Abaqus Analysis User`s Manual, vol2

Abaqus Analysis User`s Manual, vol2
Abaqus Analysis User’s Manual
Abaqus 6.12
Analysis User’s Manual
Volume II: Analysis
Abaqus Version 5.8 ID:
Printed on:
Abaqus Analysis
User’s Manual
Volume II
Abaqus Version 5.8 ID:
Printed on:
Legal Notices
CAUTION: This documentation is intended for qualified users who will exercise sound engineering judgment and expertise in the use of the Abaqus
Software. The Abaqus Software is inherently complex, and the examples and procedures in this documentation are not intended to be exhaustive or to apply
to any particular situation. Users are cautioned to satisfy themselves as to the accuracy and results of their analyses.
Dassault Systèmes and its subsidiaries, including Dassault Systèmes Simulia Corp., shall not be responsible for the accuracy or usefulness of any analysis
performed using the Abaqus Software or the procedures, examples, or explanations in this documentation. Dassault Systèmes and its subsidiaries shall not
be responsible for the consequences of any errors or omissions that may appear in this documentation.
The Abaqus Software is available only under license from Dassault Systèmes or its subsidiary and may be used or reproduced only in accordance with the
terms of such license. This documentation is subject to the terms and conditions of either the software license agreement signed by the parties, or, absent
such an agreement, the then current software license agreement to which the documentation relates.
This documentation and the software described in this documentation are subject to change without prior notice.
No part of this documentation may be reproduced or distributed in any form without prior written permission of Dassault Systèmes or its subsidiary.
The Abaqus Software is a product of Dassault Systèmes Simulia Corp., Providence, RI, USA.
© Dassault Systèmes, 2012
Abaqus, the 3DS logo, SIMULIA, CATIA, and Unified FEA are trademarks or registered trademarks of Dassault Systèmes or its subsidiaries in the United
States and/or other countries.
Other company, product, and service names may be trademarks or service marks of their respective owners. For additional information concerning
trademarks, copyrights, and licenses, see the Legal Notices in the Abaqus 6.12 Installation and Licensing Guide.
Abaqus Version 5.8 ID:
Printed on:
Locations
SIMULIA Worldwide Headquarters
SIMULIA European Headquarters
Rising Sun Mills, 166 Valley Street, Providence, RI 02909–2499, Tel: +1 401 276 4400,
Fax: +1 401 276 4408, [email protected], http://www.simulia.com
Stationsplein 8-K, 6221 BT Maastricht, The Netherlands, Tel: +31 43 7999 084,
Fax: +31 43 7999 306, [email protected]
Dassault Systèmes’ Centers of Simulation Excellence
United States
Australia
Austria
Benelux
Canada
China
Finland
France
Germany
India
Italy
Japan
Korea
Latin America
Scandinavia
United Kingdom
Fremont, CA, Tel: +1 510 794 5891, [email protected]
West Lafayette, IN, Tel: +1 765 497 1373, [email protected]
Northville, MI, Tel: +1 248 349 4669, [email protected]
Woodbury, MN, Tel: +1 612 424 9044, [email protected]
Mayfield Heights, OH, Tel: +1 216 378 1070, [email protected]
Mason, OH, Tel: +1 513 275 1430, [email protected]
Warwick, RI, Tel: +1 401 739 3637, [email protected]
Lewisville, TX, Tel: +1 972 221 6500, [email protected]
Richmond VIC, Tel: +61 3 9421 2900, [email protected]
Vienna, Tel: +43 1 22 707 200, [email protected]
Maarssen, The Netherlands, Tel: +31 346 585 710, [email protected]
Toronto, ON, Tel: +1 416 402 2219, [email protected]
Beijing, P. R. China, Tel: +8610 6536 2288, [email protected]
Shanghai, P. R. China, Tel: +8621 3856 8000, [email protected]
Espoo, Tel: +358 40 902 2973, [email protected]
Velizy Villacoublay Cedex, Tel: +33 1 61 62 72 72, [email protected]
Aachen, Tel: +49 241 474 01 0, [email protected]
Munich, Tel: +49 89 543 48 77 0, [email protected]
Chennai, Tamil Nadu, Tel: +91 44 43443000, [email protected]
Lainate MI, Tel: +39 02 3343061, [email protected]
Tokyo, Tel: +81 3 5442 6302, [email protected]
Osaka, Tel: +81 6 7730 2703, [email protected]
Mapo-Gu, Seoul, Tel: +82 2 785 6707/8, [email protected]
Puerto Madero, Buenos Aires, Tel: +54 11 4312 8700, [email protected]
Stockholm, Sweden, Tel: +46 8 68430450, [email protected]
Warrington, Tel: +44 1925 830900, [email protected]
Authorized Support Centers
Argentina
Brazil
Czech & Slovak Republics
Greece
Israel
Malaysia
Mexico
New Zealand
Poland
Russia, Belarus & Ukraine
Singapore
South Africa
Spain & Portugal
Abaqus Version 5.8 ID:
Printed on:
SMARTtech Sudamerica SRL, Buenos Aires, Tel: +54 11 4717 2717
KB Engineering, Buenos Aires, Tel: +54 11 4326 7542
Solaer Ingeniería, Buenos Aires, Tel: +54 221 489 1738
SMARTtech Mecânica, Sao Paulo-SP, Tel: +55 11 3168 3388
Synerma s. r. o., Psáry, Prague-West, Tel: +420 603 145 769, [email protected]
3 Dimensional Data Systems, Crete, Tel: +30 2821040012, [email protected]
ADCOM, Givataim, Tel: +972 3 7325311, [email protected]
WorleyParsons Services Sdn. Bhd., Kuala Lumpur, Tel: +603 2039 9000, [email protected]
Kimeca.NET SA de CV, Mexico, Tel: +52 55 2459 2635
Matrix Applied Computing Ltd., Auckland, Tel: +64 9 623 1223, [email protected]
BudSoft Sp. z o.o., Poznań, Tel: +48 61 8508 466, [email protected]m.pl
TESIS Ltd., Moscow, Tel: +7 495 612 44 22, [email protected]
WorleyParsons Pte Ltd., Singapore, Tel: +65 6735 8444, [email protected]
Finite Element Analysis Services (Pty) Ltd., Parklands, Tel: +27 21 556 6462, [email protected]
Principia Ingenieros Consultores, S.A., Madrid, Tel: +34 91 209 1482, [email protected]
Taiwan
Thailand
Turkey
Simutech Solution Corporation, Taipei, R.O.C., Tel: +886 2 2507 9550, [email protected]
WorleyParsons Pte Ltd., Singapore, Tel: +65 6735 8444, [email protected]
A-Ztech Ltd., Istanbul, Tel: +90 216 361 8850, [email protected]
Complete contact information is available at http://www.simulia.com/locations/locations.html.
Abaqus Version 5.8 ID:
Printed on:
Preface
This section lists various resources that are available for help with using Abaqus Unified FEA software.
Support
Both technical engineering support (for problems with creating a model or performing an analysis) and
systems support (for installation, licensing, and hardware-related problems) for Abaqus are offered through
a network of local support offices. Regional contact information is listed in the front of each Abaqus manual
and is accessible from the Locations page at www.simulia.com.
Support for SIMULIA products
SIMULIA provides a knowledge database of answers and solutions to questions that we have answered,
as well as guidelines on how to use Abaqus, SIMULIA Scenario Definition, Isight, and other SIMULIA
products. You can also submit new requests for support. All support incidents are tracked. If you contact
us by means outside the system to discuss an existing support problem and you know the incident or support
request number, please mention it so that we can query the database to see what the latest action has been.
Many questions about Abaqus can also be answered by visiting the Products page and the Support
page at www.simulia.com.
Anonymous ftp site
To facilitate data transfer with SIMULIA, an anonymous ftp account is available at ftp.simulia.com.
Login as user anonymous, and type your e-mail address as your password. Contact support before placing
files on the site.
Training
All offices and representatives offer regularly scheduled public training classes. The courses are offered in
a traditional classroom form and via the Web. We also provide training seminars at customer sites. All
training classes and seminars include workshops to provide as much practical experience with Abaqus as
possible. For a schedule and descriptions of available classes, see www.simulia.com or call your local office
or representative.
Feedback
We welcome any suggestions for improvements to Abaqus software, the support program, or documentation.
We will ensure that any enhancement requests you make are considered for future releases. If you wish to
make a suggestion about the service or products, refer to www.simulia.com. Complaints should be made by
contacting your local office or through www.simulia.com by visiting the Quality Assurance section of the
Support page.
Abaqus Version 5.8 ID:
Printed on:
CONTENTS
Contents
Volume I
PART I
1.
INTRODUCTION, SPATIAL MODELING, AND EXECUTION
Introduction
Introduction: general
1.1.1
Abaqus syntax and conventions
Input syntax rules
Conventions
1.2.1
1.2.2
Abaqus model definition
Defining a model in Abaqus
1.3.1
Parametric modeling
Parametric input
2.
1.4.1
Spatial Modeling
Node definition
Node definition
Parametric shape variation
Nodal thicknesses
Normal definitions at nodes
Transformed coordinate systems
Adjusting nodal coordinates
2.1.1
2.1.2
2.1.3
2.1.4
2.1.5
2.1.6
Element definition
Element definition
Element foundations
Defining reinforcement
Defining rebar as an element property
Orientations
2.2.1
2.2.2
2.2.3
2.2.4
2.2.5
Surface definition
Surfaces: overview
Element-based surface definition
Node-based surface definition
Analytical rigid surface definition
2.3.1
2.3.2
2.3.3
2.3.4
i
Abaqus ID:usb-toc
Printed on: Fri February 3 -- 18:01:12 2012
CONTENTS
Eulerian surface definition
Operating on surfaces
2.3.5
2.3.6
Rigid body definition
Rigid body definition
2.4.1
Integrated output section definition
Integrated output section definition
2.5.1
Mass adjustment
Adjust and/or redistribute mass of an element set
2.6.1
Nonstructural mass definition
Nonstructural mass definition
2.7.1
Distribution definition
Distribution definition
2.8.1
Display body definition
Display body definition
2.9.1
Assembly definition
Defining an assembly
2.10.1
Matrix definition
Defining matrices
3.
2.11.1
Job Execution
Execution procedures: overview
Execution procedure for Abaqus: overview
3.1.1
Execution procedures
Obtaining information
Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution
SIMULIA Co-Simulation Engine controller execution
Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD co-simulation execution
Abaqus/CAE execution
Abaqus/Viewer execution
Python execution
Parametric studies
Abaqus documentation
Licensing utilities
ASCII translation of results (.fil) files
Joining results (.fil) files
Querying the keyword/problem database
ii
Abaqus ID:usb-toc
Printed on: Fri February 3 -- 18:01:12 2012
3.2.1
3.2.2
3.2.3
3.2.4
3.2.5
3.2.6
3.2.7
3.2.8
3.2.9
3.2.10
3.2.11
3.2.12
3.2.13
CONTENTS
Fetching sample input files
Making user-defined executables and subroutines
Input file and output database upgrade utility
Generating output database reports
Joining output database (.odb) files from restarted analyses
Combining output from substructures
Combining data from multiple output databases
Network output database file connector
Mapping thermal and magnetic loads
Fixed format conversion utility
Translating Nastran bulk data files to Abaqus input files
Translating Abaqus files to Nastran bulk data files
Translating ANSYS input files to Abaqus input files
Translating PAM-CRASH input files to partial Abaqus input files
Translating RADIOSS input files to partial Abaqus input files
Translating Abaqus output database files to Nastran Output2 results files
Translating LS-DYNA data files to Abaqus input files
Exchanging Abaqus data with ZAERO
Encrypting and decrypting Abaqus input data
Job execution control
3.2.14
3.2.15
3.2.16
3.2.17
3.2.18
3.2.19
3.2.20
3.2.21
3.2.22
3.2.23
3.2.24
3.2.25
3.2.26
3.2.27
3.2.28
3.2.29
3.2.30
3.2.31
3.2.32
3.2.33
Environment file settings
Using the Abaqus environment settings
3.3.1
Managing memory and disk resources
Managing memory and disk use in Abaqus
3.4.1
Parallel execution
Parallel execution: overview
Parallel execution in Abaqus/Standard
Parallel execution in Abaqus/Explicit
Parallel execution in Abaqus/CFD
3.5.1
3.5.2
3.5.3
3.5.4
File extension definitions
File extensions used by Abaqus
3.6.1
FORTRAN unit numbers
FORTRAN unit numbers used by Abaqus
3.7.1
iii
Abaqus ID:usb-toc
Printed on: Fri February 3 -- 18:01:12 2012
CONTENTS
PART II
4.
OUTPUT
Output
Output
Output to the data and results files
Output to the output database
Error indicator output
4.1.1
4.1.2
4.1.3
4.1.4
Output variables
Abaqus/Standard output variable identifiers
Abaqus/Explicit output variable identifiers
Abaqus/CFD output variable identifiers
4.2.1
4.2.2
4.2.3
The postprocessing calculator
The postprocessing calculator
5.
4.3.1
File Output Format
Accessing the results file
Accessing the results file: overview
Results file output format
Accessing the results file information
Utility routines for accessing the results file
OI.1
Abaqus/Standard Output Variable Index
OI.2
Abaqus/Explicit Output Variable Index
OI.3
Abaqus/CFD Output Variable Index
5.1.1
5.1.2
5.1.3
5.1.4
iv
Abaqus ID:usb-toc
Printed on: Fri February 3 -- 18:01:12 2012
CONTENTS
Volume II
PART III
6.
ANALYSIS PROCEDURES, SOLUTION, AND CONTROL
Analysis Procedures
Introduction
Solving analysis problems: overview
Defining an analysis
General and linear perturbation procedures
Multiple load case analysis
Direct linear equation solver
Iterative linear equation solver
6.1.1
6.1.2
6.1.3
6.1.4
6.1.5
6.1.6
Static stress/displacement analysis
Static stress analysis procedures: overview
Static stress analysis
Eigenvalue buckling prediction
Unstable collapse and postbuckling analysis
Quasi-static analysis
Direct cyclic analysis
Low-cycle fatigue analysis using the direct cyclic approach
6.2.1
6.2.2
6.2.3
6.2.4
6.2.5
6.2.6
6.2.7
Dynamic stress/displacement analysis
Dynamic analysis procedures: overview
Implicit dynamic analysis using direct integration
Explicit dynamic analysis
Direct-solution steady-state dynamic analysis
Natural frequency extraction
Complex eigenvalue extraction
Transient modal dynamic analysis
Mode-based steady-state dynamic analysis
Subspace-based steady-state dynamic analysis
Response spectrum analysis
Random response analysis
6.3.1
6.3.2
6.3.3
6.3.4
6.3.5
6.3.6
6.3.7
6.3.8
6.3.9
6.3.10
6.3.11
Steady-state transport analysis
Steady-state transport analysis
6.4.1
Heat transfer and thermal-stress analysis
Heat transfer analysis procedures: overview
Uncoupled heat transfer analysis
6.5.1
6.5.2
v
Abaqus ID:usb-toc
Printed on: Fri February 3 -- 18:01:12 2012
CONTENTS
Fully coupled thermal-stress analysis
Adiabatic analysis
6.5.3
6.5.4
Fluid dynamic analysis
Fluid dynamic analysis procedures: overview
Incompressible fluid dynamic analysis
6.6.1
6.6.2
Electromagnetic analysis
Electromagnetic analysis procedures
Piezoelectric analysis
Coupled thermal-electrical analysis
Fully coupled thermal-electrical-structural analysis
Eddy current analysis
Magnetostatic analysis
6.7.1
6.7.2
6.7.3
6.7.4
6.7.5
6.7.6
Coupled pore fluid flow and stress analysis
Coupled pore fluid diffusion and stress analysis
Geostatic stress state
6.8.1
6.8.2
Mass diffusion analysis
Mass diffusion analysis
6.9.1
Acoustic and shock analysis
Acoustic, shock, and coupled acoustic-structural analysis
6.10.1
Abaqus/Aqua analysis
Abaqus/Aqua analysis
6.11.1
Annealing
Annealing procedure
7.
6.12.1
Analysis Solution and Control
Solving nonlinear problems
Solving nonlinear problems
7.1.1
Analysis convergence controls
Convergence and time integration criteria: overview
Commonly used control parameters
Convergence criteria for nonlinear problems
Time integration accuracy in transient problems
vi
Abaqus ID:usb-toc
Printed on: Fri February 3 -- 18:01:12 2012
7.2.1
7.2.2
7.2.3
7.2.4
CONTENTS
PART IV
8.
ANALYSIS TECHNIQUES
Analysis Techniques: Introduction
Analysis techniques: overview
9.
8.1.1
Analysis Continuation Techniques
Restarting an analysis
Restarting an analysis
9.1.1
Importing and transferring results
Transferring results between Abaqus analyses: overview
Transferring results between Abaqus/Explicit and Abaqus/Standard
Transferring results from one Abaqus/Standard analysis to another
Transferring results from one Abaqus/Explicit analysis to another
10.
9.2.1
9.2.2
9.2.3
9.2.4
Modeling Abstractions
Substructuring
Using substructures
Defining substructures
10.1.1
10.1.2
Submodeling
Submodeling: overview
Node-based submodeling
Surface-based submodeling
10.2.1
10.2.2
10.2.3
Generating global matrices
Generating matrices
10.3.1
Symmetric model generation, results transfer, and analysis of cyclic symmetry models
Symmetric model generation
Transferring results from a symmetric mesh or a partial three-dimensional mesh to
a full three-dimensional mesh
Analysis of models that exhibit cyclic symmetry
10.4.1
10.4.2
10.4.3
Periodic media analysis
Periodic media analysis
10.5.1
Meshed beam cross-sections
Meshed beam cross-sections
10.6.1
vii
Abaqus ID:usb-toc
Printed on: Fri February 3 -- 18:01:12 2012
CONTENTS
Modeling discontinuities as an enriched feature using the extended finite element method
Modeling discontinuities as an enriched feature using the extended finite element
method
11.
10.7.1
Special-Purpose Techniques
Inertia relief
Inertia relief
11.1.1
Mesh modification or replacement
Element and contact pair removal and reactivation
11.2.1
Geometric imperfections
Introducing a geometric imperfection into a model
11.3.1
Fracture mechanics
Fracture mechanics: overview
Contour integral evaluation
Crack propagation analysis
11.4.1
11.4.2
11.4.3
Surface-based fluid modeling
Surface-based fluid cavities: overview
Fluid cavity definition
Fluid exchange definition
Inflator definition
11.5.1
11.5.2
11.5.3
11.5.4
Mass scaling
Mass scaling
11.6.1
Selective subcycling
Selective subcycling
11.7.1
Steady-state detection
Steady-state detection
12.
11.8.1
Adaptivity Techniques
Adaptivity techniques: overview
Adaptivity techniques
12.1.1
ALE adaptive meshing
ALE adaptive meshing: overview
Defining ALE adaptive mesh domains in Abaqus/Explicit
ALE adaptive meshing and remapping in Abaqus/Explicit
Modeling techniques for Eulerian adaptive mesh domains in Abaqus/Explicit
viii
Abaqus ID:usb-toc
Printed on: Fri February 3 -- 18:01:12 2012
12.2.1
12.2.2
12.2.3
12.2.4
CONTENTS
Output and diagnostics for ALE adaptive meshing in Abaqus/Explicit
Defining ALE adaptive mesh domains in Abaqus/Standard
ALE adaptive meshing and remapping in Abaqus/Standard
12.2.5
12.2.6
12.2.7
Adaptive remeshing
Adaptive remeshing: overview
Selection of error indicators influencing adaptive remeshing
Solution-based mesh sizing
12.3.1
12.3.2
12.3.3
Analysis continuation after mesh replacement
Mesh-to-mesh solution mapping
13.
12.4.1
Optimization Techniques
Structural optimization: overview
Structural optimization: overview
13.1.1
Optimization models
Design responses
Objectives and constraints
Creating Abaqus optimization models
14.
13.2.1
13.2.2
13.2.3
Eulerian Analysis
Eulerian analysis
Defining Eulerian boundaries
Eulerian mesh motion
Defining adaptive mesh refinement in the Eulerian domain
15.
14.1.1
14.1.2
14.1.3
14.1.4
Particle Methods
Smoothed particle hydrodynamic analyses
Smoothed particle hydrodynamic analysis
Finite element conversion to SPH particles
16.
15.1.1
15.1.2
Sequentially Coupled Multiphysics Analyses
Predefined fields for sequential coupling
Sequentially coupled thermal-stress analysis
Predefined loads for sequential coupling
17.
16.1.1
16.1.2
16.1.3
Co-simulation
Co-simulation: overview
17.1.1
Preparing an Abaqus analysis for co-simulation
Preparing an Abaqus analysis for co-simulation
ix
Abaqus ID:usb-toc
Printed on: Fri February 3 -- 18:01:12 2012
17.2.1
CONTENTS
Co-simulation between Abaqus solvers
Abaqus/Standard to Abaqus/Explicit co-simulation
Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation
18.
17.3.1
17.3.2
Extending Abaqus Analysis Functionality
User subroutines and utilities
User subroutines: overview
Available user subroutines
Available utility routines
19.
18.1.1
18.1.2
18.1.3
Design Sensitivity Analysis
Design sensitivity analysis
20.
19.1.1
Parametric Studies
Scripting parametric studies
Scripting parametric studies
20.1.1
Parametric studies: commands
aStudy.combine(): Combine parameter samples for parametric studies.
aStudy.constrain(): Constrain parameter value combinations in parametric studies.
aStudy.define(): Define parameters for parametric studies.
aStudy.execute(): Execute the analysis of parametric study designs.
aStudy.gather(): Gather the results of a parametric study.
aStudy.generate(): Generate the analysis job data for a parametric study.
aStudy.output(): Specify the source of parametric study results.
aStudy=ParStudy(): Create a parametric study.
aStudy.report(): Report parametric study results.
aStudy.sample(): Sample parameters for parametric studies.
x
Abaqus ID:usb-toc
Printed on: Fri February 3 -- 18:01:12 2012
20.2.1
20.2.2
20.2.3
20.2.4
20.2.5
20.2.6
20.2.7
20.2.8
20.2.9
20.2.10
CONTENTS
Volume III
PART V
21.
MATERIALS
Materials: Introduction
Introduction
Material library: overview
Material data definition
Combining material behaviors
21.1.1
21.1.2
21.1.3
General properties
Density
22.
21.2.1
Elastic Mechanical Properties
Overview
Elastic behavior: overview
22.1.1
Linear elasticity
Linear elastic behavior
No compression or no tension
Plane stress orthotropic failure measures
22.2.1
22.2.2
22.2.3
Porous elasticity
Elastic behavior of porous materials
22.3.1
Hypoelasticity
Hypoelastic behavior
22.4.1
Hyperelasticity
Hyperelastic behavior of rubberlike materials
Hyperelastic behavior in elastomeric foams
Anisotropic hyperelastic behavior
22.5.1
22.5.2
22.5.3
Stress softening in elastomers
Mullins effect
Energy dissipation in elastomeric foams
22.6.1
22.6.2
Viscoelasticity
Time domain viscoelasticity
Frequency domain viscoelasticity
22.7.1
22.7.2
xi
Abaqus ID:usb-toc
Printed on: Fri February 3 -- 18:01:12 2012
CONTENTS
Nonlinear viscoelasticity
Hysteresis in elastomers
Parallel network viscoelastic model
22.8.1
22.8.2
Rate sensitive elastomeric foams
Low-density foams
23.
22.9.1
Inelastic Mechanical Properties
Overview
Inelastic behavior
23.1.1
Metal plasticity
Classical metal plasticity
Models for metals subjected to cyclic loading
Rate-dependent yield
Rate-dependent plasticity: creep and swelling
Annealing or melting
Anisotropic yield/creep
Johnson-Cook plasticity
Dynamic failure models
Porous metal plasticity
Cast iron plasticity
Two-layer viscoplasticity
ORNL – Oak Ridge National Laboratory constitutive model
Deformation plasticity
23.2.1
23.2.2
23.2.3
23.2.4
23.2.5
23.2.6
23.2.7
23.2.8
23.2.9
23.2.10
23.2.11
23.2.12
23.2.13
Other plasticity models
Extended Drucker-Prager models
Modified Drucker-Prager/Cap model
Mohr-Coulomb plasticity
Critical state (clay) plasticity model
Crushable foam plasticity models
23.3.1
23.3.2
23.3.3
23.3.4
23.3.5
Fabric materials
Fabric material behavior
23.4.1
Jointed materials
Jointed material model
23.5.1
Concrete
Concrete smeared cracking
Cracking model for concrete
Concrete damaged plasticity
23.6.1
23.6.2
23.6.3
xii
Abaqus ID:usb-toc
Printed on: Fri February 3 -- 18:01:12 2012
CONTENTS
Permanent set in rubberlike materials
Permanent set in rubberlike materials
24.
23.7.1
Progressive Damage and Failure
Progressive damage and failure: overview
Progressive damage and failure
24.1.1
Damage and failure for ductile metals
Damage and failure for ductile metals: overview
Damage initiation for ductile metals
Damage evolution and element removal for ductile metals
24.2.1
24.2.2
24.2.3
Damage and failure for fiber-reinforced composites
Damage and failure for fiber-reinforced composites: overview
Damage initiation for fiber-reinforced composites
Damage evolution and element removal for fiber-reinforced composites
24.3.1
24.3.2
24.3.3
Damage and failure for ductile materials in low-cycle fatigue analysis
Damage and failure for ductile materials in low-cycle fatigue analysis: overview
Damage initiation for ductile materials in low-cycle fatigue
Damage evolution for ductile materials in low-cycle fatigue
25.
24.4.1
24.4.2
24.4.3
Hydrodynamic Properties
Overview
Hydrodynamic behavior: overview
25.1.1
Equations of state
Equation of state
26.
25.2.1
Other Material Properties
Mechanical properties
Material damping
Thermal expansion
Field expansion
Viscosity
26.1.1
26.1.2
26.1.3
26.1.4
Heat transfer properties
Thermal properties: overview
Conductivity
Specific heat
Latent heat
26.2.1
26.2.2
26.2.3
26.2.4
xiii
Abaqus ID:usb-toc
Printed on: Fri February 3 -- 18:01:12 2012
CONTENTS
Acoustic properties
Acoustic medium
26.3.1
Mass diffusion properties
Diffusivity
Solubility
26.4.1
26.4.2
Electromagnetic properties
Electrical conductivity
Piezoelectric behavior
Magnetic permeability
26.5.1
26.5.2
26.5.3
Pore fluid flow properties
Pore fluid flow properties
Permeability
Porous bulk moduli
Sorption
Swelling gel
Moisture swelling
26.6.1
26.6.2
26.6.3
26.6.4
26.6.5
26.6.6
User materials
User-defined mechanical material behavior
User-defined thermal material behavior
26.7.1
26.7.2
xiv
Abaqus ID:usb-toc
Printed on: Fri February 3 -- 18:01:12 2012
CONTENTS
Volume IV
PART VI
27.
ELEMENTS
Elements: Introduction
Element library: overview
Choosing the element’s dimensionality
Choosing the appropriate element for an analysis type
Section controls
28.
27.1.1
27.1.2
27.1.3
27.1.4
Continuum Elements
General-purpose continuum elements
Solid (continuum) elements
One-dimensional solid (link) element library
Two-dimensional solid element library
Three-dimensional solid element library
Cylindrical solid element library
Axisymmetric solid element library
Axisymmetric solid elements with nonlinear, asymmetric deformation
28.1.1
28.1.2
28.1.3
28.1.4
28.1.5
28.1.6
28.1.7
Fluid continuum elements
Fluid (continuum) elements
Fluid element library
28.2.1
28.2.2
Infinite elements
Infinite elements
Infinite element library
28.3.1
28.3.2
Warping elements
Warping elements
Warping element library
28.4.1
28.4.2
Particle elements
Particle elements
Particle element library
29.
28.5.1
28.5.2
Structural Elements
Membrane elements
Membrane elements
General membrane element library
Cylindrical membrane element library
29.1.1
29.1.2
29.1.3
xv
Abaqus ID:usb-toc
Printed on: Fri February 3 -- 18:01:12 2012
CONTENTS
Axisymmetric membrane element library
29.1.4
Truss elements
Truss elements
Truss element library
29.2.1
29.2.2
Beam elements
Beam modeling: overview
Choosing a beam cross-section
Choosing a beam element
Beam element cross-section orientation
Beam section behavior
Using a beam section integrated during the analysis to define the section behavior
Using a general beam section to define the section behavior
Beam element library
Beam cross-section library
29.3.1
29.3.2
29.3.3
29.3.4
29.3.5
29.3.6
29.3.7
29.3.8
29.3.9
Frame elements
Frame elements
Frame section behavior
Frame element library
29.4.1
29.4.2
29.4.3
Elbow elements
Pipes and pipebends with deforming cross-sections: elbow elements
Elbow element library
29.5.1
29.5.2
Shell elements
Shell elements: overview
Choosing a shell element
Defining the initial geometry of conventional shell elements
Shell section behavior
Using a shell section integrated during the analysis to define the section behavior
Using a general shell section to define the section behavior
Three-dimensional conventional shell element library
Continuum shell element library
Axisymmetric shell element library
Axisymmetric shell elements with nonlinear, asymmetric deformation
xvi
Abaqus ID:usb-toc
Printed on: Fri February 3 -- 18:01:12 2012
29.6.1
29.6.2
29.6.3
29.6.4
29.6.5
29.6.6
29.6.7
29.6.8
29.6.9
29.6.10
CONTENTS
30.
Inertial, Rigid, and Capacitance Elements
Point mass elements
Point masses
Mass element library
30.1.1
30.1.2
Rotary inertia elements
Rotary inertia
Rotary inertia element library
30.2.1
30.2.2
Rigid elements
Rigid elements
Rigid element library
30.3.1
30.3.2
Capacitance elements
Point capacitance
Capacitance element library
31.
30.4.1
30.4.2
Connector Elements
Connector elements
Connectors: overview
Connector elements
Connector actuation
Connector element library
Connection-type library
31.1.1
31.1.2
31.1.3
31.1.4
31.1.5
Connector element behavior
Connector behavior
Connector elastic behavior
Connector damping behavior
Connector functions for coupled behavior
Connector friction behavior
Connector plastic behavior
Connector damage behavior
Connector stops and locks
Connector failure behavior
Connector uniaxial behavior
32.
