturated cohesive
soils under undrained conditions. The von Mises and Tresca criteria belong to what
researchers call volume preserving or J2 plasticity, as the plastic flow is independent
on the mean pressure.
MATERIAL MODELS
|
545
ORTHOTROPIC PLASTICITY
Hill (Ref. 6, Ref. 7) proposed a quadratic yield function (and associated plastic
potential) in a local coordinate system given by the principal axes of orthotropy ai
Q p = F   22 –  33  2 + G   33 –  11  2 + H   11 –  22  2 +
2
2
2
(3-60)
2L 23 + 2M 31 + 2N 12 – 1
The six parameters F, G, H, L, M, and N are related to the state of anisotropy. As with
isotropic plasticity, the elastic region Qp  0 is bounded by the yield surface Qp  0.
Hill demonstrated that this type of anisotropic plasticity is volume preserving, this is,
given the associated flow rule
Q p
ꞏ
 p =  ---------
the trace of the plastic strain rate tensor is zero, which follows from the expressions for
the diagonal elements of ꞏ p
Q p
ꞏ
 p11 =  ------------ = 2  – G   33 –  11  + H   11 –  22  
 11
Q p
ꞏ
 p22 =  ------------ = 2  F   22 –  33  – H   11 –  22  
 22
Q p
ꞏ
 p33 =  ------------ = 2  – F   22 –  33  + G   33 –  11  
 33
so the plastic volumetric strain rate is zero
ꞏ
ꞏ
ꞏ
ꞏ
ꞏ
 pvol = trace   p  =  p11 +  p22 +  p33 = 0
Hill plasticity is an extension of J2 (von Mises) plasticity, in the sense that
it is volume preserving. Due to this assumption, six parameters are needed
to define orthotropic plasticity, as opposed to orthotropic elasticity, where
nine elastic coefficients are needed.
Expressions for the Coefficients F, G, H, L, M, N
Hill noticed that the parameters L, M, and N are related to the yield stress in shear with
respect to the axes of orthotropy ai, thus they are positive parameters
546 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
1 , M = ---------------1 , N = ---------------1
L = ---------------2
2
2
2 ys23
2 ys31
2 ys12
Here, ysij represents the yield stress in shear on the plane ij.
The material parameters ys1, ys2, and ys3 represent the tensile yield stress in the
direction, a1, a2, and a3, and they are related to Hill’s parameters F, G, and H as
1- = G+H
--------2
 ys1
1
---------- = H + F
2
 ys2
1- = F+G
--------2
 ys3
or equivalently
1 - + --------1 - – --------12F = --------2
2
2
 ys2  ys3  ys1
1
1
1
2G = ---------- + ---------- – ---------2
2
2
 ys3  ys1  ys2
1
1 - – --------12H = --------- + --------2
2
2
 ys1  ys2  ys3
Note that at most one of the three coefficients F, G, and H can be negative.
In case of hardening, these coefficients (either Hill’s coefficients or the
shear and tensile yield stresses) are renamed with the “initial” prefix.
In order to define a yield function and plastic potential suitable for isotropic or
kinematic hardening, the average initial yield stress ys0 is calculated from the Hill’s
parameters F, G, and H (this is equivalent to the initial yield stress ys0 in von Mises
plasticity)
 1
1- = 2
1 - + --------1 -
---  F + G + H  = 1
---  ------------------ + --------
2
2
2
2 
3
3

 ys0
ys1  ys2  ys3
(3-61)
MATERIAL MODELS
|
547
Defining Hill’s equivalent stress as (Ref. 7)
2
2
 hill =  ys0  F   22 –  33  2 + G   33 –  11  2 + H   11 –  22  2
2
2
2
+ 2  L 23 + M 31 + N 12  
makes it possible to write the plastic potential in a similar way to von Mises plasticity.
Isotropic hardening is then applied on the average yield stress variable ys0, by using
the plastic potential
Q p =  hill –  ys
Here, the average yield stress
 ys =  ys0 +  h   pe 
now depends on the initial yield stress ys0, the hardening function h, and the
equivalent plastic strain pe.
ISOTROPIC HARDENING
In the case of isotropic hardening, the plasticity problem is defined with either
associated or nonassociated plastic flow and with the yield surface
F y =  e    –  ys   pe 
where the yield stress yspe is a function of the equivalent plastic strain pe.
There are several different kinds of isotropic hardening models for elastoplastic and
viscoplastic materials:
• Perfect Plasticity (no isotropic hardening)
• Linear Isotropic Hardening
• Ludwik
• Johnson–Cook
• Swift
• Voce
548 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
• Hockett–Sherby
• Hardening Function.
The internal variable for the equivalent plastic strain is named solid.epe.
The equivalent plastic strain evaluated at Gauss points is named
solid.epeGp.
Perfect Plasticity
For perfect (or ideal) elastoplastic materials, the yield surface is fixed in the space of
principal stresses, and therefore, plastic deformations occur only when the stress path
moves on the yield surface (the regime inside the yield surface is elastic, and stress paths
beyond the yield surface are not allowed).
Here the yield stress is directly given by the initial yield stress ys0 such that
 ys   pe  =  ys0
In the settings for plasticity you specify the equivalent stress e for the yield
function; and ys0 that defines the onset of plastic deformation.
Linear Isotropic Hardening
The yield stress yspe is for linear isotropic hardening a function of the equivalent
plastic strain pe and the initial yield stress ys0
 ys   pe  =  ys0 + E iso  pe
Here, the isotropic hardening modulus Eiso is calculated from
1 - = ------------1 - – --1---------E iso
E Tiso E
For linear isotropic hardening, the isotropic tangent modulus ETiso is defined as
(stress increment / total strain increment). A value for ETiso is entered in the isotropic
tangent modulus section for the Plasticity node. The Young’s modulus E is taken from
the parent material (Linear Elastic, Nonlinear Elastic or Hyperelastic material model).
For orthotropic and anisotropic elastic materials, E represents an equivalent Young’s
modulus.
Ludwik
In the Ludwik model for nonlinear isotropic hardening, the yield stress yspe is
defined by a nonlinear function of the equivalent plastic strain. The Ludwik equation
MATERIAL MODELS
|
549
(also called the Ludwik–Hollomon equation) for isotropic hardening is given by the
power law
n
 ys   pe  =  ys0 + k pe
Here, k is the strength coefficient and n is the hardening exponent. Setting n = 1
would result in linear isotropic hardening.
Johnson–Cook
Similar to the Ludwik hardening model, the yield stress yspe in the Johnson–Cook
model is defined as a nonlinear function of the equivalent plastic strain pe given by a
power law. The difference is that effects of the strain rate are included in the model.
The yield stress and hardening function is given by
 ꞏ pe 
n 
 ys   pe  =   ys0 + k pe   1 + C log  ------ꞏ -   1 – f  T h  

 0  
(3-62)
The Johnson–Cook model also adds the possibility to include thermal softening by
including a function which depends on the normalized homologous temperature Th.
It is a function of the current temperature T, the melting temperature of the metal Tm,
and a reference temperature Tref
T – T ref
T h = -----------------------T m – T ref
m
As a default, this dependency follows a power law, f  T h  = T h . The softening
function f(Th) should have the properties f(Th  0) = 0 and f(Th 1) = 1.
The natural logarithm is used in Equation 3-62. If material data have been
determined using a base 10 logarithm, the value of C must be adjusted
accordingly.
The strain rate strength coefficient C and the reference strain rate ꞏ in the Johnson–
0
Cook model are obtained from experimental data. The flow curve properties are
normally investigated by conducting uniaxial tension tests in a temperature range
around half the melting temperature Tm, and subjected to different strain rates like
0.1/s, 1/s, and 10/s.
550 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
It should be noted that the intent of the strain rate dependent term in Equation 3-62
is to capture the hardening at high strain rates. If extrapolated to very low strain rates,
a low or even negative yield stress will be predicted. Low strain rates can however be
expected in some regions in a general finite element model. To resolve this, the
material model as implemented, never evaluates the logarithmic term to a value smaller
than zero. This means that the reference strain rate ꞏ must be considered the
0
quasistatic limit. Below this strain rate, the hardening function will be a strain rate
independent, but temperature dependent, Ludwik law:
n
 ys   pe  =   ys0 + k pe   1 – f  T h  
Swift
For nonsaturating materials, the Swift power-law equation relates the initial yield stress
ys0 and the isotropic hardening h, to the equivalent plastic strain as
 ys   pe  =  ys0 +  h   pe  = k   0 +  pe 
n
here, k is the strength coefficient, n is the hardening exponent, and 0 is a reference
strain. Noting that at zero plastic strain the initial yield stress is related to the strength
coefficient and hardening exponent as
n
 ys  0  =  ys0 = k 0
the yield stress is written as
 ys   pe  = k   0 +  pe 
n
 pe n
=  ys0  1 + ------- for  pe  0
0 
Voce
The Voce rule for nonlinear isotropic hardening is intended for materials that exhibit
a saturating evolution of hardening. The isotropic hardening h is exponentially
related to the equivalent plastic strain as
 h   pe  =  sat  1 – e

–  pe


The yield stress yspe is then defined as
 ys   pe  =  ys0 +  h   pe  =  ys0 +  sat  1 – e
–  pe


MATERIAL MODELS
|
551
The value of the saturation exponent parameter  determines the saturation rate of
the hysteresis loop for cyclic loading. The saturation flow stress sat characterizes the
maximum distance by which the yield surface can expand in the stress space. For values
pe  , the yield stress saturates to
 ys   ys0 +  sat
Hockett–Sherby
The Hockett–Sherby rule for nonlinear isotropic hardening is also intended for
materials which yield stress saturates as equivalent plastic strain increases. It is similar
to Voce rule, but it includes an exponential dependency of the form
 ys   pe  =  ys0 +    –  ys0   1 – e
n
– m pe


where  is the steady-state flow stress, m the saturation coefficient and n the
saturation exponent. For values mpen   the yield stress saturates to
 ys   
Hardening Function
The yield stress versus the equivalent plastic strain can be specified with the help of a
hardening curve that could also depend on other variables, such as temperature.
In this case, define the (usually nonlinear) hardening function hpe such that the
yields stress reads
 ys   pe  =  ys0 +  h   pe 
KINEMATIC HARDENING
For kinematic hardening, the plasticity problem is defined with either associated or
nonassociated plastic flow and with the yield surface
F y =  e   –  b  –  ys
(3-63)
Here, ys is the yield stress (which may include a linear or nonlinear isotropic
hardening model), and e is the equivalent stress. The stress tensor used in the yield
function is shifted by what is usually called the back stress, b to impose kinematic
hardening.
552 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
There are few options for computing either linear or nonlinear kinematic hardening
for plasticity:
• No kinematic hardening (default)
• Linear kinematic hardening
• Armstrong–Frederick
• Chaboche
Linear Kinematic Hardening
The back stress is generally not only a function of the current plastic strain but also of
its history. In the case of linear kinematic hardening, the back stress back is a linear
function of the plastic strain tensor p, this is also known as Prager’s hardening rule.
The implementation of linear kinematic hardening assumes a linear evolution of the
back stress tensor with respect to the plastic strain tensor:
2
 b = --- C k  p
3
where the kinematic hardening modulus Ck is calculated from
1- = -----1- – --1-----Ck
Ek E
The value for Ek is entered in the kinematic tangent modulus section and the Young’s
modulus E is taken from the linear or nonlinear elastic material model. For orthotropic
and anisotropic elastic materials, E represents an averaged Young’s modulus. Note that
some authors define the kinematic hardening modulus as Hk = 2/3Ck.
When kinematic hardening is added, both the plastic potential and the
yield surface are calculated with effective invariants, that is, the invariants
of the tensor defined by the difference between the stress tensor minus
the back-stress, eff =  - b. The invariant of effective deviatoric tensor
is named solid.II2sEff, which is used when a von Mises, Tresca, or
Hill orthotropic plasticity is computed together with kinematic
hardening.
Armstrong–Frederick Hardening Model
Armstrong and Frederick (Ref. 1) added memory to Prager’s linear kinematic
hardening model. This nonlinear kinematic hardening model makes it possible to
MATERIAL MODELS
|
553
capture the Bauschinger effect and nonlinear behavior by nonsymmetric
tension-compression loading.
The nonlinear evolution of the back stressb is governed by the rate
2 ꞏ
ꞏ
ꞏ
 b = --- C k  p –  k  pe  b
3
here, Ck is the kinematic hardening modulus,k is a kinematic hardening parameter,
andpe the equivalent plastic strain. Setting k = 0 recovers Prager’s rule for linear
kinematic hardening.
To solve this rate, internal degrees of freedom are added to account for the back stress
components. In order to have the same units as used for the plastic strain, the
algorithm solves for the back strain b as proposed in (Ref. 2), which is related to the
back stress as
2
 b = --- C k  b
3
The nonlinear evolution for the back strain reads
ꞏ
ꞏ
ꞏ
 b =  p –  k  pe  b
Chaboche Hardening Model
Chaboche (Ref. 2) proposed a nonlinear kinematic hardening model based on the
superposition of N back stress tensors
N
b =
 b,i
i
each of these back stress tensorsb,i follows a nonlinear Armstrong–Frederick
kinematic hardening rule
2 ꞏ
ꞏ
ꞏ
 b,i = --- C i  p –  i  pe  b,i
3
(3-64)
Practitioners would normally select k = 0 for one of the back stress equations, thus
recovering Prager’s linear rule for that branch
2
 b,0 = --- C 0  p
3
554 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
The back stress tensorb is then defined by the superposition of N back stress tensors
N
2
 b = --- C 0  p +
3
 b,i
i=1
As done for Armstrong–Frederick kinematic hardening, the algorithm solves for the
back strain tensors b,i instead of the back stress tensors. The change of variables is
2
 b,i = --- C i  b,i
3
and the nonlinear evolution for the back strain tensors in Equation 3-64 reads
ꞏ
ꞏ
ꞏ
 b,i =  p –  i  pe  b,i
Multiplicative Decomposition
For multiplicative decomposition, the total deformation gradient F is decomposed
into an elastic Fel and an inelastic (plastic) Fpl deformation
F = F el F pl
as described in Inelastic Strain Contributions. When kinematic hardening is used with
multiplicative decomposition, Fpl is similarly split multiplicatively as suggested in
Ref. 8, such that
F pl = F ple F plv
Here Fple is referred to as the “elastic” part of Fpl, and Fplv as its “viscous” part of the
plastic deformation. Conceptually, Fple corresponds to a spring and Fplv to a dashpot
that are connect in series in a rheological model. Now new kinematic quantities can be
defined in a similar fashion as for Fel. For example, the tensor
T
–T
–1
C ple = F ple F ple = F plv C pl F plv
which is analogous to the elastic right Cauchy–Green deformation tensor Cel. As for
the elastic part of the model, a free energy function Wkin(Cpl,e) can be defined for the
spring of the kinematic hardening part. From Wkin different stress tensors can be
derived, for example
W kin  C ple 
S b = 2 -----------------------------C pl
MATERIAL MODELS
|
555
which represents that back stress in the material frame and is analogous to the second
Piola-Kirchoff stress of the elastic part. By applying a push-forward operation by the
total deformation gradient F, the back stress in the spatial frame is
–1
 b = J FS b F
T
Alternatively using the plastic deformation gradient leads
–1
̃ b = J pl F pl S b F pl
T
where ̃ b is a representation of the back stress in an intermediate frame defined by Fpl.
The yield function in Equation 3-63 is defined in the spatial frame for large strains,
thus to complete the formulation we need to find b, or Cple, which depends on the
kinematic hardening model used.
It is in COMSOL Multiphysics assumed that Wkin has the same format as the elastic
strain energy function and that it is always isotropic. Hence for a linear elastic material
1
W kin   ple  = --- C k  dev   ple :dev   ple  
3
where ple = 0.5(Cple-1) and Ck is the kinematic hardening modulus. For hyperelastic
materials, a compressible Neo-Hookean strain energy function is used
11
1
W kin  C ple  = --- --- C k  I 1  C ple  – 3  – --- C k ln J ple
23
3
The flow rule suggested in Plastic Flow for Multiplicative Decomposition leads to an
arbitrary plastic rotation, which is undesirable with the above formulation for large
strain kinematic hardening. Hence, when kinematic hardening is used, the plastic flow
rule is modified to
ꞏ
–1
–1
– 1 Q p
F pl = – F ---------- FF pl

such that the plastic rotation is uniquely determined.
Linear Kinematic Hardening To obtain a linear kinematic hardening model the
inelastic part of the plastic deformation is omitted by setting Fplv = 1, and thus
Cple = Cpl.
556 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
Armstrong–Frederick Kinematic Hardening To obtain an Armstrong–Frederick
kinematic hardening model, the inelastic part of the plastic deformation Fplv is
considered as an additional unknown variable determined by the flow rule
ꞏ
3 k – 1
–1
–1
C plv = – 2 ---------- F pl dev  ̃ b F pl C plv
2C k
where k is a kinematic hardening parameter. The actual unknown used by the
plasticity algorithm is the symmetric part of the inverse of Fplv.
Chaboche Kinematic Hardening The Chaboche kinematic hardening model can be
viewed as a combination of linear kinematic and Armstrong–Frederick kinematic
hardening by adding N branches. Formally each branch here corresponds to a unique
multiplicative split of Fpl such that for branch i we have
F pl = F ple i F plv,i
Conceptually, each branch corresponds to a spring and a dashpot in series and the
branches are then connected parallel. The first branch always corresponds to linear
kinematic hardening such that Fplv,1 = 1. Each consecutive branch adds an
Armstrong–Frederick kinematic hardening model, where Fplv,i is an additional
unknown with its own flow rule. The total back stress is then the sum of the stress in
all branches
N
b =
 b,i
i
SOIL PLASTICITY
The Mohr–Coulomb Criterion
The Mohr–Coulomb criterion is the most popular criterion in soil mechanics. It was
developed by Coulomb before the Tresca and von Mises criteria for metals, and it was
the first criterion to account for the hydrostatic pressure. The criterion states that
failure occurs when the shear stress and the normal stress acting on any element in the
material satisfy the equation
 +  tan  – c = 0
here,  is the shear stress, c the cohesion, and  denotes the angle of internal friction.
With the help of Mohr’s circle, this criterion can be written as
MATERIAL MODELS
|
557
1
---   1 –  3  + 1
---   1 +  3  sin  – c cos  = 0
2
2
Te
ns
ile
me
r id
ia n
The Mohr–Coulomb criterion defines an irregular hexagonal pyramid in the space of
principal stresses, which generates singularities in the derivatives of the yield function.
ss
re
mp
o
C
iv e
i
rid
me
an
Figure 3-16: The Mohr–Coulomb criterion. The cone opens toward the compressive axis.
The Mohr–Coulomb criterion can be written in terms of the invariants I1 and J2 and
the Lode angle 0    3 (Ref. 1, Ref. 11) when the principal stresses are sorted as
1  2  3. The yield function then reads
J
1
2
F y = --- I 1 sin  + -----2-   1 + sin   cos  –  1 – sin   cos   + ------  – c cos  = 0

3
3
3 
The tensile meridian is defined when  = and the compressive meridian when  = .
Rearranging terms, the Mohr–Coulomb criterion reads
Fy =
J 2 m    + I 1 – k = 0
where
m =
1
---   1 + sin   cos  –  1 – sin   cos   + 2
------  ,  = sin   3 , and
3
3
k = c cos 
558 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
In the special case of frictionless material, ( = 0,  = 0, k = c), the Mohr–Coulomb
criterion reduces to a Tresca’s maximum shear stress criterion, 1  3 = 2k or
equivalently
Fy =
J 2 cos   – --- – k = 0