31.2.1
31.2.2
31.2.3
31.2.4
31.2.5
31.2.6
31.2.7
31.2.8
31.2.9
31.2.10
Special-Purpose Elements
Spring elements
Springs
Spring element library
32.1.1
32.1.2
xvii
Abaqus ID:usb-toc
Printed on: Fri February 3 -- 18:01:12 2012
CONTENTS
Dashpot elements
Dashpots
Dashpot element library
32.2.1
32.2.2
Flexible joint elements
Flexible joint element
Flexible joint element library
32.3.1
32.3.2
Distributing coupling elements
Distributing coupling elements
Distributing coupling element library
32.4.1
32.4.2
Cohesive elements
Cohesive elements: overview
Choosing a cohesive element
Modeling with cohesive elements
Defining the cohesive element’s initial geometry
Defining the constitutive response of cohesive elements using a continuum approach
Defining the constitutive response of cohesive elements using a traction-separation
description
Defining the constitutive response of fluid within the cohesive element gap
Two-dimensional cohesive element library
Three-dimensional cohesive element library
Axisymmetric cohesive element library
32.5.1
32.5.2
32.5.3
32.5.4
32.5.5
32.5.6
32.5.7
32.5.8
32.5.9
32.5.10
Gasket elements
Gasket elements: overview
Choosing a gasket element
Including gasket elements in a model
Defining the gasket element’s initial geometry
Defining the gasket behavior using a material model
Defining the gasket behavior directly using a gasket behavior model
Two-dimensional gasket element library
Three-dimensional gasket element library
Axisymmetric gasket element library
32.6.1
32.6.2
32.6.3
32.6.4
32.6.5
32.6.6
32.6.7
32.6.8
32.6.9
Surface elements
Surface elements
General surface element library
Cylindrical surface element library
Axisymmetric surface element library
32.7.1
32.7.2
32.7.3
32.7.4
xviii
Abaqus ID:usb-toc
Printed on: Fri February 3 -- 18:01:12 2012
CONTENTS
Tube support elements
Tube support elements
Tube support element library
32.8.1
32.8.2
Line spring elements
Line spring elements for modeling part-through cracks in shells
Line spring element library
32.9.1
32.9.2
Elastic-plastic joints
Elastic-plastic joints
Elastic-plastic joint element library
32.10.1
32.10.2
Drag chain elements
Drag chains
Drag chain element library
32.11.1
32.11.2
Pipe-soil elements
Pipe-soil interaction elements
Pipe-soil interaction element library
32.12.1
32.12.2
Acoustic interface elements
Acoustic interface elements
Acoustic interface element library
32.13.1
32.13.2
Eulerian elements
Eulerian elements
Eulerian element library
32.14.1
32.14.2
User-defined elements
User-defined elements
User-defined element library
EI.1
Abaqus/Standard Element Index
EI.2
Abaqus/Explicit Element Index
EI.3
Abaqus/CFD Element Index
32.15.1
32.15.2
xix
Abaqus ID:usb-toc
Printed on: Fri February 3 -- 18:01:12 2012
CONTENTS
Volume V
PART VII
33.
PRESCRIBED CONDITIONS
Prescribed Conditions
Overview
Prescribed conditions: overview
Amplitude curves
33.1.1
33.1.2
Initial conditions
Initial conditions in Abaqus/Standard and Abaqus/Explicit
Initial conditions in Abaqus/CFD
33.2.1
33.2.2
Boundary conditions
Boundary conditions in Abaqus/Standard and Abaqus/Explicit
Boundary conditions in Abaqus/CFD
33.3.1
33.3.2
Loads
Applying loads: overview
Concentrated loads
Distributed loads
Thermal loads
Electromagnetic loads
Acoustic and shock loads
Pore fluid flow
33.4.1
33.4.2
33.4.3
33.4.4
33.4.5
33.4.6
33.4.7
Prescribed assembly loads
Prescribed assembly loads
33.5.1
Predefined fields
Predefined fields
33.6.1
PART VIII
34.
CONSTRAINTS
Constraints
Overview
Kinematic constraints: overview
34.1.1
Multi-point constraints
Linear constraint equations
34.2.1
xx
Abaqus ID:usb-toc
Printed on: Fri February 3 -- 18:01:12 2012
CONTENTS
General multi-point constraints
Kinematic coupling constraints
34.2.2
34.2.3
Surface-based constraints
Mesh tie constraints
Coupling constraints
Shell-to-solid coupling
Mesh-independent fasteners
34.3.1
34.3.2
34.3.3
34.3.4
Embedded elements
Embedded elements
34.4.1
Element end release
Element end release
34.5.1
Overconstraint checks
Overconstraint checks
34.6.1
PART IX
35.
INTERACTIONS
Defining Contact Interactions
Overview
Contact interaction analysis: overview
35.1.1
Defining general contact in Abaqus/Standard
Defining general contact interactions in Abaqus/Standard
Surface properties for general contact in Abaqus/Standard
Contact properties for general contact in Abaqus/Standard
Controlling initial contact status in Abaqus/Standard
Stabilization for general contact in Abaqus/Standard
Numerical controls for general contact in Abaqus/Standard
35.2.1
35.2.2
35.2.3
35.2.4
35.2.5
35.2.6
Defining contact pairs in Abaqus/Standard
Defining contact pairs in Abaqus/Standard
Assigning surface properties for contact pairs in Abaqus/Standard
Assigning contact properties for contact pairs in Abaqus/Standard
Modeling contact interference fits in Abaqus/Standard
Adjusting initial surface positions and specifying initial clearances in Abaqus/Standard
contact pairs
Adjusting contact controls in Abaqus/Standard
Defining tied contact in Abaqus/Standard
Extending master surfaces and slide lines
xxi
Abaqus ID:usb-toc
Printed on: Fri February 3 -- 18:01:12 2012
35.3.1
35.3.2
35.3.3
35.3.4
35.3.5
35.3.6
35.3.7
35.3.8
CONTENTS
Contact modeling if substructures are present
Contact modeling if asymmetric-axisymmetric elements are present
35.3.9
35.3.10
Defining general contact in Abaqus/Explicit
Defining general contact interactions in Abaqus/Explicit
Assigning surface properties for general contact in Abaqus/Explicit
Assigning contact properties for general contact in Abaqus/Explicit
Controlling initial contact status for general contact in Abaqus/Explicit
Contact controls for general contact in Abaqus/Explicit
35.4.1
35.4.2
35.4.3
35.4.4
35.4.5
Defining contact pairs in Abaqus/Explicit
Defining contact pairs in Abaqus/Explicit
Assigning surface properties for contact pairs in Abaqus/Explicit
Assigning contact properties for contact pairs in Abaqus/Explicit
Adjusting initial surface positions and specifying initial clearances for contact pairs
in Abaqus/Explicit
Contact controls for contact pairs in Abaqus/Explicit
36.
35.5.1
35.5.2
35.5.3
35.5.4
35.5.5
Contact Property Models
Mechanical contact properties
Mechanical contact properties: overview
Contact pressure-overclosure relationships
Contact damping
Contact blockage
Frictional behavior
User-defined interfacial constitutive behavior
Pressure penetration loading
Interaction of debonded surfaces
Breakable bonds
Surface-based cohesive behavior
36.1.1
36.1.2
36.1.3
36.1.4
36.1.5
36.1.6
36.1.7
36.1.8
36.1.9
36.1.10
Thermal contact properties
Thermal contact properties
36.2.1
Electrical contact properties
Electrical contact properties
36.3.1
Pore fluid contact properties
Pore fluid contact properties
37.
36.4.1
Contact Formulations and Numerical Methods
Contact formulations and numerical methods in Abaqus/Standard
Contact formulations in Abaqus/Standard
37.1.1
xxii
Abaqus ID:usb-toc
Printed on: Fri February 3 -- 18:01:12 2012
CONTENTS
Contact constraint enforcement methods in Abaqus/Standard
Smoothing contact surfaces in Abaqus/Standard
37.1.2
37.1.3
Contact formulations and numerical methods in Abaqus/Explicit
Contact formulation for general contact in Abaqus/Explicit
Contact formulations for contact pairs in Abaqus/Explicit
Contact constraint enforcement methods in Abaqus/Explicit
38.
37.2.1
37.2.2
37.2.3
Contact Difficulties and Diagnostics
Resolving contact difficulties in Abaqus/Standard
Contact diagnostics in an Abaqus/Standard analysis
Common difficulties associated with contact modeling in Abaqus/Standard
38.1.1
38.1.2
Resolving contact difficulties in Abaqus/Explicit
Contact diagnostics in an Abaqus/Explicit analysis
Common difficulties associated with contact modeling using contact pairs in
Abaqus/Explicit
39.
38.2.1
38.2.2
Contact Elements in Abaqus/Standard
Contact modeling with elements
Contact modeling with elements
39.1.1
Gap contact elements
Gap contact elements
Gap element library
39.2.1
39.2.2
Tube-to-tube contact elements
Tube-to-tube contact elements
Tube-to-tube contact element library
39.3.1
39.3.2
Slide line contact elements
Slide line contact elements
Axisymmetric slide line element library
39.4.1
39.4.2
Rigid surface contact elements
Rigid surface contact elements
Axisymmetric rigid surface contact element library
40.
39.5.1
39.5.2
Defining Cavity Radiation in Abaqus/Standard
Cavity radiation
40.1.1
xxiii
Abaqus ID:usb-toc
Printed on: Fri February 3 -- 18:01:12 2012
Abaqus Version 5.8 ID:
Printed on:
Part III: Analysis Procedures, Solution, and Control
•
•
Chapter 6, “Analysis Procedures”
Chapter 7, “Analysis Solution and Control”
Abaqus Version 5.8 ID:
Printed on:
ANALYSIS PROCEDURES
6.
Analysis Procedures
Introduction
6.1
Static stress/displacement analysis
6.2
Dynamic stress/displacement analysis
6.3
Steady-state transport analysis
6.4
Heat transfer and thermal-stress analysis
6.5
Fluid dynamic analysis
6.6
Electromagnetic analysis
6.7
Coupled pore fluid flow and stress analysis
6.8
Mass diffusion analysis
6.9
Acoustic and shock analysis
6.10
Abaqus/Aqua analysis
6.11
Annealing
6.12
Abaqus Version 5.8 ID:
Printed on:
INTRODUCTION
6.1
Introduction
•
•
•
•
•
•
“Solving analysis problems: overview,” Section 6.1.1
“Defining an analysis,” Section 6.1.2
“General and linear perturbation procedures,” Section 6.1.3
“Multiple load case analysis,” Section 6.1.4
“Direct linear equation solver,” Section 6.1.5
“Iterative linear equation solver,” Section 6.1.6
6.1–1
Abaqus Version 5.8 ID:
Printed on:
SOLVING ANALYSIS PROBLEMS
6.1.1
SOLVING ANALYSIS PROBLEMS: OVERVIEW
Overview
A large class of stress analysis problems can be solved with Abaqus/Standard and Abaqus/Explicit. A
fundamental division of such problems is into static or dynamic response; dynamic problems are those in
which inertia effects are significant. Abaqus/CFD solves a broad range of incompressible flow problems.
An analysis problem history is defined using steps in Abaqus (“Defining an analysis,” Section 6.1.2).
For each step you choose an analysis procedure, which defines the type of analysis to be performed during
the step. The available analysis procedures are listed below and described in more detail in the referenced
sections.
Abaqus provides multiphysics capabilities using built-in fully coupled procedures, sequential
coupling, and co-simulation as solution techniques for multiphysics simulation. An extensive selection
of additional analysis techniques that provide powerful tools for performing your Abaqus analyses more
efficiently and effectively is available; see Part IV, “Analysis Techniques.”
Abaqus/Standard analysis
Abaqus/Standard offers complete flexibility in making the distinction between static and dynamic
response; the same analysis can contain several static and dynamic phases. Thus, a static preload might
be applied, and then the linear or nonlinear dynamic response computed (as in the case of vibrations of
a component of a rotating machine or the response of a flexible offshore system that is initially moved
to an equilibrium position subject to buoyancy and steady current loads and then is excited by wave
loading). Similarly, the static solution can be sought after a dynamic event (by following a dynamic
analysis step with a step of static loading). See “Static stress/displacement analysis,” Section 6.2, and
“Dynamic stress/displacement analysis,” Section 6.3, for information on these types of procedures. In
addition to static and dynamic stress analysis, Abaqus/Standard offers the following analysis types:
•
•
•
•
•
•
•
“Steady-state transport analysis,” Section 6.4
“Heat transfer and thermal-stress analysis,” Section 6.5
“Electromagnetic analysis,” Section 6.7
“Coupled pore fluid flow and stress analysis,” Section 6.8
“Mass diffusion analysis,” Section 6.9
“Acoustic and shock analysis,” Section 6.10
“Abaqus/Aqua analysis,” Section 6.11
Abaqus/Explicit analysis
Abaqus/Explicit solves dynamic response problems using an explicit direct-integration procedure. See
“Dynamic stress/displacement analysis,” Section 6.3, for more information on the explicit dynamic
procedures available in Abaqus. Abaqus/Explicit also provides heat transfer, acoustic, and annealing
analysis capabilities: see “Heat transfer and thermal-stress analysis,” Section 6.5; “Acoustic and shock
analysis,” Section 6.10; and “Annealing,” Section 6.12, for details.
6.1.1–1
Abaqus Version 5.8 ID:
Printed on:
SOLVING ANALYSIS PROBLEMS
Abaqus/CFD analysis
Abaqus/CFD solves a broad range of incompressible flow problems using a second-order projection
method. See “Fluid dynamic analysis,” Section 6.6, for details on the incompressible flow procedures
available in Abaqus.
Multiphysics analyses
Multiphysics is a coupled approach in the numerical solution of multiple interacting physical domains.
Abaqus provides built-in fully coupled procedures, sequential coupling, and co-simulation as solution
techniques for multiphysics simulation.
Built-in fully coupled procedures
Native Abaqus multiphysics capabilities solve the physics by adding degrees of freedom representing
each of the physical fields and using a single solver. Abaqus provides the following built-in fully coupled
procedures to solve multidisciplinary simulations, where all physics fields are computed by Abaqus:
•
•
•
•
•
•
•
•
“Fully coupled thermal-stress analysis,” Section 6.5.3
“Coupled thermal-electrical analysis,” Section 6.7.3
“Fully coupled thermal-electrical-structural analysis,” Section 6.7.4
“Piezoelectric analysis,” Section 6.7.2 (electrical and mechanical coupling)
“Eddy current analysis,” Section 6.7.5 (electromagnetic)
“Coupled pore fluid diffusion and stress analysis,” Section 6.8.1
“Acoustic, shock, and coupled acoustic-structural analysis,” Section 6.10.1
“Eulerian analysis,” Section 14.1.1
Sequential coupling
A sequentially coupled multiphysics analysis can be used when the coupling between one or more of
the physical fields in a model is only important in one direction. A common example is a thermal-stress
analysis in which the temperature field does not depend strongly on the stress field. A typical sequentially
coupled thermal-stress analysis consists of two Abaqus/Standard runs: a heat transfer analysis and a
subsequent stress analysis.
You can perform sequentially coupled multiphysics analyses in Abaqus/Standard as described in
the following sections:
•
•
•
“Predefined fields for sequential coupling,” Section 16.1.1
“Sequentially coupled thermal-stress analysis,” Section 16.1.2
“Predefined loads for sequential coupling,” Section 16.1.3
6.1.1–2
Abaqus Version 5.8 ID:
Printed on:
SOLVING ANALYSIS PROBLEMS
Co-simulation
The co-simulation technique is a multiphysics capability for run-time coupling of Abaqus and another
analysis program. An Abaqus analysis can be coupled to another Abaqus analysis or to a third-party
analysis program to perform multidisciplinary simulations and multidomain (multimodel) coupling.
The co-simulation technique is described in the following sections:
•
•
•
•
“Co-simulation: overview,” Section 17.1.1
“Preparing an Abaqus analysis for co-simulation,” Section 17.2.1
“Abaqus/Standard to Abaqus/Explicit co-simulation,” Section 17.3.1
“Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation,” Section 17.3.2
6.1.1–3
Abaqus Version 5.8 ID:
Printed on:
DEFINING AN ANALYSIS
6.1.2
DEFINING AN ANALYSIS
Overview
An analysis is defined in Abaqus by:
•
•
•
dividing the problem history into steps;
specifying an analysis procedure for each step; and
prescribing loads, boundary conditions, and output requests for each step.
Abaqus distinguishes between general analysis steps and linear perturbation steps, and you can include
multiple steps in your analysis. You can control how prescribed conditions are applied throughout each
step. In addition, you can specify
•
•
•
the incrementation scheme used for controlling the solution,
the matrix storage and solution scheme in Abaqus/Standard, and
the precision level of the Abaqus/Explicit executable.
Defining an analysis
An analysis in Abaqus is defined using steps, analysis procedures, and optional history data.
Defining steps
A basic concept in Abaqus is the division of the problem history into steps. A step is any convenient
phase of the history—a thermal transient, a creep hold, a dynamic transient, etc. In its simplest form a
step can be just a static analysis in Abaqus/Standard of a load change from one magnitude to another.
You can provide a description of each step that will appear in the data (.dat) file; this description is for
convenience only.
The step definition includes the type of analysis to be performed and optional history data, such as
loads, boundary conditions, and output requests.
Input File Usage:
Use the first option to begin a step and the second option to end a step:
*STEP
*END STEP
The optional data lines on the *STEP option can be used to specify the step
description. The first data line given appears in the data (.dat) file.
Abaqus/CAE Usage:
Step module: Create Step: Description
Specifying the analysis procedure
For each step you choose an analysis procedure. This choice defines the type of analysis to be performed
during the step: static stress analysis, dynamic stress analysis, eigenvalue buckling, transient heat transfer
analysis, etc. The available analysis procedures are described in “Solving analysis problems: overview,”
Section 6.1.1. Only one procedure is allowed per step.
Input File Usage:
The procedure definition option must immediately follow the *STEP option.
6.1.2–1
Abaqus Version 5.8 ID:
Printed on:
DEFINING AN ANALYSIS
Abaqus/CAE Usage:
Step module: Create Step: choose the procedure type
Prescribing loads, boundary conditions, and output requests
The step definition includes optional history data, such as loads, boundary conditions, and output
requests, as defined in “History data” in “Defining a model in Abaqus,” Section 1.3.1. For more
information, see “Boundary conditions,” Section 33.3; “Loads,” Section 33.4; and “Output,” Section 4.1.
Details for prescribing these conditions are discussed in the individual procedure sections.
Input File Usage:
The optional history data are defined following the procedure definition within
a *STEP block.
Abaqus/CAE Usage:
You define history data (step-dependent objects) in the Interaction module,
Load module, and Step module.
General analysis steps versus linear perturbation steps
There are two kinds of steps in Abaqus: general analysis steps, which can be used to analyze linear or
nonlinear response, and linear perturbation steps, which can be used only to analyze linear problems.
General analysis steps can be included in an Abaqus/Standard or Abaqus/Explicit analysis; linear
perturbation analysis steps are available only in Abaqus/Standard. In Abaqus/Standard linear analysis is
always considered to be linear perturbation analysis about the state at the time when the linear analysis
procedure is introduced. This linear perturbation approach allows general application of linear analysis
techniques in cases where the linear response depends on preloading or on the nonlinear response
history of the model. See “General and linear perturbation procedures,” Section 6.1.3, for more details.
Multiple load case analysis
In general analysis steps Abaqus/Standard calculates the solution for a single set of applied loads. This
is also the default for linear perturbation steps. However, for static, direct steady-state dynamic, and
SIM-based steady-state dynamic linear perturbation steps it is possible to find solutions for multiple load
cases. See “Multiple load case analysis,” Section 6.1.4, for a description of this capability.
Multiple steps
The analysis procedure can be changed from step to step in any meaningful way, so you have great
flexibility in performing analyses. Since the state of the model (stresses, strains, temperatures, etc.) is
updated throughout all general analysis steps, the effects of previous history are always included in the
response in each new analysis step. Thus, for example, if natural frequency extraction is performed after
a geometrically nonlinear static analysis step, the preload stiffness will be included. Linear perturbation
steps have no effect on subsequent general analysis steps.
The most obvious reason for using several steps in an analysis is to change analysis procedure
type. However, several steps can also be used as a matter of convenience—for example, to change
output requests, contact pairs in Abaqus/Explicit, boundary conditions, or loading (any information
specified as history, or step-dependent, data). Sometimes an analysis may have progressed to a point
where the present step definition needs to be modified. Abaqus provides for this contingency with the
6.1.2–2
Abaqus Version 5.8 ID:
Printed on:
DEFINING AN ANALYSIS
restart capability, whereby a step can be terminated prematurely and a new step can be defined for the
problem continuation (see “Restarting an analysis,” Section 9.1.1).
Optional history data (see “Defining a model in Abaqus,” Section 1.3.1) prescribing the loading,
boundary conditions, output controls, and auxiliary controls will remain in effect for all subsequent
general analysis steps, including those that are defined in a restart analysis, until they are modified or reset.
Abaqus will compare all loads and boundary conditions specified in a step with the loads and boundary
conditions in effect during the previous step to ensure consistency and continuity. This comparison is
expensive if the number of individually specified loads and boundary conditions is very large. Hence,
the number of individually specified loads and boundary conditions should be minimized, which can
usually be done by using element and node sets instead of individual elements and nodes. For linear
perturbation steps only the output controls are continued from one linear perturbation step to the next if
there are no intermediate general analysis steps and the output controls are not redefined (see “Output,”
Section 4.1.1).
Within Abaqus/Standard or Abaqus/Explicit, any combination of available procedures can be used
from step to step. However, Abaqus/Standard and Abaqus/Explicit procedures cannot be used in the same
analysis. See “Transferring results between Abaqus analyses: overview,” Section 9.2.1, for information
on importing results from one type of analysis to another.
Defining time varying prescribed conditions
By default, Abaqus assumes that external parameters, such as load magnitudes and boundary conditions,
are constant (step function) or vary linearly (ramped) over a step, depending on the analysis procedure,
as shown in Table 6.1.2–1. Some exceptions in Abaqus/Standard are discussed below.
Table 6.1.2–1
Default amplitude variations for time domain procedures.
Procedure
Default amplitude variation
Coupled pore fluid diffusion/stress (steady-state)
Coupled pore fluid diffusion/stress (transient)
Coupled thermal-electrical (steady-state)
Ramp
Step
Ramp
Coupled thermal-electrical (transient)
Step
Direct-integration dynamic
Step (exception: Ramp if
quasi-static application type
is specified)
Fully coupled thermal-electrical-structural in
Abaqus/Standard (steady-state)
Ramp
Fully coupled thermal-electrical-structural in
Abaqus/Standard (transient)
Step
6.1.2–3
Abaqus Version 5.8 ID:
Printed on:
DEFINING AN ANALYSIS
Procedure
Default amplitude variation
Fully coupled thermal-stress in Abaqus/Standard
(steady-state)
Ramp
Fully coupled thermal-stress in Abaqus/Standard
(transient)
Step
Fully coupled thermal-stress in Abaqus/Explicit
Step
Incompressible flow
Step
Magnetostatic
Ramp
Mass diffusion (steady-state)
Ramp
Mass diffusion (transient)
Step
Quasi-static
Step
Static
Ramp
Steady-state transport
Ramp
Transient eddy current
Step
Transient modal dynamic
Step
Uncoupled heat transfer
Ramp
Uncoupled heat transfer (transient)
Step
No default amplitude variation is defined for a direct cyclic analysis step; for each applied load or
boundary condition, the amplitude must be defined explicitly.
Additional default amplitude variations in Abaqus/Standard
For displacement or rotation degrees of freedom prescribed in Abaqus/Standard using displacement-type
boundary conditions or displacement-type connector motions, the default amplitude variation is a ramp
function for all procedure types; the default amplitude is a step function for all procedure types when
using velocity-type boundary conditions or velocity-type connector motions.
For motions prescribed using a predefined displacement field, the default amplitude variation is a
ramp function for all procedure types; the default amplitude is a step function when using a predefined
velocity field for all procedures except steady-state transport.
The default amplitude variation is a step function for fluid flux loading in all procedure types.
When a displacement or rotation boundary condition is removed, the corresponding reaction force
or moment is reduced to zero according to the amplitude defined for the step. When film or radiation
loads are removed, the variation is always a step function.
6.1.2–4
Abaqus Version 5.8 ID:
Printed on:
DEFINING AN ANALYSIS
Prescribing nondefault amplitude variations
You can define complicated time variations of loadings, boundary conditions, and predefined fields
by referring to an amplitude curve in the prescribed condition definition (see “Amplitude curves,”
Section 33.1.2). User subroutines are also provided in Abaqus/Standard and Abaqus/Explicit for coding
general loadings (see “User subroutines: overview,” Section 18.1.1).
In Abaqus/Standard you can change the default amplitude variation for a step (except the removal
of film or radiation loads, as noted above).
Input File Usage:
Abaqus/CAE Usage:
In Abaqus/Standard use the following option to change the default amplitude
variation for a step:
*STEP, AMPLITUDE=STEP or RAMP
In Abaqus/Standard use the following input to change the default amplitude
variation for a step:
Step module: step editor: Other: Default load variation with time:
Instantaneous or Ramp linearly over step
Boundary conditions in Abaqus/Explicit
Boundary conditions applied during an explicit dynamic response step should use appropriate amplitude
references to define the time variation. If boundary conditions are specified for the step without amplitude
references, they are applied instantaneously at the beginning of the step. Since Abaqus/Explicit does not
admit jumps in displacement, the value of a nonzero displacement boundary condition that is specified
without an amplitude reference will be ignored, and a zero velocity boundary condition will be enforced.
Prescribing nondefault amplitude variations in transient procedures in Abaqus/Standard
The default amplitude is a step function for transient analysis procedures (fully coupled thermal-stress,
fully coupled thermal-electrical-structural, coupled thermal-electrical, direct-integration dynamic,
uncoupled heat transfer, and mass diffusion). Care should be exercised when the nondefault ramp
amplitude variation is specified for transient analysis procedures since unexpected results may occur.
For example, if a step of a transient heat transfer analysis uses the ramp amplitude variation and
temperature boundary conditions are removed in a subsequent step, the reaction fluxes generated in the
previous step will be ramped to zero from their initial values over the duration of the step. Therefore,
heat flux will continue to flow through the affected boundary nodes over the entire subsequent step even
though the temperature boundary conditions were removed.
Incrementation
Each step in an Abaqus analysis is divided into multiple increments. In most cases you have two choices
for controlling the solution: automatic time incrementation or user-specified fixed time incrementation.
Automatic incrementation is recommended for most cases. The methods for selecting automatic or direct
incrementation are discussed in the individual procedure sections.
6.1.2–5
Abaqus Version 5.8 ID:
Printed on:
DEFINING AN ANALYSIS
The issues associated with time incrementation in Abaqus/Standard, Abaqus/Explicit, and
Abaqus/CFD analyses are quite different. The time increments are generally much smaller in
Abaqus/Explicit than in Abaqus/Standard, while the time increments for Abaqus/CFD may be similar
to those in Abaqus/Standard in many situations.
Incrementation in Abaqus/Standard
In nonlinear problems Abaqus/Standard will increment and iterate as necessary to analyze a step,
depending on the severity of the nonlinearity. In transient cases with a physical time scale, you can
provide parameters to indicate a level of accuracy in the time integration, and Abaqus/Standard will
choose the time increments to achieve this accuracy. Direct user control is provided because it can
sometimes save computational cost in cases where you are familiar with the problem and know a
suitable incrementation scheme. Direct control can also occasionally be useful when automatic control
has trouble with convergence in nonlinear problems.
Specifying the maximum number of increments
You can define the upper limit to the number of increments in an Abaqus/Standard analysis. In a direct
cyclic analysis procedure, this upper limit should be set to the maximum number of increments in a
single loading cycle. The default is 100. The analysis will stop if this maximum is exceeded before the
complete solution for the step has been obtained. To arrive at a solution, it is often necessary to increase
the number of increments allowed by defining a new upper limit.
Input File Usage:
Abaqus/CAE Usage:
*STEP, INC=n
Step module: step editor: Incrementation: Maximum number
of increments
Extrapolation of the solution
In nonlinear analyses Abaqus/Standard uses extrapolation to speed up the solution. Extrapolation refers
to the method used to determine the first guess to the incremental solution. The guess is determined
by the size of the current time increment and by whether linear, displacement-based parabolic,
velocity-based parabolic, or no extrapolation of the previously attained history of each solution
variable is chosen. Displacement-based parabolic extrapolation is not relevant for Riks analyses, and
velocity-based parabolic extrapolation is available only for direct-integration dynamic procedures.
Linear extrapolation (the default for all procedures other than a direct-integration dynamic procedure
using the transient fidelity application setting) uses 100% extrapolation (1% for the Riks method) of the
previous incremental solution at the start of each increment to begin the nonlinear equation solution for
the next increment. No extrapolation is used in the first increment of a step.
In some cases extrapolation can cause Abaqus/Standard to iterate excessively; some common
examples are abrupt changes in the load magnitudes or boundary conditions and if unloading occurs as
a result of cracking (in concrete models) or buckling. In such cases you should suppress extrapolation.
Displacement-based parabolic extrapolation uses two previous incremental solutions to obtain the
first guess to the current incremental solution. This type of extrapolation is useful in situations when the
local variation of the solution with respect to the time scale of the problem is expected to be quadratic,
6.1.2–6
Abaqus Version 5.8 ID:
Printed on:
DEFINING AN ANALYSIS
such as the large rotation of structures. If parabolic extrapolation is used in a step, it begins after the
second increment of the step: the first increment employs no extrapolation, and the second increment
employs linear extrapolation. Consequently, slower convergence rates may occur during the first two
increments of the succeeding steps in a multistep analysis.
Velocity-based parabolic extrapolation uses the previous displacement incremental solution to
obtain the first guess to the current incremental solution. It is available only for direct-integration
dynamic procedures, and it is the default if the transient fidelity application setting is specified as part
of this procedure (see “Implicit dynamic analysis using direct integration,” Section 6.3.2). This type of
extrapolation is useful in situations with smooth solutions—i.e., when velocities do not display so called
“saw tooth” patterns—and in such cases it may provide a better first guess than other extrapolations. If
velocity-based parabolic extrapolation is used in a step, it begins after the first increment of the step; the
first increment employs initial velocities.
Input File Usage:
Use the following option to choose linear extrapolation:
*STEP, EXTRAPOLATION=LINEAR (default for all procedures
other than a direct-integration dynamic procedure using the
transient fidelity application setting)
Use the following option to choose displacement-based parabolic extrapolation:
*STEP, EXTRAPOLATION=PARABOLIC
Use the following option to choose velocity-based parabolic extrapolation:
*STEP, EXTRAPOLATION=VELOCITY PARABOLIC (default for a directintegration dynamic procedure using the transient fidelity application setting)
Use the following option to choose no extrapolation:
Abaqus/CAE Usage:
*STEP, EXTRAPOLATION= NO
Step module: step editor: Other: Extrapolation of previous state at
start of each increment: Linear, Parabolic, Velocity parabolic,
None, or Analysis product default
Incrementation in Abaqus/Explicit
The time increment used in an Abaqus/Explicit analysis must be smaller than the stability limit of
the central-difference operator (see “Explicit dynamic analysis,” Section 6.3.3); failure to use a small
enough time increment will result in an unstable solution. Although the time increments chosen by
Abaqus/Explicit generally satisfy the stability criterion, user control over the size of the time increment
is provided to reduce the chance of a solution going unstable. The small increments characteristic of an
explicit dynamic analysis product make Abaqus/Explicit well suited for nonlinear analysis.
Severe discontinuities in Abaqus/Standard
Abaqus/Standard distinguishes between regular, equilibrium iterations (in which the solution varies
smoothly) and severe discontinuity iterations (SDIs) in which abrupt changes in stiffness occur. The
most common of such severe discontinuities involve open-close changes in contact and stick-slip
6.1.2–7
Abaqus Version 5.8 ID:
Printed on:
DEFINING AN ANALYSIS
changes in friction. By default, Abaqus/Standard will continue to iterate until the severe discontinuities
are sufficiently small (or no severe discontinuities occur) and the equilibrium (flux) tolerances are
satisfied. Alternatively, you can choose a different approach in which Abaqus/Standard will continue to
iterate until no severe discontinuities occur.
For contact openings with the default approach, a force discontinuity is generated when the contact
force is set to zero, and this force discontinuity leads to force residuals that are checked against the
time average force in the usual way, as described in “Convergence criteria for nonlinear problems,”
Section 7.2.3. Similarly, in stick-to-slip transitions the frictional force is set to a lower value, which also
leads to force residuals.
For contact closures a severe discontinuity is considered sufficiently small if the penetration error is
smaller than the contact compatibility tolerance times the incremental displacement. The penetration
error is defined as the difference between the actual penetration and the penetration following from
the contact pressure and pressure-overclosure relation. In cases where the displacement increment is
essentially zero, a “zero penetration” check is used, similar to the check used for zero displacement
increments (see “Convergence criteria for nonlinear problems,” Section 7.2.3). The same checks are
used for slip-to-stick transitions in Lagrange friction.
To make sure that sufficient accuracy is obtained for contact between hard bodies, it is also required
that the estimated contact force error is smaller than the time average force times the contact force error
tolerance. The estimated contact force error is obtained by multiplying the penetration by an effective
stiffness. For hard contact this effective stiffness is equal to the stiffness of the underlying element,
whereas for softened/penalty contact the effective stiffness is obtained by adding the compliance of the
contact constraint and the underlying element.
Forcing the iteration process to continue until no severe discontinuities occur is the more
traditional, conservative method. However, this method can sometimes lead to convergence problems,
particularly in large problems with many contact points or situations where contact conditions are only
weakly determined. In such cases excessive iteration may occur and convergence may not be obtained
Input File Usage:
Abaqus/CAE Usage:
*STEP, CONVERT SDI=NO
Step module: step editor: Other: Convert severe discontinuity
iterations: Off
Matrix storage and solution scheme in Abaqus/Standard
Abaqus/Standard generally uses Newton’s method to solve nonlinear problems and the stiffness method
to solve linear problems. In both cases the stiffness matrix is needed. In some problems—for example,
with Coulomb friction—this matrix is not symmetric. Abaqus/Standard will automatically choose
whether a symmetric or unsymmetric matrix storage and solution scheme should be used based on the
model and step definition used. In some cases you can override this choice; the rules are explained
below.
Usually it is not necessary to specify the matrix storage and solution scheme. The choice is
available to improve computational efficiency in those cases where you judge that the default value is
not the best choice. In certain cases where the exact tangent stiffness matrix is not symmetric, the extra
iterations required by a symmetric approximation to the tangent matrix use less computer time than
6.1.2–8
Abaqus Version 5.8 ID:
Printed on:
DEFINING AN ANALYSIS
solving the nonsymmetric tangent matrix at each iteration. Therefore, for example, Abaqus/Standard
invokes the symmetric matrix storage and solution scheme automatically in problems with Coulomb
friction where every friction coefficient is less than or equal to 0.2, even though the resulting tangent
matrix will have some nonsymmetric terms. However, if any friction coefficient is greater than 0.2,
Abaqus/Standard will use the unsymmetric matrix storage and solution scheme automatically since it
may significantly improve the convergence history. This choice of the unsymmetric matrix storage and
solution scheme will consider changes to the friction model. Thus, if you modify the friction definition
during the analysis to introduce a friction coefficient greater than 0.2, Abaqus/Standard will activate
the unsymmetric matrix storage and solution scheme automatically. In cases in which the unsymmetric
matrix storage and solution scheme is selected automatically, you must explicitly turn it off if so desired;
it is recommended to do so if friction prevents any sliding motions.
Input File Usage:
Abaqus/CAE Usage:
*STEP, UNSYMM=YES or NO
Step module: step editor: Other: Storage: Use solver default
or Unsymmetric or Symmetric
Rules for using the unsymmetric matrix storage and solution scheme
The following rules apply to matrix storage and solution schemes in Abaqus/Standard:
1. Since Abaqus/Standard provides eigenvalue extraction only for symmetric matrices, steps with
eigenfrequency extraction or eigenvalue buckling prediction procedures always use the symmetric
matrix storage and solution scheme. You cannot change this setting. In such steps Abaqus/Standard
will symmetrize all contributions to the stiffness matrix.
2. In all steps except those with eigenfrequency extraction or eigenvalue buckling procedures,
Abaqus/Standard uses the unsymmetric matrix storage and solution scheme when any of the
following features are included in the model. You cannot change this setting.
a. Heat transfer convection/diffusion elements (element types DCCxxx)
b. General shell sections with unsymmetric section stiffness matrices (“Three-dimensional
conventional shell element library,” Section 29.6.7)
c. User-defined elements with unsymmetric element matrices (“User-defined elements,”
Section 32.15.1)
d. User-defined material models with unsymmetric material stiffness matrices (“User-defined
mechanical material behavior,” Section 26.7.1, or “User-defined thermal material behavior,”
Section 26.7.2)
e. User-defined surface interaction models with unsymmetric interface stiffness matrices (“Userdefined interfacial constitutive behavior,” Section 36.1.6)
3. The following features all trigger the unsymmetric matrix storage and solution scheme for the step.
You cannot change this setting.
a. Fully coupled thermal-stress analysis, except when a separated solution scheme is specified
for the step (“Fully coupled thermal-stress analysis,” Section 6.5.3)
6.1.2–9
Abaqus Version 5.8 ID:
Printed on:
DEFINING AN ANALYSIS
b. Coupled thermal-electrical analysis, except when a separated solution scheme is specified for
the step (“Coupled thermal-electrical analysis,” Section 6.7.3)
c. Fully coupled thermal-electrical-structural analysis (“Fully coupled thermal-electricalstructural analysis,” Section 6.7.4)
d. Coupled pore fluid diffusion/stress analysis with absorption or exsorption behavior (“Coupled
pore fluid diffusion and stress analysis,” Section 6.8.1)
e. Coupled pore fluid diffusion/stress analysis (steady-state)
f. Coupled pore fluid diffusion/stress analysis (transient with gravity loading)
g. Mass diffusion analysis (“Mass diffusion analysis,” Section 6.9.1)
h. Radiation viewfactor calculation controls (“Cavity radiation,” Section 40.1.1)
4. By default, the unsymmetric matrix storage and solution scheme is used for the complex eigenvalue
extraction procedure. You can change this setting.
5. In all other cases you can control whether a symmetric or a full matrix storage and arithmetic solution
is chosen. If you do not specify the matrix storage and solution scheme, Abaqus/Standard utilizes
the value used in the previous general analysis step.
6. If you do not specify the matrix storage and solution scheme in the first step of an analysis,
Abaqus/Standard will choose the unsymmetric scheme when any of the following are used:
a. Any Abaqus/Aqua load type
b. The concrete damaged plasticity material model
c. Friction with a friction coefficient greater than 0.2
The default value in the first step is the symmetric scheme for all other cases, except those
covered by rules 2 and 3 above and for cases in which a friction coefficient is increased above 0.2
after the first step.
7. For radiative heat transfer surface interactions (“Thermal contact properties,” Section 36.2.1),
certain follower forces (such as concentrated follower forces or moments), three-dimensional
finite-sliding analyses, any finite sliding in coupled pore fluid diffusion/stress analyses, and
certain material models (particularly nonassociated flow plasticity models and concrete) introduce
unsymmetric terms in the model’s stiffness matrix. However, Abaqus/Standard does not
automatically use the unsymmetric matrix storage and solution scheme when radiative heat
transfer surface interactions are used. Specifying that the unsymmetric scheme should be used can
sometimes improve convergence in such cases.
8. Coupled structural-acoustic and uncoupled acoustic analysis procedures in Abaqus/Standard
generally use symmetric matrix storage and solution. Exceptions are the subspace-based
steady-state dynamics or complex frequency procedures used for coupled structural-acoustic
problems, where unsymmetric matrices are a consequence of the coupling procedure used in
these cases. Using acoustic infinite elements or the acoustic flow velocity option triggers the
unsymmetric matrix storage and solution scheme in Abaqus/Standard, except for natural frequency
extraction using the Lanczos eigensolver, which uses symmetric matrix operations.
6.1.2–10
Abaqus Version 5.8 ID:
Printed on:
DEFINING AN ANALYSIS
Precision level of the Abaqus/Explicit executable
You can choose a double-precision executable (with 64-bit word lengths) for Abaqus/Explicit on
machines with a default, single-precision word length of 32 bits (see “Abaqus/Standard, Abaqus/Explicit,
and Abaqus/CFD execution,” Section 3.2.2). Most new computers have 32-bit default word lengths
even though they may have 64-bit memory addressing. The single-precision executable typically
results in a CPU savings of 20% to 30% compared to the double-precision executable, and single
precision provides accurate results in most cases. Exceptions in which single precision tends to be
inadequate include analyses that require greater than approximately 300,000 increments, have typical
nodal displacement increments less than 10−6 times the corresponding nodal coordinate values, include
hyperelastic materials, or involve multiple revolutions of deformable parts; the double-precision
executable is recommended in these cases (for example, see “Simulation of propeller rotation,”
Section 2.3.15 of the Abaqus Benchmarks Manual).
You can also run only a part of Abaqus/Explicit using double precision, while using single precision
for the rest (see “Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution,” Section 3.2.2). These
options are described below.
•
If double=explicit is used or the double option is specified without a value, the Abaqus/Explicit
analysis will run in double precision, while the packager will run in single precision. While this
choice would satisfy higher precision needs in most analyses, the data are written to the state (.abq)
file in single precision. Moreover, analysis-related computations performed in the packager will still
be executed in single precision. Thus, new steps, restart, and import analyses will commence from
data that are stored/computed in single precision despite the fact that calculations during the step
are performed in double precision. Thus, in general, one can expect somewhat noisy solutions at
the beginning of the first step, at step transitions, upon restart, and after import.
•
If double=both is used, both the Abaqus/Explicit packager and analysis will run in double
precision. This is the most expensive option but will ensure the highest overall execution precision.
Analysis database floating point data will be written to the state (.abq) file at the end of packager
or of a given step in double precision, thus ensuring in most cases the smoothest transition at step
boundaries, upon restart, and after an import.
•
There may be cases where the default single precision analysis is inadequate, while the
double=both option is too expensive. These are typically models that have complex links of
constraints (such as a complex mechanism with connector elements, complex combinations of
distributed/kinematic couplings, tie constraints and multi-point constraints, or interactions of such
constraints with boundary conditions). For such models it is desirable to solve only the constraints
in the model in double precision while the rest of the model is solved in single precision. This
combination gives the desired accuracy of the solution while increasing performance compared to
a full double precision analysis.
•
If double=constraint is used, the constraint packager and constraint solver are executed in
double precision, while the remainder of the Abaqus/Explicit packager and analysis are executed in
single precision.
6.1.2–11
Abaqus Version 5.8 ID:
Printed on:
DEFINING AN ANALYSIS
•
If double=off is used or the double option is omitted (default), both the Abaqus/Explicit packager
and the analysis will run in single precision. The double=off option is useful when you want to
override the setting in the environment file.
The significance of the precision level is indicated by comparing the solutions obtained with single
and double precision. If no significant difference is found between single- and double-precision solutions
for a particular model, the single-precision executable can be deemed adequate.
6.1.2–12
Abaqus Version 5.8 ID:
Printed on:
GENERAL AND LINEAR PERTURBATION PROCEDURES
6.1.3
GENERAL AND LINEAR PERTURBATION PROCEDURES
Products: Abaqus/Standard
Abaqus/Explicit
Abaqus/CAE
References
•
•
“Defining an analysis,” Section 6.1.2
“Linear and nonlinear procedures,” Section 14.3.2 of the Abaqus/CAE User’s Manual
Overview
An analysis step during which the response can be either linear or nonlinear is called a general analysis
step. An analysis step during which the response can be linear only is called a linear perturbation analysis
step. General analysis steps can be included in an Abaqus/Standard or Abaqus/Explicit analysis; linear
perturbation analysis steps are available only in Abaqus/Standard.
A clear distinction is made in Abaqus/Standard between general analysis and linear perturbation
analysis procedures. Loading conditions are defined differently for the two cases, time measures are
different, and the results should be interpreted differently. These distinctions are defined in this section.
Abaqus/Standard treats a linear perturbation analysis as a linear perturbation about a preloaded,
predeformed state. Abaqus/Foundation, a subset of Abaqus/Standard, is limited entirely to linear
perturbation analysis but does not allow preloading or predeformed states.
General analysis steps
A general analysis step is one in which the effects of any nonlinearities present in the model can be
included. The starting condition for each general step is the ending condition from the last general step,
with the state of the model evolving throughout the history of general analysis steps as it responds to the
history of loading. If the first step of the analysis is a general step, the initial conditions for the step can
be specified directly (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1).
Abaqus always considers total time to increase throughout a general analysis. Each step also has
its own step time, which begins at zero in each step. If the analysis procedure for the step has a physical
time scale, as in a dynamic analysis, step time must correspond to that physical time. Otherwise, step
time is any convenient time scale—for example, 0.0 to 1.0—for the step. The step times of all general
analysis steps accumulate into total time. Therefore, if an option such as creep (available only in
Abaqus/Standard) whose formulation depends on total time is used in a multistep analysis, any steps
that do not have a physical time scale should have a negligibly small step time compared to the steps
in which a physical time scale does exist.
Sources of nonlinearity
Nonlinear stress analysis problems can contain up to three sources of nonlinearity: material nonlinearity,
geometric nonlinearity, and boundary nonlinearity.
6.1.3–1
Abaqus Version 5.8 ID:
Printed on:
GENERAL AND LINEAR PERTURBATION PROCEDURES
Material nonlinearity
Abaqus offers models for a wide range of nonlinear material behaviors (see “Combining material
behaviors,” Section 21.1.3). Many of the materials are history dependent: the material’s response at
any time depends on what has happened to it at previous times. Thus, the solution must be obtained by
following the actual loading sequence. The general analysis procedures are designed with this in view.
Geometric nonlinearity
It is possible in Abaqus to define a problem as a “small-displacement” analysis, which means
that geometric nonlinearity is ignored in the element calculations—the kinematic relationships are
linearized. By default, large displacements and rotations are accounted for in contact constraints
even if the small-displacement element formulations are used for the analysis; i.e., a large-sliding
contact tracking algorithm is used (see “Contact formulations in Abaqus/Standard,” Section 37.1.1,
and “Contact formulations for contact pairs in Abaqus/Explicit,” Section 37.2.2). The elements in a
small-displacement analysis are formulated in the reference (original) configuration, using original
nodal coordinates. The errors in such an approximation are of the order of the strains and rotations
compared to unity. The approximation also eliminates any possibility of capturing bifurcation buckling,
which is sometimes a critical aspect of a structure’s response (see “Unstable collapse and postbuckling
analysis,” Section 6.2.4). You must consider these issues when interpreting the results of such an
analysis.
The alternative to a “small-displacement” analysis in Abaqus is to include large-displacement
effects. In this case most elements are formulated in the current configuration using current nodal
positions. Elements therefore distort from their original shapes as the deformation increases. With
sufficiently large deformations, the elements may become so distorted that they are no longer suitable
for use; for example, the volume of the element at an integration point may become negative. In this
situation Abaqus will issue a warning message indicating the problem. In addition, Abaqus/Standard will
cut back the time increment before making further attempts to continue the solution. Abaqus/Explicit
also offers element failure models to allow elements that reach high strains to be removed from a model;
see “Dynamic failure models,” Section 23.2.8, for details.
For each step of an analysis you specify whether a small- or large-displacement formulation
should be used (i.e., whether geometric nonlinearity should be ignored or included). By default,
Abaqus/Standard uses a small-displacement formulation and Abaqus/Explicit uses a large-displacement
formulation. The default value for the formulation in an import analysis is the same as the value at the
time of import. If a large-displacement formulation is used during any step of an analysis, it will be
used in all following steps in the analysis; there is no way to turn it off.
Almost all of the elements in Abaqus use a fully nonlinear formulation. The exceptions are the
cubic beam elements in Abaqus/Standard and the small-strain shell elements (those shell elements other
than S3/S3R, S4, S4R, and the axisymmetric shells) in which the cross-sectional thickness change is
ignored so that these elements are appropriate only for large rotations and small strains. Except for these
elements, the strains and rotations can be arbitrarily large.
The calculated stress is the “true” (Cauchy) stress. For beam, pipe, and shell elements the stress
components are given in local directions that rotate with the material. For all other elements the stress
6.1.3–2
Abaqus Version 5.8 ID:
Printed on:
GENERAL AND LINEAR PERTURBATION PROCEDURES
components are given in the global directions unless a local orientation (“Orientations,” Section 2.2.5) is
used at a point. For small-displacement analysis the infinitesimal strain measure is used, which is output
with the strain output variable E; strain output specified with output variables LE and NE is the same as
with E.
Input File Usage:
Use the following option to specify that a large-displacement formulation
should be used for the step:
*STEP, NLGEOM=YES (default in Abaqus/Explicit)
Use the following option to specify that a small-displacement formulation
should be used for the step:
*STEP, NLGEOM=NO (default in Abaqus/Standard)
Omitting the NLGEOM parameter is equivalent to using the default value.
Abaqus/CAE Usage:
Step module: Create Step: select any step type: Basic: Nlgeom: Off (for a
small-displacement formulation) or On (for a large-displacement formulation)
Boundary nonlinearity
Contact problems are a common source of nonlinearity in stress analysis—see “Contact interaction
analysis: overview,” Section 35.1.1. Other sources of boundary nonlinearity are nonlinear elastic
springs, films, radiation, multi-point constraints, etc.
Loading
In a general analysis step the loads must be defined as total values. The rules for applying loads in a
general, multistep analysis are defined in “Applying loads: overview,” Section 33.4.1.
Incrementation
The general analysis procedures in Abaqus offer two approaches for controlling incrementation.
Automatic control is one choice: you define the step and, in some procedures, specify certain tolerances
or error measures. Abaqus then automatically selects the increment size as it develops the response
in the step. Direct user control of increment size is the alternative approach, whereby you specify
the incrementation scheme. The direct approach is sometimes useful in repetitive analyses with
Abaqus/Standard, where you have a good “feel” for the convergence behavior of the problem. The
methods for selecting automatic or direct incrementation are discussed in the individual procedure
sections.
In nonlinear problems in Abaqus/Standard the challenge is always to obtain a convergent solution
in the least possible computational time. In these cases automatic control of the time increment is
usually more efficient because Abaqus/Standard can react to nonlinear response that you cannot predict
ahead of time. Automatic control is particularly valuable in cases where the response or load varies
widely through the step, as is often the case in diffusion-type problems such as creep, heat transfer, and
consolidation. Ultimately, automatic control allows nonlinear problems to be run with confidence in
Abaqus/Standard without extensive experience with the problem.
6.1.3–3
Abaqus Version 5.8 ID:
Printed on:
GENERAL AND LINEAR PERTURBATION PROCEDURES
Strong nonlinearities typically do not present difficulties in Abaqus/Explicit because of the small
time increments that are characteristic of an explicit dynamic analysis product.
Stabilization of unstable problems in Abaqus/Standard
Some static problems can be naturally unstable, for a variety of reasons.
Unconstrained rigid body motions
Instability may occur because unconstrained rigid body motions exist. Abaqus/Standard may be able
to handle this type of problem with automatic viscous damping (see “Adjusting contact controls in
Abaqus/Standard,” Section 35.3.6) when rigid body motions exist during the approach of two bodies
that will eventually come into contact.
Input File Usage:
Use one of the following options:
Abaqus/CAE Usage:
*CONTACT STABILIZATION
*CONTACT CONTROLS, STABILIZE
Automatic viscous damping is not supported in Abaqus/CAE.
Localized buckling behavior or material instability
Instability may also be caused by localized buckling behavior or by material instability; such instabilities
are especially significant when no time-dependent behavior exists in the material modeling. The
static, general analysis procedures in Abaqus/Standard can stabilize this type of problem if you request
it (see “Static stress analysis,” Section 6.2.2; “Quasi-static analysis,” Section 6.2.5; “Steady-state
transport analysis,” Section 6.4.1; “Fully coupled thermal-stress analysis,” Section 6.5.3; “Fully
coupled thermal-electrical-structural analysis,” Section 6.7.4; or “Coupled pore fluid diffusion and
stress analysis,” Section 6.8.1).
Input File Usage:
Abaqus/CAE Usage:
Use one of the following options:
*STATIC, STABILIZE
*VISCO, STABILIZE
*STEADY STATE TRANSPORT, STABILIZE
*COUPLED TEMPERATURE-DISPLACEMENT, STABILIZE
*COUPLED TEMPERATURE-DISPLACEMENT, ELECTRICAL, STABILIZE
*SOILS, CONSOLIDATION, STABILIZE
Step module: Create Step: General: any valid step type: Basic: Use
stabilization with dissipated energy fraction
Linear perturbation analysis steps
Linear perturbation analysis steps are available only in Abaqus/Standard (Abaqus/Foundation is
essentially the linear perturbation functionality in Abaqus/Standard). The response in a linear analysis
step is the linear perturbation response about the base state. The base state is the current state of the
model at the end of the last general analysis step prior to the linear perturbation step. If the first step
of an analysis is a perturbation step, the base state is determined from the initial conditions (“Initial
6.1.3–4
Abaqus Version 5.8 ID:
Printed on:
GENERAL AND LINEAR PERTURBATION PROCEDURES
conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1). In Abaqus/Foundation the base
state is always determined from the initial state of the model.
Linear perturbation analyses can be performed from time to time during a fully nonlinear analysis
by including the linear perturbation steps between the general response steps. The linear perturbation
response has no effect as the general analysis is continued. The step time of linear perturbation steps,
which is taken arbitrarily to be a very small number, is never accumulated into the total time. A simple
example of this method is the determination of the natural frequencies of a violin string under increasing
tension (see “Vibration of a cable under tension,” Section 1.4.3 of the Abaqus Benchmarks Manual). The
tension of the string is increased in several geometrically nonlinear analysis steps. After each of these
steps, the frequencies can be extracted in a linear perturbation analysis step.
If geometric nonlinearity is included in the general analysis upon which a linear perturbation study
is based, stress stiffening or softening effects and load stiffness effects (from pressure and other follower
forces) are included in the linear perturbation analysis.
Load stiffness contributions are also generated for centrifugal and Coriolis loading. In direct steadystate dynamic analysis Coriolis loading generates an imaginary antisymmetric matrix. This contribution
is accounted for currently in solid and truss elements only and is activated by using the unsymmetric
matrix storage and solution scheme in the step.
Linear perturbation procedures
The following purely linear perturbation procedures are available in Abaqus/Standard:
•
•
•
•
•
•
•
•
•
•
“Eigenvalue buckling prediction,” Section 6.2.3
“Direct-solution steady-state dynamic analysis,” Section 6.3.4
“Natural frequency extraction,” Section 6.3.5
“Complex eigenvalue extraction,” Section 6.3.6
“Transient modal dynamic analysis,” Section 6.3.7
“Mode-based steady-state dynamic analysis,” Section 6.3.8
“Subspace-based steady-state dynamic analysis,” Section 6.3.9
“Response spectrum analysis,” Section 6.3.10
“Random response analysis,” Section 6.3.11
“Time-harmonic analysis” in “Eddy current analysis,” Section 6.7.5
In addition, the following analysis techniques are treated as linear perturbation steps in an analysis:
•
•
“Defining substructures,” Section 10.1.2
“Generating matrices,” Section 10.3.1
Except for these procedures and the static procedure (explained below), all other procedures can be
used only in general analysis steps (in other words, they are not available with Abaqus/Foundation). All
linear perturbation procedures except for the complex eigenvalue extraction procedure are available with
Abaqus/Foundation.
6.1.3–5
Abaqus Version 5.8 ID:
Printed on:
GENERAL AND LINEAR PERTURBATION PROCEDURES
Linear static perturbation analysis
A linear static stress analysis (“Static stress analysis,” Section 6.2.2) can be conducted in
Abaqus/Standard.
Input File Usage:
Use both of the following options to conduct a linear static perturbation
analysis:
*STEP, PERTURBATION
*STATIC
Omitting the PERTURBATION parameter on the *STEP option implies that a
general static analysis is required.
Abaqus/CAE Usage:
Step module: Create Step: Linear perturbation: Static,
Linear perturbation
Loading
Load magnitudes (including the magnitudes of prescribed boundary conditions) during a linear
perturbation analysis step are defined as the magnitudes of the load perturbations only. Likewise, the
value of any solution variable is output as the perturbation value only—the value of the variable in the
base state is not included.
Multiple load case analysis
Multiple load cases can be analyzed simultaneously for static, direct-solution steady-state dynamic and
SIM-based steady-state dynamic (including subspace projection) linear perturbation steps. See “Multiple
load case analysis,” Section 6.1.4, for a description of this capability.
Restrictions
A linear perturbation analysis is subject to the following restrictions:
•
Since a linear perturbation analysis has no time period, amplitude references (“Amplitude curves,”
Section 33.1.2) can be used meaningfully only to specify loads or boundary conditions as functions
of frequency (in a steady-state dynamics analysis) or to define base motion (in mode-based dynamics
procedures). If loads or boundary conditions are specified as functions of time, the amplitude value
corresponding to time=0 will be used.
•
A general implicit dynamic analysis (“Implicit dynamic analysis using direct integration,”
Section 6.3.2) cannot be interrupted to perform perturbation analyses: before performing
the perturbation analysis, Abaqus/Standard requires that the structure be brought into static
equilibrium.
•
During a linear perturbation analysis step, the model’s response is defined by its linear elastic
(or viscoelastic) stiffness at the base state. Plasticity and other inelastic effects are ignored. For
hyperelasticity (“Hyperelastic behavior of rubberlike materials,” Section 22.5.1) or hypoelasticity
(“Hypoelastic behavior,” Section 22.4.1), the tangent elastic moduli in the base state are used.
6.1.3–6
Abaqus Version 5.8 ID:
Printed on:
GENERAL AND LINEAR PERTURBATION PROCEDURES
If cracking has occurred—for example, in the concrete model (“Concrete smeared cracking,”
Section 23.6.1)—the damaged elastic (secant) moduli are used.
•
Contact conditions cannot change during a linear perturbation analysis. The open/closed status of
each contact constraint remains as it is in the base state. All points in contact (i.e., with a “closed”
status) are assumed to be sticking if friction is present, except the contact nodes for which a velocity
differential is imposed by the motion of the reference frame or the transport velocity. At those nodes,
slipping conditions are assumed regardless of the friction coefficient.
•
The effects of temperature and field variable perturbations are ignored for materials that are
dependent on temperature and field variables. However, temperature perturbations will produce
perturbations of thermal strain.
6.1.3–7
Abaqus Version 5.8 ID:
Printed on:
MULTIPLE LOAD CASES
6.1.4
MULTIPLE LOAD CASE ANALYSIS
Products: Abaqus/Standard
Abaqus/CAE
References
•
•
•
*LOAD CASE
*END LOAD CASE
Chapter 34, “Load cases,” of the Abaqus/CAE User’s Manual
Overview
A multiple load case analysis:
•
•
•
•
•
is used to study the linear responses of a structure subjected to distinct sets of loads and boundary
conditions defined within a step (each set is referred to as a load case);
can be much more efficient than an equivalent multiple perturbation step analysis;
allows for the changing of mechanical loads and boundary conditions from load case to load case;
includes the effects of the base state; and
can be performed with static perturbation, direct-solution steady-state dynamic and SIM-based
steady-state dynamic analyses.
Load cases
A load case refers to a set of loads, boundary conditions, and base motions comprising a particular
loading condition. For example, in a simplified model the operational environment of an airplane might
be broken into five load cases: (1) take-off, (2) climb, (3) cruise, (4) descent, and (5) landing. Often a
load case is defined in terms of unit loads or prescribed boundary conditions, and a multiple load case
analysis refers to the simultaneous solution for the responses of each load case in a set of such load
cases. These responses can then be scaled and linearly combined during postprocessing to represent the
actual loading environment. Other postprocessing manipulations on load cases are also common, such
as finding the maximum Mises stress among all load cases. These types of load case manipulations can
be requested in the Visualization module of Abaqus/CAE (see the Abaqus/CAE User’s Manual).
Using multiple load cases
A multiple load case analysis is conceptually equivalent to a multiple step analysis in which the load
case definitions are mapped to consecutive perturbation steps. However, a multiple load case analysis is
generally much more efficient than the equivalent multiple step analysis. The exception occurs when a
large number of boundary conditions exist that are not common to all load cases (i.e., degrees of freedom
are constrained in one load case but not others). It is difficult to define what “large” is since it is model
dependent. The relative performance of the two analysis methods can be assessed by performing a data
6.1.4–1
Abaqus Version 5.8 ID:
Printed on:
MULTIPLE LOAD CASES
check analysis for both the multiple load case analysis and the equivalent multiple step analysis. The
data check analysis writes resource information for each step to the data file, including the maximum
wavefront, number of floating point operations, and minimum memory required. If these numbers are
noticeably larger for the multiple load case step compared to those across all steps of the equivalent
multiple step analysis (the number of floating point operations should be summed over all steps before
comparing), the multiple step analysis will be more efficient.