6
See also the description of the Mohr–Coulomb material model in the
Solid Mechanics interface documentation.
The Drucker–Prager Criterion
The Mohr–Coulomb criterion causes numerical difficulties when treating the plastic
flow at the corners of the yield surface. The Drucker–Prager model (Ref. 1, Ref. 2)
neglects the influence of the invariant J3 (introduced by the Lode angle) on the
cross-sectional shape of the yield surface. It can be considered as the first attempt to
approximate the Mohr–Coulomb criterion by a smooth function based on the
invariants I1 and J2 together with two material constants (which can be related to
Mohr–Coulomb’s coefficients)
Fy =
J 2 + I 1 – k = 0
The criterion is sometimes also called the extended von Mises criterion, since it is
equivalent to the von Mises criterion for metals when setting  = 
Figure 3-17: The Drucker–Prager criterion. The cone opens toward the compressive axis.
The coefficients in the Drucker–Prager model are related to the cohesion c and angle
of internal friction  in the Mohr–Coulomb criterion by the relation
MATERIAL MODELS
|
559

tan --- = -----------k
3c
The coefficients in the Drucker–Prager model can be matched to the coefficients in the
Mohr–Coulomb criterion by (Ref. 1)
2
sin 
3c cos  = -------  -------------------------- and k = 2
------------------------- 3  sin  
3  3  sin  
The symbol ± is related to either matching the tensile meridian (positive sign) or the
compressive meridian (negative sign) of Mohr–Coulomb’s pyramid.
The matching at the tensile meridian ( = ) comes from setting
m  0  =  3 + sin     2 3 
in the Mohr–Coulomb criterion, and the matching at the compressive meridian ( = 
3) from setting
m    3  =  3 – sin     2 3 
compressive meridian
tensile meridian

Figure 3-18: The Drucker–Prager criterion showing the tensile and compressive meridians
(inner and outer circles), and the Lode angle compared to the cross section of the Mohr–
Coulomb criterion in the -plane.
In the special case of frictionless material, ( = 0,  = 0, k = 2c  3 ), the Drucker–
Prager criterion reduces to the von Mises criterion
560 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
J 2 = 2c  3
When the Drucker–Prager criterion is matched to the Mohr–Coulomb criterion in 2D
plane-strain applications, the parameters are
tan 
3c
 = ------------------------------------ and k = -----------------------------------2
2
9 + 12 tan 
9 + 12 tan 
when matching the criterion in 2D generalized plane-strain, the matching parameters
are:
2 sin 
2 3  = ---------------------------------- and k = ------------------- c cos 
3  3 – sin  
3 – sin 
and when matching the criterion in 2D plane-stress, the matching parameters are:
1
2
 = -------  sin  and k = -------  c cos 
3
3
Dilatation Angle
The Mohr–Coulomb criterion is sometimes used with a nonassociated plastic
potential. This plastic potential could be either a Drucker–Prager criterion, or the same
Mohr–Coulomb yield function but with a different slope with respect to the
hydrostatic axis, in which case the angle of internal friction is replaced by the dilatation
angle, which is normally smaller (Ref. 7).
Also, when using a Drucker–Prager criterion matched to the Mohr–Coulomb
criterion, the plastic potential could also be nonassociated, in which case the difference
between the dilatation angle and the angle of internal friction results in a yield surface
and plastic potential portrayed by two cones with different angles with respect to the
hydrostatic angle.
Elliptic Cap
The Mohr–Coulomb and Drucker–Prager criteria portray a conic yield surface which
opens in the hydrostatic axis direction. Normally, these soil models are not accurate
above a given limit pressure because real-life materials cannot bear infinite loads and
still behave elastically. A simple way to overcome this problem is to add an elliptical end
cap on the compressive side to these models.
MATERIAL MODELS
|
561
The elliptic cap is an elliptic yield surface of semi-axes as shown in Figure 3-19. The
initial pressure pa (SI units: Pa) denotes the pressure at which the elastic range
circumscribed by either a Mohr–Coulomb pyramid or a Drucker–Prager cone is not
valid any longer, so a cap surface is added. The limit pressure pb gives the curvature of
the ellipse, and denotes the maximum admissible hydrostatic pressure for which the
material starts deforming plastically. Pressures higher than pb are not allowed.
q
pa
pb
p
Figure 3-19: Elliptic cap model in Haigh–Westergaard coordinate system.
The sign convention for the pressure is taken from the Structural Mechanics Module:
positive sign under compression, so pa and pb are positive parameters. Figure 3-19
shows the cap in terms of the variables p and q
q =
3J 2    and p = – I 1     3
In terms of these variables, the equation for the elliptic cap reads
p – pa  2  q  2
 -------------------- p b – p a +  q a = 1
the point (pa, qa) in the Haigh–Westergaard coordinate system is where the elliptic cap
intersects either the Mohr–Coulomb or the Drucker–Prager cone.
When the Mohr–Coulomb or the Drucker–Prager equations are represented in
J 2  I1 plane, the equation for the elliptic cap reads
I 1 – I a 2  J 2
 --------------- +  ----------
 I b – I a
 Ja 
562 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
2
= 1
where Ia  3pa, Ib  3pb, and Ja is the ellipse semiaxis in the
by the intersection with the Drucker–Prager criterion
J 2  I1 plane, given
J a = k – I a
This makes it easier to compute the ellipse’s semiaxis Ja in terms of Drucker–Prager
parameters  and k.
Elliptic Cap with Hardening
It is also possible to add isotropic hardening to the cap surface. In this case, the center
of the ellipse is shifted as the volumetric plastic strain increases, also, the size of the
ellipse’s semi-axes grow as hardening evolves. The intersection of the elliptic cap with
the pressure axis is given by
 pvol 
p b = p b0 – K iso log  1 + ------------------- pvol,max
here, pb0 is the initial value for the limit pressure pb, Kiso is the isotropic hardening
modulus, pvol the volumetric plastic strain, and pvol,max the maximum volumetric
plastic strain. The volumetric plastic strain pvol is negative in compression, so the limit
pressure pb is increased from pb0 as hardening evolves.
Instead of providing the value for the initial pressure pa (SI units: Pa), the ellipse’s
aspect ratio R is entered. The ellipse aspect ratio R is given by
pb – pa
Ia – Ib
R = --------------- = 3 3 ------------------ where q a =
qa
Ja
The ellipse semiaxis in the
3J a
J 2  I1 plane is given by the aspect ratio R
k – I a
J a = -----------------------------------------2 2
R + 1 +  R
In order to have a smooth transition, the cap intersects the failure surface at the point
of tangency (Ref. 3). The intersection coordinates (Ic, Jc) are given by
Ja
k and J =
I c = ------------------------------- – --c
2 2 
 1+ R
2
Ja
----------------------2 2
1+ R
MATERIAL MODELS
|
563
See also the description of the Drucker–Prager material model in the
Solid Mechanics interface documentation.
The Matsuoka–Nakai Criterion
Matsuoka and Nakai (Ref. 5) discovered that the sliding of soil particles occurs in the
plane in which the ratio of shear stress to normal stress has its maximum value, which
they called the mobilized plane. They defined the yield surface as
F y =  9 + 9 2 I 3 – I 1 I 2 = 0
where the parameter  = /nSTP equals the maximum ratio between shear stress
and normal stress in the spatially mobilized plane (STP-plane), and the invariants are
applied over the effective stress tensor (this is the stress tensor minus the fluid pore
pressure).
The Matsuoka–Nakai criterion circumscribes the Mohr–Coulomb criterion in dry
soils, when
2 2
 = ----------- tan 
3
564 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
and  denotes the angle of internal friction in the Mohr–Coulomb criterion.
Figure 3-20: The Matsuoka–Nakai and Mohr–Coulomb criteria in the principal stress
space.
See also the description of the Matsuoka–Nakai material model in the
Solid Mechanics interface documentation.
The Lade–Duncan Criterion
The Lade–Duncan criterion was originally developed to model a large volume of
laboratory sample test data of cohesionless soils. This criterion is defined as
3
F y = kI 3 – I 1 = 0
where I1 and I3 are the first and third stress invariants, respectively, and k is a parameter
related to the direction of the plastic strain increment in the triaxial plane. The
parameter k can vary from 27 for hydrostatic stress conditions (1 = 2 = 3), up to a
critical value kc at failure. In terms of the invariants I1, J2, and J3, this criterion can be
written as
3
1
1- – 1
F y = J 3 – --- I 1 J 2 +  ------- I = 0
3
27 k 1
The Lade–Duncan criterion can be fitted to the compressive meridian of the Mohr–
Coulomb surface by choosing
k =  3 – sin   3 /  cos  2   1 – sin   
MATERIAL MODELS
|
565
with  as the angle of internal friction in the Mohr–Coulomb criterion.
Lade–Duncan
Matsuoka–Nakai
Mohr–Coulomb
Figure 3-21: Comparing the Mohr–Coulomb, Matsuoka–Nakai, and Lade–Duncan
criteria when matching the tensile meridian.
The Lade–Duncan criterion does not match the Mohr–Coulomb
criterion (nor the Matsuoka–Nakai criterion) at the tensile meridian.
See also the description of the Lade–Duncan material model in the Solid
Mechanics interface documentation.
Tension Cutoff
It appears that the Mohr–Coulomb and Drucker–Prager criteria predict tensile
strengths larger than the experimental measurements on soil samples. This discordance
can be mended by the introduction of a tension cutoff criterion.
The Rankine criterion states that a material stops deforming elastically when the largest
principal stress 1 reaches a maximum tensile stress, also called tension cutoff limit t.
In terms of the principal stress, the Rankine criterion reads
F = 1 – t = 0
For soils and clays, the maximum tensile stress can be estimated from the material
parameters, such as the cohesion c and the friction angle .For instance, the tip of the
cone in Mohr–Coulomb criterion is reached when
cos 
 1 = c -----------sin 
therefore, the tension cutoff should be chosen such as
566 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
cos 
 t  c -----------sin 
The Mohr–Coulomb criterion together with a tension cutoff is sometimes called the
modified Mohr–Coulomb criterion (Ref. 21).
There might be numerical problems when implementing Rankine cutoff criterion, as
the intersection of the cone in Mohr–Coulomb criterion with the tensile plane
produces sharp edges in the stress space. A better approach is to use the mean stress
instead of the principal stress, then the mean stress cutoff reads
F = p + m = 0
here, m is the maximum mean stress and p  I13 is the pressure, which is negative
in tension.
The Rankine tension cutoff criterion is also available with Concrete and
Rocks material models.
POROUS PLASTICITY
The modeling of plastic deformation in soils, porous metals and aggregates has a main
difference with respect to traditional metal plasticity; the yield function and plastic
potential are not only defined in terms of the deviatoric stress tensor (or the deviatoric
stress invariant J2), but also include dependencies on the hydrostatic pressure.
A key concept for porous plasticity models is the evolution of the relative density,
which is the solid volume fraction in a porous mixture. The relative density is related
to the porosity (or void volume fraction)  by
 rel =  1 –  
When compacting a mixture of metal particles, the porosity tends to zero and the
relative density tends to one. There are different porous plasticity models to account
for the mechanism of compaction and void growth.
The Shima–Oyane Criterion
Shima and Oyane (Ref. 9) proposed a yield surface for modeling the compaction of
porous metallic structures fabricated by sintering. The criterion can be applied for
powder compaction at both low and high temperatures. The yield function and
associated plastic potential is defined by an ellipsoid in the stress space. The plastic
potential Qp is written in terms of both von Mises equivalent stress and mean pressure,
MATERIAL MODELS
|
567
and it also considers isotropic hardening due to changes in porosity. The plastic
potential is defined by
2
e 2
 pm
m
Q p    =  ---------- +   1 –  rel   ---------- –  rel
  ys0
  ys0
here, e is the equivalent stress, ys0 is the initial yield stress, pm is the pressure, and
rel is the relative density. The material parameters , , and m are obtained from curve
fitting experimental data. Typical material parameter values for copper aggregates are
 = 6.2,  = 1.03, and m = 5.
The Gurson Criterion
The Gurson criterion (Ref. 10) consists in a pressure dependent yield function to
describe the constitutive response of porous metals, this yield function is derived from
the analytical expression of an isolated void immersed in a continuum medium. The
void volume fraction, or porosity , is chosen as main variable. The yield function and
associated plastic potential is not an ellipse in the stress space, as in The Shima–Oyane
Criterion, but it is defined in terms of the hyperbolic cosine function. The plastic
potential for the Gurson criterion reads
e 2
3p m
2
Q p    =  ---------- + 2 cosh  ------------- –  1 +  
  ys0
 2 ys0
here, e is the equivalent stress, ys0 is the initial yield stress, pm is the pressure, and 
is the porosity.
The Gurson–Tvergaard–Needleman Criterion
Tvergaard and Needleman modified The Gurson Criterion for porous plasticity to
include parameters to better fit experimental data (Ref. 11-12). The resulting criterion
is called the Gurson–Tvergaard–Needleman (GTN) criterion in the literature. The
plastic potential for the GTN criterion reads
e 2
 3q 2 p m
2
Q p    =  ---------- + 2q 1  e cosh  ----------------- –  1 + q 3  e 
  ys0
 2 ys0 
here, e is the equivalent stress, ys0 is the initial yield stress, pm is the pressure, and
e is the effective void volume fraction (effective porosity). Typical correction
parameter values are q1 = , q2 = , and q3 = q12.
568 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
The effective void value fraction (or effective porosity)e used in the plastic potential
is a function of the current porosity  and other material parameters. It is often given
using a bilinear definition
 
if    c


m – c
 e =   + ------------------   –   if     
c
c
f
 c f – c

if    f
 m
where c is the critical void volume fraction (critical porosity) at which void coalescence
begins, and f is the void volume fraction at failure. When the porosity increases up to
the value of failure, the effective porosity takes a maximum value of m and the porous
material loses the capacity to carry stresses. The maximum porosity value is derived
from other parameters
q 1 + q 12 – q 3
 m = ---------------------------------q3
Since typical values for the parameters are q3 = q12, the maximum porosity value is
given by m = 1/q1.
A similar definition for e that gives a smoother response as the material reaches failure
can was suggested in Ref. 14. It is based on a modification such that the effective void
volume fraction reaches its maxim value asymptotically
 
if    c


m – c
  + -----------------   – c 
if  c     i
e =  c f – c

 – i

   m –  s  1 – exp  – --------------- +  s if    i


f – i
where i = 0.75(f  c) + c, and
m – c
 s =  c + ------------------   i –  c 
f – c
The Fleck–Kuhn–McMeeking Criterion
The Fleck–Kuhn–McMeeking criterion (Ref. 15), also called the FKM criterion, was
developed to model the plastic yielding of metal aggregates of high porosity. The yield
MATERIAL MODELS
|
569
function and associated plastic potential is derived from expressions for randomly
distributed particles. The criterion is considered relevant for aggregates with porosity
between 10% and 35%. The plastic potential for the FKM criterion reads
5 e 2 2
5 pm 2
Q p =  ------ ----- + --- +  --- ------- – 1
18 p f 3
3 pf
here, e is the equivalent stress and pm is the pressure. The flow strength of the
material under hydrostatic loading, pf, is computed from
2 m – 
p f = 2.97  1 –   ----------------  ys0
m
here, ys0 is the initial yield stress, and  is the void volume fraction (porosity). The
maximum void volume fraction m typically takes the value of 36%, the limit of dense
random packing of sintered powder.
The FKM–GTN Criterion
The FKM–GTN criterion is a combination of The Fleck–Kuhn–McMeeking Criterion
and The Gurson–Tvergaard–Needleman Criterion, intended to cover a wider range of
porosities (Ref. 16–17). The GTN model is used for low void volume fractions
(porosity lower than 10%), and for void volume fractions higher than 25%, the FKM
criterion is used. In the transition zone, a linear combination of both criteria is used.
Capped Drucker–Prager
See the sections The Drucker–Prager Criterion and Elliptic Cap for details.
Void Nucleation and Growth
For the porous plasticity criteria, the change in relative density is by default computed
from the change in plastic volumetric strain
ꞏ
ꞏ
 rel = –  rel  p,vol
Since the relative density is related to the porosity  by rel =   , the change in
porosity is also controlled by the change in plastic volumetric strain
ꞏ
ꞏ
 =  1 –   p,vol
and the change in volumetric plastic strain ꞏ p,vol is given by the porous plasticity
model.
Nucleation and shear growth are other mechanism that can trigger an increase of
porosity. The increment in porosity based on growth nucleation is given by
570 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
1 
–
2
pm
N
– ---  -----------------fN

 ꞏ
ꞏ
 nucleation = ------------------ e 2 sN
 pm for p  0
s N 2
here, N is the mean strain for nucleation, fN is the void volume fraction for nucleating
particles, and sN is the standard deviation. Typical values for these parameters are
N = , sN = , and fN = . It is assumed that nucleation appears only in tension,
and that there is no nucleation in compression.
The other possible mechanism to change the porosity is the so-called void growth in
shear
ꞏ
ꞏ
 shear = k w wn D : pl
here, kw is a material parameter,  is the current porosity, nD is a deviatoric tensor
coaxial to the stress tensor, and ꞏ pl is the plastic strain rate, which depends on the
porous plasticity model. The weight w is computed from stress invariants as
2
27 J 3
w = 1 – ------ -----3- = sin2  3 
4J
2
where  is the Lode angle. The weight variable has a value of w = at the compressive
and tensile meridians ( =  and  = 3), and it attains its maximum w =  for  = 6.
Isotropic Hardening
Porous plasticity implements different kinds of isotropic hardening models to describe
the hardening of the porous matrix. When applying isotropic hardening, the average
flow stress
 fm =  ys0 +  h   pm 
now depends on the initial yield stress ys0, the hardening function h, and the
equivalent plastic strain in the porous matrix pm.
Different isotropic hardening models are implemented for porous plasticity models,
which are described for elastoplastic materials:
• Perfect Plasticity (no isotropic hardening)
• Linear Isotropic Hardening
• Ludwik
MATERIAL MODELS
|
571
• Hardening Function
• Exponential Hardening (Elliptic Cap with Hardening)
It is also possible to include a power law relation between the equivalent plastic strain
in the porous matrix pm, and the flow stress (yield level) fm. For uniaxial loading, the
strain stress relation is written as (ref. Ref. 12)
 ys0  fm n
 = -----------  ----------- for  fm   ys0
E   ys0
where ys0 is the initial yield stress, n is the hardening exponent, and the Young’s
modulus E is taken from the elastic material properties. By writing the onset of
plasticity as 0 = ys0E, and noting that  = 0 + pm for fm > ys0, this reads
 fm n
 0 +  pm =  0  ----------- for  fm   ys0
 ys0
which is equivalent to Swift isotropic hardening
 pm 1 / n
 fm   pm  =  ys0  1 + -------
0 
NUMERICAL SOLUTION OF THE ELASTOPLASTIC CONDITIONS
A backward Euler discretization of the pseudo-time derivative is used in the plastic flow
rule. For small plastic strains, this gives
Q p
 p –  p, old =  ---------
where “old” denotes the previous time step and   t, where t is the pseudo-time
step length.
For large plastic strains, Equation 3-55 is numerically solved with the so-called
exponential mapping technique
Q p
–1
C p– 1 = F – 1 exp  – 2 ---------- FC p,
old

 
–1
–1
–T
where C p–1 = F p– 1 F p–T and C p,
old = F p, old F p, old . The purpose of the exponential
mapping is to ensure volume preservation of the discretized equations. For plasticity
models that are not volume preserving, for example soil plasticity, the computationally
leaner backward Euler discretization is used also for large plastic strains.
572 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
For each Gauss point, the plastic state variables (p or Fp1, depending on whether
small strain or large strain plasticity is selected) and the plastic multiplier, , are
computed by solving either of the above time-discretized flow rules together with the
complementarity conditions
  0,
F y  0,
F y = 0
This is done as follows (Ref. 3):
–1
1 Elastic-predictor: Try the elastic solution p  p,old (or F p–1 = F p,
old ) and   0.
If this satisfies Fy   it is done.
2 Plastic-corrector: If the elastic solution does not work (this is Fy  ), solve the
nonlinear system consisting of the flow rule and the equation Fy   using a damped
Newton method.
The numerical tolerance to fulfill the condition Fy   is given in SI units
of Pascals, and it depends on the initial yield stress (in case of plasticity and
porous plasticity) or it is defined in terms of other material parameter (for
soil plasticity).
It is possible to specify the maximum number of iterations and the relative tolerance
used to solve the plastic flow rule. Under the Advanced section enter the following
settings:
• Maximum number of local iterations. To determine the maximum number of iteration
when solving the local plasticity equations. The default value is 25 iterations.
• Relative tolerance. To check the convergence of the local plasticity equations based
on the step size. The final tolerance is computed based on the current solution of
the local variable and the entered value. The default value is 1e-6.
To display the Advanced section, click the Show More Options button (
Advanced Physics Options in the Show More Options dialog box.
) and select
ENERGY DISSIPATION
Since plasticity is an inelastic process, the dissipated energy density can be calculated
by integrating the pseudo-rate given by
Q p
ꞏ
ꞏ
W p = : p = : ---------
MATERIAL MODELS
|
573
As plasticity is rate independent, the plastic dissipation density Wp is obtained after
integrating an extra variable in the plastic flow rule.
The total energy dissipated by plasticity in a given volume can be calculated by a
volume integration of the plastic dissipation density Wp.
When the Calculate dissipated energy check box is selected, the plastic
dissipation density is available under the variable solid.Wp and the total
plastic dissipation under the variable solid.Wp_tot.
NONLOCAL PLASTICITY
The nonlocal plasticity model implemented in COMSOL Multiphysics is based on the
so-called implicit gradient method suggested in Ref. 23, and it incorporates some of
the generalizations introduced by the micromorphic theory (Ref. 24). The theory
assumes that the free energy of the elastoplastic material not only depends on the
macroscopic displacement u and macrostate variables, such as the equivalent plastic
strain pe, but also on some micromotion  and its gradient. If the micromotion
variable is identified as a nonlocal version of the equivalent plastic strain, pe,nl, the free
energy potential is written as
2
1
  u u  p  pe  pe,nl  pe,nl  = W s  u u  p  + --- E iso   pe  +
2
1
--- H nl   pe –  pe,nl  2 + 1
--- H nl  l int  2  pe,nl   pe,nl
2
2
(3-65)
here Ws is the elastic free energy, Hnl is a model parameter that determines the strength
of the coupling between the macro- and micromotions, and lint is the length scale that
determines the influence radius of the interaction. For simplicity, Equation 3-65
assumes linear isotropic hardening, but the same concept is applicable for more general
isotropic hardening laws and can for example also be extended with kinematic
hardening.
Taking the variation of Equation 3-65 with respect to state variables pe, pe,nl, and
pe,nl leads to the following set of equations related to the plasticity model:
2
2
 pe,nl – H nl  l int    pe,nl =  pe
in 
 pe,nl  n = 0
on
 ys   pe  pe,nl  =  ys0 + E iso  pe + H nl   pe –  pe,nl 
574 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
here,  is the domain of the elastoplastic problem. Variation of Equation 3-65 with
respect to the remaining state variables leads to the standard elasticity equations. In the
nonlocal (or regularized) plasticity problem, pe,nl is an additional dependent variable
that is solved as part of the global problem. The structure of the local plasticity
problem is not changed and the numerical solution remains the same as discussed
above, but the hardening law now depends on pe,nl.
For porous plasticity, the same equation applies, but pe and pe,nl are replaced by the
equivalent plastic strains in the matrix material, pm and pm,nl. It is also possible to
add nonlocal effects to the void volume fraction .The porous plasticity model is then
extended with the following set of equations
2
2
 nl –  l int,f    nl =  in 
 nl  n = 0
on
where nl is the nonlocal void volume fraction. In contrast to the equivalent plastic
strain, it is assumed that there is a perfect coupling between  and nl, and that the
nonlocal void volume fraction nl directly replaces its local counterpart in the model
equations.
RESETTING ELASTOPLASTIC VARIABLES
For some industrial applications, plastic strains are released due to manufacturing
processes such as welding or stress relief annealing. To model these type of
phenomena, it is possible to reset the internal plasticity variables to zero, or to prescribe
them to user defined expressions or values.
Add a Set Variables subnode to the Plasticity, Porous Plasticity, Soil Plasticity, or
Elastoplastic Soil Models to set up the plastic strain tensor, plastic deformation
gradient, the equivalent plastic strain, and other internal elastoplastic variables.
Failure Criteria for Concrete and Rocks
In this section:
• The Bresler–Pister Yield Criterion
• The Willam–Warnke Criterion
• The Ottosen Criterion
• The Original Hoek–Brown Criterion
• The Generalized Hoek–Brown Criterion
MATERIAL MODELS
|
575
THE BRESLER–PISTER YIELD CRITERION
The Bresler–Pister yield criterion (Ref. 4, Ref. 19) was originally devised to predict the
strength of concrete under multiaxial stresses. This failure criterion is an extension of
The Drucker–Prager Criterion to brittle materials, and it can be expressed in terms of
the stress invariants as
Fy =
2
J2 + k1 I1 + k2 I1 + k3
(3-66)
here, k1, k2, and k3 are parameters obtained from the uniaxial compressive strength
cs, the uniaxial tensile strength ts, and the biaxial compressive strength bc
 bc  cs + 2 cs  ts – 3 bc  ts
k 1 = ---------------------------------------------------------------------------------------------3   cs +  ts   2 bc –  cs   2 bc +  ts 
  ts –  cs    bc   cs +  ts – 4 bc  –  cs  ts 
k 2 = -------------------------------------------------------------------------------------------------------3   cs +  ts   2 bc –  cs   2 bc +  ts 
–  cs  bc  ts   ts + 8 bc – 3 cs 
k 3 = ---------------------------------------------------------------------------------------------3   cs +  ts   2 bc –  cs   2 bc +  ts 
All the strengths are considered with a positive sign. Note that for typical strength
values, the parameters k1 and k2 are positive while k3 is negative.
THE WILLAM–WARNKE CRITERION
The Willam–Warnke criterion (Ref. 12) is used to predict failure in concrete and other
cohesive-frictional materials such as rock, soil, and ceramics. Just as The Bresler–Pister
Yield Criterion, it depends only on three parameters. It was developed to describe
initial concrete failure under triaxial conditions. The failure surface is convex,
continuously differentiable, and it is fitted to test data in the low compression range.
The original “three-parameter” Willam–Warnke failure criterion was defined as
Fy =
 oct
3
1 -  – 1
1- – --------- --------- + r      -----
 oct

5  cs

ts
bc
(3-67)
where cs is the uniaxial compressive strength, ts is uniaxial tensile strength, and bc
is the biaxial compressive strength (all parameters are positive). The octahedral normal
and shear stresses are defined as usual; see Other Stress Invariants
 oct = I 1 /3 and  oct =
576 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
2J 2 /3
so the criterion in Equation 3-67 can be written in term of stress invariants as
Fy =
I1
 1

1 - ---- – 1
J2 + 5
--- r    cs   ------ – ------

3
2


 ts

bc
The dimensionless function r( describes the segment of an ellipse on the octahedral
plane as a function of the Lode angle 
2
2r c  r c2 – r t2  cos  + r c  2r t – r c  4  r c2 – r t2  cos  + 5r t2 – 4 r c r
r    = ---------------------------------------------------------------------------------------------------------------------------------------------------------------t
2
4  r c2 – r t2  cos  +  r c – 2r t  2
Here, the tensile and compressive meridian rt and rc are defined in terms of the
strengths cs, bc, and ts:
1  bc  ts
rt = 6
--- ------- ------------------------5  cs 2 bc +  ts
 bc  ts
rc = 6
--- --------------------------------------------------------------5 3 bc  ts +  bc  cs –  ts  cs
MATERIAL MODELS
|
577
The function r( can be interpreted as the friction angle which depends on the Lode
angle (Ref. 12).

rc
r

rt
Figure 3-22: The deviatoric section of the Willam–Warnke failure criterion.
THE OTTOSEN CRITERION
The Ottosen criterion is a four-parameter failure criterion proposed for short-time
loading of concrete. It corresponds to a smooth convex failure surface with curved
meridians, which is open in the negative (compressive) direction of the hydrostatic
axis. The curve in the pi-plane changes from almost triangular to a more circular shape
with increasing hydrostatic pressure. The criterion agrees with experimental results
over a wide range of stress states, including both triaxial tests along the tensile and the
compressive meridian and biaxial tests (Ref. 20).
The Ottosen criterion is commonly written as (Ref. 19, Ref. 20):
a
F y = ------- J 2 +     J 2 + bI 1 –  cs
 cs
Here, cs is the uniaxial compressive strength of concrete, and a > 0 and b > 0 are
dimensionless parameters. The dimensionless function depends on the Lode angle
 and two dimensionless parameters k1 > 0 and k2 > 0.
578 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY

 k cos  1

--k
 1
 3 acos  2 cos  3  

 = 

 k cos  
--- – 1
--- acos  – k 2 cos  3  
 1
3 3


J3  0
J 3  0.
The parameter k1 is called the size factor. The parameter k2 (also called shape factor)
is positive and bounded to 0  k2  1(Ref. 19, Ref. 20).
Typical values for these parameters are obtained by curve-fitting the uniaxial
compressive strength cs, uniaxial tensile strength ts, and from the biaxial and triaxial
data (for instance, a typical biaxial compressive strength of concrete is 16% higher than
the uniaxial compressive strength). The parameters cs, bc, and ts are positive.
TABLE 3-3: TYPICAL PARAMETER VALUES FOR OTTOSEN FAILURE CRITERION ( Ref. 20).
ts/ cs
a
b
k1
k2
t
c
0.08
1.808
4.096
14.486
0.991
14.472
7.783
0.10
1.276
3.196
11.736
0.980
11.711
6.531
0.12
0.922
2.597
9.911
0.965
9.872
5.698
The compressive and tensile meridians (as defined in The Willam–Warnke Criterion)
are
1
1
1
1
r c = ----- = ------------------- and r t = ----- = ---------- c   /3 
t   0 
The ratio rt/rc = c/t normally lies between 0.54~0.58 for concrete.
The Ottosen criterion is equivalent to the Drucker–Prager criterion when
a = 0 and  independent of the Lode angle.
THE ORIGINAL HOEK–BROWN CRITERION
The Hoek–Brown criterion is an empirical type of model which is commonly used
when dealing with rock masses of variable quality. The Hoek–Brown criterion is widely
used within civil engineering and is popular because the material parameters can be
estimated based on simple field observations together with knowledge of the uniaxial
compressive strength of the intact rock material. The Hoek–Brown criterion is one of
MATERIAL MODELS
|
579
the few nonlinear criteria widely accepted and used by engineers to estimate the yield
and failure of rock masses. The original Hoek–Brown failure criterion states (Ref. 7)
2
 1 =  3 + m cs  3 + s cs
where 1  2  3  0 are the principal stresses at failure (as defined in geotechnical
engineering; that is, an absolute value), cs is the uniaxial compressive strength of the
intact rock, and m and s are positive material parameters.
If the expression is converted into to the sign convention for principal stresses in the
Structural Mechanics Module, it becomes
2
 1 =  3 + – m cs  1 + s cs
with cs, m, and s positive material parameters. (In this case, note that 1  scs/m).
As developed originally, there is no relation between the parameters m and s and the
physical characteristics of a rock mass measured in laboratory tests. However, for intact
rock, s  1 and m  mi, which is measured in a triaxial test.
For jointed rock masses, 0  s  1 and m  mi. The parameter m usually lies in the
range 5  m  30 (Ref. 9).
TABLE 3-4: CHARACTERISTIC VALUES FOR DIFFERENT ROCK TYPES.
m
ROCK TYPE
5
Carbonate rocks, dolomite, limestone
10
Consolidated rocks, mudstone, shale
15
Sandstone
20
Fine-grained rocks
25
Coarse grained rocks
The Hoek–Brown criterion can be written in terms of the invariants I1 and J2 and the
Lode angle 0    3, so
1

F y = 2 J 2 sin   + --- –  cs s – m ------ = 0
c
3
THE GENERALIZED HOEK–BROWN CRITERION
The generalized Hoek–Brown criterion was developed to fit the Geological Strength
Index (GSI) classification of isotropic rock masses (Ref. 8). A new relationship
between GSI, m, s, and the newly introduced parameter a was developed to give a
580 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
smoother transition between very poor quality rock masses (GSI < 25) and stronger
rocks
1 a
 1 –  3 =  cs  s – m b --------

 cs
where cs is the compressive strength of the intact rock. In terms of the invariants J2
and the Lode angle 0    3 this equals
1 a
F y = 2 J 2 sin   + --- –  cs  s – m b -------- = 0
 cs
3
where 1  2  3 are the principal stresses (using the Structural Mechanics Module
conventions) of the effective stress tensor (that is, the stress tensor minus the fluid pore
pressure).
The positive parameter mb is a reduced value of the material constant mi:
GSI – 100
m b = m i exp  --------------------------
28 – 14D
s and a are positive parameters for the rock mass given by the following relationships:
GSI – 100
s = exp  --------------------------
9 – 3D
1 1
– GSI
– 20
a = --- + ---  exp  ------------- – exp  --------- 
2 6
15
3
The disturbance factor D was introduced to account for the effects of stress relaxation
and blast damage, and it varies from 0 for undisturbed in situ rock masses to 1 for very
damaged rock masses.
TABLE 3-5: DISTURBANCE FACTOR IN ROCK MASSES.
D
DESCRIPTION OF ROCK MASS
0
Undisturbed rock mass
0~0.5
Poor quality rock mass
0.8
Damaged rock mass
1.0
Severely damaged rock mass
MATERIAL MODELS
|
581
Damage Models
The deformation of quasi-brittle materials under mechanical loads is characterized by
an initial elastic deformation. If a critical level of stress or strain is exceeded, a nonlinear
fracture phase will follow the elastic phase.
As this critical value is reached, cracks grow and spread until the material fractures. The
occurrence and growth of the cracks play an important role in the failure of brittle
materials, and there are a number of theories to describe such behavior.
In the continuum damage mechanics formalism, a damage variable represents the
amount of deterioration due to crack growth. This damage variable controls the
weakening of the material’s stiffness, and it produces a nonlinear relation between
stress and strain.
For a linear elastic material, Hooke’s law relates the undamaged stress tensorun to
the elastic strain tensor:
 un =  ex + C  el =  ex + C    –  inel 
(3-68)
here, C is the fourth order elasticity tensor, “:” stands for the double-dot tensor
product (or double contraction). The elastic strain el is the difference between the
total strain  and inelastic strains inel. There may also be an external stress contribution
ex, with contributions from initial, viscoelastic, or other inelastic stresses. For a
hyperelastic material, the undamaged stress tensor follows from the definition of the
second Piola–Kirchhoff stress in Hyperelastic Materials.
For the scalar damage models, the damaged stress tensord is computed from the
undamaged stress as
 d =  1 – d  un
(3-69)
This damaged stress is then used in the weak formulation. There are different ways to
compute the scalar damage variable d that controls the material weakening. These are
listed in the following sections. When a large strain formulation is used, un and d
should be interpreted as the second Piola–Kirchoff stress.
The undamaged stress tensor un is used when combining the Damage
feature with Elastoplastic Materials, Elastoplastic Soil Models, Creep and
Viscoplasticity, or Linear Viscoelasticity.
582 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
STRAIN-BASED DAMAGE MODELS
The strain-based formulation for the Scalar damage and the Mazars damage for concrete
models is based on the loading function f such as
f =  eq –   0
(3-70)
here, eq is the equivalent strain, a scalar measure of the elastic strain; and is a state
variable. The evolution of the state variable follows the Kuhn–Tucker loading/
unloading conditions
f  0 , ꞏ  0 , and ꞏ f = 0
In this formulation,  is the maximum value of eq in the load history. The damage
variable d is then computed as a function of the state variable  and other parameters.
Equivalent Strain
Different damage models use different definitions for the equivalent strain eq. The
Rankine, stress damage model defines the equivalent strain from the largest undamaged
principal stress p1 as
  p1
 eq = ------------E
(3-71)
Here, “<·>” represent the Macaulay brackets and E is Young’s modulus. The Macaulay
brackets are used since in this formulation only tensile (positive) stresses cause damage.
Similarly, the Rankine, strain damage model defines the equivalent strain from the
largest principal elastic strain elp1 as
 eq =   elp1
(3-72)
The Smooth Rankine, stress damage model defines the equivalent strain from the three
undamaged principal stresses
  p1 2 +   p2 2 +   p3 2
 eq = -------------------------------------------------------------------E
(3-73)
In the same way, the Smooth Rankine, strain damage model defines the equivalent strain
from the three elastic principal strains
 eq =
  elp1 2 +   elp2 2 +   elp3 2
(3-74)
MATERIAL MODELS
|
583
By default, only the principal stresses in tension contribute to the damage evolution,
for both the Rankine and the Smooth Rankine damage models; but it is also possible
to include damage in compression by incorporating the compressive stresses in the
computation of the damaged stress tensord.
The Euclidean Norm of the elastic strain tensor can also be used as a measure for the
equivalent strain
 eq =
 el : el
(3-75)
The Euclidean norm considers both tensile and compressive strains.
For the Mazars damage for concrete model, it is also possible to select from Mazars or
Modified Mazars equivalent strain. Mazars equivalent strain is defined as
 eq =
  el :   el
(3-76)
In the modified Mazars equivalent strain (Ref. 2 and Ref. 3), a correction factor  is
added to improve the approximation of the failure surface of concrete in multiaxial
compression.
 eq =    el :   el
(3-77)
It is also possible to apply a User defined expression for defining the equivalent strain
as a function of undamaged stress, stress components or strains.
Damage Evolution
A key component in a scalar damage model is the definition of the damage evolution
law. The Linear strain softening law defines the damage variable from
f

d    =  1 – ----0-  ---------------
 f – 0
  0
d = 0
  0
,
(3-78)
Here,0 denotes the onset of damage, computed from the tensile strength ts and
Young’s modulus E, so that 0  tsE. The parameter f is derived from other material
parameters such as the tensile strength, the characteristic element size hcb and the
fracture energy per unit area Gf, or the fracture energy per unit volume gf.