Although generally more efficient, the multiple load case analysis may consume more memory and
disk space than an equivalent multiple step analysis. Thus, for large problems or problems with many
load cases it is again advisable, as described above, to compare resource usage between the multiple load
case analysis and the equivalent multiple step analysis. If resource requirements for the multiple load
case analysis are deemed too large, consider dividing the load cases among a few steps. The resulting
analysis (a hybrid of multiple load cases and multiple steps) will require fewer resources while retaining
an efficiency advantage over an equivalent pure multiple step analysis.
Defining load cases
You define a load case within a static perturbation, direct-solution steady-state dynamic, and SIM-based
steady-state dynamic analyses. Load case definitions do not propagate to subsequent steps. Only the
following types of prescribed conditions can be specified within a load case definition:
•
•
•
•
•
•
Boundary conditions
Concentrated loads
Distributed loads
Distributed surface loads
Inertia-based loads
Base motions
Additional rules governing these prescribed conditions are described in the sections that follow. No other
types of prescribed conditions can appear in a step that contains load case definitions. All other valid
analysis components, such as output requests, must be specified outside load case definitions.
Each load case definition is assigned a name for postprocessing purposes.
Input File Usage:
Use the first option to begin a load case and the second option to end a load
case:
*LOAD CASE, NAME=name
*END LOAD CASE
Prescribed conditions specified within a load case definition apply only
to that load case. In static perturbation and direct-solution steady-state
dynamic analyses, prescribed conditions can be specified outside the load case
definitions (in this case they apply to all load cases in the step).
Abaqus/CAE Usage:
Load module: Create Load Case: Name: name
In Abaqus/CAE if a step contains load cases, all prescribed conditions in the
step must be included in one or more load cases.
6.1.4–2
Abaqus Version 5.8 ID:
Printed on:
MULTIPLE LOAD CASES
Procedures
Load cases can be defined only in perturbation steps with the following procedures:
•
•
•
Static
Direct-solution, steady-state dynamic
SIM-based, steady-state dynamic
As with other perturbation steps, a multiple load case analysis will include the nonlinear effects of the
previous general step (base state). The following analysis techniques are not supported in the context of
a load case step:
•
•
•
•
•
•
Restart from a particular load case
Submodeling using results from other than the first load case in the global analysis
Importing and transferring results
Cyclic symmetry analysis
Contour integrals
Design sensitivity analysis
Boundary conditions
Boundary conditions can be specified both outside and inside load case definitions in the same step.
Specifying a boundary condition outside the load case definitions in a step is equivalent to including it
in all load case definitions in the step (i.e., the boundary condition will be applied to all load cases).
Unless any boundary conditions are removed in the perturbation step, the boundary conditions that
are active in the base state will propagate to all load cases in the perturbation step. If any boundary
condition is removed in a step with load cases (either outside or inside load case definitions), the base
state boundary conditions will not be propagated to any load case in the step. See “Boundary conditions
in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1, for more information.
Note: In Abaqus/CAE if a step contains load cases, all boundary conditions in the step must be included
in one or more load cases. Boundary conditions can only be used with load cases in static perturbation
and direct-solution steady-state dynamic analyses.
Loads
In static perturbation and direct-solution steady-state dynamic analyses concentrated, distributed, and
distributed surface loads can be specified both outside and inside load case definitions in the same step.
Inertia relief loads can be specified either outside load case definitions or inside load case definitions
in the same step but not both simultaneously. Specifying one of these load types outside the load case
definitions in a step is equivalent to including it in all load case definitions in the step (i.e., the loading
will be applied to all load cases).
6.1.4–3
Abaqus Version 5.8 ID:
Printed on:
MULTIPLE LOAD CASES
In SIM-based steady-state dynamic analyses concentrated, distributed, distributed surface loads,
and base motion can be specified only inside load case definitions in the same step. Inertia relief loads
are not supported.
Load cases cannot be used in models that include aqua loads (see “Abaqus/Aqua analysis,”
Section 6.11.1).
As with any perturbation step, perturbation loads must be defined completely within the perturbation
step (see “Applying loads: overview,” Section 33.4.1).
Note: In Abaqus/CAE if a step contains load cases, all loads in the step must be included in one or more
load cases.
Predefined fields
Field variables cannot be specified in a step with load cases.
Elements
Load cases cannot be used in models that include piezoelectric elements (see “Piezoelectric analysis,”
Section 6.7.2).
Output
In a step containing one or more load cases, field and history output requests to the output database and
output requests to the data file are supported. Output requests to the results file are not supported. Output
requests can be specified only outside load case definitions, and they apply to all load cases in a step.
The step propagation rules for output requests are the same as for other perturbation steps (see “Output,”
Section 4.1.1).
Most of the field and history output variables normally available within a particular procedure are
also available during a multiple load case analysis (see “Abaqus/Standard output variable identifiers,”
Section 4.2.1). Additional restrictions apply for a SIM-based steady-state dynamic analysis; see “Using
the SIM architecture for modal superposition dynamic analyses” in “Dynamic analysis procedures:
overview,” Section 6.3.1, for more information.
The field output corresponding to each load case is stored in a separate frame on the output database
with the load case name included as a frame attribute. To distinguish between load cases for history
output variables, the name of the load case is appended to the history variable name. The Visualization
module of Abaqus/CAE and the Abaqus Scripting Interface (see Chapter 9, “Using the Abaqus Scripting
Interface to access an output database,” of the Abaqus Scripting User’s Manual) can be used to access
and manipulate load case output. Abaqus/Standard does not perform consistency checks on the physical
validity of the load case manipulations. For example, the linear superposition of two load cases, each
with different boundary conditions, is allowed even though the combined results may not be physically
meaningful.
Input file template
*HEADING
…
6.1.4–4
Abaqus Version 5.8 ID:
Printed on:
MULTIPLE LOAD CASES
*STEP, PERTURBATION
*STATIC or *STEADY STATE DYNAMICS, DIRECT
…
*OUTPUT, FIELD
…
*BOUNDARY
Data lines to specify boundary conditions for all load cases.
*DLOAD
Data lines to specify distributed loads for all load cases.
*CLOAD
Data lines to specify point loads for all load cases.
*DSLOAD
Data lines to specify distributed surface loads for all load cases.
*INERTIA RELIEF
Data lines to specify inertia relief loading directions.
(This option cannot be used inside load cases if it is used here.)
…
*LOAD CASE, NAME=name1
*BOUNDARY
Data lines to specify boundary conditions for first load case.
*DLOAD
Data lines to specify distributed loads for first load case.
*CLOAD
Data lines to specify point loads for first load case.
*DSLOAD
Data lines to specify distributed surface loads for first load case.
*INERTIA RELIEF
Data lines to specify inertia relief loading directions.
(This option cannot be used outside load cases if it is used here.)
*END LOAD CASE
*LOAD CASE, NAME=name2
Load and boundary condition options for second load case
*END LOAD CASE
…
Subsequent load case definitions
…
*END STEP
*STEP, PERTURBATION
*FREQUENCY, SIM or *FREQUENCY, EIGENSOLVER=AMS
*END STEP
…
*STEP, PERTURBATION
6.1.4–5
Abaqus Version 5.8 ID:
Printed on:
MULTIPLE LOAD CASES
*STEADY STATE DYNAMICS
*LOAD CASE, NAME=name3
*BASE MOTION
Data lines to specify base motion for first load case.
*DLOAD
Data lines to specify distributed loads for first load case.
*CLOAD
Data lines to specify point loads for first load case.
*DSLOAD
Data lines to specify distributed surface loads for first load case.
*END LOAD CASE
*LOAD CASE, NAME=name4
Load and base motion options for second load case.
*END LOAD CASE
…
Subsequent load case definitions
…
*OUTPUT, HISTORY
…
*END STEP
6.1.4–6
Abaqus Version 5.8 ID:
Printed on:
DIRECT LINEAR EQUATION SOLVER
6.1.5
DIRECT LINEAR EQUATION SOLVER
Products: Abaqus/Standard
Abaqus/CAE
References
•
•
•
•
•
“Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution,” Section 3.2.2
“Using the Abaqus environment settings,” Section 3.3.1
“Iterative linear equation solver,” Section 6.1.6
“Parallel execution in Abaqus/Standard,” Section 3.5.2
“Configuring analysis procedure settings,” Section 14.11 of the Abaqus/CAE User’s Manual, in the
online HTML version of this manual
Overview
Linear equation solution is used in linear and nonlinear analysis. In nonlinear analysis Abaqus/Standard
uses the Newton method or a variant of it, such as the Riks method, within which it is necessary
to solve a set of linear equations at each iteration. The direct linear equation solver finds the exact
solution to this system of linear equations (up to machine precision). The direct linear equation solver
in Abaqus/Standard:
•
•
uses a sparse, direct, Gauss elimination method; and
often represents the most time consuming part of the analysis (especially for large models)—the
storage of the equations occupies the largest part of the disk space during the calculations.
The sparse solver
The direct sparse solver uses a “multifront” technique that can reduce the computational time to solve the
equations dramatically if the equation system has a sparse structure. Such a matrix structure typically
arises when the physical model is made from several parts or branches that are connected together; a
spoked wheel is a good example of a structure that has a sparse stiffness matrix. Space frames and other
structures modeled with beams, trusses, and shells often have sparse stiffness matrices. In contrast,
a blocky structure—such as a single, solid, three-dimensional block (see “Elastic-plastic line spring
modeling of a finite length cylinder with a part-through axial flaw,” Section 1.4.3 of the Abaqus Example
Problems Manual)—provides little opportunity for the sparse solver to reduce the computer time. For
large blocky structures, the iterative linear equation solver may be more efficient (see “Iterative linear
equation solver,” Section 6.1.6).
Input File Usage:
Use the following option to use the default direct sparse solver:
Abaqus/CAE Usage:
*STEP
Step module: step editor: Other: Method: Direct
6.1.5–1
Abaqus Version 5.8 ID:
Printed on:
DIRECT LINEAR EQUATION SOLVER
Setting controls for the direct linear solver
The linear equation solver can optimize elimination of constraint equations associated with hard contact
and hybrid elements. There are two potential undesirable side-effects associated with this option:
•
Possible small degradation of solution accuracy may adversely impact the nonlinear convergence
behavior.
•
Possible minor performance degradation for models without hard contact constraints and/or hybrid
elements.
Input File Usage:
Use the following option to turn on constraint optimization:
Abaqus/CAE Usage:
*SOLVER CONTROLS, CONSTRAINT OPTIMIZATION
You cannot specify constraint optimization in Abaqus/CAE.
6.1.5–2
Abaqus Version 5.8 ID:
Printed on:
ITERATIVE LINEAR EQUATION SOLVER
6.1.6
ITERATIVE LINEAR EQUATION SOLVER
Products: Abaqus/Standard
Abaqus/CAE
References
•
•
•
•
*STEP
*SOLVER CONTROLS
“Parallel execution in Abaqus/Standard,” Section 3.5.2
“Customizing solver controls,” Section 14.15.2 of the Abaqus/CAE User’s Manual, in the online
HTML version of this manual
Overview
The iterative linear equation solver in Abaqus/Standard:
•
can be used for linear and nonlinear static, quasi-static, heat transfer, geostatic, and coupled pore
fluid diffusion and stress analysis solution procedures;
•
should be used only for large, well-conditioned models for which the direct sparse solver (see
“Direct linear equation solver,” Section 6.1.5) requires a prohibitively large number of floating point
operations;
•
is likely to be dramatically faster than the direct equation solver for large, well-conditioned, blocky
structures;
•
•
•
runs totally in-core and uses less storage than the direct sparse solver (memory and disk combined);
•
cannot be used with automatic stabilization with an adaptive damping factor (see “Adaptive
automatic stabilization scheme” in “Solving nonlinear problems,” Section 7.1.1);
•
can be used with a constant damping factor if stabilization is necessary (see “Automatic stabilization
of static problems with a constant damping factor” in “Solving nonlinear problems,” Section 7.1.1);
•
cannot be used if the system of equations includes Lagrange multiplier degrees of freedom (i.e.,
associated with distributing couplings, hybrid elements, connector elements, contact with direct
enforcement); and
•
will degrade performance if used with models containing dense linear constraints (e.g., equations,
kinematic couplings, MPCs) that eliminate a large number of slave degrees of freedom per master
degree of freedom and/or eliminate some slave degrees of freedom in favor of a large number of
master degrees of freedom.
can be used only with three-dimensional models;
must be the only solver invoked in the analysis (i.e., you cannot use the iterative solver in one step
and the direct solver in another);
6.1.6–1
Abaqus Version 5.8 ID:
Printed on:
ITERATIVE LINEAR EQUATION SOLVER
Iterative solver basics
The iterative solver in Abaqus/Standard can be used to find the solution to a linear system of equations and
can be invoked in a linear or nonlinear static, quasi-static, geostatic, pore fluid diffusion, or heat transfer
analysis step. Since the technique is iterative, a converged solution to a given system of linear equations
cannot be guaranteed. In cases where the iterative solver fails to converge to a solution, modifications
to the model may be necessary to improve the convergence behavior. In some cases the only choice
may be to use the direct solver to obtain a solution. When the iterative solver converges, the accuracy of
this solution depends on the relative tolerance that is used; the default tolerance is sufficiently accurate
for most purposes. However, tolerance adjustments for particular analyses may improve the overall
performance of the simulation. In addition, the performance of the iterative solver relative to the direct
sparse solver is highly sensitive to the model geometry, favoring blocky type structures (i.e., models that
look more like a cube than a plate) with a high degree of mesh connectivity and a relatively low degree
of sparsity. These types of models often demand the most computational and storage resources for the
direct sparse solver. Models with a lesser degree of connectivity (often said to have a higher degree of
sparsity), such as thin, shell-like structures, are much more suited to the direct sparse solver (see “Direct
linear equation solver,” Section 6.1.5).
Input File Usage:
Use the following option to invoke the iterative solver:
Abaqus/CAE Usage:
*STEP, SOLVER=ITERATIVE
Step module: step editor: Other: Method: Iterative
The iterative solution technique
The iterative solution technique in Abaqus/Standard is based on Krylov methods employing a
preconditioner. This solver uses the following general strategy:
1. The Krylov method solver iterates on the system of equations generated by the finite element method
while a preconditioner is applied at each iteration.
2. The preconditioner is calculated only once at the beginning of each linear system solve and is used
to accelerate the convergence of the Krylov method.
3. In parallel, all components of the iterative solution process (including matrix assembly,
preconditioner setup, and the actual solve using the Krylov method) are handled locally on each
core with all necessary communication handled through an MPI-based implementation.
The process outlined above is performed entirely internal to Abaqus/Standard, with no user intervention
required.
Convergence of the linear system of equations
To generate the solution to the system of linear algebraic equations (denoted by the matrix equation
, where K is the global stiffness matrix, f is the load vector, and u is the desired displacement
solution), a sequence of Krylov solver iterations is performed, whereby an approximate solution gets
closer to the exact solution at each iteration. The error in the approximate solution is measured by
the relative residual of the linear system, defined by
, where
is the
norm.
6.1.6–2
Abaqus Version 5.8 ID:
Printed on:
ITERATIVE LINEAR EQUATION SOLVER
The term “convergence” is used to describe this process, and the approximate solution is said to be
converged when the relative residual is below a specified tolerance. By default, this tolerance is 10−3
for general nonlinear procedures. Linear perturbation procedures have the default tolerance of 10−6 .
While the default tolerance may seem loose for general nonlinear procedures, it is important to note
that the linear solver convergence tolerance is independent from the nonlinear convergence process (i.e.,
Newton-Raphson method) tolerances that are used to determine if analysis increments converge. The
latter are the same regardless of the choice of linear equation solver, iterative or direct.
The rate at which the approximate solution converges is directly related to the conditioning of
the original system of equations. A linear system that is well conditioned will converge faster than
an ill-conditioned system. If the residual does not converge to tolerance within the maximum number of
iterations, the iterative solver is said to have encountered a non-convergence and Abaqus/Standard issues
a warning message. However, the analysis will continue running and in some cases the Newton-Raphson
iterations within increments may continue to converge.
Setting controls for the iterative linear solver
The default controls provided in Abaqus/Standard are usually sufficient. However, a method for
overriding the default relative convergence tolerance and maximum number of solver iterations is
provided.
Resetting the solver controls
You can specify that the solver controls be reset to their default values.
Input File Usage:
Abaqus/CAE Usage:
*SOLVER CONTROLS, RESET
Step module: Other→Solver Controls→Edit: Reset all parameters
to their system-defined defaults
Specifying the relative convergence tolerance
By default, this tolerance is 10−3 for procedures other than linear perturbation. Linear perturbation
procedures have the default tolerance of 10−6 . For nonlinear problems the accuracy of the linear solution
can impact the convergence of the Newton method. In some cases it may be necessary to manually
specify the iterative solver relative tolerance to improve the convergence of the Newton-Raphson method
or to improve performance.
Input File Usage:
*SOLVER CONTROLS
relative tolerance for convergence
Abaqus/CAE Usage:
Step module: Other→Solver Controls→Edit: Specify: Relative
tolerance: Specify: relative tolerance for convergence
Specifying the maximum number of solver iterations
In rare instances the linear solver may require more than the default number of iterations to converge to
the desired level of accuracy. In this case you can increase the maximum number of iterations allowed
by the iterative solver (the default value is 300).
6.1.6–3
Abaqus Version 5.8 ID:
Printed on:
ITERATIVE LINEAR EQUATION SOLVER
Input File Usage:
*SOLVER CONTROLS
, max number of solver iterations
Abaqus/CAE Usage:
Step module: Other→Solver Controls→Edit: Specify: Max. number
of iterations: Specify: max number of solver iterations
Specifying the incomplete factorization fill-in levels for soils and geostatic analyses
The preconditioner used for soils and geostatic analyses employs a factorization-based method, also
known as ILU(k). In rare instances the linear solver may require more than the default number
of incomplete factorization fill-in levels to converge to the desired accuracy level. Incomplete
LU factorization of a matrix is a sparse approximation of the LU factorization. LU factorization
typically changes the nonzero structure of the stiffness matrices by adding many nonzero entries; ILU
factorization approximates the fully factorized matrices by limiting the number of nonzero entries
introduced during the factorization. By default, the ILU factorization fill-in level used by the iterative
solver is 0 and no nonzero entries are added. You can increase the fill-in level (maximum value is 3) to
allow nonzero entries to be added based on the connectivity of the stiffness matrices and obtain a better
approximation of the full factorization but with increased computational cost.
Input File Usage:
*SOLVER CONTROLS
, , ILU factorization fill-in level
Abaqus/CAE Usage:
Step module: Other→Solver Controls→Edit: Specify: ILU factorization
fill-in level: Specify: ILU factorization fill-in level
Deciding to use the iterative solver
Many factors must be carefully weighed before deciding to use the iterative solver in Abaqus/Standard,
such as element type, contact and constraint equations, material and geometric nonlinearities, and
material properties, all of which can impact robustness and performance. In cases where the model is
ill-conditioned the iterative solver may converge very slowly or fail to converge. This may occur, for
example, if many elements have poor aspect ratios.
In addition to the robustness issues (relating mainly to the rate of convergence or stagnation), the
iterative solver is expected to outperform the direct sparse solver only for blocky models (even when the
model is well conditioned) that require a very large number of floating point operations for factorization.
Typically, for a well-conditioned solid model, the number of degrees of freedom in the global model
must be greater than one million before the iterative solver will be comparable to the direct solver in
terms of run time.
Element type and model geometry
The most basic modeling issue that will affect the performance of the iterative solver is the model
geometry, which must be carefully considered when deciding if the iterative solver is suited for a
particular model. In general, models that are blocky in nature (i.e., look more like a cube than a plate)
and are dominated by solid elements will behave well with the iterative solver. Although structural
elements such as beams and shells are supported, models with structural elements will not perform
6.1.6–4
Abaqus Version 5.8 ID:
Printed on:
ITERATIVE LINEAR EQUATION SOLVER
optimally; the direct sparse solver should be used instead for such models. Common modeling
techniques such as coating solid elements with a thin layer of membrane elements to recover accurate
stresses on the boundary or fixing rigid body motion with weak springs may not work with the iterative
solver. Applying loads or boundary conditions to large node sets using locally transformed coordinate
systems can also cause convergence difficulties. All of these techniques are likely to lead to extremely
slow convergence or stagnation.
Another factor that can influence the convergence of the iterative solver is the quality of the
elements. Blocky models, such as an engine block, that contain many poorly shaped elements with high
aspect ratios can also lead to poor iterative solver convergence. It is a good idea to look for warning
messages about poorly shaped elements when evaluating the performance of the iterative solver.
Currently, hybrid elements and connectors are not supported with the iterative solver.
Using cohesive elements with the iterative solver will likely lead to nonconvergence.
Constraint equations
Although the iterative solver can be used for models that include constraint equations (such as multi-point
constraints, surface-based tie constraints, kinematic couplings, etc.), certain limitations may exist in the
following situations:
•
•
linear or nonlinear multi-point constraints containing more than a few thousand degrees of freedom;
•
•
rigid body definition of elements containing more than a few thousand degrees of freedom; or
more than a few thousand linear or nonlinear multi-point constraints containing shared master
degrees of freedom;
kinematic coupling constraints containing more than a few thousand slave degrees of freedom.
If any of these conditions apply to a model, the solution cost of the linear system of equations will
grow linearly with the number of such constraints. Furthermore, it is usually recommended to tighten
the iterative solver tolerance and increase the number of maximum iterations in the linear iterative solver
for nonlinear analysis to achieve convergence. Therefore, it is recommended to keep such constraints to
a minimum if possible; otherwise, the increased cost may offset the performance gains that come from
using the iterative solver.
Distributing couplings are not supported with the iterative solver.
Contact
Since contact is a form of nonlinear analysis, special care must be taken in selecting the convergence
tolerance for the iterative solver (see “Nonlinear analysis” below). Therefore, it is recommended to run
the model through a static perturbation analysis before proceeding to the nonlinear problem. This will
demonstrate how the iterative solver will perform for the specific model geometry without the added
difficulty of nonlinear convergence.
The iterative solver will work only with the penalty-based contact formulation with reasonable
penalty stiffness. If contact with direct enforcement (i.e., the Lagrange multiplier method) or penalty
contact with an extremely high penalty stiffness is used, Abaqus/Standard may fail to converge. The
iterative solver does not support pore fluid contact, regardless of the contact formulation used.
6.1.6–5
Abaqus Version 5.8 ID:
Printed on:
ITERATIVE LINEAR EQUATION SOLVER
Material properties
When deciding to use the iterative solver, the variation of material properties in the model should be
considered. Models that have very large discontinuities in material behavior (many orders of magnitude)
will most likely converge slowly and possibly stagnate.
Nonlinear analysis
The iterative solver can be used to solve the linear system of algebraic equations that arises at each
iteration of the Newton procedure. However, the convergence of the nonlinear problem will be affected
by the convergence of the iterative linear solver. The actual impact depends on the particular model and
type of nonlinearities present. In some cases the default iterative solver tolerance of 10−3 is sufficient
to maintain the convergence of the Newton method; in other cases a smaller linear solver tolerance (for
example, 10−6 ) must be used.
If a nonlinear analysis that uses the iterative solver fails to converge, it is often difficult to
determine if this is due to the approximate linear equation solution of the iterative solver or if the
Newton process itself is failing to converge. If nonlinear convergence problems occur, the direct solver
can be used—given the problem is solvable using the direct solver due to solution cost—to eliminate
the approximate linear solution as a possible source of the problem.
6.1.6–6
Abaqus Version 5.8 ID:
Printed on:
STATIC STRESS/DISPLACEMENT ANALYSIS
6.2
Static stress/displacement analysis
•
•
•
•
•
•
•
“Static stress analysis procedures: overview,” Section 6.2.1
“Static stress analysis,” Section 6.2.2
“Eigenvalue buckling prediction,” Section 6.2.3
“Unstable collapse and postbuckling analysis,” Section 6.2.4
“Quasi-static analysis,” Section 6.2.5
“Direct cyclic analysis,” Section 6.2.6
“Low-cycle fatigue analysis using the direct cyclic approach,” Section 6.2.7
6.2–1
Abaqus Version 5.8 ID:
Printed on:
STATIC STRESS ANALYSIS
6.2.1
STATIC STRESS ANALYSIS PROCEDURES: OVERVIEW
A static stress procedure is one in which inertia effects are neglected. Several static stress analysis procedures
are available in Abaqus/Standard:
•
Static analysis:
•
Eigenvalue buckling analysis:
“Static stress analysis,” Section 6.2.2, is used for stable problems and can include
linear or nonlinear response.
“Eigenvalue buckling prediction,” Section 6.2.3, is used to estimate
the critical (bifurcation) load of “stiff” structures. It is a linear perturbation procedure.
•
Unstable collapse and postbuckling analysis: “Unstable collapse and postbuckling analysis,”
Section 6.2.4, is used to estimate the unstable, geometrically nonlinear collapse of a structure. The
method can also be helpful in obtaining a solution in other types of unstable problems, and it is often
suitable for limit load analyses.
•
Quasi-static analysis: “Quasi-static analysis,” Section 6.2.5, is used to analyze the transient response
of structures considering time-dependent material behavior (creep and swelling, viscoelasticity, and
viscoplasticity). A quasi-static analysis can be linear or nonlinear.
•
Direct cyclic analysis:
•
Low-cycle fatigue analysis:
“Direct cyclic analysis,” Section 6.2.6, is used to calculate the stabilized cyclic
response of the structure directly. It uses a combination of Fourier series and time integration of the
nonlinear material behavior to obtain the stabilized cyclic solution iteratively.
“Low-cycle fatigue analysis using the direct cyclic approach,”
Section 6.2.7, is used to predict progressive damage and failure for ductile bulk materials and/or to
predict delamination/debonding growth at the interfaces in laminated composites based on the direct
cyclic approach in conjunction with the damage extrapolation technique.
6.2.1–1
Abaqus Version 5.8 ID:
Printed on:
STATIC STRESS ANALYSIS
6.2.2
STATIC STRESS ANALYSIS
Products: Abaqus/Standard
Abaqus/CAE
References
•
•
•
•
“Defining an analysis,” Section 6.1.2
“Static stress analysis procedures: overview,” Section 6.2.1
*STATIC
“Configuring a static, general procedure” in “Configuring general analysis procedures,”
Section 14.11.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual
Overview
A static stress analysis:
•
•
•
is used when inertia effects can be neglected;
can be linear or nonlinear; and
ignores time-dependent material effects (creep, swelling, viscoelasticity) but takes rate-dependent
plasticity and hysteretic behavior for hyperelastic materials into account.
Time period
During a static step you assign a time period to the analysis. This is necessary for cross-references to the
amplitude options, which can be used to determine the variation of loads and other externally prescribed
parameters during a step (see “Amplitude curves,” Section 33.1.2). In some cases this time scale is quite
real—for example, the response may be caused by temperatures varying with time based on a previous
transient heat transfer run; or the material response may be rate dependent (rate-dependent plasticity),
so that a natural time scale exists. Other cases do not have such a natural time scale; for example, when
a vessel is pressurized up to limit load with rate-independent material response. If you do not specify a
time period, Abaqus/Standard defaults to a time period in which “time” varies from 0.0 to 1.0 over the
step. The “time” increments are then simply fractions of the total period of the step.
Linear static analysis
Linear static analysis involves the specification of load cases and appropriate boundary conditions. If
all or part of a problem has linear response, substructuring is a powerful capability for reducing the
computational cost of large analyses (see “Using substructures,” Section 10.1.1).
Nonlinear static analysis
Nonlinearities can arise from large-displacement effects, material nonlinearity, and/or boundary
nonlinearities such as contact and friction (see “General and linear perturbation procedures,”
6.2.2–1
Abaqus Version 5.8 ID:
Printed on:
STATIC STRESS ANALYSIS
Section 6.1.3) and must be accounted for. If geometrically nonlinear behavior is expected in a step, the
large-displacement formulation should be used. In most nonlinear analyses the loading variations over
the step follow a prescribed history such as a temperature transient or a prescribed displacement.
Input File Usage:
Abaqus/CAE Usage:
Use the following option to specify that a large-displacement formulation
should be used for a static step:
*STEP, NLGEOM
Step module: Create Step: General: Static, General: Basic: Nlgeom:
On (to activate the large-displacement formulation)
Unstable problems
Some static problems can be naturally unstable, for a variety of reasons.
Buckling or collapse
In some geometrically nonlinear analyses, buckling or collapse may occur. In these cases a quasistatic solution can be obtained only if the magnitude of the load does not follow a prescribed history;
it must be part of the solution. When the loading can be considered proportional (the loading over the
complete structure can be scaled with a single parameter), a special approach—called the “modified Riks
method”—can be used, as described in “Unstable collapse and postbuckling analysis,” Section 6.2.4.
Input File Usage:
Abaqus/CAE Usage:
*STATIC, RIKS
Step module: Create Step: General: Static, Riks
Local instabilities
In other unstable analyses the instabilities are local (e.g., surface wrinkling, material instability, or local
buckling), in which case global load control methods such as the Riks method are not appropriate.
Abaqus/Standard offers the option to stabilize this class of problems by applying damping throughout
the model in such a way that the viscous forces introduced are sufficiently large to prevent instantaneous
buckling or collapse but small enough not to affect the behavior significantly while the problem is
stable. The available automatic stabilization schemes are described in detail in “Automatic stabilization
of unstable problems” in “Solving nonlinear problems,” Section 7.1.1.
Incrementation
Abaqus/Standard uses Newton’s method to solve the nonlinear equilibrium equations. Many problems
involve history-dependent response; therefore, the solution usually is obtained as a series of increments,
with iterations to obtain equilibrium within each increment. Increments must sometimes be kept small
(in the sense that rotation and strain increments must be small) to ensure correct modeling of historydependent effects. Most commonly the choice of increment size is a matter of computational efficiency:
if the increments are too large, more iterations will be required. Furthermore, Newton’s method has a
finite radius of convergence; too large an increment can prevent any solution from being obtained because
the initial state is too far away from the equilibrium state that is being sought—it is outside the radius of
convergence. Thus, there is an algorithmic restriction on the increment size.
6.2.2–2
Abaqus Version 5.8 ID:
Printed on:
STATIC STRESS ANALYSIS
Automatic incrementation
In most cases the default automatic incrementation scheme is preferred because it will select increment
sizes based on computational efficiency.
Input File Usage:
Abaqus/CAE Usage:
*STATIC
Step module: Create Step: General: Static, General: Incrementation:
Type: Automatic (default)
Direct incrementation
Direct user control of the increment size is also provided because if you have considerable experience
with a particular problem, you may be able to select a more economical approach.
Input File Usage:
Abaqus/CAE Usage:
*STATIC, DIRECT
Step module: Create Step: General: Static, General:
Incrementation: Type: Fixed
With direct user control, the solution to an increment can be accepted after the maximum
number of iterations allowed has been completed (as defined in “Commonly used control parameters,”
Section 7.2.2), even if the equilibrium tolerances are not satisfied. This approach is not recommended; it
should be used only in special cases when you have a thorough understanding of how to interpret results
obtained in this way. Very small increments and a minimum of two iterations are usually necessary if
this option is used.
Input File Usage:
Abaqus/CAE Usage:
*STATIC, DIRECT=NO STOP
Step module: Create Step: General: Static, General: Other: Accept
solution after reaching maximum number of iterations
Steady-state frictional sliding
In a static analysis procedure you can model steady-state frictional sliding between two deformable
bodies or between a deformable and a rigid body that are moving with different velocities by specifying
the motions of the bodies as predefined fields. In this case it is assumed that the slip velocity follows
from the difference in the user-specified velocities and is independent of the nodal displacements, as
described in “Coulomb friction,” Section 5.2.3 of the Abaqus Theory Manual.
Since this frictional behavior is different from the frictional behavior used without steady-state
frictional sliding, discontinuities may arise in the solutions between an analysis step in which relative
velocity is determined from predefined motions and prior steps. An example is the discontinuity that
occurs between the initial preloading of the disc pads in a disc brake system and the subsequent braking
analysis where the disc spins with a prescribed rotation. To ensure a smooth transition in the solution, it is
recommended that all analysis steps prior to the analysis step in which predefined motion is specified use
a zero coefficient of friction. You can then modify the friction properties in the steady-state analysis to use
the desired friction coefficient (see “Changing friction properties during an Abaqus/Standard analysis”
in “Frictional behavior,” Section 36.1.5).
6.2.2–3
Abaqus Version 5.8 ID:
Printed on:
STATIC STRESS ANALYSIS
Input File Usage:
Abaqus/CAE Usage:
*MOTION
Predefined motion fields are not supported in Abaqus/CAE.
Initial conditions
Initial values of stresses, temperatures, field variables, solution-dependent state variables, etc. can be
specified. “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1, describes all of
the available initial conditions.
Boundary conditions
Boundary conditions can be applied to any of the displacement or rotation degrees of freedom (1–6); to
warping degree of freedom 7 in open-section beam elements; or, if hydrostatic fluid elements are included
in the model, to fluid pressure degree of freedom 8. If boundary conditions are applied to rotation degrees
of freedom, you must understand how finite rotations are handled by Abaqus (see “Boundary conditions
in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1). During the analysis prescribed boundary
conditions can be varied using an amplitude definition (see “Amplitude curves,” Section 33.1.2).
Loads
The following loads can be prescribed in a static stress analysis:
•
Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6); see
“Concentrated loads,” Section 33.4.2.
•
Distributed pressure forces or body forces can be applied; see “Distributed loads,” Section 33.4.3.
The distributed load types available with particular elements are described in Part VI, “Elements.”
Predefined fields
The following predefined fields can be specified in a static stress analysis, as described in “Predefined
fields,” Section 33.6.1:
•
Although temperature is not a degree of freedom in a static stress analysis, nodal temperatures
can be specified as a predefined field. Any difference between the applied and initial temperatures
will cause thermal strain if a thermal expansion coefficient is given for the material (“Thermal
expansion,” Section 26.1.2). The specified temperature also affects temperature-dependent material
properties, if any.
•
The values of user-defined field variables can be specified. These values only affect field-variabledependent material properties, if any.
Material options
Most material models that describe mechanical behavior are available for use in a static stress analysis.
The following material properties are not active during a static stress analysis: acoustic properties,
6.2.2–4
Abaqus Version 5.8 ID:
Printed on:
STATIC STRESS ANALYSIS
thermal properties (except for thermal expansion), mass diffusion properties, electrical conductivity
properties, and pore fluid flow properties.
Rate-dependent yield (“Rate-dependent yield,” Section 23.2.3), hysteresis (“Hysteresis
in elastomers,” Section 22.8.1), and two-layer viscoplasticity (“Two-layer viscoplasticity,”
Section 23.2.11) are the only time-dependent material responses that are active during a static
analysis. The rate-dependent yield response is often important in rapid processes such as metal-working
problems. The hysteresis model is useful in modeling the large-strain, rate-dependent response of
elastomers that exhibit a pronounced hysteresis under cyclic loading. The two-layer viscoplasticity
model is useful in situations where a significant time-dependent behavior as well as plasticity is
observed, which for metals typically occurs at elevated temperatures. An appropriate time scale must
be specified so that Abaqus/Standard can treat the rate dependence of the material responses correctly.
Static creep and swelling problems and time-domain viscoelastic models are analyzed by the quasistatic procedure (“Quasi-static analysis,” Section 6.2.5). When any of these time-dependent material
models are used in a static analysis, a rate-independent elastic solution is obtained and the chosen time
scale does not have an effect on the material response. For creep and swelling behavior this implies that
the loading is applied instantaneously compared with the natural time scale over which creep effects take
place.
The same concept of instantaneous load application applies to time-domain viscoelastic behavior.
You can also obtain the fully relaxed long-term viscoelastic solution directly in a static procedure without
having to perform a transient analysis; this choice is meaningful only when time-domain viscoelastic
material properties are defined. If the long-term viscoelastic solution is requested, the internal stresses
associated with each of the Prony series terms are increased gradually from their values at the beginning
of the step to their long-term values at the end of the step.
For the two-layer viscoplastic material model, you can obtain the long-term response of the elasticplastic network alone.
When frequency-domain viscoelastic material properties are defined (see “Frequency domain
viscoelasticity,” Section 22.7.2), the corresponding elastic moduli must be specified as long-term elastic
moduli. This implies that the response corresponds to the long-term elastic solution, regardless of the
time period specified for the step.
Input File Usage:
Abaqus/CAE Usage:
Use the following option to obtain the fully relaxed long-term elastic solution
with time-domain viscoelasticity or the long-term elastic-plastic solution for
two-layer viscoplasticity:
*STATIC, LONG TERM
Step module: Create Step: General: Static, General or Static, Riks:
Other: Obtain long-term solution with time-domain material properties
Elements
Any of the stress/displacement elements in Abaqus/Standard can be used in a static stress analysis (see
“Choosing the appropriate element for an analysis type,” Section 27.1.3). Although velocities are not
available in a static stress analysis, dashpots can still be used (they can be useful in stabilizing an unstable
problem). The relative velocity will be calculated as described in “Dashpots,” Section 32.2.1.
6.2.2–5
Abaqus Version 5.8 ID:
Printed on:
STATIC STRESS ANALYSIS
Acoustic elements are not active in a static step. Consequently, if an acoustic-solid analysis includes
a static step, only the solid elements will deform. If the deformations are large, the acoustic and solid
meshes may not conform, and subsequent acoustic-structural analysis steps may produce misleading
results. See “ALE adaptive meshing: overview,” Section 12.2.1, for information on using the adaptive
meshing technique to deform the acoustic mesh.
Output
The element output available for a static stress analysis includes stress; strain; energies; the values of
state, field, and user-defined variables; and composite failure measures. The nodal output available
includes displacements, reaction forces, and coordinates. All of the output variable identifiers are
outlined in “Abaqus/Standard output variable identifiers,” Section 4.2.1.
Input file template
*HEADING
…
*BOUNDARY
Data lines to specify zero-valued boundary conditions
*INITIAL CONDITIONS
Data lines to specify initial conditions
*AMPLITUDE
Data lines to define amplitude variations
**
*STEP (,NLGEOM)
Once NLGEOM is specified, it will be active in all subsequent steps
*STATIC, DIRECT
Data line to define direct time incrementation
*BOUNDARY
Data lines to prescribe zero-valued or nonzero boundary conditions
*CLOAD and/or *DLOAD
Data lines to specify loads
*TEMPERATURE and/or *FIELD
Data lines to specify values of predefined fields
*END STEP
**
*STEP
*STATIC
Data line to control automatic time incrementation
*BOUNDARY, OP=MOD
Data lines to modify or add zero-valued or nonzero boundary conditions
6.2.2–6
Abaqus Version 5.8 ID:
Printed on:
STATIC STRESS ANALYSIS
*CLOAD, OP=NEW
Data lines to specify new concentrated loads; all previous concentrated
loads will be removed
*DLOAD, OP=MOD
Data lines to specify additional or modified distributed loads
*TEMPERATURE and/or *FIELD
Data lines to specify additional or modified values of predefined fields
*END STEP
6.2.2–7
Abaqus Version 5.8 ID:
Printed on:
BUCKLING
6.2.3
EIGENVALUE BUCKLING PREDICTION
Products: Abaqus/Standard
Abaqus/CAE
References
•
•
•
•
•
•
“Defining an analysis,” Section 6.1.2
“General and linear perturbation procedures,” Section 6.1.3
“Static stress analysis procedures: overview,” Section 6.2.1
*BUCKLE
“Configuring a buckling procedure” in “Configuring linear perturbation analysis procedures,”
Section 14.11.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual
“Creating and modifying prescribed conditions,” Section 16.4 of the Abaqus/CAE User’s Manual
Overview
Eigenvalue buckling analysis:
•
•
•
•
•
•
is generally used to estimate the critical (bifurcation) load of “stiff” structures;
is a linear perturbation procedure;
can be the first step in an analysis of an unloaded structure, or it can be performed after the structure
has been preloaded—if the structure has been preloaded, the buckling load from the preloaded state
is calculated;
can be used in the investigation of the imperfection sensitivity of a structure;
works only with symmetric matrices (hence, unsymmetric stiffness contributions such as the load
stiffness associated with follower loads are symmetrized); and
cannot be used in a model containing substructures.
General eigenvalue buckling
In an eigenvalue buckling problem we look for the loads for which the model stiffness matrix becomes
singular, so that the problem
has nontrivial solutions.
is the tangent stiffness matrix when the loads are applied, and the
are nontrivial displacement solutions. The applied loads can consist of pressures, concentrated forces,
nonzero prescribed displacements, and/or thermal loading.
Eigenvalue buckling is generally used to estimate the critical buckling loads of stiff structures
(classical eigenvalue buckling). Stiff structures carry their design loads primarily by axial or membrane
action, rather than by bending action. Their response usually involves very little deformation prior to
buckling. A simple example of a stiff structure is the Euler column, which responds very stiffly to a
6.2.3–1
Abaqus Version 5.8 ID:
Printed on:
BUCKLING
compressive axial load until a critical load is reached, when it bends suddenly and exhibits a much
lower stiffness. However, even when the response of a structure is nonlinear before collapse, a general
eigenvalue buckling analysis can provide useful estimates of collapse mode shapes.
The base state
The buckling loads are calculated relative to the base state of the structure. If the eigenvalue buckling
procedure is the first step in an analysis, the initial conditions form the base state; otherwise, the base
state is the current state of the model at the end of the last general analysis step (see “General and linear
perturbation procedures,” Section 6.1.3). Thus, the base state can include preloads (“dead” loads),
.
The preloads are often zero in classical eigenvalue buckling problems.
If geometric nonlinearity was included in the general analysis steps prior to the eigenvalue buckling
analysis (see “General and linear perturbation procedures,” Section 6.1.3), the base state geometry is the
deformed geometry at the end of the last general analysis step. If geometric nonlinearity was omitted,
the base state geometry is the original configuration of the body.
The eigenvalue problem
An incremental loading pattern,
, is defined in the eigenvalue buckling prediction step. The
magnitude of this loading is not important; it will be scaled by the load multipliers, , found in the
eigenvalue problem:
where
is the stiffness matrix corresponding to the base state, which includes the effects
of the preloads,
(if any);
is the differential initial stress and load stiffness matrix due to the incremental
loading pattern,
;
are the eigenvalues;
are the buckling mode shapes (eigenvectors);
M and N
refer to degrees of freedom M and N of the whole model; and
i
refers to the ith buckling mode.
. Normally, the lowest value of
is of interest. The
The critical buckling loads are then
preload pattern,
, and perturbation load pattern,
, may be different. For example,
might be
thermal loading caused by temperature changes, while
is caused by application of pressure.
, are normalized vectors and do not represent actual magnitudes of
The buckling mode shapes,
deformation at critical load. They are normalized so that the maximum displacement component is 1.0.
If all displacement components are zero, the maximum rotation component is normalized to 1.0. These
buckling mode shapes are often the most useful outcome of the eigenvalue analysis, since they predict
the likely failure mode of the structure.
6.2.3–2
Abaqus Version 5.8 ID:
Printed on:
BUCKLING
Abaqus/Standard can extract eigenvalues and eigenvectors for symmetric matrices only; therefore,
and
are symmetrized. If the matrices have significant unsymmetric parts, the eigenproblem
may not be exactly what you expected to solve.
Selecting the eigenvalue extraction method
Abaqus/Standard offers the Lanczos and the subspace iteration eigenvalue extraction methods. The
Lanczos method is generally faster when a large number of eigenmodes is required for a system with
many degrees of freedom. The subspace iteration method may be faster when only a few (less than 20)
eigenmodes are needed.
By default, the subspace iteration eigensolver is employed. Subspace iteration and the Lanczos
solver can be used for different steps in the same analysis; there is no requirement that the same
eigensolver be used for all appropriate steps.
For both eigensolvers you specify the desired number of eigenvalues; Abaqus/Standard will choose
a suitable number of vectors for the subspace iteration procedure or a suitable block size for the Lanczos
method (although you can override this choice, if needed). Significant overestimation of the actual
number of eigenvalues can create very large files. If the actual number of eigenvalues is underestimated,
Abaqus/Standard will issue a corresponding warning message.
In general, the block size for the Lanczos method should be as large as the largest expected
multiplicity of eigenvalues (that is, the largest number of modes with the same eigenvalue). A block
size larger than 10 is not recommended. If the number of eigenvalues requested is n, the default
block size is the minimum of (7, n). The number of block Lanczos steps is usually determined by
Abaqus/Standard, but you can change it when you define the eigenvalue buckling prediction step. In
general, if a particular type of eigenproblem converges slowly, providing more block Lanczos steps will
reduce the analysis cost. On the other hand, if you know that a particular type of problem converges
quickly, providing fewer block Lanczos steps will reduce the amount of in-core memory used. If the
number of eigenvalues requested is n, the default is
Block size
n ≤ 10
n > 10
1
40
70
2
40
60
3
30
60
≥ 4
30
30
If the subspace iteration technique is requested, you can also specify the maximum eigenvalue of
interest; Abaqus/Standard will extract eigenvalues until either the requested number of eigenvalues has
been extracted or the last eigenvalue extracted exceeds the maximum eigenvalue of interest.
If the Lanczos eigensolver is requested, you can also specify the minimum and/or maximum
eigenvalues of interest; Abaqus/Standard will extract eigenvalues until either the requested number of
eigenvalues has been extracted in the given range or all the eigenvalues in the given range have been
extracted.
6.2.3–3
Abaqus Version 5.8 ID:
Printed on:
BUCKLING
Input File Usage:
Use the following option to perform an eigenvalue buckling analysis using the
subspace iteration method:
*BUCKLE, EIGENSOLVER=SUBSPACE (default)
Use the following option to perform an eigenvalue buckling analysis using the
Lanczos method:
Abaqus/CAE Usage:
*BUCKLE, EIGENSOLVER=LANCZOS
Step module: Create Step: Linear perturbation: Buckle:
Eigensolver: Lanczos or Subspace
Limitations associated with applying the Lanczos eigensolver to a buckling analysis
The Lanczos eigensolver cannot be used for buckling analyses in which the stiffness matrix is indefinite,
as in the following cases:
•
•
A model containing hybrid elements or connector elements.
•
•
•
A model containing contact pairs or contact elements.
A model containing distributing coupling constraints, defined either directly (“Coupling
constraints,” Section 34.3.2; “Shell-to-solid coupling,” Section 34.3.3; or “Mesh-independent
fasteners,” Section 34.3.4) or by the distributing coupling elements (DCOUP2D and DCOUP3D).
A model that has been preloaded above the bifurcation (buckling) load.
A model that has rigid body modes.
In such cases Abaqus/Standard will issue an error message and terminate the analysis.
Order of calculation and formation of the stiffness matrices
In an eigenvalue buckling prediction step Abaqus/Standard first does a static perturbation analysis
to determine the incremental stresses,
, due to
. If the base state did not include geometric
nonlinearity, the stiffness matrix used in this static perturbation analysis is the tangent elastic stiffness.
If the base state did include geometric nonlinearity, initial stress and load stiffness terms (due to the
preload,
) are included. The stiffness matrix
corresponding to
and
is then formed.
corresponding
In the eigenvalue extraction portion of the buckling step, the stiffness matrix
to the base state geometry is formed. Initial stress and the load stiffness terms due to the preload,
,
are always included regardless of whether or not geometric nonlinearity is included and are calculated
based on the geometry of the base state.
When forming the stiffness matrices
and
, all contact conditions are fixed in the base
state.
Buckling modes with closely spaced eigenvalues
Some structures have many buckling modes with closely spaced eigenvalues, which can cause numerical
problems. In these cases it often helps to apply enough preload,
, to load the structure to just below
the buckling load before performing the eigenvalue extraction.
6.2.3–4
Abaqus Version 5.8 ID:
Printed on:
BUCKLING
If
—where is a scalar constant and the structure is “stiff” and elastic—and if the
problem is linear, the structural stiffness changes to
and the buckling loads are given
by
. The process is equivalent to a dynamic eigenfrequency extraction with shift . The
structure should not be preloaded above the buckling load. In that case the subspace iteration process
may fail to converge or produce incorrect results; the Lanczos eigensolver cannot be used (as discussed
earlier).
In many cases a series of closely spaced eigenvalues indicates that the structure is imperfection
sensitive. An eigenvalue buckling analysis will not give accurate predictions of the buckling load
for imperfection-sensitive structures; the static Riks procedure should be used instead (see “Unstable
collapse and postbuckling analysis,” Section 6.2.4).
Understanding negative eigenvalues
Sometimes, negative eigenvalues are reported in an eigenvalue buckling analysis. In most cases such
negative eigenvalues indicate that the structure would buckle if the load were applied in the opposite
direction. A classical example is a plate under shear loading; the plate will buckle at the same value for
positive and negative applied shear load. Buckling under reverse loading can also occur in situations
where it may not be expected. For example, a pressure vessel under external pressure may exhibit
a negative eigenvalue (buckling under internal pressure) due to local buckling of a stiffener. Such
“physical” negative buckling modes are usually readily understood once they are displayed and can
usually be avoided by applying a preload before the buckling analysis.
Negative eigenvalues sometimes correspond to buckling modes that cannot be understood readily
in terms of physical behavior, particularly if a preload is applied that causes significant geometric
nonlinearity. In this case a geometrically nonlinear load-displacement analysis should be performed
(“Unstable collapse and postbuckling analysis,” Section 6.2.4).
Including large geometry changes in a buckling analysis
Because buckling analysis is usually done for “stiff” structures, it is not usually necessary to include
the effects of geometry change in establishing equilibrium for the base state. However, if significant
geometry change is involved in the base state and this effect is considered to be important, it can be
included by specifying that geometric nonlinearity should be considered for the base state step (see
“General and linear perturbation procedures,” Section 6.1.3). In such cases it is probably more realistic to
perform a geometrically nonlinear load-displacement analysis (Riks analysis) to determine the collapse
loads, especially for imperfection-sensitive structures.
While large deformation can be included in the preload, the eigenvalue buckling theory relies on
there being little geometric change due to the “live” buckling load,
. If the live load produces
significant geometric change, a nonlinear collapse (Riks) analysis must be used. The total buckling
load predicted by the eigenvalue analysis,
, may be a good estimate for the limit load in
the nonlinear buckling analysis. The Riks method is described in “Unstable collapse and postbuckling
analysis,” Section 6.2.4.
6.2.3–5
Abaqus Version 5.8 ID:
Printed on:
BUCKLING
Initial conditions
The initial values of quantities such as stress, temperature, field variables, and solution-dependent
variables can be specified for an eigenvalue buckling analysis. If the buckling step is the first step
in the analysis, these initial conditions form the base state of the structure. “Initial conditions in
Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1, describes all of the available initial conditions.
Boundary conditions
Boundary conditions can be applied to any of the displacement or rotation degrees of freedom (1–6) or to
warping degree of freedom 7 in open-section beam elements (“Boundary conditions in Abaqus/Standard
and Abaqus/Explicit,” Section 33.3.1). A nonzero prescribed boundary condition in a general analysis
step preceding the eigenvalue buckling analysis can be used to preload the structure. Nonzero boundary
conditions prescribed in an eigenvalue buckling step will contribute to the incremental stress
and,
thus, will contribute to the differential initial stress stiffness. When prescribing nonzero boundary
conditions, you must interpret the resulting eigenproblem carefully. Nonzero prescribed boundary
conditions will be treated as constraints (i.e., as if they were fixed) during the eigenvalue extraction.
Therefore, unless the prescribed boundary conditions are removed for the eigenvalue extraction by
specifying buckling mode boundary conditions (see the discussion below), the mode shapes may be
altered by these boundary conditions.
Amplitude definitions (“Amplitude curves,” Section 33.1.2) cannot be used to vary the magnitudes
of prescribed boundary conditions during an eigenvalue buckling analysis.
You can define perturbation load and buckling mode boundary conditions in an eigenvalue buckling
prediction step.
Input File Usage:
Use either of the following two options to define perturbation load boundary
conditions:
*BOUNDARY
*BOUNDARY, LOAD CASE=1
Use the following option to define buckling mode boundary conditions:
*BOUNDARY, LOAD CASE=2, OP=NEW
The OP=NEW parameter is required when you define buckling mode boundary
conditions in an eigenvalue buckling prediction step; however, the perturbation
load boundary conditions in the step can use either OP=NEW or OP=MOD.
Abaqus/CAE Usage:
Load module: Create Boundary Condition: choose Mechanical for the
Category and Symmetry/Antisymmetry/Encastre for the Types for
Selected Step: select region: toggle on Stress perturbation only to
define a perturbation load boundary condition; toggle on Buckling mode
calculation only to define a buckling mode boundary condition; toggle on
Stress perturbation and buckling mode calculation to define both types
of boundary conditions
6.2.3–6
Abaqus Version 5.8 ID:
Printed on:
BUCKLING
Combining boundary conditions
The buckling mode shapes depend on the stresses in the base state as well as the incremental stresses due
to the perturbation loading in the buckling step. These stresses are influenced by the boundary conditions
used in each step. In a general eigenvalue buckling analysis the following types of boundary conditions
can influence the stresses:
1. The boundary conditions in the base state.
2. The boundary conditions used to calculate the linear perturbation stresses,
conditions will be:
. These boundary
a. the perturbation load boundary conditions specified in the eigenvalue buckling step; or
b. the base-state boundary conditions if no perturbation load boundary conditions are specified
in the eigenvalue buckling step; or
c. the buckling mode boundary conditions if neither perturbation load boundary conditions nor
base-state boundary conditions exist.
3. The boundary conditions used for the eigenvalue extraction. These boundary conditions will be:
a. the buckling mode boundary conditions; or
b. the perturbation load boundary conditions if buckling mode boundary conditions are not
specified in the eigenvalue buckling step; or
c. the base-state boundary conditions if no boundary condition definition is used in the eigenvalue
buckling step.
Table 6.2.3–1 summarizes the use of boundary conditions during an eigenvalue buckling step. When
buckling mode boundary conditions are specified, all boundary conditions to be imposed during
eigenvalue extraction must be specified.
Buckling of symmetric structures
The buckling mode shapes of symmetric structures subjected to symmetric loadings are either symmetric
or antisymmetric. In such cases it is often more efficient to model only part of the structure and then
perform the buckling analysis twice for each symmetry plane: once with symmetric boundary conditions
and once with antisymmetric boundary conditions.
The live load pattern is usually symmetric, so symmetric boundary conditions are required for
the calculation of the perturbation stresses used in the formation of the initial stress stiffness matrix.
The boundary conditions must be switched to antisymmetric for the eigenvalue extraction to obtain the
antisymmetric modes. “Buckling of a cylindrical shell under uniform axial pressure,” Section 1.2.3 of
the Abaqus Benchmarks Manual, illustrates such a case.
If the model includes more than one symmetry plane, it may be necessary to study all permutations
of symmetric and antisymmetric boundary conditions for each symmetry plane.
6.2.3–7
Abaqus Version 5.8 ID:
Printed on:
BUCKLING
Table 6.2.3–1 Boundary conditions in effect during the different
portions of an eigenvalue buckling analysis.
User-defined boundary conditions
Boundary conditions used by Abaqus
Base state
Eigenvalue
buckling
prediction step
Linear
perturbation
Eigenvalue
extraction
B
0
B
B
0
1
1
1
0
2
2
2
B
1
1
1
B
2
B
2
0
1, 2
1
2
B
1, 2
1
2
B = base-state boundary conditions; 0 = no boundary conditions specified
1 = perturbation load boundary conditions
2 = buckling mode boundary conditions
Asymmetric buckling of axisymmetric structures
Axisymmetric structures subjected to compressive loading often collapse in nonaxisymmetric modes.
These modes cannot be found with purely axisymmetric modeling such as that provided by shell elements
SAX1 and SAX2 (“Axisymmetric shell element library,” Section 29.6.9) or continuum elements CAX4
or CAX8 (“Axisymmetric solid element library,” Section 28.1.6). Such analyses must be done with
three-dimensional shell or continuum elements.
Loads
The following types of loading can be prescribed in an eigenvalue buckling analysis:
•
•
Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6); see
“Concentrated loads,” Section 33.4.2.
Distributed pressure forces or body forces can be applied; see “Distributed loads,” Section 33.4.3.
The distributed load types available with particular elements are described in Part VI, “Elements.”
The load stiffness can have a significant effect on the critical buckling load; therefore,
Abaqus/Standard will take the load stiffness due to preloads into account when solving the eigenvalue
buckling problem. It is important that the structure not be preloaded above the critical buckling load.
Any load applied during the eigenvalue buckling analysis is called a “live” load. This incremental
load,
, describes the load pattern for which buckling sensitivity is being investigated; its magnitude
6.2.3–8
Abaqus Version 5.8 ID:
Printed on:
BUCKLING
is not important. This incremental loading definition represents linear perturbation loads, as described
in “Applying loads: overview,” Section 33.4.1.
Follower forces (such as concentrated loads assumed to rotate with the nodal rotation or pressure
loads) lead to an unsymmetric load stiffness. Since eigenvalue extraction in Abaqus/Standard can be
performed only on symmetric matrices, eigenvalue analysis with follower loads may not yield correct
results.
Amplitude definitions cannot be used during an eigenvalue buckling analysis. “Applying loads:
overview,” Section 33.4.1, describes all of the available loads.
Prescribed boundary conditions can also be used to load the structure in an eigenvalue buckling
analysis, as discussed earlier.
Predefined fields
In an eigenvalue buckling prediction step, nodal temperatures can be specified (see “Predefined
fields,” Section 33.6.1). The specified temperatures will cause thermal strain during the static
perturbation analysis if a thermal expansion coefficient is given for the material (“Thermal expansion,”
Section 26.1.2), and incremental stresses
will be generated. Hence, Abaqus/Standard can analyze
buckling due to thermal stress. The specified temperature will not affect temperature-dependent
material properties during the eigenvalue buckling prediction step; the material properties are based
on the temperature in the base state. Amplitude definitions cannot be used to vary the magnitudes of
prescribed temperatures during an eigenvalue buckling analysis.
Material options
During an eigenvalue buckling analysis, the model’s response is defined by its linear elastic stiffness in
the base state. All nonlinear and/or inelastic material properties, as well as effects involving time or strain
rate, are ignored during an eigenvalue buckling analysis. In classical eigenvalue buckling the response
in the base state is also linear.
If temperature-dependent elastic properties are used, the eigenvalue buckling analysis will not
account for changes in the stiffness matrix due to temperature changes. The material properties of the
base state will be used.
Acoustic properties, thermal properties (except for thermal expansion), mass diffusion properties,
electrical properties, and pore fluid flow properties are not active during an eigenvalue buckling analysis.
Elements
Any of the stress/displacement elements in Abaqus/Standard (including those with temperature or
pressure degrees of freedom) can be used in an eigenvalue buckling analysis, with the exception that
hybrid and contact elements cannot be used with the Lanczos eigensolver (as discussed earlier). See
“Choosing the appropriate element for an analysis type,” Section 27.1.3.
6.2.3–9
Abaqus Version 5.8 ID:
Printed on:
BUCKLING
Output
The values of the eigenvalues, , will be listed in the printed output file. If output of stresses, strains,
reaction forces, etc. is requested, this information will be printed for each eigenvalue; these quantities are
perturbation values and represent mode shapes, not absolute values. All of the output variable identifiers
are outlined in “Abaqus/Standard output variable identifiers,” Section 4.2.1.
Buckling mode shapes can be plotted in the Visualization module of Abaqus/CAE.
Input file template
The following template describes a very general eigenvalue buckling problem, where as many eigenvalue
buckling prediction steps as needed can be specified.
Symmetric boundary conditions are specified in the model definition part of the Abaqus/Standard
input and, therefore, belong to the base state (see “General and linear perturbation procedures,”
Section 6.1.3). In the first buckling step Abaqus/Standard uses the base-state boundary conditions to
solve for the perturbation stresses as well as for the eigenvalue extraction.
In the second buckling step the boundary conditions for the base state, the initial stress calculation,
and the eigenvalue extraction are all different. Abaqus/Standard uses the specified symmetry boundary
conditions to solve for the perturbation stresses but uses the specified antisymmetry boundary conditions
for the eigenvalue extraction.