2G f
 f = --------------- + ----0 ts h cb 2
584 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
(3-79)
The Exponential strain softening law defines the damage evolution from
–

d    = 1 – ----0- exp  – --------------0-
f – 0

  0
d = 0
  0
(3-80)
where

Gf
 f = --------------- + ----0 ts h cb 2
(3-81)
The Polynomial strain softening law defines the damage evolutions from
 – 0 2  – 0

d    = 1 – ----0- 1 +  ---------------  2 --------------- – 3

f – 0

f – 0
  0
d  = 0
  0
(3-82)
with f according to Equation 3-79.
The Multilinear strain softening law defines the damage evolutions from
 f – 
d    = 1 – ----0- -------------- f – p

d    = 1 – ----0
d = 0
  p
0    p
(3-83)
  0
with f according to Equation 3-79 and
Gf
 p =  ---------------- +  0  1 – 
---
 ts h cb
2
(3-84)
where is an input parameter that defines the shape of the curve.
Mazars Damage for Concrete
The Mazars damage for concrete utilizes two different damage evolution laws, one for
tensile damage and another for compressive damage. These two damage functions are
combined as


d    = t dt    + c dc   
(3-85)
MATERIAL MODELS
|
585
here, t and c are weight functions depending on the current stress state, and  is the
so-called shear exponent, which determines the response in shear, that is, the evolution
of the combined damage function in states where both damage functions are active.
To define the tensile damage evolution law dt(Ref. 3), it is possible to use either
Linear strain softening, Exponential strain softening, described in Damage Evolution
section; or Mazars damage evolution function. A tensile Mazars damage evolution
function is obtained by a combination of linear and exponential strain softening
 0t
d t    = 1 –  1 – A t  ------- – A t exp  – B t   –  0t  

dt    = 0
   0t
(3-86)
   0t
Here, At and Bt are tensile damage evolution parameters, and 0t is the tensile strain
threshold.
The compressive Mazars damage evolution function dcis obtained by
 0c
d c    = 1 –  1 – A c  ------- – A c exp  – B c   –  0c  

dc    = 0
   0c
(3-87)
   0c
Here, Ac and Bc are compressive damage evolution parameters, and 0c is the
compressive strain threshold. Both the tensile and compressive damage evolution laws
can also be specified by User defined expressions.
Spatial Regularization
The most common application for the damage models is to describe strain localization,
due to cracking in quasi-brittle materials. In a damage model without regularization,
the deformation during strain softening will always localize in the narrowest possible
band, following the principle of least action. This means that large strains will develop
in a narrow band of elements (or even Gauss points). As a consequence, the amount
of energy dissipated during softening will decrease upon mesh refinement. The results
of a damage model without regularization will therefore be mesh dependent and
possibly unstable; hence the need for these models to be regularized for the solution
to maintain its mesh objectivity.
The simplest regularization method is to modify the stress-strain relation to account
for the mesh size. More advanced regularization techniques introduce length scales in
the constitutive equation, and additional equations and variables acting as localization
586 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
limiters. The following sections describe the two methods for damage regularization
available in COMSOL Multiphysics.
The Crack Band Method
This simplest regularization technique is based on stress-strain curves (damage
evolution laws) that depend on the mesh and element characteristics. The method is
often called the Crack Band method (Ref. 4, Ref. 5). The method regularizes the
solution from a global viewpoint, which dissipates the correct amount of energy during
strain localization. The main difficulty when using the crack band method is to find the
correct width of the crack band, hcb; which can depend on the element size and shape,
as well as the order of the interpolation and the current stress state (that is, the
inclination of the crack with respect to the mesh).
hcb
hcb
The length scale used in the crack band method is computed by using the volume to
area ratio in the mesh elements. By using the element volume v in 3D or the area a in
2D, the crack bandwidth hcb is defined as:
• h cb =
2a , for 2D triangles
• h cb =
a , for 2D rectangles
• h cb =
3
6  2v , for 3D tetrahedra
• h cb =
3
6v  2 , for 3D pyramids
• h cb = 3 2v , for 3D wedges
• h cb = 3 v , for 3D hexahedra
The crack band width hcb is then used to modify the Damage Evolution law in which
the damage variable d is computed. Note that the damage evolution laws
(Equation 3-86 and Equation 3-87) are unaffected by the crack band method.
MATERIAL MODELS
|
587
The Implicit Gradient Method
The Implicit Gradient method (Ref. 6) enforces a predefined width of the damage
zone through a localization limiter. This is achieved by adding a nonlocal strain
variable, the nonlocal equivalent strain nl, through an additional PDE where the
equivalent strain eq acts as source term. This PDE is solved simultaneously with the
displacement field:
2
 nl – c  nl =  eq
(3-88)
Here, the parameter c controls the width of the localization band. This parameter is
defined from the internal length scale, lint, and the geometry dimension n (two or
three dimension)
2
l int
c = -----2n
(3-89)
If the fracture energy per unit area is used to define the softening behavior, the size of
the damage zone is also needed as input. This parameter does not necessarily have the
same value as lint.
The strain-based formulation for the damage model (Equation 3-70) is then redefined
by the nonlocal equivalent strainnl instead of the equivalent strain eq
f =  nl –   0
(3-90)
Viscous Regularization
A rate dependency can be introduced to the damage model by using the Delayed
damage viscous regularization method available for time-dependent studies. The
method can be used to model a real rate-dependent fracture problem, as well as for
stabilizing a rate-independent problem. In both cases, a viscous damage variable dv is
introduced. This variable is defined through the following ODE

d v
+ dv = d   
t
(3-91)
where  is the characteristic relaxation time. For the case when the viscous
regularization is used to stabilize a rate-independent fracture problem, should be
significantly smaller than the time step used by the solver in order not to modify the
properties of the problem too much. The viscous damage variable dv is then used in
Equation 3-69 to define the damaged stress tensor.
588 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
PHASE FIELD DAMAGE MODELS
The Phase field damage model is closely related to the Strain-based Damage Models,
but it is derived from a different starting point. Following a similar derivation as
reported in Ref. 7, the model is based on the regularization of a variational formulation
of the classical theory by Griffith for brittle fracture; where the geometric crack
discontinuity is regularized by a second-order phase field. Including a viscous
regularization of the crack phase field , the energy functional governing the crack
propagation takes the following form:
E  x t u u    =

  1 – d    Ws0 dx +    t dx


1 2 l int
2
+ G c  ------------  + ---------   dx
 2l int

2
(3-92)


where d is the damage function, Ws0 is the elastic strain energy density,  is the
viscosity, Gc is the critical energy release rate, and lint is the internal length scale that
appears form the regularization of the discrete fracture.
Given the two dependent variables, u and the main contributions to the coupled
initial boundary value problem (including inertial terms), are:
2 u
- =   d + FV
 --------t 2
on 
 d

2
2
= --------------- H d –   – l int    on 
t

on 
 0 = –   n

(3-93)
where the characteristic time  and the state variable Hd have been introduced. The
state variable Hd is a function of the crack driving force Dd, and it satisfies the Kuhn–
Tucker conditions so that:
H d  t u  = max    0 t  D d   u 
(3-94)
The momentum balance in Equation 3-93 is included for completeness but is not
implemented directly as part of the phase field damage model. However, the equation
gives an indication that the damaged stress, as defined by Equation 3-69, is used for
the mechanical equilibrium.
MATERIAL MODELS
|
589
Crack Driving Force
The crack driving force, Dd, can be either a function of the elastic strain energy density,
or it can also include dissipation processes.
By selecting the Elastic strain energy density, the crack driving force is derived from
l int
G c0
+
D d = ----------------------  W s0 – --------
G c – G c0
l int
(3-95)
where Ws0+ is the tensile part of the undamaged elastic strain energy density. The
strain energy threshold Gc0 is an ad hoc variable introduced to establish an elastic
threshold before damage occurs. By setting Gc0 equal to zero recovers the model
reported in Ref. 7.
By selecting Total strain energy density, additional contributions from dissipative
material features, such as creep, plasticity, and viscoelasticity, are added. Select the
Calculate energy dissipation check box in the parent material model to compute these
variables.
An alternative definition for the crack driving force based on stress measures is
suggested in Ref. 9. By selecting the Principal stress criterion, the crack driving force is
defined as
3
Dd =  
 pi 2
- 
  ------c 
(3-96)
i=1
where c is the critical fracture stress, pi are the undamaged principal stresses, and
 is a dimensionless parameter which determines the post peak slope.
It is also possible to enter a User defined expression for the crack driving force Dd.
Damage Evolution for Phase Field Damage
The damage variable d is in the phase field damage model a function of the crack phase
field . By selecting Power law, the damage evolution function is defined as
d  = 1 – 1 –  
m
(3-97)
where the exponent m is a user input. Often a quadratic function is used so that m  2.
An alternative damage function was suggested in Ref. 10. By selecting Cubic, Borden,
the damage evolution function d reads
3
2
2
d = 1 – s 1 –  – 1 –   – 31 –  + 21 – 
590 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
3
(3-98)
where the model parameter s controls the shape of the damage evolution function.
The Cubic, Borden option is only available when the crack driving force is defined
through the strain energy density.
It is also possible to enter a User defined expression for the damage evolution d as a
function of the phase field variable .
Strain Energy Split
Typically, phase field damage models use a decomposition of the undamaged strain
energy density Ws0 into a tensile and compressive parts. Only the tensile part Ws0+
affects the phase field, and consequently the damage growth and fracture. Several
alternative definitions of Ws0+ are available in COMSOL Multiphysics.
The simplest alternative is to set Ws0+ equal to the complete strain energy density Ws0,
which means that no split is made into tensile and compressive counterparts. Select No
split in the Exclude compressive energy list to achieve this. This option has the advantage
that it greatly simplifies the structure of the equations, although that comes at the cost
of physical correctness, especially for shear and cyclic loading.
A more accurate method is to use the volumetric-deviatoric split by selecting
Volumetric only in the Exclude compressive energy list. Here, only the positive part of
the volumetric stress is considered while the entire undamaged deviatoric stress
dev  dev(un) is included in Ws0+. The definition of Ws0+ then reads
+
1  I 1
W s0 = ---  ----------  el,vol +  dev : el,dev

2 3
(3-99)
where I1  trace(un) is the first invariant of the undamaged stress tensor defined in
Equation 3-68 (see Invariants of the Stress Tensor); and el,vol and el,dev are the
volumetric and deviatoric parts of the elastic strain tensor, respectively (see Invariants
of Strain). For hyperelastic materials, Equation 3-99 is replaced by

 W + W vol if
+
W s0 =  iso
if
 W iso

J el  1
J el  1
where Wiso is the isochoric strain energy density, Wvol is the volumetric strain energy
density, and Jel is the elastic volume ratio. The split is only available if the parent
hyperelastic model permits a clear split of Ws into two parts.
Another alternative is to define Ws0+ by performing a spectral decomposition of the
stress tensor such that
MATERIAL MODELS
|
591
3
+
1
W s0 = --2
  pi el pi
(3-100)
i=1
where pi are the principal values of the undamaged stress tensor un, and el,pi are the
principal values of the elastic strain tensorel (see Principal Strains).
Similarly, a spectral decomposition can be made directly on the elastic strain tensor as
suggested in Ref. 7. The tensile part of the elastic strain tensor is then
3
+
 el =
  el pi ni  ni
(3-101)
i=1
and the tensile part of the undamaged stress tensor is defined as
+
+
 = C  el
(3-102)
Using these two tensors, the tensile part of the elastic strain energy density is
+
1 + +
W s0 = ---  : el
2
(3-103)
Both the Spectral decomposition, stress and Spectral decomposition, strain options
involve computing the principal values and principal vectors. Such operations are
comparatively expensive and typically increase the computational cost of the phase field
damage method, however, these are the most physically correct formulations to use.
The choice of how to split the elastic strain energy density also affects how the
damaged stress tensor is constructed form the tensile part of the undamaged stress
tensor.
Coupled Damage–Plasticity
The coupled damage–plasticity material model combines damage mechanics with a
plasticity model to describe important characteristics of the mechanical response and
failure of concrete and similar materials subjected to multiaxial and cyclic loading
592 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
conditions. Specifically, it implements the constitutive model for concrete suggested in
Ref. 29 and Ref. 30.
The behavior of the coupled damage–plasticity model when subjected to
different loading conditions is exemplified in Concrete Damage–
Plasticity Material Tests: Application Library path Geomechanics_Module/
Verification_Examples/concrete_damage_plasticity.
GENERAL EQUATIONS
The general constitutive equations for the coupled damage–plasticity model uses the
concept of the damaged stress tensor d and the undamaged stress tensor un. The
former is used in the weak formulation while the latter describe the behavior of the
intact material.
The damaged stress is computed from the following constitutive equation
+
-
 d =  1 – d t  un +  1 – d c  un
where un is split into a positive and negative part by a spectral decomposition in order
to account for the anisotropic behavior of concrete in tension and compression. For
the same reason, two damage variables introduced: the tensile damage variable dt and
the compressive damage variable dc. These variables introduce a weakening of the
material’s stiffness, and varies from 0 for an undamaged state to 1 for a fully damaged
state. Their definitions are described in Damage Model.
The behavior of the intact material is commonly described by a linear elastic material
such that Hooke’s law relates un to the elastic strain tensor
 un =  ex + C  el =  ex + C    –  inel 
where, C is the fourth order elasticity tensor, “:” stands for the double-dot tensor
product (or double contraction). The elastic strain el is the difference between the
total strain  and inelastic strains inel. The coupled damage–plasticity model always
adds a plastic strain tensor pl to inel, but other contributions such as thermal strains
can also be considered. There may also be an external stress contribution ex, with
contributions from initial, viscoelastic, or other inelastic stresses.
PLASTICITY MODEL
The evolution of the plastic strains are based on the undamaged stress and thus
independent of damage. A flow plasticity model with isotropic hardening is used that
MATERIAL MODELS
|
593
introduces a yield function Fp, a plastic potential Qp, a scalar hardening variable p,
and the plastic multiplier p. The model can be summarized by the following evolution
equations for the plastic strain and the hardening variable
ꞏ
ꞏ Q p   un  p 
 pl =  p --------------------------------- un
ꞏ
 p = h p   un  pl 
together with the Kuhn-Tucker loading-unloading conditions
ꞏ
ꞏ
F p  0  p  0  p F p = 0
The yield function used is a generalization of The Willam–Warnke Criterion written as
a function of the Haigh–Westergaard coordinates in the space of the undamaged stress
tensor (un, run, un), as described in Invariants of the Stress Tensor, and p. It is
defined as
r un 2
 r un
 un 2

F p   un r un  un  p  =   1 – q h1   p    --------------- + -------- + 3
--- -------- 
2  cs 
 6 cs  cs 

(3-104)
r un
 un
2
2
+ m 0 q h1   p q h2   p  ---------------- r   un  + -------- + q h1   p q h2   p 
 cs
6 cs
where qh1 and qh2 are dimensionless hardening functions, and cs is the uniaxial
compressive strength. The friction parameter
2
2
3   cs –  ts  e
m 0 = ------------------------------- ----------- cs  ts e + 1
where ts is the uniaxial tensile strength and e is the eccentricity parameter. The
meridians of the corresponding yield surface Fp are parabolic, while the deviatoric
sections are triangular at low confinement but changes toward a circular shape at high
confinement. The shape of the deviatoric section is given by a dimensionless function
of the Lode angle un
2
2
2
4  1 – e cos  un +  2e – 1 
r   un  = ------------------------------------------------------------------------------------------------------------------------------------------------2
2
2
2
2  1 – e  cos  un +  2e – 1  4  1 – e cos  un + 5e – 4e
As suggested in Ref. 29 and Ref. 30, the eccentricity is in COMSOL Multiphysics
computed as
594 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
2
2
 ts  bc –  cs
1+
e = ------------- , with  = -------- ---------------------2–
 bc  2 –  2
bc
ts
where bc is the biaxial compressive strength.
A graphical representation of yield surface Fp = 0 in the undamaged principal stress
space and how evolves during hardening is shown in Figure 3-23 and Figure 3-24.
3
1 + 2 + 3
2
1
Figure 3-23: Graphical representation of the yield surface in the undamaged principal
stress space at different levels of hardening (p < 0.7). The red surface shows the initial
yield surface with p = 0.
MATERIAL MODELS
|
595
3
1 + 2 + 3
2
1
Figure 3-24: Graphical representation of the yield surface in the undamaged principal
stress space at different levels of hardening (p > 0.7).
Plastic Flow
The plastic flow is determined by a non-associative flow rule; an associative flow rule
typically leads to an overestimation of the strength of concrete due to an unrealistically
large volume expansion during plastic flow. Here the plastic potential is a simplified
version of the yield function in that it is independent of un, and is given as
r un 2
 r un
 un 2

Q p   un r un  p  =   1 – q h1   p    --------------- + -------- + 3
--- -------- 
2  cs 
 6 cs  cs 

(3-105)
m 0 r un m q   un  p 
2
+ q h1   p  ---------------- + ------------------------------ cs
6 cs
with
 ts
 un – q h2   p  -------3
m q   un  p  = A q   p B q   p  cs exp -------------------------------------------B   p  cs
where Aq(p) and Bq(p) are auxiliary functions derived from assumptions on the
plastic flow in the post-peak regime in uniaxial loading, see Ref. 30. They are defined as
 ts q h2   p  m 0
A q   p  = ---------------------------- + -------2
 cs
596 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
and
q h2   p  
 ts
-------------------- 1 + ------
3
 cs
B q   p  = --------------------------------------------------------------------------------------------------------------------------------------------------------m
ln A q   p  + ln  2D f – 1  – ln 3q h2   p  + -------0- + ln  D f + 1 
2
where Df is a model parameter that controls the dilatancy of the plastic flow. COMSOL
Multiphysics by default uses Df = 0.85.
Hardening
An isotropic hardening model is used to control the evolution of the yield surface
during plastic flow. The evolution of the scalar hardening variable p is proportional to
the norm of the plastic strain tensor and follows the evolution equation
 pl
2
ꞏ
 p = --------------------  2 cos  un 
x h   un 
From this equation it can be seen that the rate of p depends on the direction of
loading such that it grows faster in uniaxial compression while it is constant in uniaxial
tension. The rate of p is, furthermore, scaled by a ductility measure

h   un 
 A +  A – B  exp – R
--------------------if R h   un   0
h
h
 h
Ch

x h   un  = 
A h – B h R h   un 
  B – D  exp ----------------------------------------------+ Dh
otherwise
h
h

 B h – D h C h

such that the model is more ductile in compression. Here Ah, Bh, Ch, and Dh are
model parameters, and
 un 1
R h   un  = – -------- – -- cs 3
COMSOL Multiphysics uses default suggestions for these model parameters according
to suggestions in Ref. 29, where also a calibration procedure can be found if measured
data is available.
The hardening variable p enters the two dimensionless hardening functions qh1 and
qh2 that appear in Equation 3-104 and Equation 3-105. These functions control the
MATERIAL MODELS
|
597
evolution of the size and shape of the yield function and the plastic potential. They are
defined as

3
2
3
2
q h1   p  =  q h0 +  1 – qh0    p – 3 p + 3 p  – H p   p – 3 p – 2 p  if  p  1

else
 1
and
 1
if  p  1
q h2   p  = 
+


–
1

else
1
H
p p

where qh0 defines the initial yield limit, and Hp is a dimensionless hardening modulus
that controls the hardening in the post-peak regime. For the functions to be
well-defined it is required that 0 < Hp < (1 - qh0).
DAMAGE MODEL
The definition of the two damage variables, dt and dc, are defined in the framework of
isotropic damage mechanics, It can described by a damage loading function Fdi and
Kuhn-Tucker loading-unloading conditions
F di =  eq   un  –  di
(3-106)
ꞏ
ꞏ
F di  0  di  0  di F di = 0
(3-107)
where i = [t, c] for tension and compression, respectively. In the aboveeq is the
equivalent strain and di is a history variable. The damage variables are then defined
on the form
d i = g di   di  di1  di2 
where di1 and di2 are additional history variables.
The equivalent strain is the same for both tension and compression, and is derived from
the plastic yield surface Fp = 0. Using qh1 = 1 and qh2 = eq / 0 one can derive
598 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
 0 m 0 r un
 un
 eq   un r un  un  = ------------- ---------------- r   un  + -------2
 cs
6 cs
2
2
2 2
 0 m 0 r un
 un 2 3 0 r un
+ ------------- ---------------- r   un  + -------- + -----------------2
4
 cs
6
2
cs
cs
where 0 = ts / E. Noteworthy is that this definition of eq reduces to
 un
 eq = --------E
in uniaxial tension, and
 un  ct
 eq = --------- -------E  cs
in uniaxial compression.
History Variables, Tension
The equivalent strain in tension is given by the evolution equation
ꞏ
ꞏ
 eqt =  eq
or directly as eqt = eq. The definition of dt then follows from Equation 3-106 and
Equation 3-107. The two additional history variables dt1 and dt2 are introduced to
account for how damage evolves during different stress states. The first variable is a
function of the rate of the plastic strain tensor and is given by the evolution equation

1
ꞏ
 ------------------------------- 
if
 dt  1 and  dt   0
ꞏ
 dt1 =   s   un r un  pl

otherwise
 0
and the second is a function of dt given by
1
ꞏ
ꞏ
 dt2 = --------------------------------  dt
 s   un r un 
The evolution of these variables and thus also the softening response of the model are
sensitive to the multiaxial stress state which enters in the equations through the
ductility measure s. It is defined as
MATERIAL MODELS
|
599
 s   un r un  = 1 +  A s – 1 R s
(3-108)
with

6 un
 – ---------------- if
 un  0
Rs = 
r un

 0
otherwise
In uniaxial compression we get Rs = 1 and s = As, which can be useful for calibrating
the model parameter As. COMSOL Multiphysics by default uses As = 10.
History Variables, Compression
The equivalent strain in compression is given by the evolution equation
ꞏ
ꞏ
 eqc =  c  eq
The definition of dc then follows from Equation 3-106 and Equation 3-107. The two
additional history variables dc1 and dc2 are introduced to account for how damage
evolves during different stress states. The first variable is a function of the rate of the
plastic strain tensor and is given by the evolution equation

c c
ꞏ
 ------------------------------ꞏ
 dt  1 and  dt   0
 dt1 =      r   pl if
s un un

 0
otherwise
and the second is a function of dt given by
1
ꞏ
ꞏ
 dt2 = --------------------------------  dt
 s   un r un 
The factor c is introduced to distinguish between tensile and compressive stress, and
follows from the spectral decomposition of un as
3
c =
–  –  un i    un i –  –  un i 
 --------------------------------------------------------------------------2

i=1
un
where un,i is th ith principal value of un, and “<·>” denote the positive parts
operator. Note that c varies from 0 in pure tension to 1 in pure compression.
600 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
The factor c is introduced to accomplish a smooth transition between the case of pure
damage to damage–plasticity softening, which may occur during cyclic loading. It is
defined as
c =
 ct q h1   p 
2
---------------------------- ----------------------------2
r un
3  1 + 2D f 
where Df is the same model parameter used for the plasticity flow. The ductility
measure s is defined in Equation 3-108.
Damage Variables
Given the damage history variables, the definition of both damage variables dt and dc
follows the same format and the subscript is dropped for simplicity. Assuming
monotonic and uniaxial loading, the damaged stress in the softening regime can be
described by an enhanced inelastic strain, inel,d, such that
 dmg =  1 – d  un =  1 – d E   –  inel  = E   –  inel,d 
(3-109)
The damage variable is then defined such that the post-peak (or softening) is described
by an equation on the form
 dmg = f s   inel,d 
(3-110)
where fs(·) is the softening law; often referred to as a traction-separation law, although
here given in a terms of strain since we are working with a continuum.
Now since damage is an irreversible process, it is postulated that inel,d can be
described by the damage history variables. We can call this strain measure the inelastic
damage strain (or crack-opening strain) and define it as
 dmg =  d1 + d d2
Finally, replacing  - inel in Equation 3-109 with d such that
 dmg =  1 – d E d
and using it together with Equation 3-110 results in an equation for the damage
variable in terms of the known history variables on the form
f s   d1 + d d2  =  1 – d E d
(3-111)
MATERIAL MODELS
|
601
This equation is typically nonlinear and we need to solve it for d using Newton’s
method at each material point. COMSOL Multiphysics here provides a number of
built-in definitions of fs(·) for both tension and compression:
• Linear
• Bilinear
• Exponential
• Cornelissen (only tension)
These are depicted in a Figure 3-25. The linear and bilinear definitions have
closed-form solutions to Equation 3-111, which makes them computationally
attractive since it negates solving a nonlinear equation to find d.
Figure 3-25: Built-in softening laws.
When combined with the crack-band method, the stress versus strain curves in
Figure 3-25 are defined in terms of stress versus displacement. The stress versus
displacement curves are then converted to unique stress versus strains curves at each
material point using the crack-band width hcb, see The Crack Band Method.
In addition to the built-in softening laws, COMSOL Multiphysics allows user-defined
definitions of fs(·) and for this purpose provides the variables
<phys>.<feat>.<feat>.edmgt and <phys>.<feat>.<feat>.edmgc for the
damaged strain in tension and compression, respectively. Alternatively, the
user-defined softening behavior can be specified in terms of a stress versus
displacement curve fw(·). Equation 3-111 is then replaced by
602 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
f w  w dmg  = f w    d1 + d d2 h cb  =  1 – d E d
assuming that the crack-band method is used. If chosen, COMSOL Multiphysics
provides the variables <phys>.<feat>.<feat>.wdmgt and
<phys>.<feat>.<feat>.wdmgc for the damaged displacement in tension and
compression, respectively. For both these options, the a nonlinear equation needs to
be solved to find d.
Elastoplastic Soil Models
In this section:
• The Modified Cam-Clay Soil Model
• The Modified Structured Cam-Clay Soil Model
• The Extended Barcelona Basic Soil Model
• The Hardening Soil Model
• The Hardening Soil Small Strain Model
THE MODIFIED CAM-CLAY SOIL MODEL
The Cam-clay material model was developed in the 1970s at the University of
Cambridge, and since then it has experienced many modifications. The Modified
Cam-Clay (MCC) model is the most commonly used model due to its smooth yield
surface, and it is the one implemented in COMSOL Multiphysics.
The modified Cam-clay model is a so-called critical state model, where the loading
and unloading of the material follow different paths in stress space. The model also
features hardening and softening of clays. Different formulations can be found in
textbooks, see for instance Ref. 15, Ref. 16, and Ref. 17.
The yield function is written in terms of the stress invariants
q=
3J 2   
p = –I1     3
Following the Structural Mechanics Module sign convention (the pressure is positive
in compression), the yield function reads:
F y = q 2 + M 2  p – p c p = 0
MATERIAL MODELS
|
603
This is an ellipse in the pq-plane, with a cross section independent of the Lode angle.
Note that p, q, and pc are positive variables.
The parameter M  0 defines the slope of the critical state line in the pq-plane. This
parameter can be matched to the angle of internal friction  in the Mohr–Coulomb
criterion as
6 sin    M = ------------------------3 – sin   
(3-112)
critical state line
q=Mp
q
hardening
softening
nonlinear elastic region
pc/2
pc
p
Figure 3-26: Modified Cam-clay ellipse in the pq-plane. The ellipse circumscribes a
nonlinear elastic region.
The slope of the critical state line M can either be a material property or
it can be matched The Mohr–Coulomb Criterion and derived from the
angle of internal friction . It can also be matched to The Matsuoka–Nakai
Criterion; see Equation 3-121.
The soil response to isotropic compression is described by the curve of the void ratio
(or specific volume or volumetric strain) versus the logarithm of pressure as shown in
Figure 3-27.
The void ratio e is the ratio between the pore space and solid volume. It
can be written in terms of the porosity  as e = /(1  ).
604 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
.
e
eref

virgin consolidation line
e0

swelling line
pref
pi
pc0
ln(p)
Figure 3-27: Slopes of the virgin isotropic consolidation line and swelling line in the e
versus ln  p  plane.
The compression index  is the slope of the virgin isotropic consolidation line, and
the swelling index  is the slope of the swelling line (also called unloading-reloading
line) in the e versus ln(p) plane. The reference void ratio eref is measured at the
reference pressure pref and initial void ratio e0 is measured at the initial mean stress pi.
The starting value of initial mean stress pi is the reference pressure pref. The equation
for the virgin isotropic consolidation line is written as
p
e = e ref –  ln  ----------
 p ref
The void ratio at the initial consolidation pressure pc0 is given by
p c0
e c0 = e ref –  ln  ----------
 p ref
The equation for the swelling line is
p
e = e 0 –  ln  -----
 p i
where e0 is the initial void ratio calculated as
MATERIAL MODELS
|
605
p c0
e 0 = e c0 +  ln  --------
pi
The initial void ratio e0 can be directly entered as user input. In this case,
the void ratio at initial consolidation pressure, ec0, is not needed as
intermediate variable.
Assuming small deformations and adopting the sign convention of Structural
Mechanics, the volumetric strain is related to the void ratio as
e–e
V–V
 vol = ----------------0- = --------------0V0
1 + e0
For elastic response, the incremental volumetric elastic strain is written as
de - = –  dp
------d el, vol = -------------p
1 + e0
(3-113)
Integrating Equation 3-113, the equation is reformulated as
p
 1 + e 0  el, vol = –  ln  -----
 p i
Then the nonlinear relation between pressure and volumetric strain is obtained by
p = pi e
– B el 
el , vol
(3-114)
where
1+e
B el = --------------0
The contribution to initial mean stress pi also comes from the first
invariant of the initial or external stress tensor of Initial Stress and Strain or
External Stress feature. The reference pressure is generally a unit pressure
in the used unit system, in the literature the value varies from 1 kPa to
100 kPa. In COMSOL Multiphysics the default value is 100 kPa.
606 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
At zero volumetric elastic strain and with zero contribution from Initial Stress and
Strain or External Stress features the initial mean stress is nonzero and equal to the
reference pressure pref. The reference pressure acts as an in situ stress.
p i = p ref
(3-115)
The tangent bulk modulus Kt is written as
1 + e0
K t = --------------- p

The secant bulk modulus Ks (or bulk modulus K) is written as
pi – p
K s = -------------- el, vol
When a constant Poisson’s ratio is specified in the modified Cam-clay
model, the shear modulus is calculated from the secant bulk modulus and
Poisson’s ratio, which in turn gives a variable shear modulus.
The total volumetric strain increment in written as
 dp  –  dp c
de d vol = -------------= – --------------- ------- – --------------- --------+
1
e0 p 1 + e0 pc
1 + e0
The evolution of void ratio is then written as
e =  1 + e 0  vol + e 0 or
(3-116)
pc
pc
p
e = e ref –  ln  ----- –  ln  -------- +  ln  -----
p ref
pi
pi
(3-117)
Equation 3-116 is used to compute the void ratio which matches exactly with
Equation 3-117 which may be used for verification purposes.
In the modified Cam-clay model, hardening is controlled by the consolidation
pressure pc, which depends on the volumetric plastic strain p,vol as
MATERIAL MODELS
|
607
1+e
ꞏ
pꞏ c = – --------------0- p c  p,vol
–
(3-118)
The elastic and plastic volumetric strains are available in the variable
solid.eelvol and solid.epvol, respectively. The consolidation
pressure is available in the variable item.pc.
The evolution of the consolidation pressure depends on the values for the initial void
ratio e0, the swelling index , and the compression index , which are positive
parameters that fulfill
0     and e ref  0
If an Initial Stress and Strain node is added to the Cam-clay material, the
initial consolidation pressure pc0 must be equal or larger than one third
of minus the trace of the initial stress tensor, otherwise the initial stress
state is outside the Cam-clay ellipse.
Volumetric Elastic Deformation
The stress-strain relation beyond the elastic range is of great importance in soil
mechanics. For additive decomposition of strains, Cauchy’s stress tensor is written as
 = dev   0  + p i e
– B el 
el , vol
+ 2Gdev   el 
with
1+e
B el = --------------0
Here,  is the stress tensor,  is the total strain tensor, el is the elastic strain tensor, 0
is the initial or external stress tensor, and G is the shear modulus.
At zero volumetric strain, and with zero contribution from Initial Stress and Strain or
External Stress features, the pressure in the MCC model is equal to the reference
pressure (see Equation 3-114 and Equation 3-115). This is needed as the MCC model
do not have stiffness at zero stress. The reference pressure appears as an additional term
in the variational formulation (weak equation).
608 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
As opposed to the Linear Elastic Material, the MCC model introduces a nonlinear
relation for the hydrostatic pressure as a function of the volumetric elastic strain given
by Equation 3-114.
Hardening and Softening
The yield surface for the modified Cam-clay model reads
2
F y = q 2 + M  p – p c p
The plastic strain tensor p is computed from the flow rule
Q p
Q p I 1 Q p J 2
ꞏ
 p =  p ---------- =  p  ---------- -------- + ---------- ---------

I 1  J 2 
where p is the plastic multiplier and the derivatives of the plastic potential Qp with
respect to the stress tensor An associated flow rule is used such that Qp = Fy.
See also Plastic Flow for Additive Decomposition and Numerical Solution
of the Elastoplastic Conditions. If a multiplicative decomposition of
strains is used, the flow rule is reformulated according to Plastic Flow for
Multiplicative Decomposition.
The plastic strain rate tensor ꞏ p includes both deviatoric and isotropic parts. Note that
I 1   = I
and
J 2   = dev   
These relations can be used for writing the plastic flow as
Q p 3
1 Q p
ꞏ
 p =  p  – --- ---------- I + ---------- ------- dev   
 3 p

q 2q
since the associated flow rule implies a plastic potential such as
2
Q p = F y = q 2 + M  p – p c p
the plastic flow rule simplifies to
MATERIAL MODELS
|
609
1 2
ꞏ
 p =  p  – --- M  2p – p c I + 3dev   
3
The trace of the plastic strain rate tensor (the volumetric plastic strain rate ꞏ pvol )
then reads
2
ꞏ
ꞏ
 pvol = trace   p  =  p M  p c – 2p 
This relation explains why there is isotropic hardening when the pressure is p > pc2
and isotropic softening when p < pc2. As opposed to what happens in J2 plasticity, in
the modified Cam-clay soil model the volumetric plastic strain can either increase or
decrease as plastic deformation occurs.
In the MCC model, hardening is controlled by the consolidation pressure pc as a
function of volumetric plastic strain, as described in Equation 3-118.
Hardening introduces changes in the shape of the Cam-clay ellipse, since its major
semiaxis depends on the value of the consolidation pressure pc. The initial
consolidation pressure pc0 defines the size of the ellipse before plastic deformation
occurs.
Including Pore Pressure
When an external pore pressure pf is added to the MCC material, the yield function is
shifted along the p axis, and the yield function reads:
2
Fy = q 2 + M  p – pf – pc   p – pf 
The quantity p  pf is normally regarded as the effective pressure, or effective stress,
which should not be confused with the equivalent von Mises stress. To add the effect
of a fluid pressure in the pores pf to the modified Cam-clay material, add an External
Stress feature.
See also the description of the Elastoplastic Soil Material materials in the
Solid Mechanics interface documentation.
THE MODIFIED STRUCTURED CAM-CLAY SOIL MODEL
The Structured Cam-Clay (SCC) model was developed (Ref. 22, Ref. 23) to
circumvent the limitations of the Cam-clay model when applied to structured soils and
clays. The SCC model, however, does not consider the influence of the soil structure
610 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
neither on strength characteristics (especially cohesion) nor in the softening behavior,
and it is also not suitable to model cemented clays.
The Modified Structured Cam-Clay (MSCC) model was further developed to model
destructured, naturally structured and artificially structured clays (Ref. 22), and it is
the one implemented in the Geomechanics Module.
In the MSCC model, the reduction of mean effective stress due to structure
degradation, pb, depends on the shear plastic strain p,dev. The destructuring
mechanism is the process of reducing structure strength due to the degradation and
crushing of the structure. The structure degradation is given by
pb =
p bi e –  p,dev
p bf e
if  p,dev   p,deve
– d s   p,dev –  p,deve 
(3-119)
otherwise
Here, pbi is the initial structural strength, pbf the failure structural strength, p,devc is
the equivalent plastic strain at failure, and ds is the destructuring index due to shear
deformation.
The equivalent deviatoric plastic strain at which the crushing of the
structure begins, p,devc, has a typical value between 0.15 and 0.3 for
most clays.
Structured clays show a higher void ratio than destructured clays at the same effective
mean stress. The virgin compression behavior during the destructuring process is
expressed by
e = e  + e
e = e i  p c0  p c 
dv
where is e void ratio of the structured clay, e is additional void ratio, e* is void ratio
of the destructured clay at the same stress state. The void ratio can be found by using
Equation 3-117. Further, ei is the additional void ratio at consolidation pressure, and
dv is the destructuring index due to volumetric deformation.
The yield surface for the modified structured Cam-clay model reads
2
Fy = q 2 + M  p + pb   p – pc 
MATERIAL MODELS
|
611
The nonassociated plastic potential reads
2
p + pb 2  
2
2
2
M
Q p = q + -----------   p + p b  –  ------------------  p c + p b  



–1
p c + p b
Here,  is a parameter to smooth the shape of the plastic potential. The slope of the
critical state line, M can be found by using Equation 3-112.
In the modified structured Cam-clay soil model, hardening is controlled by the
consolidation pressure pc as a function of volumetric plastic strain, and is described as
1 + e0
ꞏ
– ------------------------------------------------------- p c  p,vol
M


 –  + d v e -------------- M – 
pꞏ c =
1 + e0
ꞏ
– ---------------------------------- p c  p,vol

 –  + d v e
if   M
otherwise
Here, * is the compression index for destructured clay,  is the swelling index, and 
is ratio of shear stress to mean stress.
The MSCC and MCC models are equivalent when ei = 0,  = 2, and
pb = 0.
The relationship between hydrostatic pressure and volumetric elastic strain is the same
as the one outlined in The Modified Cam-Clay Soil Model,
p = pi e
– B el 
el , vol
1+e
with B el = --------------0
(3-120)
The stress tensor is then computed from
 = dev   0  + p i e
– B el 
el , vol
+ 2Gdev   el 
At zero volumetric strain, and with zero contribution from Initial Stress and Strain or
External Stress features, the pressure in the MSCC model is equal to the reference
pressure (see Equation 3-120 and Equation 3-115). This is needed as the MSCC
model do not have stiffness at zero stress. The reference pressure appears as an
additional term in the variational formulation (weak equation).
612 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
THE EXTENDED BARCELONA BASIC SOIL MODEL
The Barcelona Basic Model (BBM) was developed to simulate the loading of
unsaturated and partially saturated soils, by incorporating an extra state variable for the
pore suction. The suction value depends on the amount of water in the soil, and it
affects the flow in porous soils as well as the deformation and stress distribution.
The BBM model uses the concepts of plasticity theory, incorporating the critical state
model (Ref. 24). This soil model matches the results obtained with the modified
Cam-clay model in fully saturated soils.
The so-called Extended Barcelona Basic Model (BBMx) was further developed to
overcome numerical limitations of the original BBM model (Ref. 25). The model
implemented in COMSOL Multiphysics follows Ref. 25 with certain modifications
described in this section.
The BBMx model presents a smooth yield surface with respect to both stress and
suction
Fy
2
= q2 + M  p – p
b  s – sy 
– bs y
-----------------------------p ref
p ref
2 


p
+
p

+
p
e
–
e


cs
s
ref


Here, p and q are stress invariants as defined in The Modified Cam-Clay Soil Model,
pcs is the consolidation pressure at current suction, ps is the tensile strength due to
current suction, s is the current suction, b is a dimensionless smoothing parameter, sy
is the yield value at current suction, and pref is the reference pressure at which the
reference void ratio eref was measured.
The tensile strength due to current suction, ps, is linearly related to the suction level
as ps = ks, where k is the tension to suction ratio.
The consolidation pressure at current suction pcs is calculated from
0 –  
 -------------------
p c    s  – 
p cs = p ref  ---------
 p ref
where sis the compression index at current suction, 0 is the compression index at
saturation, and  is the swelling index. The compression index at current suction, s,
is given by
  s  =  0   1 – w e
–s  m
+ w
MATERIAL MODELS
|
613
where w and m are weighting and soil stiffness parameters.
The slope of the critical state line M can be computed from the Matsuoka–Nakai
criterion, in which case it depends on both the Lode angle  and the angle of internal
friction 

1  4


6
sin



2


M =  --------------------------  ---------------------------------------------------------------------
3 – sin    
 