*HEADING
…
*BOUNDARY
Data lines to specify zero-valued boundary conditions contributing to the base state
**
*STEP, NLGEOM
The load stiffness terms will be included in the eigenvalue buckling steps
since the NLGEOM parameter is used in this (optional) preload step
*STATIC
Data line to control incrementation
*BOUNDARY
Data lines to specify nonzero boundary conditions (dead loads)
*CLOAD and/or *DLOAD and/or *TEMPERATURE
Data lines to specify dead loads,
*END STEP
**
*STEP
*BUCKLE
Data line to request the desired number of symmetric modes
*CLOAD and/or *DLOAD and/or *TEMPERATURE
Data lines to specify perturbation loading,
*END STEP
6.2.3–10
Abaqus Version 5.8 ID:
Printed on:
BUCKLING
**
*STEP
*BUCKLE
Data line to request the desired number of antisymmetric modes
*CLOAD and/or *DLOAD and/or *TEMPERATURE
Data lines to specify perturbation loading,
*BOUNDARY, LOAD CASE=1
Data lines to specify all boundary conditions for perturbation loading
*BOUNDARY, LOAD CASE=2, OP=NEW
Data lines to specify all antisymmetric boundary conditions for eigenvalue extraction
*END STEP
6.2.3–11
Abaqus Version 5.8 ID:
Printed on:
RIKS ANALYSIS
6.2.4
UNSTABLE COLLAPSE AND POSTBUCKLING ANALYSIS
Products: Abaqus/Standard
Abaqus/CAE
References
•
•
•
•
•
•
“Defining an analysis,” Section 6.1.2
“Static stress analysis procedures: overview,” Section 6.2.1
“Introducing a geometric imperfection into a model,” Section 11.3.1
*STATIC
*IMPERFECTION
“Configuring a static, Riks procedure” in “Configuring general analysis procedures,”
Section 14.11.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this
manual
Overview
The Riks method:
•
•
•
•
is generally used to predict unstable, geometrically nonlinear collapse of a structure;
can include nonlinear materials and boundary conditions;
often follows an eigenvalue buckling analysis to provide complete information about a structure’s
collapse; and
can be used to speed convergence of ill-conditioned or snap-through problems that do not exhibit
instability.
Unstable response
Geometrically nonlinear static problems sometimes involve buckling or collapse behavior, where the
load-displacement response shows a negative stiffness and the structure must release strain energy to
remain in equilibrium. Several approaches are possible for modeling such behavior. One is to treat the
buckling response dynamically, thus actually modeling the response with inertia effects included as
the structure snaps. This approach is easily accomplished by restarting the terminated static procedure
(“Restarting an analysis,” Section 9.1.1) and switching to a dynamic procedure (“Implicit dynamic
analysis using direct integration,” Section 6.3.2) when the static solution becomes unstable. In some
simple cases displacement control can provide a solution, even when the conjugate load (the reaction
force) is decreasing as the displacement increases. Another approach would be to use dashpots to
stabilize the structure during a static analysis. Abaqus/Standard offers an automated version of this
stabilization approach for the static analysis procedures (see “Static stress analysis,” Section 6.2.2;
“Quasi-static analysis,” Section 6.2.5; “Fully coupled thermal-stress analysis,” Section 6.5.3; or
“Coupled pore fluid diffusion and stress analysis,” Section 6.8.1).
6.2.4–1
Abaqus Version 5.8 ID:
Printed on:
RIKS ANALYSIS
Alternatively, static equilibrium states during the unstable phase of the response can be found by
using the “modified Riks method.” This method is used for cases where the loading is proportional;
that is, where the load magnitudes are governed by a single scalar parameter. The method can provide
solutions even in cases of complex, unstable response such as that shown in Figure 6.2.4–1.
A
1.0
B
Load, P
Displacement
Figure 6.2.4–1
Proportional loading with unstable response.
The Riks method is also useful for solving ill-conditioned problems such as limit load problems or
almost unstable problems that exhibit softening.
The Riks method
In simple cases linear eigenvalue analysis (“Eigenvalue buckling prediction,” Section 6.2.3) may be
sufficient for design evaluation; but if there is concern about material nonlinearity, geometric nonlinearity
prior to buckling, or unstable postbuckling response, a load-deflection (Riks) analysis must be performed
to investigate the problem further.
The Riks method uses the load magnitude as an additional unknown; it solves simultaneously
for loads and displacements. Therefore, another quantity must be used to measure the progress of the
solution; Abaqus/Standard uses the “arc length,” l, along the static equilibrium path in load-displacement
space. This approach provides solutions regardless of whether the response is stable or unstable. See
6.2.4–2
Abaqus Version 5.8 ID:
Printed on:
RIKS ANALYSIS
the “Modified Riks algorithm,” Section 2.3.2 of the Abaqus Theory Manual, for a detailed description
of the method.
Proportional loading
If the Riks step is a continuation of a previous history, any loads that exist at the beginning of the step
and are not redefined are treated as “dead” loads with constant magnitude. A load whose magnitude is
defined in the Riks step is referred to as a “reference” load. All prescribed loads are ramped from the
initial (dead load) value to the reference values specified.
The loading during a Riks step is always proportional. The current load magnitude,
, is defined
by
where
is the “dead load,”
is the reference load vector, and is the “load proportionality factor.”
The load proportionality factor is found as part of the solution. Abaqus/Standard prints out the current
value of the load proportionality factor at each increment.
Incrementation
Abaqus/Standard uses Newton’s method (as described in “Static stress analysis,” Section 6.2.2) to solve
the nonlinear equilibrium equations. The Riks procedure uses only a 1% extrapolation of the strain
increment.
You provide an initial increment in arc length along the static equilibrium path,
, when you
define the step. The initial load proportionality factor,
, is computed as
where
is a user-specified total arc length scale factor (typically set equal to 1). This value of
is used during the first iteration of a Riks step. For subsequent iterations and increments the value
of is computed automatically, so you have no control over the load magnitude. The value of is part of
the solution. Minimum and maximum arc length increments,
and
, can be used to control
the automatic incrementation.
Input File Usage:
Abaqus/CAE Usage:
*STATIC, RIKS
Step module: Create Step: General: Static, Riks
Direct user control of the increment size is also provided; in this case the incremental arc length, ,
is kept constant. This method is not recommended for a Riks analysis since it prevents Abaqus/Standard
from reducing the arc length when a severe nonlinearity is encountered.
Input File Usage:
Abaqus/CAE Usage:
*STATIC, RIKS, DIRECT
Step module: Create Step: General: Static, Riks:
Incrementation: Type: Fixed
6.2.4–3
Abaqus Version 5.8 ID:
Printed on:
RIKS ANALYSIS
Ending a Riks analysis step
Since the loading magnitude is part of the solution, you need a method to specify when the step is
completed. You can specify a maximum value of the load proportionality factor,
, or a maximum
displacement value at a specified degree of freedom. The step will terminate when either value is crossed.
If neither of these finishing conditions is specified, the analysis will continue for the number of increments
specified in the step definition (see “Defining an analysis,” Section 6.1.2).
Bifurcation
The Riks method works well in snap-through problems—those in which the equilibrium path in
load-displacement space is smooth and does not branch. Generally you do not need take any special
precautions in problems that do not exhibit branching (bifurcation). “Snap-through buckling analysis
of circular arches,” Section 1.2.1 of the Abaqus Example Problems Manual, is an example of a smooth
snap-through problem.
The Riks method can also be used to solve postbuckling problems, both with stable and unstable
postbuckling behavior. However, the exact postbuckling problem cannot be analyzed directly due to
the discontinuous response at the point of buckling. To analyze a postbuckling problem, it must be
turned into a problem with continuous response instead of bifurcation. This effect can be accomplished
by introducing an initial imperfection into a “perfect” geometry so that there is some response in the
buckling mode before the critical load is reached.
Introducing geometric imperfections
Imperfections are usually introduced by perturbations in the geometry. Unless the precise shape
of an imperfection is known, an imperfection consisting of multiple superimposed buckling modes
must be introduced (“Eigenvalue buckling prediction,” Section 6.2.3). Abaqus allows you to define
imperfections; see “Introducing a geometric imperfection into a model,” Section 11.3.1.
In this way the Riks method can be used to perform postbuckling analyses of structures that show
linear behavior prior to (bifurcation) buckling. An example of this method of introducing geometric
imperfections is presented in “Buckling of a cylindrical shell under uniform axial pressure,” Section 1.2.3
of the Abaqus Benchmarks Manual.
By performing a load-displacement analysis, other important nonlinear effects, such as material
inelasticity or contact, can be included. In contrast, all inelastic effects are ignored in a linear eigenvalue
buckling analysis and all contact conditions are fixed in the base state. Imperfections based on linear
buckling modes can also be useful for the analysis of structures that behave inelastically prior to reaching
peak load.
Introducing loading imperfections
Perturbations in loads or boundary conditions can also be used to introduce initial imperfections. In
this case fictitious “trigger” loads can be used to initiate the instability. The trigger loads should perturb
the structure in the expected buckling modes. Typically, these loads are applied as dead loads prior to
the Riks step so that they have fixed magnitudes. The magnitudes of trigger loads must be sufficiently
6.2.4–4
Abaqus Version 5.8 ID:
Printed on:
RIKS ANALYSIS
small so that they do not affect the overall postbuckling solution. It is your responsibility to choose
appropriate magnitudes and locations for such fictitious loads; Abaqus/Standard does not check that they
are reasonable.
Obtaining a solution at a particular load or displacement value
The Riks algorithm cannot obtain a solution at a given load or displacement value since these are treated
as unknowns—termination occurs at the first solution that satisfies the step termination criterion. To
obtain solutions at exact values of load or displacement, the solution must be restarted at the desired
point in the step (“Restarting an analysis,” Section 9.1.1) and a new, non-Riks step must be defined.
Since the subsequent step is a continuation of the Riks analysis, the load magnitude in that step must be
given appropriately so that the step begins with the loading continuing to increase or decrease according
to its behavior at the point of restart. For example, if the load was increasing at the restart point and
was positive, a larger load magnitude than the current magnitude should be given in the restart step to
continue this behavior. If the load was decreasing but positive, a smaller magnitude than the current
magnitude should be specified.
Restrictions
A Riks analysis is subject to the following restrictions:
•
A Riks step cannot be followed by another step in the same analysis. Subsequent steps must be
analyzed by using the restart capability.
•
If a Riks analysis includes irreversible deformation such as plasticity and a restart using another Riks
step is attempted while the magnitude of the load on the structure is decreasing, Abaqus/Standard
will find the elastic unloading solution. Therefore, restart should occur at a point in the analysis
where the load magnitude is increasing if plasticity is present.
•
For postbuckling problems involving loss of contact, the Riks method will usually not work; inertia
or viscous damping forces (such as those provided by dashpots) must be introduced in a dynamic
or static analysis to stabilize the solution.
Initial conditions
Initial values of stresses, temperatures, field variables, solution-dependent state variables, etc. can be
specified; “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1, describes all of
the available initial conditions.
Boundary conditions
Boundary conditions can be applied to any of the displacement or rotation degrees of freedom (1–6) or to
warping degree of freedom 7 in open-section beam elements (“Boundary conditions in Abaqus/Standard
and Abaqus/Explicit,” Section 33.3.1). Amplitude definitions (“Amplitude curves,” Section 33.1.2)
cannot be used to vary the magnitudes of prescribed boundary conditions during a Riks analysis.
6.2.4–5
Abaqus Version 5.8 ID:
Printed on:
RIKS ANALYSIS
Loads
The following loads can be prescribed in a Riks analysis:
•
•
Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6); see
“Concentrated loads,” Section 33.4.2.
Distributed pressure forces or body forces can be applied; see “Distributed loads,” Section 33.4.3.
The distributed load types available with particular elements are described in Part VI, “Elements.”
Since Abaqus/Standard scales loading magnitudes proportionally based on the user-specified
magnitudes, amplitude references are ignored when the Riks method is chosen.
If follower loads are prescribed, their contribution to the stiffness matrix may be unsymmetric; the
unsymmetric matrix storage and solution scheme can be used to improve computational efficiency in
such cases (see “Defining an analysis,” Section 6.1.2).
Predefined fields
Nodal temperatures can be specified (see “Predefined fields,” Section 33.6.1). Any difference between
the applied and initial temperatures will cause thermal strain if a thermal expansion coefficient is given for
the material (“Thermal expansion,” Section 26.1.2). The loads generated by the thermal strain contribute
to the “reference” load specified for the Riks analysis and are ramped up with the load proportionality
factor. Hence, the Riks procedure can analyze postbuckling and collapse due to thermal straining.
The values of other user-defined field variables can be specified. These values affect only fieldvariable-dependent material properties, if any. Since the concept of time is replaced by arc length in a
Riks analysis, the use of properties that change due to changes in temperatures and/or field variables is
not recommended.
Material options
Most material models that describe mechanical behavior are available for use in a Riks analysis.
The following material properties are not active during a Riks analysis: acoustic properties, thermal
properties (except for thermal expansion), mass diffusion properties, electrical properties, and pore fluid
flow properties. Materials with history dependence can be used; however, it should be realized that the
results will depend on the loading history, which is not known in advance.
The concept of time is replaced by arc length in a Riks analysis. Therefore, any effects involving
time or strain rate (such as viscous damping or rate-dependent plasticity) are no longer treated correctly
and should not be used.
See Part V, “Materials,” for details on the material models available in Abaqus/Standard.
Elements
Any of the stress/displacement elements in Abaqus/Standard (including those with temperature or
pressure degrees of freedom) can be used in a Riks analysis (see “Choosing the appropriate element for
an analysis type,” Section 27.1.3). Dashpots should not be used since velocities will be calculated as
displacement increments divided by arc length, which is meaningless.
6.2.4–6
Abaqus Version 5.8 ID:
Printed on:
RIKS ANALYSIS
Output
Output options are provided to allow the magnitudes of individual load components (pressure, point
loads, etc.) to be printed or to be written to the results file. The current value of the load proportionality
factor, LPF, will be given automatically with any results or output database file output request. These
output options are recommended when the Riks method is used so that load magnitudes can be
seen directly. All of the output variable identifiers are outlined in “Abaqus/Standard output variable
identifiers,” Section 4.2.1.
Input file template
*HEADING
…
*INITIAL CONDITIONS
Data lines to define initial conditions
*BOUNDARY
Data lines to specify zero-valued boundary conditions
**
*STEP, NLGEOM
*STATIC
*CLOAD and/or *DLOAD and/or *TEMPERATURE
Data lines to specify preload (dead load),
*END STEP
**
*STEP, NLGEOM
*STATIC, RIKS
Data line to define incrementation and stopping criteria
*CLOAD and/or *DLOAD and/or *TEMPERATURE
Data lines to specify reference loading,
*END STEP
6.2.4–7
Abaqus Version 5.8 ID:
Printed on:
QUASI-STATIC ANALYSIS
6.2.5
QUASI-STATIC ANALYSIS
Products: Abaqus/Standard
Abaqus/CAE
References
•
•
•
•
“Defining an analysis,” Section 6.1.2
“Static stress analysis procedures: overview,” Section 6.2.1
*VISCO
“Configuring a transient, static, stress/displacement analysis with time-dependent material
response” in “Configuring general analysis procedures,” Section 14.11.1 of the Abaqus/CAE
User’s Manual, in the online HTML version of this manual
Overview
A quasi-static stress analysis in Abaqus/Standard:
•
•
•
is used to analyze problems with time-dependent material response (creep, swelling, viscoelasticity,
and two-layer viscoplasticity);
is used when inertia effects can be neglected; and
can be linear or nonlinear.
See “Mass scaling,” Section 11.6.1, and “Explicit dynamic analysis,” Section 6.3.3, for information
on conducting quasi-static analysis in Abaqus/Explicit. See “Implicit dynamic analysis using direct
integration,” Section 6.3.2, for information on conducting quasi-static analysis using a dynamic
procedure in Abaqus/Standard.
Incrementation
You can control the time incrementation in a quasi-static analysis directly, or it can be controlled
automatically by Abaqus/Standard. Automatic incrementation is preferred in almost all cases.
Fixed incrementation
If you specify the time increments in a quasi-static analysis directly, fixed time increments equal to the
specified initial time increment will be used throughout the analysis.
Input File Usage:
Abaqus/CAE Usage:
*VISCO
Step module: Create Step: General: Visco
Automatic incrementation
If you select automatic incrementation, the size of the time increment is limited by the accuracy of the
integration. The user-specified accuracy tolerance parameter limits the maximum inelastic strain rate
change allowed over an increment:
6.2.5–1
Abaqus Version 5.8 ID:
Printed on:
QUASI-STATIC ANALYSIS
where t is the time at the beginning of the increment,
is the time increment (so that
is the time
at the end of the increment), and
is the equivalent creep strain rate. To achieve accuracy, the value
chosen for the accuracy tolerance parameter should be on the order of
for creep problems, where
is an acceptable level of error in the stress and E is a typical elastic modulus, or on the order of the
elastic strains for viscoelasticity problems.
Input File Usage:
Abaqus/CAE Usage:
*VISCO, CETOL=tolerance
Step module: Create Step: General: Visco: Incrementation:
Creep/swelling/viscoelastic strain error tolerance: tolerance
Selecting explicit creep integration
Nonlinear creep problems (“Rate-dependent plasticity: creep and swelling,” Section 23.2.4) that exhibit
no other nonlinearities can be solved efficiently by forward-difference integration of the inelastic strains
if the inelastic strain increments are smaller than the elastic strains. This explicit method is efficient
computationally because, unlike implicit methods, iteration is not required. Although this method is
only conditionally stable, the numerical stability limit of the explicit operator is in many cases sufficiently
large to allow the solution to be developed in a reasonable number of time increments.
For creep at very low stress levels, however, the unconditional stability of the backward difference
operator (implicit method) is desirable. In such cases Abaqus/Standard will invoke the implicit
integration scheme automatically.
Explicit integration can be less expensive computationally and simplifies implementation of userdefined creep laws in user subroutine CREEP; you can restrict Abaqus/Standard to using this method
for creep problems (with or without geometric nonlinearity included). See “Rate-dependent plasticity:
creep and swelling,” Section 23.2.4, for further details.
Input File Usage:
Abaqus/CAE Usage:
*VISCO, CETOL=tolerance, CREEP=EXPLICIT
Step module: Create Step: General: Visco: Incrementation:
Creep/swelling/viscoelastic strain error tolerance: tolerance and
Creep/swelling/viscoelastic integration: Explicit
Integration scheme for viscoelasticity and rate-dependent yield
Problems including “Time domain viscoelasticity,” Section 22.7.1, are always integrated with an
unconditionally stable operator. The time step in these problems is limited only by the accuracy
tolerance parameter defined above.
Problems including “Rate-dependent yield,” Section 23.2.3, and “Parallel network viscoelastic
model,” Section 22.8.2, are always integrated using an implicit, unconditionally stable method. The
accuracy tolerance parameter does not limit the inelastic strain rate change and can be set equal to any
nonzero value to activate automatic time incrementation.
6.2.5–2
Abaqus Version 5.8 ID:
Printed on:
QUASI-STATIC ANALYSIS
Unstable problems
Some types of analyses may develop local instabilities, such as surface wrinkling, material instability,
or local buckling. In such cases it may not be possible to obtain a quasi-static solution, even with the aid
of automatic incrementation. Abaqus/Standard offers the ability to stabilize this class of problems by
applying damping throughout the model in such a way that the viscous forces introduced are sufficiently
large to prevent instantaneous buckling or collapse but small enough not to affect the behavior
significantly while the problem is stable. The available automatic stabilization schemes are described in
detail in “Automatic stabilization of unstable problems” in “Solving nonlinear problems,” Section 7.1.1.
Initial conditions
Initial values of stresses, temperatures, field variables, solution-dependent state variables, etc. can be
specified, as described in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1.
Boundary conditions
Boundary conditions can be applied to any of the displacement or rotation degrees of freedom (1–6);
to warping degree of freedom 7 in open-section beam elements; or, if hydrostatic fluid elements are
included in the model, to fluid pressure degree of freedom 8. If boundary conditions are applied to
rotation degrees of freedom, you must understand how Abaqus handles finite rotations. See “Boundary
conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1.
Loads
The following types of loading can be prescribed in a quasi-static analysis:
•
Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6); see
“Concentrated loads,” Section 33.4.2.
•
Distributed pressure forces or body forces can be applied; see “Distributed loads,” Section 33.4.3.
The distributed load types available with particular elements are described in Part VI, “Elements.”
Predefined fields
The following predefined fields can be specified in a quasi-static analysis, as described in “Predefined
fields,” Section 33.6.1:
•
Although temperature is not a degree of freedom in quasi-static analysis, nodal temperatures can be
specified. Any difference between the applied and initial temperatures will cause thermal strain if a
thermal expansion coefficient is given for the material (“Thermal expansion,” Section 26.1.2). The
specified temperature also affects temperature-dependent material properties, if any.
•
The values of user-defined field variables can be specified. These values affect only field-variabledependent material properties, if any.
6.2.5–3
Abaqus Version 5.8 ID:
Printed on:
QUASI-STATIC ANALYSIS
Material options
The quasi-static procedure in Abaqus/Standard is generally used to analyze quasi-static creep and
swelling problems, which occur over fairly long time periods (“Rate-dependent plasticity: creep and
swelling,” Section 23.2.4). This procedure can also be used to analyze viscoelastic materials (“Time
domain viscoelasticity,” Section 22.7.1, and “Parallel network viscoelastic model,” Section 22.8.2) and
two-layer viscoplastic materials (“Two-layer viscoplasticity,” Section 23.2.11). In addition, all material
models that are valid in a static analysis procedure can be used.
Elements
Any of the stress/displacement elements in Abaqus/Standard (including those with temperature or
pressure degrees of freedom) can be used in a quasi-static stress analysis—see “Choosing the appropriate
element for an analysis type,” Section 27.1.3.
Output
In addition to the usual output variables available in Abaqus/Standard (see “Abaqus/Standard output
variable identifiers,” Section 4.2.1), the following variables are provided specifically for creep problems:
Element integration point variables:
CEEQ
CESW
Equivalent creep strain,
.
Magnitude of the swelling strain.
CEMAG
Magnitude of the creep strain,
CEP
CE
Principal creep strains.
Output of all of the creep strain components and CEEQ, CESW, and CEMAG.
.
Input file template
*HEADING
…
*BOUNDARY
Data lines to specify zero-valued boundary conditions
*INITIAL CONDITIONS
Data lines to specify initial conditions
*AMPLITUDE
Data lines to define amplitude variations
**
*STEP (,NLGEOM)
*VISCO, CETOL=tolerance
Data line to define time incrementation and a “real” time scale
*BOUNDARY
6.2.5–4
Abaqus Version 5.8 ID:
Printed on:
QUASI-STATIC ANALYSIS
Data lines to describe nonzero boundary conditions
*CLOAD and/or *DLOAD and/or *TEMPERATURE and/or *FIELD
Data lines to specify loading
*END STEP
6.2.5–5
Abaqus Version 5.8 ID:
Printed on:
DIRECT CYCLIC ANALYSIS
6.2.6
DIRECT CYCLIC ANALYSIS
Products: Abaqus/Standard
Abaqus/CAE
References
•
•
•
•
•
“Defining an analysis,” Section 6.1.2
*DIRECT CYCLIC
*TIME POINTS
*CONTROLS
“Configuring a direct cyclic procedure” in “Configuring general analysis procedures,”
Section 14.11.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual
Overview
A direct cyclic analysis:
•
•
•
•
•
•
•
•
•
is a quasi-static analysis;
uses a combination of Fourier series and time integration of the nonlinear material behavior to obtain
the stabilized cyclic response of the structure iteratively;
avoids the considerable numerical expense associated with a transient analysis;
is ideally suited for very large problems in which many load cycles must be applied to obtain the
stabilized response if transient analysis is performed;
can be performed with linear or nonlinear material with localized plastic deformation;
can be used to predict the likelihood of plastic ratchetting;
assumes geometrically linear behavior and fixed contact conditions;
uses the elastic stiffness, so the equation system is inverted only once; and
can also be used to predict progressive damage and failure for ductile bulk materials and/or to predict
delamination/debonding growth at the interfaces in laminated composites in a low-cycle fatigue
analysis.
Introduction
It is well known that after a number of repetitive loading cycles, the response of an elastic-plastic
structure, such as an automobile exhaust manifold subjected to large temperature fluctuations and
clamping loads, may lead to a stabilized state in which the stress-strain relationship in each successive
cycle is the same as in the previous one. The classical approach to obtain the response of such a structure
is to apply the periodic loading repetitively to the structure until a stabilized state is obtained. This
approach can be quite expensive, since it may require the application of many loading cycles before the
stabilized response is obtained. To avoid the considerable numerical expense associated with a transient
analysis, a direct cyclic analysis can be used to calculate the cyclic response of the structure directly.
6.2.6–1
Abaqus Version 5.8 ID:
Printed on:
DIRECT CYCLIC ANALYSIS
The basis of this method is to construct a displacement function
that describes the response of the
structure at all times t during a load cycle with period T as shown in Figure 6.2.6–1.
u
stabilized solution
solution at iteration n+1
solution at iteration n
tn
∇
o
t n-1
t1
tn
t n+1
T
t
∇
Figure 6.2.6–1 A displacement function at all times t during
a load cycle with period T at different iterations.
A truncated Fourier series is used for this purpose,
where n stands for the number of terms in the Fourier series,
is the angular frequency,
and
, and
are unknown displacement coefficients associated with each degree of freedom in
the problem. Abaqus/Standard solves for the unknown displacement coefficients by using a modified
Newton method, with the elastic stiffness matrix at the beginning of the analysis step serving as the
Jacobian in the scheme. We expand the residual vector in the modified Newton method using a Fourier
series of the same form as the displacement solution:
where each residual vector coefficient , , and
in the Fourier series corresponds to a displacement
coefficient
, and , respectively. The residual coefficients are obtained by tracking through the
entire load cycle. At each instant in time in the cycle Abaqus/Standard obtains the residual vector
by
6.2.6–2
Abaqus Version 5.8 ID:
Printed on:
DIRECT CYCLIC ANALYSIS
using standard element-by-element calculations, which—when integrated over the entire cycle—provide
the Fourier coefficients
The displacement solution is obtained by solving for corrections to the displacement Fourier
coefficients corresponding to each residual coefficient. The updated displacement solution is used in
the next iteration to obtain the displacements at each instant in time. This process is repeated until
convergence is obtained. Each pass through the complete load cycle can, therefore, be thought of as a
single iteration of the solution to the nonlinear problem. Convergence is measured by ensuring that all
entries of the residual coefficients are small.
The algorithm to obtain a stabilized cycle is described in detail in “Direct cyclic algorithm,”
Section 2.2.3 of the Abaqus Theory Manual.
Direct cyclic analysis
A direct cyclic step can be the only step in an analysis, can follow a general or linear perturbation step,
or can be followed by a general or linear perturbation step. If a direct cyclic step is followed by a general
step, the solution at the end of the direct cyclic step will be the initial state of the general step. If a
direct cyclic step follows a general or linear perturbation step, the elastic stiffness matrix at the end of
the last general analysis step prior to the direct cyclic step will serve as the Jacobian in the direct cyclic
procedure. Any prior (non-cyclic) loads are simply included in the constant part of the Fourier expansion
of the residual vectors, and the plastic strains at the end of the preloading step are used as initial conditions
for the direct cyclic step.
Multiple direct cyclic analysis steps can be included in a single analysis. In such a case the Fourier
series coefficients obtained in the previous step can be used as starting values in the current step. By
default, the Fourier coefficients are reset to zero, thus allowing application of cyclic loading conditions
that are very different from those defined in the previous direct cyclic step.
You can specify that a direct cyclic step in a restart analysis should use the Fourier coefficients from
the previous step, thus allowing continuation of an analysis that has not reached a stabilized cycle. In a
direct cyclic analysis a restart file is written at the end of the cycle or time period. Consequently, a restart
analysis that is a continuation of a previous direct cyclic analysis will start with a new iteration at
(see “Restarting an analysis,” Section 9.1.1).
Input File Usage:
Use the following option to reset the Fourier series coefficients to zero:
*DIRECT CYCLIC, CONTINUE=NO (default)
Use the following option to specify that the current step is a continuation of the
previous direct cyclic step:
*DIRECT CYCLIC, CONTINUE=YES
6.2.6–3
Abaqus Version 5.8 ID:
Printed on:
DIRECT CYCLIC ANALYSIS
Abaqus/CAE Usage:
Use the following option to reset the Fourier series coefficients to zero (default):
Step module: Create Step: General: Direct cyclic
Use the following option to specify that the current step is a continuation of the
previous direct cyclic step:
Step module: Create Step: General: Direct cyclic; Basic: Use
displacement Fourier coefficients from previous direct cyclic step
Using the direct cyclic approach to perform low-cycle fatigue analysis
The direct cyclic procedure can also be used in conjunction with the damage extrapolation
technique to predict progressive damage and failure for ductile bulk materials and/or to predict
delamination/debonding at the interfaces in laminated composites in a low-cycle fatigue analysis. In
this case multiple cycles can be included in a single direct cyclic analysis, as described in “Low-cycle
fatigue analysis using the direct cyclic approach,” Section 6.2.7.
Input File Usage:
Abaqus/CAE Usage:
*DIRECT CYCLIC, FATIGUE
Step module: Create Step: General: Direct cyclic; Fatigue:
Include low-cycle fatigue analysis
Controlling the solution accuracy
Direct cyclic analysis combines a Fourier series approximation with time integration of the nonlinear
material behavior to obtain the stabilized cyclic solution iteratively using a modified Newton method.
The accuracy of the algorithm depends on the number of Fourier terms used, the number of iterations
taken to obtain the stabilized solution, and the number of time points within the load period at which the
material response and residual vector are evaluated. Abaqus/Standard allows you to control the solution
in several ways, as described below.
Controlling the iterations in the modified Newton method
In the direct cyclic method global Newton iterations are performed to determine corrections to the
displacement Fourier coefficients. During each global iteration Abaqus/Standard tracks through the
entire time cycle to compute the residual vector at a suitable number of time points. This involves
standard element-by-element finite element calculations in which history-dependent material variables
are integrated. The residual vector is integrated over the period to obtain the Fourier residual
coefficients, which in turn yield corrections in displacement coefficients when the system of equations is
solved. Abaqus/Standard will continue with the iterative process until convergence is obtained or until
the maximum number of iterations allowed has been reached. You can specify the maximum number of
iterations when you define the direct cyclic step; the default is 200 iterations.
Input File Usage:
*DIRECT CYCLIC
, , , , , , , max number of iterations
Abaqus/CAE Usage:
Step module: Create Step: General: Direct cyclic; Incrementation:
Maximum number of iterations: max number of iterations
6.2.6–4
Abaqus Version 5.8 ID:
Printed on:
DIRECT CYCLIC ANALYSIS
Specifying convergence criteria
Convergence is best measured by ensuring that all the residual coefficients are sufficiently small
compared to the time averaged force and that all the corrections to displacement Fourier coefficients
are sufficiently small compared to the displacement Fourier coefficients. The time averaged force is
defined in “Convergence criteria for nonlinear problems,” Section 7.2.3. Abaqus/Standard requires
that the ratio of the maximum residual coefficient to the time averaged force,
, and the ratio of
the maximum correction to the displacement coefficients to the largest displacement coefficient,
,
are less than the tolerances. The default values are
= 0.005 and
= 0.005. To change these
values, you must define direct cyclic controls.
When a stabilized cyclic response does not exist, the method will not converge. In the case where
plastic ratchetting occurs, the displacement and residual coefficients of all the periodic terms (
, and
) in the Fourier series converge. However, the displacement and the residual coefficients of the
constant term ( and ) in the Fourier series continue to grow from one iteration to another iteration.
The user-specified tolerances
and
are used to detect the plastic ratchetting. The default values
are
= 0.005 and
= 0.005. For more information, see “Controlling the solution accuracy in
direct cyclic analysis” in “Commonly used control parameters,” Section 7.2.2.
Input File Usage:
Abaqus/CAE Usage:
*CONTROLS, TYPE=DIRECT CYCLIC
Step module: Other→General Solution Controls→Edit;
Specify: Direct Cyclic
Controlling the Fourier representations
The number of Fourier terms required to obtain an accurate solution depends on the variation of the load
as well as the variation of the structural response over the period. In determining the number of terms,
keep in mind that the objective of this kind of analysis is to make low-cycle fatigue predictions. Hence,
the goal is to obtain good approximation of the plastic strain cycle at each point; local inaccuracies in
the stresses are less important. More Fourier terms usually provide a more accurate solution but at the
expense of additional data storage and computational time. In addition, an accurate integration of the
Fourier residual coefficients requires that the residual vector be evaluated at an adequate number of time
points during the cycle. Abaqus/Standard uses a trapezoidal rule, which assumes a linear variation of the
residual over a time increment, to integrate the residual coefficients. For accurate integration the number
of time points must be larger than the number of Fourier coefficients (which is equal to
, where
n represents the number of Fourier terms). Abaqus/Standard will automatically reduce the number of
Fourier coefficients used for the next iteration if it is found to be greater than the number of increments
taken to complete an iteration.
Abaqus/Standard uses an adaptive algorithm to determine the number of Fourier terms. By default,
Abaqus/Standard starts with 11 terms and determines the response of the structure by using the iterative
method described before. Once convergence is obtained (which is measured by ensuring that all the
residual vector coefficients and all the corrections to displacement coefficients in the Fourier series
are sufficiently small), Abaqus/Standard evaluates if a sufficient number of Fourier terms are used by
determining if equilibrium was satisfied at all the time points during the cycle. If equilibrium is satisfied
at all time points, the solution is accepted. Otherwise, Abaqus/Standard increases the number of Fourier
6.2.6–5
Abaqus Version 5.8 ID:
Printed on:
DIRECT CYCLIC ANALYSIS
terms (by default, 5 terms are added) and continues with the iterative scheme until convergence with the
new number of Fourier terms is obtained. This process is repeated until equilibrium is reached or until
the maximum number of Fourier terms has been used. This scheme is best illustrated in Figure 6.2.6–2,
where both local equilibrium and overall convergence are obtained when the number of Fourier terms
is equal to 21. A maximum number of 25 Fourier terms is used by default. You can specify the initial
and maximum number of Fourier terms and the increment in the number of terms when you define the
direct cyclic step.
ratio of maximum residual to time average force
equilibrium
tolerance
stabilized iteration with 11 terms
stabilized iteration with 16 terms
stabilized iteration with 21 terms
T
t
equilibrium
tolerance
Figure 6.2.6–2
Stabilized iterations with different Fourier terms.
You can also define the convergence criteria for determining convergence and for determining
whether equilibrium is achieved at all time points through the period (see “Commonly used control
parameters,” Section 7.2.2), with suitable defaults set by Abaqus/Standard.
In a direct cyclic analysis that has not reached a stabilized cycle, you can increase the number of
iterations or Fourier terms upon restart, thus allowing continuation of an analysis.
Abaqus/Standard provides detailed output of the maximum residual at each time point, the
maximum residual coefficient, the maximum displacement coefficient, the maximum correction to
displacement coefficients, and the number of Fourier terms at the end of each iteration in the message
(.msg) file. This output is described in more detail below.
Input File Usage:
*DIRECT CYCLIC
, , , , initial number of terms, max number of terms, increment in number of terms
Abaqus/CAE Usage:
Step module: Create Step: General: Direct cyclic; Incrementation:
Number of Fourier terms: Initial: initial number of terms, Maximum:
max number of terms, Increment: increment in number of terms
6.2.6–6
Abaqus Version 5.8 ID:
Printed on:
DIRECT CYCLIC ANALYSIS
Controlling the incrementation during the cyclic time period
To ensure an accurate solution, the material history as well as the residual vector must be evaluated at a
sufficient number of time points during the cycle. The number of time points, , at which the response
is computed must be larger than the number of Fourier coefficients; i.e.,
. Abaqus/Standard
will automatically adjust the number of Fourier coefficients if such a condition is not satisfied. You
can specify the time incrementation over the cycle directly, or it can be determined automatically by
Abaqus/Standard.
You should specify the maximum number of increments allowed in the time period as part of the
step definition. The default is 100.
Automatic incrementation
There are several ways to choose the automatic incrementation scheme. If you specify only the maximum
allowable nodal temperature change in an increment, the time increments are selected automatically
based on this value. Abaqus/Standard will restrict the time increments to ensure that the maximum
temperature change is not exceeded at any node during any increment of the analysis.
For rate-dependent constitutive equations you can limit the size of the time increment by the
accuracy of the integration. The user-specified accuracy tolerance parameter limits the maximum
inelastic strain rate change allowed over an increment:
where t is the time at the beginning of the increment,
is the time increment (so that
is the time
at the end of the increment), and
is the equivalent creep strain rate. To achieve sufficient accuracy, the
value chosen for the accuracy tolerance parameter should be on the order of
for creep problems,
where
is an acceptable level of error in the stress and E is a typical elastic modulus, or on the order
of the elastic strains for viscoelasticity problems.
If rate-dependent constitutive equations are used in combination with a varying temperature, both
controls can be used simultaneously. Abaqus/Standard will then choose the increments that satisfy both
criteria.
If the time integration accuracy measure specified by either or both of the above controls is satisfied
after
consecutive increments without cutbacks, the next time increment will be increased by a factor
of
. Both and
are user-defined parameters (see “Increasing the time increment size” in “Time
integration accuracy in transient problems,” Section 7.2.4). The defaults are
= 3 and
= 1.5.
Input File Usage:
Use the following option to specify the maximum allowable nodal temperature
change:
*DIRECT CYCLIC, DELTMX=
Use the following option to specify the accuracy tolerance parameter:
Abaqus/CAE Usage:
*DIRECT CYCLIC, CETOL=tolerance
Use the following option to specify the maximum allowable nodal temperature
change:
Step module: Create Step: General: Direct cyclic; Incrementation:
Max. allowable temperature change per increment:
6.2.6–7
Abaqus Version 5.8 ID:
Printed on:
DIRECT CYCLIC ANALYSIS
Use the following option to specify the accuracy tolerance parameter:
Step module: Create Step: General: Direct cyclic; Incrementation:
Creep/swelling/viscoelastic strain error tolerance: tolerance
Fixed time incrementation
If neither the accuracy tolerance parameter nor the maximum allowable nodal temperature change is
specified, the size of the time increment is fixed. You must specify the time increment
and the time
period T.
Input File Usage:
*DIRECT CYCLIC
, T
Abaqus/CAE Usage:
Step module: Create Step: General: Direct cyclic; Basic: Cycle time
period: T; Incrementation: Type: Fixed, Increment size:
Defining the time points at which the response must be evaluated
The user-defined time incrementation for a direct cyclic step can be augmented or superseded by
specifying particular time points in the loading history at which the response of the structure should
be evaluated. This feature is particularly useful if you know prior to the analysis at which time points
in the analysis the load reaches a maximum and/or minimum value or when the response will change
rapidly. An example is the analysis of the heating/cooling thermal cycle of an engine component where
you typically know when the temperature reaches a maximum value.
When time points are used with fixed time incrementation, the time incrementation specified for
the direct cyclic step is ignored and instead the time incrementation precisely follows the specified time
points. If time points are used with automatic incrementation, the time incrementation is variable; but
the response of the structure will be evaluated at the specified time points.
The time points can be listed individually, or they can be generated automatically by specifying the
starting time point, ending time point, and increment in time between the two specified time points.
Input File Usage:
Use the following options to list time points individually:
*TIME POINTS, NAME=time points name
*DIRECT CYCLIC, TIME POINTS=time points name
Use the following options to generate time points automatically:
Abaqus/CAE Usage:
*TIME POINTS, NAME=time points name, GENERATE
*DIRECT CYCLIC, TIME POINTS=time points name
Use the following options to list time points individually:
Step module: Create Step: General: Direct cyclic; Incrementation:
Evaluate structure response at time points: time points name
Use the following options to generate time points automatically:
Step module: Create Step: General: Direct cyclic; Incrementation:
Evaluate structure response at time points: Create; Edit Time
Points: Specify using delimiters: Start, End, Increment
6.2.6–8
Abaqus Version 5.8 ID:
Printed on:
DIRECT CYCLIC ANALYSIS
Controlling the application of periodicity conditions
By default, Abaqus/Standard imposes periodic conditions during the iterative solution process by using
the state obtained at the end of the previous iteration as the starting state for the current iteration; i.e.,
, where s is a solution variable such as plastic strain.
In cases where the periodic solution is not easily found (for example, when the loading is close
to causing ratchetting), the state around which the periodic solution is obtained may show considerably
more “drift” than would be obtained in a transient analysis. In such cases you may wish to delay the
application of periodic conditions as an artificial method to reduce this drift. Figure 6.2.6–3 compares
the response of two identical structures subjected to the same set of cyclic loads and boundary conditions,
where each structure experienced a different loading history prior to the application of the cyclic loads.
Figure 6.2.6–3 shows that the prior loading history only affects the mean value of stress and strain; it
does not affect the shape of the stress-strain curves or the amount of energy dissipated during the cycle.
periodicity condition imposed
from iteration 5
periodicity condition imposed
from iteration 1
Figure 6.2.6–3
Influence of periodicity condition on mean value of the strains over a stabilized cycle.
By delaying the application of periodicity conditions, you can influence the mean stress and strain level.
However, this is rarely necessary since the average stress and strain levels are usually not needed for
low-cycle fatigue life predictions.
You can control when the periodicity conditions are applied by defining direct cyclic controls to
specify the variable
. This variable defines from which iteration onward the application of periodic
conditions will be activated. For example, setting
means that the periodicity conditions are
applied from iteration 6 onwards. The default is
, which is appropriate for most analyses.
6.2.6–9
Abaqus Version 5.8 ID:
Printed on:
DIRECT CYCLIC ANALYSIS
Input File Usage:
*CONTROLS, TYPE=DIRECT CYCLIC
Abaqus/CAE Usage:
Step module: Other→General Solution Controls→Edit;
Direct Cyclic:
Initial conditions
Initial values of stresses, temperatures, field variables, solution-dependent state variables, etc. can be
specified (see “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1).
Boundary conditions
Boundary conditions can be applied to any of the displacement or rotation degrees of freedom. During
the analysis, prescribed boundary conditions must have an amplitude definition that is cyclic over the
step: the start value must be equal to the end value (see “Amplitude curves,” Section 33.1.2). If the
analysis consists of several steps, the usual rules apply (see “Boundary conditions in Abaqus/Standard
and Abaqus/Explicit,” Section 33.3.1). At each new step the boundary condition can either be modified
or completely defined. All boundary conditions defined in previous steps remain unchanged unless they
are redefined.
Loads
The following loads can be prescribed in a direct cyclic analysis:
•
•
Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6); see
“Concentrated loads,” Section 33.4.2.
Distributed pressure forces or body forces can be applied; see “Distributed loads,” Section 33.4.3.
The distributed load types available with particular elements are described in Part VI, “Elements.”
During the analysis each load must have an amplitude definition that is cyclic over the step where the start
value must be equal to the end value (see “Amplitude curves,” Section 33.1.2). If the analysis consists
of several steps, the usual rules apply (see “Applying loads: overview,” Section 33.4.1). At each new
step the loading can either be modified or completely defined. All loads defined in previous steps remain
unchanged unless they are redefined.
Predefined fields
The following predefined fields can be specified in a direct cyclic analysis, as described in “Predefined
fields,” Section 33.6.1:
•
Temperature is not a degree of freedom in a direct cyclic analysis, but nodal temperatures can be
specified as a predefined field. The temperature values specified must be cyclic over the step:
the start value must be equal to the end value (see “Amplitude curves,” Section 33.1.2). If the
temperatures are read from the results file, you should specify initial temperature conditions equal
to the temperature values at the end of the step (see “Initial conditions in Abaqus/Standard and
Abaqus/Explicit,” Section 33.2.1). Alternatively, you can ramp the temperatures back to their initial
6.2.6–10
Abaqus Version 5.8 ID:
Printed on:
DIRECT CYCLIC ANALYSIS
condition values, as described in “Predefined fields,” Section 33.6.1. Any difference between the
applied and initial temperatures will cause thermal strain if a thermal expansion coefficient is given
for the material (“Thermal expansion,” Section 26.1.2). The specified temperature also affects
temperature-dependent material properties, if any.
•
The values of user-defined field variables can be specified. These values affect only field-variabledependent material properties, if any. The field variable values specified must be cyclic over the
step.
Material options
Most material models, including user-defined materials (defined using user subroutine UMAT), that
describe mechanical behavior are available for use in a direct cyclic analysis.
The following material properties are not active during a direct cyclic analysis: acoustic properties,
thermal properties (except for thermal expansion), mass diffusion properties, electrical conductivity
properties, piezoelectric properties, and pore fluid flow properties.
Rate-dependent yield (“Rate-dependent yield,” Section 23.2.3), rate-dependent creep
(“Rate-dependent plasticity: creep and swelling,” Section 23.2.4), and two-layer viscoplasticity
(“Two-layer viscoplasticity,” Section 23.2.11) can also be used during a direct cyclic analysis.
Elements
Any of the stress/displacement elements in Abaqus/Standard can be used in a direct cyclic analysis (see
“Choosing the appropriate element for an analysis type,” Section 27.1.3).
Output
Different types of output are available for postprocessing and for monitoring a direct cyclic analysis.
Message file information
Abaqus/Standard prints the residual force, time average force, and a flag to indicate if equilibrium was
satisfied in the message (.msg) file at different time increments for each iteration. You can control the
frequency in increments at which information is printed to the message file, and you can suppress the
output; the default is to print output every 10 increments (see “The Abaqus/Standard message file” in
“Output,” Section 4.1.1, for more information).
Abaqus/Standard also prints the number of Fourier terms used, the maximum residual coefficient,
the maximum correction to displacement coefficients, and the maximum displacement coefficient in the
Fourier series in the message file at the end of each iteration. An example of the output is shown below:
INC
10
TIME
INC
0.250
ITERATION
STEP
TIME
2.50
26 STARTS
LARG. RESI.
FORCE
1.008E+01
6.2.6–11
Abaqus Version 5.8 ID:
Printed on:
TIME AVG.
FORCE
50.9
FORCE
EQUV.
N
DIRECT CYCLIC ANALYSIS
20
30
0.250
0.250
5.00
7.50
1.622E+01
4.622E-02
76.8
99.8
N
Y
ITERATION
26 SUMMARY
NUMBER OF FOURIER TERMS USED 40, TOTAL NUMBER OF INCREMENTS
CYCLE/STEP TIME
30.0,
TOTAL TIME COMPLETED
31.0
AVERAGE FORCE
21.2
TIME AVG. FORCE
25.7
MAX.
MAX.
MAX.
MAX.
MAX.
COEFFICIENT OF DISP.
COEFF. OF RESI. FORCE ON
COEFF. OF RESI. FORCE ON
CORR. TO COEFF. OF DISP.
CORR. TO COEFF. OF DISP.
CONST. TERM
PERI. TERMS
ON CONST. TERM
ON PERI. TERMS
0.142
31.7
0.82
0.002
0.015
AT
AT
AT
AT
AT
NODE
NODE
NODE
NODE
NODE
120
24
44
6
50
50
DOF
DOF
DOF
DOF
DOF
2
1
3
3
3
Results output
Element and nodal output are written only when the stabilized cycle is reached. If a stabilized cycle
has not been reached at the end of an analysis, output is written for the last iteration of the step. The
element output available for a direct cyclic analysis includes stress; strain; energies; and the values of
state, field, and user-defined variables. All the energies are set equal to zero at the beginning of each
iteration since energies dissipated over an entire stabilized cycle are of interest in making fatigue life
predictions in direct cyclic analysis. The nodal output available includes displacements, reaction forces,
and coordinates. All of the output variable identifiers are outlined in “Abaqus/Standard output variable
identifiers,” Section 4.2.1.
Recovering additional results for an iteration
You may want to recover additional results for an iteration rather than for the stabilized cycle. You can
extract these results from the restart data (see “Recovering additional results output from restart data in
Abaqus/Standard” in “Output,” Section 4.1.1). This feature is particularly useful if you want to evaluate
the shift of the strain from one iteration to another iteration when plastic ratchetting occurs.
Input File Usage:
Abaqus/CAE Usage:
*POST OUTPUT, ITERATION=n
Recovering additional results for an iteration is not supported in Abaqus/CAE.
Specifying output at exact times
Output at exact times is not supported for direct cyclic analysis. If output at exact times is requested,
Abaqus will issue a warning message and change the output to an output at approximate times.
Limitations
A direct cyclic analysis is subject to the following limitations:
6.2.6–12
Abaqus Version 5.8 ID:
Printed on:
DIRECT CYCLIC ANALYSIS
•
Contact conditions cannot change during a direct cyclic analysis; they remain as they were defined
at the beginning of the analysis or at the end of any general step prior to the direct cyclic step.
Frictional slipping is not allowed during direct cyclic analyses; all points in contact are assumed to
be sticking if friction is present.
•
Geometric nonlinearity can be included only in any general step prior to a direct cyclic step;
however, only small displacements and strains will be considered during the cyclic step.
Input file template
*HEADING
…
*BOUNDARY
Data lines to specify zero-valued boundary conditions
*INITIAL CONDITIONS
Data lines to specify initial conditions
*AMPLITUDE
Data lines to define amplitude variations
**
*STEP (,INC=)
Set INC equal to the maximum number of increments in a single loading cycle
*DIRECT CYCLIC
Data line to define time increment, cycle time, initial number of Fourier terms,
maximum number of Fourier terms, increment in number of Fourier terms,
and maximum number of iterations
*TIME POINTS
Data lines to list time points
*BOUNDARY, AMPLITUDE=
Data lines to prescribe zero-valued or nonzero boundary conditions
*CLOAD and/or *DLOAD, AMPLITUDE=
Data lines to specify loads
*TEMPERATURE and/or *FIELD, AMPLITUDE=
Data lines to specify values of predefined fields
*END STEP
**
*STEP(,INC=)
*DIRECT CYCLIC, DELTMX
Data line to control automatic time incrementation and Fourier representations
*BOUNDARY, OP=MOD,AMPLITUDE=
Data lines to modify or add zero-valued or nonzero boundary conditions
*CLOAD, OP=NEW, AMPLITUDE=
Data lines to specify new concentrated loads; all previous concentrated
loads will be removed
6.2.6–13
Abaqus Version 5.8 ID:
Printed on:
DIRECT CYCLIC ANALYSIS
*DLOAD, OP=MOD, AMPLITUDE=
Data lines to specify additional or modified distributed loads
*TEMPERATURE and/or *FIELD, AMPLITUDE=
Data lines to specify additional or modified values of predefined fields
*END STEP
6.2.6–14
Abaqus Version 5.8 ID:
Printed on:
LOW-CYCLE FATIGUE ANALYSIS
6.2.7
LOW-CYCLE FATIGUE ANALYSIS USING THE DIRECT CYCLIC APPROACH
Products: Abaqus/Standard
Abaqus/CAE
References
•
•
•
•
•
•
•
•
•
•
•
•
•
“Defining an analysis,” Section 6.1.2
“Static stress analysis procedures: overview,” Section 6.2.1
“Direct cyclic analysis,” Section 6.2.6
“Crack propagation analysis,” Section 11.4.3
“Damage and failure for ductile materials in low-cycle fatigue analysis,” Section 24.4
“Modeling discontinuities as an enriched feature using the extended finite element method,”
Section 10.7.1
*DAMAGE EVOLUTION
*DAMAGE INITIATION
*DEBOND
*DIRECT CYCLIC
*FRACTURE CRITERION
*CONTROLS
“Configuring a direct cyclic procedure” in “Configuring general analysis procedures,”
Section 14.11.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual
Overview
A low-cycle fatigue analysis:
•
•
•
•
•
is characterized by states of stress high enough for inelastic deformation to occur in most cases;
•
models propagation of a discrete crack along an arbitrary, solution-dependent path without
remeshing in the bulk material based on the principles of linear elastic fracture mechanics (LEFM)
with the extended finite element method, in which case the onset and growth of fatigue crack are
characterized by the relative fracture energy release rate;
is a quasi-static analysis on a structure subjected to sub-critical cyclic loading;
can be associated with thermal as well as mechanical loading;
uses the direct cyclic approach to obtain the stabilized cyclic response of the structure directly;
models progressive damage and failure in bulk ductile material based on a continuum damage
mechanics approach, in which case damage initiation and evolution are characterized by the
accumulated inelastic hysteresis strain energy per stabilized cycle;
6.2.7–1
Abaqus Version 5.8 ID:
Printed on:
LOW-CYCLE FATIGUE ANALYSIS
•
models progressive delamination growth along a predefined path at the interfaces in laminated
composites, in which case the onset and growth of fatigue delamination at the interfaces are
characterized by the relative fracture energy release rate;
•
•
uses the damage extrapolation technique to accelerate the low-cycle fatigue analysis; and
assumes geometrically linear behavior and fixed contact conditions within each loading cycle.
Approaches to low-cycle fatigue analysis
The traditional approach for determining the fatigue limit for a structure is to establish the
curves
(load versus number of cycles to failure) for the materials in the structure. Such an approach is still
used as a design tool in many cases to predict fatigue resistance of engineering structures. However, this
technique is generally conservative, and it does not define a relationship between the cycle number and
the degree of damage or crack length.
One alternative approach is to predict the fatigue life by using a crack/damage evolution law
based on the inelastic strain/energy when the structure’s response is stabilized after many cycles.
Because the computational cost to simulate the slow progressive damage in a material over many
load cycles is prohibitively expensive for all but the simplest models, numerical fatigue life studies
usually involve modeling the response of the structure subjected to a small fraction of the actual loading
history. This response is then extrapolated over many load cycles using empirical formulae such as the
Coffin-Manson relationship (see Coffin, 1954, and Manson, 1953) to predict the likelihood of crack
initiation and propagation. Since this approach is based on a constant crack/damage growth rate, it may
not realistically predict the evolution of the crack or damage.
Low-cycle fatigue analysis in Abaqus/Standard
The direct cyclic analysis capability in Abaqus/Standard provides a computationally effective modeling
technique to obtain the stabilized response of a structure subjected to periodic loading and is ideally
suited to perform low-cycle fatigue calculations on a large structure. The capability uses a combination
of Fourier series and time integration of the nonlinear material behavior to obtain the stabilized response
of the structure directly. The theory and algorithm to obtain a stabilized response using the direct cyclic
approach are described in detail in “Direct cyclic algorithm,” Section 2.2.3 of the Abaqus Theory Manual.
The direct cyclic low-cycle fatigue procedure models the progressive damage and failure both in
bulk materials (such as in solder joints in an electronic chip packaging or intra-laminar crack growth in
laminated composites) and at material interfaces (such as delamination in laminated composites). The
former can be based on either a continuum damage mechanics approach or the principles of linear elastic
fracture mechanics with the extended finite element method. The response is obtained by evaluating the
behavior of the structure at discrete points along the loading history (see Figure 6.2.7–1). The solution
at each of these points is used to predict the degradation and evolution of material properties that will
take place during the next increment, which spans a number of load cycles,
. The degraded material
properties are then used to compute the solution at the next increment in the load history. Therefore, the
crack/damage growth rate is updated continually throughout the analysis.
The elastic material stiffness at a material point remains constant and contact conditions remain
unchanged when the stabilized solution is computed at a given point in the loading history. Each of the
6.2.7–2
Abaqus Version 5.8 ID:
Printed on:
LOW-CYCLE FATIGUE ANALYSIS
E
N
N
Figure 6.2.7–1
Elastic stiffness degradation as a function of the cycle number.
solutions along the loading history represents the stabilized response of the structure subjected to the
applied period loads, with a level of material damage at each point in the structure computed from the
previous solution. This process is repeated up to a point in the loading history at which a fatigue life
assessment can be made.
In bulk material, there are two approaches to modeling the progressive damage and failure. One
approach is based on continuum damage mechanics. This approach is more appropriate for ductile
material, in which the cyclic loading leads to stress reversals and the accumulation of plastic strains,
which in turn cause the initiation and propagation of cracks. The damage initiation and evolution are
characterized by the stabilized accumulated inelastic hysteresis strain energy per cycle as illustrated in
Figure 6.2.7–2. The other approach is based on the principles of linear elastic fracture mechanics with the
extended finite element method. This approach is more appropriate for brittle material or material with
small scale yielding, in which the cyclic loading leads to material strength degradation causing fatigue
crack growth along an arbitrary path. The onset and growth of the crack are characterized by the relative
fracture energy release rate at the crack tip based on the Paris law (Paris, 1961).
At interfaces of laminated composites the cyclic loading leads to interface strength degradation
causing fatigue delamination growth. The onset and growth of delamination are also characterized by
the relative fracture energy release rate at the crack tip based on the Paris law (Paris, 1961).
Both the progressive damage mechanism in the bulk material and the progressive delamination
growth mechanism at interfaces can be considered simultaneously, with the failure occurring first at the
weakest link in a model.
Defining a low-cycle fatigue analysis using the direct cyclic approach is similar to defining a direct
cyclic analysis. See “Direct cyclic analysis,” Section 6.2.6, for details on how to specify the number
of Fourier terms, number of iterations, and the increment sizes. You specify the maximum numbers of
cycles,
, when you define the low-cycle fatigue analysis step.
Input File Usage:
Abaqus/CAE Usage:
*DIRECT CYCLIC, FATIGUE
first data line
, ,
Step module: Create Step: General: Direct cyclic; Fatigue: Include
low-cycle fatigue analysis, Maximum number of cycles: Value:
6.2.7–3
Abaqus Version 5.8 ID:
Printed on:
LOW-CYCLE FATIGUE ANALYSIS
3
2
1
time
1
2
stabilized
plastic shakedown
Figure 6.2.7–2
Plastic shakedown in a direct cyclic analysis.
Determining whether to use the Fourier coefficients from the previous step
A low-cycle fatigue step using the direct cyclic approach can be the only step in an analysis, can follow a
general or linear perturbation step, or can be followed by a general or linear perturbation step. Multiple
low-cycle fatigue analysis steps can be included in a single analysis. In such a case the Fourier series
coefficients obtained in the previous step can be used as starting values in the current step. By default,
the Fourier coefficients are reset to zero, thus allowing application of cyclic loading conditions that are
very different from those defined in the previous low-cycle fatigue step.
As in a direct cyclic analysis, you can specify that a low-cycle fatigue step in a restart analysis
should use the Fourier coefficients from the previous step, thus allowing continuation of an analysis to
simulate more loading cycles. In a low-cycle fatigue analysis a restart file is written at the end of the
stabilized cycle. Consequently, a restart analysis that is a continuation of a previous low-cycle fatigue
analysis will start with a new loading cycle at
(see “Restarting an analysis,” Section 9.1.1).
Input File Usage:
Use the following option to specify that the current step is a continuation of the
previous low-cycle fatigue step using the direct cyclic approach:
*DIRECT CYCLIC, FATIGUE, CONTINUE=YES
Use the following option to reset the Fourier series coefficients to zero:
Abaqus/CAE Usage:
*DIRECT CYCLIC, FATIGUE, CONTINUE=NO (default)
Use the following option to specify that the current step is a continuation of the
previous low-cycle fatigue step using the direct cyclic approach:
6.2.7–4
Abaqus Version 5.8 ID:
Printed on:
LOW-CYCLE FATIGUE ANALYSIS
Step module: Create Step: General: Direct cyclic; Basic: Use
displacement Fourier coefficients from previous direct cyclic
step; Fatigue: Include low-cycle fatigue analysis
Use the following option to reset the Fourier series coefficients to zero:
Step module: Create Step: General: Direct cyclic; Fatigue:
Include low-cycle fatigue analysis
Progressive damage and damage extrapolation in bulk ductile material based on continuum
damage mechanics approach
Low-cycle fatigue analysis in Abaqus/Standard allows modeling of progressive damage and failure for
ductile materials in any elements whose response is defined in terms of a continuum-based constitutive
model (“Material library: overview,” Section 21.1.1). This includes cohesive elements modeled using a
continuum approach (“Modeling of an adhesive layer of finite thickness” in “Defining the constitutive
response of cohesive elements using a continuum approach,” Section 32.5.5). The inelastic definition
in a material point must be used in conjunction with the linear elastic material model (“Linear elastic
behavior,” Section 22.2.1), the porous elastic material model (“Elastic behavior of porous materials,”
Section 22.3.1), or the hypoelastic material model (“Hypoelastic behavior,” Section 22.4.1).
After damage initiation the elastic material stiffness is degraded progressively in each cycle (as
shown in Figure 6.2.7–1) based on the accumulated stabilized inelastic hysteresis energy. It is impractical
and computationally expensive to perform a cycle-by-cycle simulation for a low-cycle fatigue analysis;
Instead, to accelerate the low-cycle fatigue analysis, each increment extrapolates the current damaged
state in the bulk material forward over many cycles to a new damaged state after the current loading
cycle is stabilized.
Damage initiation and evolution
Damage initiation refers to the beginning of degradation of the response of a material point. In a
low-cycle fatigue analysis the damage initiation criterion is characterized by the accumulated inelastic
hysteresis energy per cycle,
.
and material constants are used to determine the number of the
cycle in which damage is initiated,
. At the end of a stabilized loading cycle, , Abaqus/Standard
checks to see if the damage initiation criterion
is satisfied in any material point; material
stiffness at a material point will not be degraded unless this criterion is satisfied. The calculations
and output associated with damage initiation are discussed in detail in “Damage initiation for ductile
materials in low-cycle fatigue,” Section 24.4.2.