 1 +  –  1 –   sin  3 – --2- 
(3-121)
where
3 – sin    4
 =  ---------------------------
 3 + sin   
At the tensile or compressive meridians, where the Lode angle is =  or  = , the
slope of the critical state line achieves the same expression as when matched to The
Mohr–Coulomb Criterion, see Equation 3-112
6 sin    M = ------------------------3 – sin   
It can also be matched to The Matsuoka–Nakai Criterion.
The associated plastic potential for the BBMx model reads
Qp = Fy
The plastic strain increments are computed from the derivatives of the plastic potential
with respect to stress only.
As in The Modified Cam-Clay Soil Model, hardening is controlled by the evolution of
the consolidation pressure pc, which depends on the volumetric plastic strain p,vol.
1+e
ꞏ
pꞏ c = – --------------0- p c  p,vol
0 – 
(3-122)
The initial void ratio e0, the swelling index , and the compression index at saturation
0, are positive parameters.
The evolution of the yield value at current suction, sy, is also governed by the
volumetric plastic strain pl,vol as
614 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
1 + e0
ꞏ
-  s + p atm  p,vol
sꞏ y = – ---------------s – s y
(3-123)
Here, s is the compression index for changes in suction, s is the swelling index for
changes in suction, and patm is the atmospheric pressure, all positive parameters. Note
that Equation 3-122 and Equation 3-123 are normally given with opposite sign. Here,
however, the structural mechanics convention is used, so the increments in
consolidation pressure and suction are positive in compression.
The evolution of void ratio is then written as
e =  1 + e 0  vol + e 0 or
p cs
p cs
p
e = e s ref –   s  ln  --------- +  ln  -------- –  ln  -----
 p ref
 pi 
 p i
where
e s ref = e ref –  s ln   s + p atm   p atm 
In the BBMx model, the total volumetric elastic response is combination of elastic
response by pressure and suction,

s
ds el,vol =  el,vol +  el,vol = – dp
------- – ------K K cs
where
K cs =  1 + e 0   s + p atm    s
Here K is the bulk modulus, and Kcs the stiffness to suction. Note that the pressure p
in compression and suction s is positive variables, but the elastic volumetric strain
el,vol is negative in compression. The volumetric elastic response due to suction is
given by
s
 s + p atm 
s
 el,vol = – --------------- ln  ------------------------
1 + e 0  s 0 + p atm
Here, s0 is the initial suction. The volumetric elastic response due to suction is
accounted in the total strain tensor for BBMx model, so any changes in suction with
keeping pressure constant can cause volumetric strains.
MATERIAL MODELS
|
615
The relationship between hydrostatic pressure and volumetric elastic strain is the same
as the one outlined in The Modified Cam-Clay Soil Model
p = pi e
– B el 
el , vol
1+e
with B el = --------------0
(3-124)
The stress tensor is then computed from
 = dev   0  + p i e
– B el 
el , vol
+ 2Gdev   el 
At zero volumetric strain, and with zero contribution from Initial Stress and Strain or
External Stress features, the pressure in the BBMx model is equal to the reference
pressure (see Equation 3-124 and Equation 3-115). This is needed as the BBMx
model does not have stiffness at zero stress. The reference pressure appears as an
additional term in the variational formulation (weak equation form).
Note that the material property 0 is the compression index at saturation,
which does not depend on the suction. The variable (s), which is a
function of the current suction, is the compression index (slope) in the
void ratio versus logarithm of the mean stress plot. The material property
s is the compression index (slope) in the void ratio versus logarithm of
the matrix suction plot, which does not depend on the mean stress.
THE HARDENING SOIL MODEL
The Hardening Soil model is an elastoplastic material model with a stress and stress
path-dependent stiffness. It is a so-called double stiffness model, meaning that the soil
stiffness is different during primary loading and unloading/reloading load paths
(Ref. 26).
The yield surface for the hardening soil model is a combination of a conical surface and
an elliptic cap surface in stress space.
In the original hardening soil model, failure in shear occurs according to The Mohr–
Coulomb Criterion. In the so-called Hardening Soil Smooth model (Ref. 26), failure
in shear occurs according to the The Matsuoka–Nakai Criterion. In Ref. 28, the
so-called Panteghini and Lagioia version of Matsuoka–Nakai criterion is used.
The 50% failure stiffness for primary loading, E50, and the stiffness for unloading
and reloading, Eur, are used to define the plastic potential and failure criterion. These
are given by
616 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
ref c cot    –  1
E 50 = E 50  -----------------------------------
c cot    + p ref
m
ref c cot    –  1
E ur = E ur  -----------------------------------
c cot    + p ref
m
and
ref
Here E 50 is the reference failure stiffness for primary loading at reference pressure,
ref
E ur is the reference stiffness for unloading and reloading at reference pressure, c is
the cohesion,  is the angle of internal friction, and m is the stress exponent.
The ultimate deviatoric stress qf and the stress to failure qa are derived from The
Mohr–Coulomb Criterion
2c cos    – 2 1 sin   
q
q f = --------------------------------------------------------and q a = ------f
1 – sin   
Rf
where Rf is the failure ratio. Consider the stress invariants q = 3J 2 and
p = – I 1  3 , the yield function and plastic potential for the shear hardening are given
by
qa q
2q
F y = q a  ----------------------------– --------- –  
E 50  q a – q  E ur p
q
q
Q p = --- –  p + --- sin   m 
2
6
where p is the accumulated plastic shear strain and m is the mobilized dilatancy
angle.
The definition of the shear strain p in the original hardening soil model
is not compatible with pure volumetric loading as it does not vanish
during pure volumetric straining. Therefore, the shear strain measure p
is defined as  p = 2 J 2   pl  , see Nonlinear Elastic Materials.
The yield function for the elliptic cap, and the associated plastic potential, are also
defined in terms of stress invariants, and given by
MATERIAL MODELS
|
617
2
2
 Rc q 
F y = Q p = -----------------+p
------ – p c
pc
pc
Here, Rc is the ellipse aspect ratio, and it can directly entered, or given in terms of the
nc
coefficient of earth pressure at rest k 0
1R c = ------nc
k0
nc
The coefficient of earth pressure at rest k 0 is computed from the angle of internal
friction 
nc
k 0 = 1 – sin   
The modified deviatoric stress q is defined as
q =  1 –   – 1  2 –  3
where
3 + sin   
 = --------------------------3 – sin   
The internal variables pc and p depend on the volumetric plastic strain pl,vol and the
plastic strain invariant J2 pl, and their evolution is defined as
ꞏ
pꞏ c = – H  pl,vol
ꞏ
ꞏ
 p = 2 J 2   pl 
where H is the hardening modulus which depends on the bulk modulus in
compression Kc and the bulk modulus in swelling Ks
ref
E ur
1- = ----1- – ----1- where K = -------------------------------s
3  1 – 2 ur 
H
Kc Ks
The dilatancy cutoff is implemented by setting the mobilized dilatancy angle m equal
to zero when the void ratio reaches the critical void ratio emax.
Cauchy’s stress tensor is then written as
 –  0 = C:   –  inel 
618 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
where C is a function of the stiffness modulus Eur and Poisson’s ratio .
Mobilized Dilatancy Angle
The mobilized dilatancy angle m is explicitly used in the definition for the plastic
potential Qp. Different authors define this variable using different expressions. The
original expression for the mobilized dilatancy derived by Rowe (Ref. 26) is
sin  m – sin  c
sin  m = ---------------------------------------1 – sin  m sin  c
(3-125)
here, c is the critical friction angle and m is the mobilized friction angle, and these
are derived from
sin  – sin sin  c = ---------------------------------1 – sin  sin 
1 – 3
sin  m = ------------------------------------------ 1 +  3 + 2c cot 
where is the dilatancy angle, i are the principal stresses, c is the cohesion, and  is
the angle of internal friction.
Rowe’s original model for the mobilized dilatancy angle is highly contractive at low
angles, so in the original hardening soil model it is modified to
sin  m – sin  c
sin  m = max  0 ----------------------------------------
 1 – sin  m sin  c
(3-126)
however, this modification also gives too little plastic volumetric contraction.
Other expressions (Ref. 26) for the mobilized dilatancy angle include the Wehnert
correction
sin  m – sin  c
sin  m = max  0.07 ----------------------------------------

1 – sin  m sin  c
(3-127)
the Soreide correction
sin  m – sin  c sin  m
sin  m =  ----------------------------------------  ----------------
 1 – sin  m sin  c  sin  
(3-128)
and the correction by Li and Dafalias
MATERIAL MODELS
|
619
1 p
1
sin  m = ------  p
--- – Mexp  ------ ln ----c- 
 15 p  
10  q
(3-129)
The Rowe–Li–Dafalias model uses Equation 3-126 to define the mobilized dilatancy
angle when sin  m  sin  c , and Equation 3-129 otherwise.
THE HARDENING SOIL SMALL STRAIN MODEL
The Hardening Soil Small Strain model is a combination of Small Strain Overlay
model and The Hardening Soil Model.
The initial shear modulus is computed from other material parameters, as done in the
hardening soil model
ref c cot    –  1
G 0 = G 0  -----------------------------------
c cot    + p ref
m
ref
Here G 0 is the reference initial shear modulus for primary loading at reference
pressure, c is the cohesion,  is the angle of internal friction, and m is the stress
exponent.
The critical shear strain, defined as
 G ref

0
 c =  ref  --------- – 1


ref
 G ur

is used to switch between the shear stiffness derived from the small strain overlay and
the hardening soil models
G =
G 0 when    c
G ur when    c
here, Gur is the shear modulus for unloading/reloading, as defined in the The
Hardening Soil Model.
m
ref c cot    –  1
G ur = G ur  -----------------------------------
c cot    + p ref
620 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
Creep and Viscoplasticity
In this section:
• Creep
- Creep Material Models
- Creep Rate Function
- Equivalent Stress, Creep Flow and Hardening Rule
- Hardening Function
- Thermal Function
- Combining Creep Models
- Time Integration
- Converting Between Different Data Representations
• Viscoplasticity
- Anand Model
- Chaboche Model
- Perzyna Model
- Bingham Model
- Peric Model
• Creep and Viscoplasticity for Large Strains
• Polymer Viscoplasticity
- Bergstrom–Boyce Model
- Bergstrom–Bischoff Model
- Parallel Network Model
• Energy Dissipation
In the literature, the terms viscoplasticity and creep are often used
interchangeably to refer to the class of problems related to
rate-dependent plasticity. A distinction is sometimes made so that creep
refers to models without a yield surface.
MATERIAL MODELS
|
621
CREEP
Creep is an inelastic time-dependent deformation that occurs when a material is
subjected to stress (typically much less than the plastic yield stress) at sufficiently high
temperatures.
The creep strain rate depends in a general case on stress, temperature, and time, usually
in a nonlinear manner:
ꞏ
 cr = F cr   T t 
It is often possible to separate these effects multiplicatively:
ꞏ
 cr   t T  = f   g  T h  t 
Experimental data shows three different types of behavior for the creep strain rate at
constant stress as function of time. Researchers normally subdivide the creep curve into
these three regimes, based on the fact that many different materials show similar
responses:
• In the initial primary creep regime (also called transient creep) the creep strain rate
decreases with time to a minimum steady-state value.
• In the secondary creep regime the creep strain rate is almost constant. This is also
called steady-state creep.
• In the tertiary creep regime the creep strain increases with time until a failure
occurs.
When this distinction is assumed, the total creep rate can be additively split into
primary, secondary, and tertiary creep rates
ꞏ
 cr = F cr1 + F cr2 + F cr3
In most cases, Fcr1 and Fcr3 depend on stress, temperature, and time, while secondary
creep, Fcr2, depends only on stress level and temperature. Normally, secondary creep
622 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
is the dominant process. Tertiary creep is seldom important because it only accounts
for a small fraction of the total lifetime of a structure or mechanical component.
cr
1
primary creep
2
tertiary creep
secondary creep
1 >2
log time
Figure 3-28: Uniaxial creep as a function of logarithmic time.
Creep Material Models
The mathematical description of a general creep model can be summarized by a set of
equations given in a similar format as the flow theory of plasticity. The creep strain is
given by a flow rule that defines the relationship between the rate of the creep strain
tensor cr and the current state of stress. This flow rule can be written as
Q cr
ꞏ
 cr =  cr ----------
where cr is the creep multiplier, Qcr is the creep potential, and  is the stress tensor.
The creep multiplier is an explicit function of stress , temperature T, time t, and the
equivalent creep strain ce, and can be given on a general format as
 cr = f   e g  T h   ce t 
where the generic functions f, g, and h that define the creep rate and can be combined
to construct different types of creep models. The hardening rule, h(ce, t), defines the
relationship between the creep strain tensor cr and the equivalent creep strain ce. The
equivalent stress e is a scalar representation of the Cauchy stress tensor, and given
associative creep flow, it also defines the creep potential so that
MATERIAL MODELS
|
623
Q cr =  e
Creep Rate Function
The creep rate function f is typically a function of the equivalent stress e or any other
scalar measure of the current stress state. In COMSOL Multiphysics, there are several
built-in creep rate functions:
• Norton (Power law)
• Garofalo (Hyperbolic sine law)
• Nabarro–Herring (Diffusional Creep)
• Coble (Diffusional Creep)
• Weertman (Dislocation Creep)
It is also possible to define an arbitrary expression for f so that, in principle, any creep
model can be implemented. The expressions used for the built-in creep rate functions
are described in the following sections.
The Norton model is the most common secondary creep model, where the creep rate
is assumed proportional to a power law of the equivalent stress e such that
e n
f   e  = A  ---------
 ref
(3-130)
where A is the creep rate coefficient, n is the stress exponent, ref is a reference stress
level.
At very high stress levels the creep rate is proportional to the exponential of e.
Garofalo showed (Ref. 8, Ref. 9) that the power-law and exponential creep are limiting
cases for the general empirical expression
n
ꞏ
 cr   sinh   e  
This equation reduces to a power-law (the Norton model) when e  0.8 and
approaches exponential creep for e  1.2, where 1 is a reference equivalent stress
level. The Garofalo (Hyperbolic sine law) creep model implemented in COMSOL
Multiphysics is given as
e n
f   e  = A  sinh  --------- 

  ref 
624 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
For metals at low stress levels and high temperatures, Nabarro and Herring (Ref. 6,
Ref. 7) independently derived an expression for the creep rate as a function of atomic
diffusion, so called diffusional creep. The Nabarro–Herring model implemented in
COMSOL Multiphysics is given as
7D v b 3
f   e  = -----------------2-  e
k B Td
where d is the grain diameter, Dv is the volume diffusivity through the grain interior,
b is the Burgers vector, kB is the Boltzmann’s constant, T is the absolute temperature.
Another model for diffusional creep is the Coble creep model (Ref. 6, Ref. 7), which
is closely related to Nabarro–Herring creep, but takes into account the grain boundary
diffusivity through the parameter Dgb. The Coble creep model implemented in
COMSOL Multiphysics is given as
50D gb b 4
-
f   e  = ---------------------k B Td 3 e
For metals at intermediate to high stress levels and temperatures close to the melting
temperature of the solid, the creep mechanism can be assumed to be
diffusion-controlled movements of dislocations in the crystal lattices (Ref. 7). This
type of creep deformation can be described by the Weertman model, which is given as
e n
Db
f   e  = -----------  ref  ---------
  ref
kB T
Generally, the stress exponent n in the Weertman model takes a value between 3 and
5 when modeling dislocational creep.
Coble creep is more sensitive to grain diameter than Nabarro–Herring
creep.
Equivalent Stress, Creep Flow and Hardening Rule
For metals and alloys, creep is in most cases deviatoric (volume preserving), and can
often be described by a von Mises equivalent stress
e =
3J 2    =
3
--- dev   :dev   
2
MATERIAL MODELS
|
625
where J2 is the second invariant of the stress deviator. If creep is orthotropic, the Hill
orthotropic equivalent stress can be used, which is given by
2
3
 e = ------------------------------  F   22 –  33  2 + G   33 –  11  2
2F + H + G
2
2
(3-131)
2
+ H   11 –  22  2 + 2  L 23 + M 31 + N 12  
where F, G, H, L, M, and N are Hill’s coefficients that relate the anisotropy to the local
coordinates. In the above equation it is assumed that an average equivalent stress can
be computed from F, G, and H using a von Mises like expression; this assumption leads
to the first term on the right-hand-side of Equation 3-131.
For soils and other geological materials, creep is often volumetric and can be described
by a Pressure equivalent stress
1
 e = p = --- tr   
3
where p is the pressure.
It is also possible to specify a user defined equivalent stress in terms of the stress tensor
and its invariants.
For more information and the background on the equivalent stress
definitions, see Elastoplastic Materials.
Assuming associative creep flow, the creep flow rule is given as function of the
equivalent stress
 e
Q cr
ꞏ
 cr =  ----------- =  --------

The hardening rule is also assumed to be associative.
The dimensionless tensor N, which gives the direction of the creep flow, is computed
from the creep potential Qcr as
Q cr
N = ----------
When von Mises equivalent stress is used, the potential equals Qcr  mises, and the
deviatoric tensor Ndev is defined as done for J2 plasticity (see Isotropic Plasticity)
626 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
3 dev   
N dev = --- ----------------2 e
the creep flow rule is then written as
Q cr
ꞏ
 cr =  ----------- = N dev

Given the property N dev :N dev = 3  2 , the evolution of the equivalent creep strain
reads
ꞏ
 ce =
2
--- ꞏ cr :ꞏ cr = 
3
(3-132)
The same hardening rule is also used when the Hill orthotropic equivalent stress is
selected.
For the Pressure equivalent stress, the flow direction is volumetric
Q cr
1
= --- I
N vol = ----------3

the volumetric creep flow rule is given as
Q cr
ꞏ
 cr =  ----------- = N vol

and the hardening rule reads
ꞏ
ꞏ
ꞏ
 ce = tr   cr  =  cr,vol = 
When a user-defined equivalent stress is used, a von Mises like hardening rule is used
according to Equation 3-132.
Hardening Function
The creep hardening function h is typically a function of time t and the equivalent
creep strain ce. In COMSOL Multiphysics, there are two built-in hardening
functions, Strain hardening and Time hardening, and it is also possible to specify a
user defined expression. Also, it is possible to add hardening to any of the built-in creep
models.
A common model for modeling primary and secondary creep together is the so-called
Norton–Bailey (or Bailey–Norton) model. Here, the creep strain is proportional to a
power of the equivalent stress (Norton law) and a power of time (Bailey law)
MATERIAL MODELS
|
627
n m
 cr   e t
by taking the time derivative of this generic expression at constant stress, it is found
that the creep strain rate and stress are related by the time hardening function
n m–1
n
ꞏ
 cr  m e t
= e h  t 
where the time hardening function is given by the power law
t + t shift m – 1
h  t  = m  -------------------
 t ref 
here, tshift is a time shift, tref is a reference time, and m is the hardening exponent.
Similarly, the strain hardening function is given by the power law
  ce +  shift 
h   ce  = m  ----------------------------------
 t ref f   e g  T 
m – 1------------m
where shift is the equivalent creep strain shift, tref is a reference time, and m is the
hardening exponent.
The strain shift shift and the time shift tshift in the hardening functions serve two
purposes:
• To initialize a study where hardening has already taken place.
• To remove singularities. The strain rate expressions actually predict an infinite creep
rate at t = 0, unless a shift is used. This singularity is weak in the sense that the time
integral is well defined, but it will cause numerical problems. Adding a small shift
overcomes this problem.
Both the strain hardening function h(ce) and the time hardening
function h(t) return a dimensionless expression, but for elastoplastic
material models with Numerical Solution of the Elastoplastic Conditions,
the Hardening Function returns an expression in units of stress (SI unit:
Pa).
628 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
Thermal Function
The temperature shift function g typically depends on the absolute temperature T. In
COMSOL Multiphysics, an Arrhenius temperature function is built-in, but it is also
possible to specify a user defined expression.
The Arrhenius temperature function is given as
Q 1
1 -
g  T  = exp – ----  --- – -------R T T ref
where Q is the activation energy (J/mol), R is the gas constant, T is the absolute
temperature, and Tref is a reference temperature.
Combining Creep Models
Using a combination of f, g, and h together with the definition of the equivalent stress
e makes it possible to construct sophisticate creep models. For example, the often
used temperature-dependent isotropic Norton creep model is obtained by the
following settings:
• Creep model: Norton
• Equivalent stress: von Mises
• Thermal effects: Arrhenius
The resulting creep model is then given by the following equations:
e n
Q cr
Q 1
ꞏ
1 - N
 cr =  ----------- = A  --------- exp – ----  --- – -------dev

 ref
R T T ref
Furthermore, selecting a time hardening function results in the Norton–Bailey creep
model:
 e n t + t shift m – 1
Q cr
Q 1
ꞏ
1 - N
 cr =  ----------- = A  --------- m  -------------------
exp – ----  --- – -------dev

 ref
t ref
R T T ref
Several creep rate contributions can be added to the total creep rate to construct more
elaborate models. This is done by adding one or more Additional Creep subnodes to an
existing Creep node. There are no restrictions on how to combine models; for example,
MATERIAL MODELS
|
629
a von Mises based creep flow contribution can be combined with a Pressure based
creep flow contribution.
• In the example Combining Creep Material Models:
Application Library path Nonlinear_Structural_Materials_Module/Creep/
combined_creep
a Norton–Bailey model for primary creep is combined with a Norton
model for secondary creep. Both creep models are temperature
dependent. The resulting creep-rate equation becomes
 e n t + t shift m – 1
Q1 1 1 
ꞏ
 cr = A 1  --------- m  -------------------
exp – -------  --- – ------ N dev
  ref
 t ref 
R T T 
1
Q2 1 1 
e
+ A 2  --------- exp – -------  --- – ------ N dev
  ref
R T T 
2
Time Integration
The rate equations given by the creep flow and hardening rules have to be integrated
in time to compute the value of the creep strain tensor cr and the equivalent creep
strain ce at each time step. This can be done using any of the following methods:
• Backward Euler
• Forward Euler
• Domain ODEs
For an arbitrary number of contributions to the creep deformation, the general
equations to be solved can be formulated as
ꞏ
 cr =
Q cr
 =
   ----------  Ncr i
  i
i
ꞏ
 ce =
(3-133)
i
  Nce i
(3-134)
i
where Ncr and Nce are tensors that describe the direction of cr and ce, respectively.
The Backward Euler method is used to discretize these equations as
n + 1 –  n = t
 cr
cr
  n + 1 Ncrn + 1 i
i
630 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
(3-135)
n + 1 –  n = t
 ce
ce
  n + 1 Ncen + 1 i
(3-136)
i
where n+1 indicates that the variable is evaluated at the current time step, and t is the
n and equivalent creep strain  n at the previous
time step. The creep strain tensor  cr
ce
time step are stored as internal state variables. Equation 3-135 and Equation 3-136
define a system of nonlinear equations that is solved locally at each Gauss point for
n + 1 and  n + 1 using Newton’s method.
 cr
ce
The Forward Euler method is used to discretize Equation 3-133 and Equation 3-134
as
n + 1 –  n = t
 cr
cr
  Ncr in
(3-137)
i
n + 1 –  n = t
 ce
ce
  Nce in
(3-138)
i
such that all quantities on the right-hand-side are evaluated at the previous time step.
This means that Equation 3-137 and Equation 3-138 define an explicit update of
n + 1 and  n + 1 given only known quantities from the previous time step. The
 cr
ce
forward Euler method is only conditionally stable, and the time step of the global time
marching scheme has to be constrained to preserve stability and accuracy of the
method. In COMSOL Multiphysics the limit for a stable time step is estimated as





1
el
t max = min  --- ----------------------------
4
 N ce  in




i
where el is the elastic strain tensor. This estimate in principle restricts the creep
increment to be smaller than the current state of stress, and 1/4 is a constant to make
the estimate conservative. The final value is computed as the minimum value over all
Gauss points in the domain where the creep feature is active.
For Domain ODEs, Equation 3-133 and Equation 3-134 are converted to weak-form
and solved as part of the general initial-boundary value problem. The components of
MATERIAL MODELS
|
631
the creep strain tensor cr and the equivalent creep strain ce are then treated as
degrees-of-freedom.
For more information see the Modeling with ODEs and DAEs and The
ODE and DAE Interfaces chapters in the COMSOL Multiphysics
Reference Manual.
Converting Between Different Data Representations
The equations described in the previous sections about the different creep models
differ from the forms most commonly found in the literature. The main difference lies
in the introduction of normalizing reference values such as the reference stress ref and
reference time tref. These values are in a sense superfluous and can in principle be
chosen arbitrarily. The choice of reference values, however, affects the numerical values
to be entered for the material data. The implementation in COMSOL Multiphysics has
two advantages:
• It is possible to use the built-in unit management system.
• There is not any need to perform any difficult unit conversions when creep data are
available in units other than the units in the model. Since many creep models
contain the stress or time raised to a noninteger power, such conversions are error
prone.
Norton Law
Material data for a Norton law is often available as the parameters AN and n in the
equation
n
ꞏ
 cr = A N  e
The coefficient AN has a physical dimension that depends on the value of n, and the
unit has an implicit dependence on the stress and time units. Converting the data to
the format used in COMSOL Multiphysics (for example, Equation 3-130) requires
the introduction of the reference stress ref. It is convenient here to use the implicit
stress unit for which AN is given as the reference stress. The creep rate coefficient A
will then have the same numerical value as AN, and you do not need to do any
conversions.
The physical dimension of A is, however, (time)1, whereas the physical dimension of
AN is (stress)n(time)1.
632 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
Another popular way of representing creep data is to supply the stress giving a certain
creep rate. As an example, c7 is the stress at which the creep strain rate is 107/h. Data
on this form is also easy to enter: You set the reference stress ref to the value of c7
and enter the creep rate coefficient A as 1e-7[1/h].
Example
Assume that a carbon steel has the following two equivalent descriptions of its creep
properties at a certain temperature:
• c7 = 70 MPa, and stress exponent n = 4.5.
• AN = 4.98·10-16 with respect to units MPa and hours, and stress exponent n = 4.5.
In the first case, enter:
• ref as 70[MPa]
• n as 4.5
• A as 1e-7[1/h].
In the second case, enter:
• ref as 1[MPa]
• n as 4.5
• A as 4.98e-16[1/h]
These two sets of data describe the same material.
Garofalo Law
Since the stress inside in the Garofalo law appears as an argument to a sinh() function,
it must necessarily be dimensionless. Most commonly this is however written as
n
ꞏ
 cr   sinh   e  
Comparing with the expression in COMSOL Multiphysics,
e n
ꞏ
 cr   sinh  --------- 

  ref 
it is evident that the reference stress should be chosen as
1
 ref = --
MATERIAL MODELS
|
633
In this case, there is no arbitrariness in the choice of ref, since  is an actual material
parameter.
VISCOPLASTICITY
Viscoplasticity, as well as Creep, is an inelastic time-dependent deformation that occurs
when the material is subjected to stress (typically much less than the yield stress). The
growth of unrecoverable strains depend on the rate at which loads are applied, effect
that is normally enhanced by high temperatures.
The viscoplastic strain vp is computed by a flow rule that defines the relationship
between the rate of vp and the current state of stress and temperature.
When an associative flow and von Mises equivalent stress e are used, so Qvp  e, the
rate of vp is coaxial to the stress deviator and the viscoplastic flow rule is written as
Q vp
3 dev   
ꞏ
 vp =  vp ------------ =  vp --- ------------------- =  vp N dev

2 e
where Qvp is the viscoplastic potential,  is the stress tensor, and Ndev  Qvp   is
the flow direction.
The viscoplastic multiplier vp depicts a different expression for different viscoplastic
models (Anand, Chaboche, and so on), and it is equal to the equivalent viscoplastic
ꞏ
strain rate  vpe
ꞏ
 vpe =
2
--- ꞏ vp :ꞏ vp =
3
2
2 N
---  vp
dev :N dev =  vp
3
given the property N dev :N dev = 3  2 .
Setting different measures for the equivalent stress e (von Mises, Tresca, Hill) allows
to define different viscoplastic multiplier and flow directions, see Equivalent Stress,
Creep Flow and Hardening Rule for details.
Anand Model
Anand viscoplasticity (Ref. 9) is a deviatoric viscoplastic model suitable for isotropic
viscoplastic deformations. As for the models described in Creep, the Anand model has
no yield surface.
The rate of vp is determined by the viscoplastic multiplier vp which is a function of
stress  and temperature T, and it is given by
634 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
 vp = Ae
– Q  RT
e
sinh   -----
 sa
1
----m
here, A is the viscoplastic rate coefficient, Q is the activation energy (J/mol),  is the
stress multiplier, m is the stress sensitivity, and R is the gas constant.
The deformation resistance, sa (SI unit: Pa), controls the hardening behavior of the
Anand model. In COMSOL Multiphysics it is derived for the normalized resistance
factor, sf, and the deformation resistance saturation coefficient, ssat, such that
sa = ssat sf. The resistance factor sf is a dimensionless internal variable that is
computed by the evolution equation
sꞏ f = h vp
with the initial condition sf(0)  sinit / ssat. The evolution of the resistance factor sf is
controlled by the dimensionless hardening function
h0
h0

s a
s a – 1
s
sf 
h = --------- 1 – ----f- sign  1 – ----f- = --------- 1 – ----f 1 – ----*-
*
*
*
s sat
s sat


sf
sf 
sf
sf 
were h0 (SI unit: Pa) represents a constant rate of athermal hardening in the curve
stress versus strain (Ref. 9). The use of the sign function and the absolute value in the
hardening function permits the modeling of either strain hardening or strain softening,
depending on whether sf is greater or smaller than the saturation value sf*.
The saturation value sf* is calculated from the expression
 vp Q  RT
*
s f =  -------- e

A
n
where n is the deformation resistance sensitivity exponent.
The Anand model computes the equivalent viscoplastic strain rate (viscoplastic
multiplier) using the evolution equation for the internal variable
1----
e m
– Q  RT
ꞏ
sinh   -----
 vpe =  vp = Ae
 sa
Anand–Narayan Model
Anand–Narayan model (Ref. 10) is suitable for modeling the viscoplastic deformation
of lithium.
MATERIAL MODELS
|
635
The equivalent viscoplastic strain rate (viscoplastic multiplier) is given by
ꞏ
 vp =  vpe = Ae
1
-----
 e m
----  s a
– Q  RT 
where A is the viscoplastic rate coefficient, Q is the activation energy (J/mol),  is the
stress multiplier, m is the stress sensitivity, and R is the gas constant.
The deformation resistance, sa (SI unit: Pa), is computed with an extra dependent
variable as done for Anand Model.
Chaboche Model
The equivalent viscoplastic strain rate (viscoplastic multiplier) is given by
 e –  ys n
ꞏ
 vp =  vpe = A  ------------------- for  e –  ys  0
 ref
and the viscoplastic strain rate tensor is given by
ꞏ
 vp =  vp N dev
Here, A is the viscoplastic rate coefficient (SI unit: 1/s), n is the stress exponent
(dimensionless), and ref is a reference stress level (SI unit: Pa).
The Macaulay brackets   are applied on the yield function, which is defined as done
for plasticity
F =  e –  ys
The equivalent stress e is either the von Mises, Tresca, or Hill orthotropic stress, or a
user defined expression; and ys is the yield stress (which may include an Numerical
Solution of the Elastoplastic Conditions model). The stress tensor used in the
equivalent stress e is shifted by what is usually called the back stress, back when
Kinematic Hardening is included.
The deviatoric tensor Ndev is computed from the viscoplastic potential Qvp
Q vp
N dev = -----------
636 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
When von Mises equivalent stress is used, the associated flow rule reads Qvp  F, and
the deviatoric tensor Ndev is defined as done for deviatoric creep.
For more information see Converting Between Different Data
Representationsthe for the relation between the viscoplastic rate
coefficient A, the stress exponent n, and the reference stress ref.
Perzyna Model
The Perzyna model defines the equivalent viscoplastic strain rate (viscoplastic
multiplier) by
n

ꞏ
 vp =  vpe = A  ------e- – 1 for F =  e –  ys  0
 ys
and the viscoplastic strain rate tensor is given by
ꞏ
 vp =  vp N dev
As described for Chaboche Model, the equivalent stress e can be either von Mises
(default), Tresca, Hill orthotropic stress, or a user defined expression. The flow
direction Ndev  Qvp   is computed from the viscoplastic potential Qvp, which can
be associated or nonassociated.
Bingham Model
Bingham model is equivalent to Chaboche Model when setting the exponent n  1,
and denoting the viscosity as the quotient   ref/A. The equivalent viscoplastic
strain rate (viscoplastic multiplier) is given by
1
ꞏ
 vp =  vpe = ---   e –  ys for F =  e –  ys  0

and the viscoplastic strain rate tensor is given by
ꞏ
 vp =  vp N dev
As described for Chaboche Model, the equivalent stress e can be either von Mises
(default), Tresca, Hill orthotropic stress, or a user defined expression. The flow
direction Ndev  Qvp   is computed from the viscoplastic potential Qvp, which can
be associated or nonassociated.
MATERIAL MODELS
|
637
Peric Model
The Peric model defines the equivalent viscoplastic strain rate (viscoplastic multiplier)
by
e n
ꞏ
 vp =  vpe = A   ------- – 1 for F =  e –  ys  0
 ys
and the viscoplastic strain rate tensor is given by
ꞏ
 vp =  vp N dev
As described for Chaboche Model, the equivalent stress e can be either von Mises
(default), Tresca, Hill orthotropic stress, or a user defined expression. The flow
direction Ndev  Qvp   is computed from the viscoplastic potential Qvp, which can
be associated or nonassociated.
User Defined
It is possible to freely define the viscoplastic rate vp
ꞏ
 vp =  vpe for F =  e –  ys  0
The conditional evaluation F  0 is handled automatically.
By default, an associative flow and von Mises equivalent stress e are used, so Qvp  F,
the rate of vp is coaxial to the stress deviator, and the viscoplastic flow rule is written as
Q vp
3 dev   
ꞏ
 vp =  vp ------------ =  vp --- ------------------- =  vp N dev

2 e
Thermal Effects
The temperature function g typically depends on the absolute temperature T. In
COMSOL Multiphysics, an Arrhenius temperature function is built-in, but it is also
possible to specify a user defined expression.
The Arrhenius temperature function is given as
Q 1
1 -
g  T  = exp – ----  --- – -------R  T T ref
638 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
where Q is the activation energy (J/mol), R is the gas constant, T is the absolute
temperature, and Tref is a reference temperature.
See also the description of Viscoplasticity in the physics interface
documentation.
Time Stepping
The rate equations given by the viscoplastic flow rule and evolution equations for the
two internal variables are integrated in time to compute the value of the viscoplastic
strain tensor vp, the equivalent creep strain vpe, and other possible internal variables
(for instance, the resistance factor sf in Anand model) at each time step. This can be
done using any of the following methods:
• Backward Euler
• Domain ODEs
The Backward Euler method is used to discretize these equations as
n + 1 –  n = t n + 1 N n + 1
 vp
vp
vp
vp
(3-139)
n + 1 – n
n+1 n+1
 vpe
vpe = t vp N vpe
(3-140)
where Nvp and Nvpe are tensors that describe the direction of vp and vpe,
respectively, n+1 indicates that the variable is evaluated at the current time step, and
t is the time step.
For Anand Model an extra equation is solved for the resistance factor, sf,
n + 1hn + 1
s fn + 1 – s fn = t vp
(3-141)
n , equivalent viscoplastic strain  n , and the resistance
The viscoplastic strain tensor  vp
vpe
n
factor s f at the previous time step are stored as internal state variables.
Equation 3-139 to Equation 3-141 define a system of nonlinear equations that is
n + 1 ,  n + 1 , and s n + 1 using Newton’s
solved locally at each Gauss point for  vp
vp
f
method.
MATERIAL MODELS
|
639
For Domain ODEs, the evolution equations of the viscoplastic model are converted
to weak-form and solved as part of the general initial-boundary value problem. The
components of vp, vpe, and sf are then treated as degrees of freedom.
For more information see the Modeling with ODEs and DAEs and The
ODE and DAE Interfaces chapters in the COMSOL Multiphysics
Reference Manual.
CREEP AND VISCOPLASTICITY FOR LARGE STRAINS
When the Large strains formulation is selected in the Creep or Viscoplasticity nodes, a
Multiplicative Decomposition of deformation gradients is used
F = F el F in
here, F is the deformation gradient, Fel is the elastic deformation, and Fin is inelastic
deformation due to creep or viscoplasticity.
The velocity gradient then reads (see Strain Rate and Spin for details)
ꞏ
ꞏ
ꞏ
ꞏ
ꞏ
–1 F
–1
L = F F –1 =  F el F in + F el F in F –1 = F el F el + FF in
in F
The velocity gradient can then be split into the elastic and inelastic parts, L = Lel + Lin.
The inelastic velocity gradient
ꞏ
–1
–1 F
L in = FF in
in F
is energy conjugate to the stress tensor, and it is coaxial to it for maximum dissipation.
Neglecting the inelastic spin, so the inelastic deformation gradient is symmetric, the
formulation for large strain viscoplasticity or creep is similar to the formulation
described in the Plastic Flow for Multiplicative Decomposition section. The
time-derivative of the inverse inelastic deformation gradient is given by the rate
Q in
ꞏ –1
–1
F in
= –  in F – 1 ------------ FF in

(3-142)
where in is the equivalent creep or viscoplastic strain rate, and Qin is the creep or
viscoplastic potential. For creep and viscoplasticity in metals (so-called J2 plasticity)
the viscoplastic potential depends on the deviatoric stress, Qin  QinJ2 , and the
flow direction is deviatoric, Ndev  Qin  .
640 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
For large strains, Equation 3-142 is numerically solved with the so-called exponential
mapping technique, as described in Numerical Solution of the Elastoplastic
Conditions, and the elastic deformation gradient then obtained from
–1
F el = FF in
POLYMER VISCOPLASTICITY
Elastomers and biological materials exhibit strain rate dependent mechanical behavior
and hysteresis when subjected to cyclical loads
Bergstrom–Boyce Model
The Bergstrom–Boyce model (Ref. 35–36) is a viscoplastic material that successfully
capture such phenomena, and it is suitable for modeling rubbers and elastomers.
The rheology of this material model is similar to the Standard Linear Solid Model, but
the deformation in the spring-dashpot branch is nonlinear.
The stiffness in the spring is defined by the energy factor v. This factor multiplies the
isochoric strain energy density defined in the main hyperelastic branch, in a similar way
as done for Large Strain Viscoelasticity. For instance, if the main branch is defined by
an Arruda–Boyce hyperelastic material with a shear modulus 0, then the shear
modulus in the spring is 1  v0.
The rate of viscoplastic deformation is given by a Multiplicative Decomposition of
deformation gradients
F = F el F vp
here, F is the deformation gradient in the hyperelastic branch, Fel is the elastic
deformation in the spring, and Fvp is inelastic deformation in the dashpot.
The velocity gradient reads (see Creep and Viscoplasticity for Large Strains)
ꞏ
ꞏ
ꞏ
ꞏ
ꞏ
–1 F
–1
L = F F – 1 =  F el F vp + F el F vp F – 1 = F el F el + FF vp
vp F
The viscoplastic velocity gradient, Lvp, is energy conjugate to the stress tensor  in the
branch. For volume-preserving viscoplasticity, it is defined as
3
  ꞏ
–1 =  N
–1 F
--- dev
---------------L vp = FF vp
vp F
vp dev with N dev = 2 
e
The equivalent viscoplastic strain rate (viscoplastic multiplier) is similar to the rate
defined for the Chaboche Model, but it also incorporates strain hardening
MATERIAL MODELS
|
641
 e –  co n
ꞏ
 vp =  vpe = Ah   vpe   -------------------- for  e –  co  0
 res
here, A is the viscoplastic rate coefficient, e is the von Mises stress in the network, co
is a cutoff stress, res is the flow resistance, and n is the stress exponent.
For more information see Converting Between Different Data
Representations the for the relation between the viscoplastic rate
coefficient A, the stress exponent n, and the flow resistance res.
The strain hardening function hvpe is defined by the power-law
h   vpe  =   vpe – 1 +   c
Here, c is the strain hardening exponent and  is a small numerical constant. The
equivalent viscoplastic stretch vpe is computed from the viscoplastic deformation
 vpe =
F vp :F vp
--------------------3
Bergstrom–Bischoff Model
The Bergstrom–Bischoff model, also known as the three network model (Ref. 35,
Ref. 37) is suitable for modeling elastomers and thermoplastics. The rheology is similar
to the Bergstrom–Boyce model, but it adds two parallel branches instead of one.
The stiffness in the spring in the first branch is defined by the energy factor v1. This
factor multiplies the isochoric strain energy density defined in the main hyperelastic
branch, in a similar way as done for Bergstrom–Boyce Model. For instance, if the main
branch is defined by an Arruda–Boyce hyperelastic material with a shear modulus 0,
then the stiffness in the spring is 1  v10.
The viscoplastic rate in the first branch includes a power law to represent stress
hardening or softening
n1
 e,1
ꞏ
 vp1 =  vpe1 = A  -----------------------------
  res,1 + a 1 p
here, A is the viscoplastic rate coefficient, e,1 is the von Mises stress in the branch,
res,1 is the flow resistance, a1 is a material parameter to control the influence of the
hydrostatic stress, and n1 is the stress exponent.
642 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
The energy factor in the second branch v2 is computed after solving the rate equation
ꞏ
 v2 = –    v2 –  vf  vp1
Here, v2 is the final energy factor after saturation. The energy factor is initialized to a
value equal to v2  vi. The energy factor v2 then multiplies the isochoric strain
energy density defined in the main hyperelastic branch to define the stiffness of the
spring in the second branch, in a similar way as done in the first branch.
The viscoplastic rate in the second branch also includes a power law to represent stress
hardening or softening
n2
 e,2
ꞏ
 vp2 =  vpe2 = A  -----------------------------
  res,2 + a 2 p
here, e,2 is the von Mises stress in the branch, res,2 is the flow resistance, a2 is a
material parameter to control the influence of the hydrostatic stress, and n2 is the stress
exponent.
The material model also includes a power law expression to model thermal softening,
see Thermal Effects for details.
Parallel Network Model
The Parallel Network model (Ref. 35, Ref. 37) can be seen as a generalized version of
the Bergstrom–Boyce Model, where several viscoplastic branches can be added in
parallel to the main hyperelastic branch.
It is possible to choose a different elastic strain energy for the viscoplastic branch as
compared to that of the main hyperelastic branch, however, all the additional
viscoplastic branches are assumed to have the same type of hyperelastic strain energy
density as the first branch.
For example, it is possible to combine a Neo-Hookean material in the main
hyperelastic branch with two parallel spring-dashpot branches characterized by an
Arruda–Boyce model.
Several networks can be added to build more elaborate viscoplasticity models, and the
energy factors vi are used to differentiate the response of the additional stiffnesses.
This is done by adding one or more Additional Network subnodes to an existing Polymer
MATERIAL MODELS
|
643
Viscoplasticity node. The rheological representation of this model can be seen in
Figure 3-29.
d
Wiso
v1
v2
1
2
.....
vm
m
Fel
F
Fvp
d
Figure 3-29: Parallel network model.
The dashpots in the additional viscoplastic branches can showcase strain hardening,
like in the Bergstrom–Boyce Model, or pressure-dependent stress hardening like in the
Bergstrom–Bischoff Model.
User Defined
Enter the equivalent viscoplastic strain rate (viscoplastic multiplier). This can be any
expression of the von Mises stress, e, and the equivalent viscoplastic stretch vpe
ꞏ
 vp =  vpe   e  vpe 
The viscoplastic velocity gradient, Lvp, is then defined as
3
  ꞏ
–1 =  N
–1 F
--- dev
---------------L vp = FF vp
vp F
vp dev with N dev = 2 
e
Thermal Effects
The temperature function g(T) depends on the absolute temperature T, and it acts as
a multiplier for the viscoplastic rate.
The Arrhenius temperature function is given as
Q 1
1 -
g  T  = exp – ----  --- – -------RT T 
ref
where Q is the activation energy (J/mol), R is the gas constant, T is the absolute
temperature, and Tref is a reference temperature.
The Power law temperature function is given as
644 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
T m
g  T  =  ---------
T ref
where T is the absolute temperature, Tref is a reference temperature, and m is the
temperature exponent.
It is also possible to specify a user defined expression for the temperature function
g(T).
ENERGY DISSIPATION
Since creep and viscoplasticity are inelastic processes, the dissipated energy density can
be calculated by integrating the creep dissipation rate density or viscoplastic
dissipation rate density given by
ꞏ
ꞏ
W cr = : cr
ꞏ
ꞏ
W vp = : vp
in time. The total energy dissipated in a given volume can be calculated by a volume
integration of the dissipated creep energy density Wcr or dissipated viscoplastic energy
density Wvp.
When the Calculate dissipated energy check box is selected, the dissipation
rate density due to creep is available under the variable solid.Wcdr and
the dissipation rate density due to viscoplasticity is available under the
variable solid.Wvpdr. The dissipated energy density due to creep is
available under the variable solid.Wc and due to viscoplasticity under the
variable solid.Wvp. Here solid denotes the name of the physics
interface node.
Inelastic Strain Rate
The inelastic behavior of materials is often described by the rate of the inelastic
quantity, especially if the behavior is time dependent and nonlinear. For example,
Elastoplastic Materials, Linear Viscoelasticity, Creep and Viscoplasticity all describe
material models that are implemented in dedicated features. The Inelastic Strain Rate
node provides functionality to specify a general expression for the rate of inelastic
deformation, entered either as strain tensor ie; deformation gradient Fie; deformation
MATERIAL MODELS
|
645
–1
gradient inverse F ie ; or stretch ie. The user defined expression can be a function of
any variable in the model.
Given a generic inelastic quantity Uie, the feature sets up and solves the following type
of distributed ODE
dU ie
------------- = f  t u U ie  
dt
(3-143)
where t is the time, u is the displacement, and f(t, u, Uie,...) is a user defined
expression. Equation 3-143 is also subjected to the initial condition
init
U ie  t 0  = U ie
init is a user defined input.
where U ie
Time Integration
The distributed ODE in Equation 3-143 is integrated in time to compute the value of
the inelastic quantity Uie at each time step. This can be done using any of the following
methods:
• Backward Euler
• Domain ODEs
The Backward Euler method is used to discretize Equation 3-143 as
n + 1 – Un
U ie
ie
n + 1  
------------------------------ = f  t n + 1 u n + 1 U ie
t
(3-144)
where n+1 indicates the current time step, and t is the time step. The inelastic
n is stored as internal state variables, their initial
quantity at the previous time step U ie
init
value is given by U ie . Equation 3-144 defines a system of nonlinear equations that is
n + 1 using Newton’s method.
solved locally at each Gauss point for U ie
For Domain ODEs, Equation 3-143 is converted to weak-form and solved as part of
the general initial-boundary value problem. The components of the inelastic quantity
Uie are here treated as a degrees-of-freedom of the model.
For more information see the Modeling with ODEs and DAEs and The
ODE and DAE Interfaces chapters in the COMSOL Multiphysics
Reference Manual.
646 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
Shape Memory Alloy
The term shape memory alloy (SMA) normally refers to alloys that can undergo large
strains, effect called superelasticity or pseudoelasticity; and also to materials that after
undergoing large deformations can remember their original shape when heated above
a certain temperature, so-called memory effect.
These alloys are mixtures of metals such as copper, aluminum, nickel, titanium, and
other. Nickel-titanium (NiTi) alloys have applications in many industries due to their
thermal and mechanical properties. Most of the industrial applications of NiTi alloys
take advantage of the different mechanical properties of the two crystalline structures
found around room temperature: austenite and martensite.
Hot NiTi alloys are composed by a pure austenite phase. The martensite phase
develops upon cooling the alloy below the martensite start temperature, Ms. The
martensite volume fraction M will increase until the cooling temperature reaches the
martensite finish temperature, Mf, below which the alloy microstructure will be pure
martensite.
The reverse process has different transition temperatures: A pure martensite alloy will
develop an austenite microstructure if it is heated above the austenite start
temperature, As. The austenite phase will increase upon heating the material to the
austenite finish temperature, Af, above which the alloy microstructure becomes 100%
austenite.
Many industrial applications take advantage of this hysteresis loop, as the transition
temperatures are not the same in a heating-cooling cycle.
Under stress free conditions, these phase transformation temperatures (also called
critical temperatures) are such that Mf <Ms<As<Af.
There are two shape memory alloy models available with the Nonlinear Structural
Material Module: the Souza–Auricchio model and the Lagoudas model. These
material models differ in the expression for the free energy density.
SOUZA–AURICCHIO MODEL
For the Souza–Auricchio model, Helmholtz free energy density depends on two state
variables: the total strain tensor  and the temperature T. An additional internal variable
is used to compute the transformation strain tensor tr (Ref. 38-40)
K 2
2 Hk
2
   T  tr  = cT  1 – ln  T   + ----  vol + G   –  tr  + -------   tr  +  m  T   tr + I   tr 
2
2
MATERIAL MODELS
|
647
Here, c is the heat capacity at constant pressure, K and G are the bulk and shear
moduli, vol is the volumetric strain, Hk is the hardening modulus, and I(tr) is the
indicator function for the strain limit constraint. The equivalent transformation
strain tre is used as a measure of the transformation strain tensor
 tre =  tr =
2
---  tr : tr
3
The indicator function is defined by
 0 for  tre   tr, max
I   tr  = 
otherwise

The indicator function plays the role of a penalty function for the equivalent
transformation strain tre.
The term ch  mTtr is denoted as the chemical energy density due to the
thermally induced martensite transformation. The function mT corresponds to the
temperature-dependent martensite to austenite equilibrium stress, defined from the
slope of the limit curve and the reference temperature T*
*
m  T  =   T – T 
Here, the operator   denotes the Macaulay brackets.
The conjugated thermodynamic stress tr associated to the transformation strain
variable is
  tr
- = dev    – H 
I- – ------- tr = -------k tr –  m  T  ---------- tr  tr
 tr
(3-145)
The evolution of the transformation strain tr is given by the so-called limit function,
which takes the same form as the yield function for von Mises plasticity.
F y =  tr –  0
where 0 is the elastic domain radius.
In Ref. 39 it was suggested to consider the asymmetric behavior that many alloys show
in tension and compression. In this case, the limit function depends on the Lode
angle , the elastic radius in tension t, and elastic radius in compression c.
648 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
c – t
2 c  t
F y =  tr +  tr ----------------- cos  3  – ---------------c + t
c + t
Denoting the elastic domain radius in tension 0  t, and the compression to
tension stress ratio k such as c  kt  k0, the asymmetric limit function reads
k–1
2k
F y =  tr +  tr ------------- cos  3  – -------------  0
k+1
k+1
In Ref. 39, the stability for the limit function Fy is achieved when k  1.286.
For an additive strain decomposition, the evolution equation for the transformation
straintr is computed from the flow rule
F y
ꞏ
 tr =  p --------
where the plastic multiplierp is solved with the Kuhn–Tucker conditions, as done for
plasticity, see Plastic Flow for Additive Decomposition.
When a multiplicative decomposition is used for the Souza–Auricchio model, an
evolution equation is formulated for the transformation deformation gradient Ftr in
terms of the flow rule
ꞏ
–1
–1
– 1 F y
F tr = –  p F --------- FF tr

where F is the total deformation gradient. See also Plastic Flow for Multiplicative
Decomposition. The last three terms in Equation 3-145 can, moreover, be recognized
as the back stress in a linear kinematic hardening model. Hence the framework for
kinematic hardening with Multiplicative Decomposition is used.
LAGOUDAS MODEL
For Lagoudas model, Gibbs free energy density depends on two state variables: the
total stress tensor  and the temperature field T. Additional internal variables are used
to compute the transformation strain tensor tr and the martensite volume fraction 
(Ref. 41)
1
T
1 :S: – 1
--- :   th –  tr  + u 0 + --- f   
G   T  tr   = c   T – T 0  – Tln ------ – s 0 T – -----
T0

2
Here, c is the heat capacity at constant pressure, s0 is the specific entropy at reference
state, S is the compliance matrix,th is the thermal strain tensor,tr is the
transformation strain tensor, u0 is the specific internal energy at reference state, and
MATERIAL MODELS
|
649
f() is the transformation hardening function. The compliance matrix S, is obtained
by a volume average of the elastic properties of martensite and austenite
S    = S M +  1 –  S A = S A + S
where S  SM  SA. Also, other material parameters are averaged this way.
As opposed to Souza–Auricchio model, the evolution equation for the transformation
straintr is computed from the flow rule
ꞏ
ꞏ
 tr =  
where the normalized transformation tensor  changes principal directions
depending on the direction of the martensitic transformation.
The maximum transformation strain in Lagoudas model can be considered constant,
or stress-dependent as described in Ref. 42. A stress-dependent maximum
transformation strain can be used at low stress levels, where the martensite turns into
detwinned structures.
ꞏ
The variable for the direction of the martensitic transformation,  , is calculated from
the previous state to determine the expected increment or decrement of the
transformation strain tensor tr. This calculation is computational expensive and it can
ꞏ
lead to convergence issues. Since in many applications the transformation direction 
is known a priori (for instance, mechanical loading or unloading, or temperature
increment/decrement) a user input enables to set the transformation direction
manually to 1 or -1, thus speeding up the computational time.
For Lagoudas model, it is possible to choose from different transformation hardening
functions f()
• Quadratic
• Cosine
• Smooth
• User defined
The quadratic hardening function is defined as
2
1
--- b  +   1 +  2 
2 M
f = 
1
--- b  2 +   1 –  2 
2 A
650 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
ꞏ
for   0
ꞏ
for   0
where the parameters bM and bA are computed from
b M = s 0  M f – M s  and b A = s 0  A f – A s  ,
and the parameters 1 and 2 from
1
1
 1 = --- s 0  M s + A f  – u 0 and  2 = --- s 0  A s – A f – M f + M s 
2
4
The smooth hardening function is defined with four smoothing parameters n1, n2, n3,
and n4:

n +1
n +1

1 –   2 - for ꞏ  0
 1 - + ---------------------------1
-+
--------------
b


2 M
n1 + 1
n2 + 1 


f  = 
n +1
n +1
1

ꞏ
1 –   4 -
 3 - + --------------------------- --- b A   + -------------- for   0
n3 + 1
n4 + 1 
2


EQUIVALENT MATERIAL PROPERTIES FOR LAGOUDAS MODEL
In Lagoudas model, the phase transformation is described by six parameters: the
transition temperatures Mf, Ms, As, Af, and the two slopes of austenite and martensite
limit curves CA and CM.
When the experimental data consists of a uniaxial stress-strain curve taken at a constant
temperature T above the austenite finish temperature Af, it is possible to observe the
pseudoelastic or superelastic effect. In this case it is convenient to enter the transition
stress levels instead of the transition temperatures since these are easily derived from
the uniaxial curve.
Consider a NiTi alloy composed by 100% of austenite at room temperature T>Af.
Upon loading, the slope in the stress-strain curve would be the Young’s modulus of
austenite, EA. The martensite phase starts to develop when the axial stress reaches the
martensite start stress, Ms. If the alloy is further loaded, the slope reduces, entering
a region called loading plateau. Above the martensite finish stress, Mf, the
microstructure becomes 100% martensite. This process is commonly called the
forward transformation.
The reverse process has different transition stresses: When the 100% martensite alloy
is unloaded at constant temperature T>Af, the slope follows the martensite Young’s
modulus EM. When the axial stress reaches the austenite start stress, As, the austenite
volume fraction A starts to develop until the axial stress falls below the austenite
MATERIAL MODELS
|
651
finish stress, Af, at which level the alloy microstructure is 100% austenite. This process
is commonly called the reverse transformation. Figure 3-30 illustrates this process.
axial stress
100% martensite
loading plateau
Mf
Ms
EM
EA
As
Af
unloading plateau
100% austenite
axial strain
Figure 3-30: Uniaxial stress-strain curve at constant temperature, Lagoudas parameters.
The relations between the start and finish temperatures and stresses are
 Ms = C M  T  – M s  ,  Mf = C M  T  – M f 
 As = C A  T  – A s  ,  Af = C A  T  – A f 
here, T is the constant temperature at which the stress-strain curve for the
pseudoelastic effect was measured. This curve is observed when the temperature T is
higher than the austenite finish temperature Af.
The transition temperatures defined in terms of transition stresses read
 Ms
 Mf
M s = T  – --------- , M f = T  – -------CM
CM
 As
 Af
A s = T  – ------- , A f = T  – ------CA
CA
The two slopes of austenite and martensite limit curves CA and CM are sometimes
referred to as the Clausius-Clapeyron constants are measured in a strain-temperature
curve at constant stress (Ref. 41).
652 |
CHAPTER 3: STRUCTURAL MECHANICS THEORY
EQUIVALENT MATERIAL PROPERTIES FOR THE SOUZA–AURICCHIO
MODEL
Lagoudas model contains more parameters than the Souza–Auricchio model. The
latter model assumes that the slope of limit curves to martensite and austenite are
equal, this is, CM  CA. These two parameters influence the slopes of the loading and
unloading plateaus, respectively. For the Souza–Auricchio model, the slope of limit
curve  can be taken from the martensite limit curve CM, or as the average between
the austenite and martensite limit curves.
The function mT corresponds to the temperature-dependent martensite to austenite
equilibrium stress. It is defined from the slope of the limit curve  and the reference
temperature T*. At the current temperature T it equals
*
m  T  =   T – T 
The relations between the start and finish stresses and Souza–Auricchio parameters are
derived from the so-called limit function, F =  tr –  0 evaluated at a constant
temperature T
 Ms =  0 +  m  T   ,  Mf =  0 +  m  T   + H k  tr,max
 As = –  0 +  m  T   + H k  tr,max ,  Af = –  0 +  m  T  
The elastic radius 0 represents half of the height of the hysteresis loop, and it depends
on the temperature at which the superelastic effect was measured
 Mf –  As
 Ms –  Af
 0 = ----------------------- = ----------------------2
2
The hardening parameter Hk relates the slope in the loading plateau with the
difference between the martensite finish stress, Mf, and the martensite start stress,
Ms
 Mf =  Ms + H k  tr,max
here, tr,max is the maximum transformation strain measured in a strain-temperature
curve at constant stress (Ref. 40).
The Souza–Auricchio model assumes that the width of the transition zones in the
phase diagram are equal, that is, the temperature difference Af  As and Ms  Mf are
the same, which is not the case in the Lagoudas model. In the Souza–Auricchio model,
MATERIAL MODELS
|
653
the reference temperature T* is taken as the average temperature between the
martensite start temperature and the austenite finish temperature
Ms + A
*
T = -------------------f
2
Considering, CM  CA  , it is possible to write the reference temperature T* in terms
of the martensite start stress, the austenite finish stress, and the measurement
temperature T
m  T 
 Ms +  Af
*
- = T  – -----------------------T = T  – -----------------,

2
Figure 3-31 illustrates the material parameters for the Souza–Auricchio model.
axial stress
100% martensite
Mf
Ms
mT
As
Hk
0
EM
EA
Af
100% austenite
tr,max
axial strain
Figure 3-31: Uniaxial stress-strain curve at constant temperature, Souza–Auricchio
parameters.
DISSIPATION
Since phase transformation is an inelastic process, the dissipated energy density can be
calculated by integrating the pseudo-rate given by
ꞏ
ꞏ
W tr = : tr
For the Souza–Auricchio model the dissip">