Once the damage initiation criterion is satisfied at a material point, the damage state is calculated
and updated based on the inelastic hysteresis energy for the stabilized cycle. Abaqus/Standard assumes
that the degradation of the elastic stiffness can be modeled using the scalar damage variable, . The
rate of the damage in a material point per cycle,
, is calculated based on the accumulated inelastic
hysteresis energy, the characteristic length associated with an integration point, and material constants.
For details, see “Damage evolution for ductile materials in low-cycle fatigue,” Section 24.4.3.
6.2.7–5
Abaqus Version 5.8 ID:
Printed on:
LOW-CYCLE FATIGUE ANALYSIS
Typically, a material has completely lost its load carrying capacity when
. You can remove
an element from the mesh if all of the section points at all integration locations of the element have lost
their load carrying capability.
Damage extrapolation technique in the bulk material
If the damage initiation criterion is satisfied in any material point at the end of a stabilized cycle, ,
Abaqus/Standard extrapolates the damage variable
from the current cycle forward to the next
increment over a number of cycles,
. The new damage state,
, is given by
where is the characteristic length associated with an integration point, and
and
are material
constants (see “Damage evolution for ductile materials in low-cycle fatigue,” Section 24.4.3, for more
information).
You specify the minimum (
) and maximum (
) number of cycles over which
the damage is extrapolated forward in any given increment. The default values are 100 and 1000,
respectively.
Input File Usage:
Abaqus/CAE Usage:
*DIRECT CYCLIC, FATIGUE
first data line
,
Step module: Create Step: General: Direct cyclic; Fatigue:
Include low-cycle fatigue analysis, Cycle increment size:
, Maximum:
Minimum:
Discrete crack propagation along an arbitrary path based on the principles of linear elastic
fracture mechanics with the extended finite element method
Low-cycle fatigue analysis in Abaqus/Standard allows the modeling of discrete crack growth along an
arbitrary path based on the principles of linear elastic fracture mechanics with the extended finite element
method. You complete the definition of the crack propagation capability by defining a fracture-based
surface behavior and specifying the fracture criterion in enriched elements. The fracture energy release
rates at the crack tips in enriched elements are calculated based on the modified virtual crack closure
technique (VCCT). VCCT uses the principles of linear elastic fracture mechanics. Therefore, VCCT
is appropriate for problems in which brittle fatigue crack growth occurs, although nonlinear material
deformations can occur somewhere else in the bulk materials. For more information about defining
fracture criteria and VCCT in enriched elements, see “Modeling discontinuities as an enriched feature
using the extended finite element method,” Section 10.7.1.
To accelerate the low-cycle fatigue analysis, the damage extrapolation technique is used, which
advances the crack by at least one element length after each stabilized cycle.
6.2.7–6
Abaqus Version 5.8 ID:
Printed on:
LOW-CYCLE FATIGUE ANALYSIS
Onset and growth of fatigue crack
The onset and growth of fatigue crack at an enriched element are characterized by using the Paris law,
which relates the relative fracture energy release rate,
, to crack growth rates. Two criteria must be
met to initiate fatigue crack growth: one criterion is based on material constants,
, and the current
cycle number, ; the other criterion is based on the maximum fracture energy release rate,
, which
corresponds to the cyclic energy release rate when the structure is loaded up to its maximum value. Once
the onset of fatigue crack growth criterion is satisfied at the enriched elements, the crack growth rate,
, is a piecewise function based on material constants and
(the Paris law). The criteria for fatigue
crack onset and growth are discussed in detail in “Modeling discontinuities as an enriched feature using
the extended finite element method,” Section 10.7.1.
Damage extrapolation technique
If the onset of crack growth criterion is satisfied at any crack tip in the enriched element at the end of a
stabilized cycle, , Abaqus/Standard extends the crack length,
, from the current cycle forward over
a number of cycles,
, to
by fracturing at least one enriched element ahead of the crack tips.
Given the material constants and (as defined in “Modeling discontinuities as an enriched feature
using the extended finite element method,” Section 10.7.1), combined with the known element length and
likely propagation direction
at the enriched elements ahead of the crack tips, the
number of cycles necessary to fail each enriched element ahead of the crack tip can be calculated as
,
where represents the enriched element ahead of the th crack tip. The analysis is set up to advance the
crack by at least one enriched element per increment after the loading cycle is stabilized. The element
with the fewest cycles is identified to be fractured, and its
is represented as the
number of cycles to grow the crack equal to its element length,
. The most
critical element is completely fractured with a zero constraint and a zero stiffness at the cracked surfaces
at the end of the stabilized cycle. As the enriched element is fractured, the load is redistributed, and a
new relative fracture energy release rate must be calculated for the enriched elements ahead of the crack
tips for the next cycle. This capability allows at least one enriched element ahead of the crack tips to
be fractured after each stabilized cycle and precisely accounts for the number of cycles needed to cause
fatigue crack growth over that length.
Progressive delamination growth along a pre-defined path at interfaces
Low-cycle fatigue analysis in Abaqus/Standard also allows the modeling of progressive delamination
growth at the interfaces in laminated composites. The interface along which the delamination (or crack)
propagates must be indicated in the model using a fracture criterion definition. The fracture energy
release rates at the crack tips in the interface elements are calculated based on the virtual crack closure
technique (VCCT). VCCT uses the principles of linear elastic fracture mechanics. Therefore, VCCT is
appropriate for problems in which brittle fatigue delamination growth occurs along predefined surfaces,
although nonlinear material deformations can occur in the bulk materials. For more information about
defining fracture criteria and VCCT, see “Crack propagation analysis,” Section 11.4.3.
To accelerate the low-cycle fatigue analysis, the damage extrapolation technique is used, which
releases at least one element length at the crack tip along the interface after each stabilized cycle. When
6.2.7–7
Abaqus Version 5.8 ID:
Printed on:
LOW-CYCLE FATIGUE ANALYSIS
both brittle fatigue delamination at interfaces and ductile damage or discrete crack growth in bulk
materials are considered in an analysis, failure occurs first at the weakest link.
Onset and growth of fatigue delamination
The onset and growth of fatigue delamination at a defined crack interface are characterized by using
the Paris law, which relates the relative fracture energy release rate,
, to crack growth rates. Two
criteria must be met to initiate fatigue delamination growth: one criterion is based on material constants,
, and the current cycle number, ; the other criterion is based on the maximum fracture energy
release rate,
, which corresponds to the cyclic energy release rate when the structure is loaded up
to its maximum value. Once the onset of delamination growth criterion is satisfied at the interface, the
delamination growth rate,
, is a piecewise function based on material constants and
(the Paris
law). The criteria for fatigue delamination onset and growth are discussed in detail in “Low-cycle fatigue
criterion” in “Crack propagation analysis,” Section 11.4.3.
Damage extrapolation technique at the interface elements
If the onset of delamination growth criterion is satisfied at any crack tip in the interface at the end of
a stabilized cycle, , Abaqus/Standard extends the crack length,
, from the current cycle forward
over a number of cycles,
, to
by releasing at least one element at the interface. Given the
material constants and (as defined in “Low-cycle fatigue criterion” in “Crack propagation analysis,”
Section 11.4.3), combined with the known node spacing
at the interface elements
at the crack tips, the number of cycles necessary to fail each interface element at the crack tip can be
calculated as
, where j represents the node at the jth crack tip. The analysis is set up to release
at least one interface element per increment after the loading cycle is stabilized. The element with the
fewest cycles is identified to be released, and its
is represented as the number of
cycles to grow the crack equal to its element length,
. The most critical element
is completely released with a zero constraint and a zero stiffness at the end of the stabilized cycle. As
the interface element is released, the load is redistributed, and a new relative fracture energy release rate
must be calculated for the interface elements at the crack tips for the next cycle. This capability allows
at least one interface element at the crack tips to be released after each stabilized cycle and precisely
accounts for the number of cycles needed to cause fatigue crack growth over that length.
Controlling the solution accuracy
Low-cycle fatigue analysis utilizes the direct cyclic approach to obtain the stabilized cyclic solution
iteratively by combining a Fourier series approximation with time integration of the nonlinear material
behavior using a modified Newton method. The accuracy of the algorithm depends on the number of
Fourier terms used, the number of iterations taken to obtain the stabilized solution, and the number of
time points within the load period at which the material response and residual vector are evaluated. Some
methods for controlling the solution accuracy in a direct cyclic analysis are described in detail in “Direct
cyclic analysis,” Section 6.2.6. They all remain valid in a low-cycle fatigue analysis using the direct
cyclic approach. In addition, the accuracy of a low-cycle fatigue analysis depends on the number of
cycles over which the damage is extrapolated forward, as described below.
6.2.7–8
Abaqus Version 5.8 ID:
Printed on:
LOW-CYCLE FATIGUE ANALYSIS
Controlling the accuracy of damage extrapolation in the bulk material when using continuum
damage mechanics approach
To accelerate the low-cycle fatigue analysis, the damage extrapolation technique is used at the end of
a stabilized cycle. In addition to specifying the minimum and maximum number of cycles over which
the damage is extrapolated (see “Damage extrapolation technique in the bulk material” above), you can
specify the damage extrapolation tolerance,
, to control the accuracy of damage extrapolation in
the bulk material. The default is
.
Input File Usage:
Use the following option to specify the damage extrapolation tolerance:
*DIRECT CYCLIC, FATIGUE
first data line
, , ,
Abaqus/CAE Usage:
Step module: Create Step: General: Direct cyclic; Fatigue: Include
low-cycle fatigue analysis, Damage extrapolation tolerance:
Determining the increment over which damage is extrapolated forward
Abaqus/Standard uses an adaptive algorithm to determine the number of cycles over which the damage
is extrapolated forward in each increment. By default, Abaqus/Standard starts with 500 cycles (half of
the default value of maximum increment in number of cycles) and determines the maximum damage
increment at any material points based on
If the maximum damage increment,
, is greater than the damage extrapolation tolerance that you
specify, the number of cycles over which the damage is extrapolated forward is reduced accordingly
to ensure the maximum damage increment is less than the damage extrapolation tolerance. On the
other hand, if the maximum damage increment at all material points is less than half of the damage
extrapolation tolerance that you specify, the number of cycles is increased accordingly to ensure the
maximum damage increment is equal to the damage extrapolation tolerance.
Initial conditions
Initial values of stresses, temperatures, field variables, solution-dependent state variables, etc. can be
specified (see “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1).
Boundary conditions
Boundary conditions can be applied to any of the displacement or rotation degrees of freedom. During
the analysis, prescribed boundary conditions must have an amplitude definition that is cyclic over the
step: the start value must be equal to the end value (see “Amplitude curves,” Section 33.1.2). If the
analysis consists of several steps, the usual rules apply (see “Boundary conditions in Abaqus/Standard
and Abaqus/Explicit,” Section 33.3.1). At each new step the boundary condition can either be modified
6.2.7–9
Abaqus Version 5.8 ID:
Printed on:
LOW-CYCLE FATIGUE ANALYSIS
or completely defined. All boundary conditions defined in previous steps remain unchanged unless they
are redefined.
Loads
The following loads can be prescribed in a low-cycle fatigue analysis using the direct cyclic approach:
•
•
Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6); see
“Concentrated loads,” Section 33.4.2.
Distributed pressure forces or body forces can be applied; see “Distributed loads,” Section 33.4.3.
The distributed load types available with particular elements are described in Part VI, “Elements.”
During the analysis each load must have an amplitude definition that is cyclic over the step where the start
value must be equal to the end value (see “Amplitude curves,” Section 33.1.2). If the analysis consists
of several steps, the usual rules apply (see “Applying loads: overview,” Section 33.4.1). At each new
step the loading can either be modified or completely defined. All loads defined in previous steps remain
unchanged unless they are redefined.
Predefined fields
The following predefined fields can be specified in a low-cycle fatigue analysis using the direct cyclic
approach, as described in “Predefined fields,” Section 33.6.1:
•
•
Temperature is not a degree of freedom in a low-cycle fatigue analysis using the direct cyclic
approach, but nodal temperatures can be specified as a predefined field. The temperature values
specified must be cyclic over the step: the start value must be equal to the end value (see
“Amplitude curves,” Section 33.1.2). If the temperatures are read from the results file, you should
specify initial temperature conditions equal to the temperature values at the end of the step (see
“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1). Alternatively,
you can ramp the temperatures back to their initial condition values, as described in “Predefined
fields,” Section 33.6.1. Any difference between the applied and initial temperatures will cause
thermal strain if a thermal expansion coefficient is given for the material (“Thermal expansion,”
Section 26.1.2). The specified temperature also affects temperature-dependent material properties,
if any.
The values of user-defined field variables can be specified. These values affect only field-variabledependent material properties, if any. The field variable values specified must be cyclic over the
step.
Material options
Most ductile material models that describe mechanical behavior are available for use in a low-cycle
fatigue analysis. The inelastic definition in a material point must be used in conjunction with the linear
elastic material model (“Linear elastic behavior,” Section 22.2.1), the porous elastic material model
(“Elastic behavior of porous materials,” Section 22.3.1), or the hypoelastic material model (“Hypoelastic
behavior,” Section 22.4.1).
6.2.7–10
Abaqus Version 5.8 ID:
Printed on:
LOW-CYCLE FATIGUE ANALYSIS
The following material properties are not active during a low-cycle fatigue analysis: acoustic
properties, thermal properties (except for thermal expansion), mass diffusion properties, electrical
conductivity properties, piezoeletric properties, and pore fluid flow properties.
Rate-dependent yield (“Rate-dependent yield,” Section 23.2.3), rate-dependent creep
(“Rate-dependent plasticity: creep and swelling,” Section 23.2.4), and two-layer viscoplasticity
(“Two-layer viscoplasticity,” Section 23.2.11) can also be used during a low-cycle fatigue analysis.
Elements
Any of the stress/displacement elements in Abaqus/Standard can be used in a low-cycle fatigue analysis
(see “Choosing the appropriate element for an analysis type,” Section 27.1.3). This includes cohesive
elements with finite thickness (“Modeling of an adhesive layer of finite thickness” in “Defining the
constitutive response of cohesive elements using a continuum approach,” Section 32.5.5). However,
when modeling fatigue crack growth based on the principles of linear elastic fracture mechanics with the
extended finite element method, only first-order continuum stress/displacement elements and secondorder stress/displacement tetrahedron elements can be associated with an enriched feature (see “Modeling
discontinuities as an enriched feature using the extended finite element method,” Section 10.7.1).
Output
Different types of output are available for postprocessing and for monitoring a low-cycle fatigue analysis
using the direct cyclic approach.
Message file information
As in a direct cyclic analysis, low-cycle fatigue analysis using the direct cyclic approach in
Abaqus/Standard prints the residual force, time average force, and a flag to indicate if equilibrium was
satisfied in the message (.msg) file at different time increments for each iteration in each loading cycle.
You can control the frequency in increments at which information is printed to the message file, and you
can suppress the output; the default is to print output every 10 increments (see “The Abaqus/Standard
message file” in “Output,” Section 4.1.1, for more information).
Abaqus/Standard also prints the number of Fourier terms used, the maximum residual coefficient,
the maximum correction to displacement coefficients, and the maximum displacement coefficient in the
Fourier series in the message file at the end of each iteration in each cycle. An example of the output is
shown below:
CYCLE
INC
10
20
30
TIME
INC
0.250
0.250
0.250
5 STARTS
ITERATION
STEP
TIME
2.50
5.00
7.50
26 STARTS
LARG. RESI.
FORCE
1.008E+01
1.622E+01
4.622E-02
6.2.7–11
Abaqus Version 5.8 ID:
Printed on:
TIME AVG.
FORCE
50.9
76.8
99.8
FORCE
EQUV.
N
N
Y
LOW-CYCLE FATIGUE ANALYSIS
ITERATION
26 SUMMARY
NUMBER OF FOURIER TERMS USED 40, TOTAL NUMBER OF INCREMENTS
CYCLE/STEP TIME
30.0,
TOTAL TIME COMPLETED
31.0
AVERAGE FORCE
21.2
TIME AVG. FORCE
25.7
MAX.
MAX.
MAX.
MAX.
MAX.
COEFFICIENT OF DISP.
COEFF. OF RESI. FORCE ON
COEFF. OF RESI. FORCE ON
CORR. TO COEFF. OF DISP.
CORR. TO COEFF. OF DISP.
CONST. TERM
PERI. TERMS
ON CONST. TERM
ON PERI. TERMS
0.142
31.7
0.82
0.002
0.015
AT
AT
AT
AT
AT
NODE
NODE
NODE
NODE
NODE
120
24
44
6
50
50
DOF
DOF
DOF
DOF
DOF
2
1
3
3
3
Results output
Element and nodal output are written only when the stabilized cycle is reached. If a stabilized cycle has
not been reached at the end of a cycle, output is written for the last iteration of the cycle. All standard
output variables in Abaqus/Standard (“Abaqus/Standard output variable identifiers,” Section 4.2.1) are
available. In addition, the following variables are available for progressive damage in bulk ductile
material based on the continuum damage mechanics approach:
STATUS
SDEG
CYCLEINI
Status of element (the status of an element is 1.0 if the element is active, 0.0 if the
element is not).
Scalar stiffness degradation, D.
Number of cycles to initialize the damage at the material point.
The following variables are available for discrete crack propagation along an arbitrary path based
on the principles of linear elastic fracture mechanics with the extended finite element method:
STATUSXFEM
Status of the enriched element. (The status of an enriched element is 1.0 if the
element is completely cracked, 0.0 if the element is not. If the element is partially
cracked, the value lies between 1.0 and 0.0.)
CYCLEINIXFEM Number of cycles to initialize the crack at the enriched element.
ENRRTXFEM
All components of strain energy release rate range; i.e., the difference between the
energy release rate at the maximum loading and at the minimum loading.
Recovering additional results for a stabilized cycle
You may want to recover additional results for a stabilized cycle. You can extract these results from the
restart data (see “Recovering additional results output from restart data in Abaqus/Standard” in “Output,”
Section 4.1.1).
Input File Usage:
Abaqus/CAE Usage:
*POST OUTPUT, CYCLE=n
Recovering additional results for a stabilized cycle is not supported in
Abaqus/CAE.
6.2.7–12
Abaqus Version 5.8 ID:
Printed on:
LOW-CYCLE FATIGUE ANALYSIS
Specifying output at exact times
Output at exact times is not supported for low-cycle fatigue analysis. If output at exact times is requested,
Abaqus will issue a warning message and change the output to an output at approximate times.
Limitations
A low-cycle fatigue analysis using the direct cyclic approach is subject to the following limitations:
•
•
Contact conditions cannot change during a given cycle when direct cyclic analysis is used iteratively
to obtain a stabilized solution.
Geometric nonlinearity can be included only in any general step prior to a direct cyclic step;
however, only small displacements and strains will be considered during the cyclic step.
Input file template
The following is an example of modeling progressive damage and failure in the bulk material based on
the continuum damage mechanics approach and progressive delamination growth at the interface:
*HEADING
…
*BOUNDARY
Data lines to specify zero-valued boundary conditions
*INITIAL CONDITIONS
Data lines to specify initial conditions
*AMPLITUDE
Data lines to define amplitude variations
**
*MATERIAL
Options to define material properties
*DAMAGE INITIATION, CRITERION=HYSTERESIS ENERGY
Data lines to define material constants for bulk ductile material damage initiation
*DAMAGE EVOLUTION, TYPE=HYSTERESIS ENERGY
Data lines to define material constants for bulk ductile material damage evolution
**
*SURFACE, NAME=slave
Data lines to define slave surface at delamination interface
*SURFACE, NAME=master
Data lines to define master surface at delamination interface
*CONTACT PAIR
slave, master
**
*STEP (,INC=)
Set INC equal to the maximum number of increments in a single loading cycle
6.2.7–13
Abaqus Version 5.8 ID:
Printed on:
LOW-CYCLE FATIGUE ANALYSIS
*DIRECT CYCLIC, FATIGUE
Data line to define time increment, cycle time, initial number of Fourier terms,
maximum number of Fourier terms, increment in number of Fourier terms,
and maximum number of iterations
Data line to define minimum increment in number of cycles,
maximum increment in number of cycles, total number of cycles,
and damage extrapolation tolerance
*DEBOND, SLAVE=slave, MASTER=master
*FRACTURE CRITERION, TYPE=FATIGUE
Data lines to define material constants used in Paris law and fracture criterion
**
*BOUNDARY, AMPLITUDE=
Data lines to prescribe zero-valued or nonzero boundary conditions
*CLOAD and/or *DLOAD, AMPLITUDE=
Data lines to specify loads
*TEMPERATURE and/or *FIELD, AMPLITUDE=
Data lines to specify values of predefined fields
**
*END STEP
The following is an example of modeling discrete crack growth in the bulk material based on the
principles of linear elastic fracture mechanics with the extended finite element method and progressive
delamination growth at the interface:
*HEADING
…
*ENRICHMENT, TYPE=PROPAGATION CRACK, INTERACTION=INTERACTION,
ELSET=ENRICHED
*BOUNDARY
Data lines to specify zero-valued boundary conditions
*INITIAL CONDITIONS
Data lines to specify initial conditions
*AMPLITUDE
Data lines to define amplitude variations
**
*MATERIAL
Options to define material properties
*SURFACE, INTERACTION=INTERACTION
*SURFACE BEHAVIOR
*FRACTURE CRITERION, TYPE=FATIGUE
Data lines to define material constants used in the Paris law and fracture criterion in the bulk
material for enriched elements
**
6.2.7–14
Abaqus Version 5.8 ID:
Printed on:
LOW-CYCLE FATIGUE ANALYSIS
*SURFACE, NAME=slave
Data lines to define slave surface at delamination interface
*SURFACE, NAME=master
Data lines to define master surface at delamination interface
*CONTACT PAIR
slave, master
**
*STEP (,INC=)
Set INC equal to the maximum number of increments in a single loading cycle
*DIRECT CYCLIC, FATIGUE
Data line to define time increment, cycle time, initial number of Fourier terms,
maximum number of Fourier terms, increment in number of Fourier terms,
and maximum number of iterations
Data line to define minimum increment in number of cycles,
maximum increment in number of cycles, total number of cycles,
and damage extrapolation tolerance
*DEBOND, SLAVE=slave, MASTER=master
*FRACTURE CRITERION, TYPE=FATIGUE
Data lines to define material constants used in the Paris law and fracture criterion at the interface
**
*BOUNDARY, AMPLITUDE=
Data lines to prescribe zero-valued or nonzero boundary conditions
*CLOAD and/or *DLOAD, AMPLITUDE=
Data lines to specify loads
*TEMPERATURE and/or *FIELD, AMPLITUDE=
Data lines to specify values of predefined fields
**
*END STEP
Additional references
•
Coffin, L., “A Study of the Effects of Cyclic Thermal Stresses on a Ductile Metal,” Transactions of
the American Society of Mechanical Engineering, vol. 76, pp. 931–951, 1954.
•
Manson, S., “Behavior of Materials under Condition of Thermal Stress,” Heat Transfer Symposium,
University of Michigan Engineering Research Institute, Ann Arbor, MI, pp. 9–75, 1953.
•
Paris, P., M. Gomaz, and W. Anderson, “A Rational Analytic Theory of Fatigue,” The Trend in
Engineering, vol. 15, 1961.
6.2.7–15
Abaqus Version 5.8 ID:
Printed on:
DYNAMIC STRESS/DISPLACEMENT ANALYSIS
6.3
Dynamic stress/displacement analysis
•
•
•
•
•
•
•
•
•
•
•
“Dynamic analysis procedures: overview,” Section 6.3.1
“Implicit dynamic analysis using direct integration,” Section 6.3.2
“Explicit dynamic analysis,” Section 6.3.3
“Direct-solution steady-state dynamic analysis,” Section 6.3.4
“Natural frequency extraction,” Section 6.3.5
“Complex eigenvalue extraction,” Section 6.3.6
“Transient modal dynamic analysis,” Section 6.3.7
“Mode-based steady-state dynamic analysis,” Section 6.3.8
“Subspace-based steady-state dynamic analysis,” Section 6.3.9
“Response spectrum analysis,” Section 6.3.10
“Random response analysis,” Section 6.3.11
6.3–1
Abaqus Version 5.8 ID:
Printed on:
DYNAMIC ANALYSIS OVERVIEW
6.3.1
DYNAMIC ANALYSIS PROCEDURES: OVERVIEW
Overview
Abaqus offers several methods for performing dynamic analysis of problems in which inertia effects
are considered. Direct integration of the system must be used when nonlinear dynamic response is being
studied. Implicit direct integration is provided in Abaqus/Standard; explicit direct integration is provided
in Abaqus/Explicit. Modal methods are usually chosen for linear analyses because in direct-integration
dynamics the global equations of motion of the system must be integrated through time, which makes
direct-integration methods significantly more expensive than modal methods. Subspace-based methods
are provided in Abaqus/Standard and offer cost-effective approaches to the analysis of systems that are
mildly nonlinear.
In Abaqus/Standard dynamic studies of linear problems are generally performed by using the
eigenmodes of the system as a basis for calculating the response. In such cases the necessary modes and
frequencies are calculated first in a frequency extraction step. The mode-based procedures are generally
simple to use; and the dynamic response analysis itself is usually not expensive computationally,
although the eigenmode extraction can become computationally intensive if many modes are required
for a large model. The eigenvalues can be extracted in a prestressed system with the “stress stiffening”
effect included (the initial stress matrix is included if the base state step definition included nonlinear
geometric effects), which may be necessary in the dynamic study of preloaded systems. It is not
possible to prescribe nonzero displacements and rotations directly in mode-based procedures. The
method for prescribing motion in mode-based procedures is explained in “Base motions in modal-based
procedures,” Section 2.5.9 of the Abaqus Theory Manual.
Density must be defined for all materials used in any dynamic analysis, and damping (both viscous
and structural) can be specified either at the material or step level, as described below in “Damping in
dynamic analysis.”
Implicit versus explicit dynamics
The direct-integration dynamic procedure provided in Abaqus/Standard offers a choice of implicit
operators for integration of the equations of motion, while Abaqus/Explicit uses the central-difference
operator. In an implicit dynamic analysis the integration operator matrix must be inverted and a set of
nonlinear equilibrium equations must be solved at each time increment. In an explicit dynamic analysis
displacements and velocities are calculated in terms of quantities that are known at the beginning
of an increment; therefore, the global mass and stiffness matrices need not be formed and inverted,
which means that each increment is relatively inexpensive compared to the increments in an implicit
integration scheme. The size of the time increment in an explicit dynamic analysis is limited, however,
because the central-difference operator is only conditionally stable; whereas the implicit operator
options available in Abaqus/Standard are unconditionally stable and, thus, there is no such limit on the
size of the time increment that can be used for most analyses in Abaqus/Standard (accuracy governs
the time increment in Abaqus/Standard).
The stability limit for the central-difference method (the largest time increment that can be taken
without the method generating large, rapidly growing errors) is closely related to the time required for a
6.3.1–1
Abaqus Version 5.8 ID:
Printed on:
DYNAMIC ANALYSIS OVERVIEW
stress wave to cross the smallest element dimension in the model; thus, the time increment in an explicit
dynamic analysis can be very short if the mesh contains small elements or if the stress wave speed in the
material is very high. The method is, therefore, computationally attractive for problems in which the total
dynamic response time that must be modeled is only a few orders of magnitude longer than this stability
limit; for example, wave propagation studies or some “event and response” applications. Many of the
advantages of the explicit procedure also apply to slower (quasi-static) processes for cases in which it is
appropriate to use mass scaling to reduce the wave speed (see “Mass scaling,” Section 11.6.1).
Abaqus/Explicit offers fewer element types than Abaqus/Standard. For example, only first-order,
displacement method elements (4-node quadrilaterals, 8-node bricks, etc.) and modified second-order
elements are used, and each degree of freedom in the model must have mass or rotary inertia associated
with it. However, the method provided in Abaqus/Explicit has some important advantages:
1. The analysis cost rises only linearly with problem size, whereas the cost of solving the nonlinear
equations associated with implicit integration rises more rapidly than linearly with problem size.
Therefore, Abaqus/Explicit is attractive for very large problems.
2. The explicit integration method is often more efficient than the implicit integration method for
solving extremely discontinuous short-term events or processes.
3. Problems involving stress wave propagation can be far more efficient computationally in
Abaqus/Explicit than in Abaqus/Standard.
In choosing an approach to a nonlinear dynamic problem you must consider the length of time for which
the response is sought compared to the stability limit of the explicit method; the size of the problem; and
the restriction of the explicit method to first-order, pure displacement method or modified second-order
elements. In some cases the choice is obvious, but in many problems of practical interest the choice
depends on details of the specific case. Experience is then the only useful guide.
Direct-solution versus modal superposition procedures
Direct solution procedures must be used for dynamic analyses that involve a nonlinear response. Modal
superposition procedures are a cost-effective option for performing linear or mildly nonlinear dynamic
analyses.
Direct-solution dynamic analysis procedures
The following direct-solution dynamic analyses procedures are available in Abaqus:
•
•
Implicit dynamic analysis: Implicit direct-integration dynamic analysis (“Implicit dynamic
analysis using direct integration,” Section 6.3.2) is used to study (strongly) nonlinear transient
dynamic response in Abaqus/Standard.
explicit dynamic analysis: The subspace projection method in
Abaqus/Standard uses direct, explicit integration of the dynamic equations of equilibrium
written in terms of a vector space spanned by a number of eigenvectors (“Implicit dynamic analysis
using direct integration,” Section 6.3.2). The eigenmodes of the system extracted in a frequency
extraction step are used as the global basis vectors. This method can be very effective for systems
Subspace-based
6.3.1–2
Abaqus Version 5.8 ID:
Printed on:
DYNAMIC ANALYSIS OVERVIEW
•
•
with mild nonlinearities that do not substantially change the mode shapes. It cannot be used in
contact analyses.
Explicit dynamic analysis: Explicit direct-integration dynamic analysis (“Explicit dynamic
analysis,” Section 6.3.3) is available in Abaqus/Explicit.
Direct-solution steady-state harmonic response analysis: The steady-state harmonic
response of a system can be calculated in Abaqus/Standard directly in terms of the physical
degrees of freedom of the model (“Direct-solution steady-state dynamic analysis,” Section 6.3.4).
The solution is given as in-phase (real) and out-of-phase (imaginary) components of the solution
variables (displacement, stress, etc.) as functions of frequency. The main advantage of this method
is that frequency-dependent effects (such as frequency-dependent damping) can be modeled. The
direct method is the most accurate but also the most expensive steady-state harmonic response
procedure. The direct method can also be used if nonsymmetric terms in the stiffness are important
or if model parameters depend on frequency.
Modal superposition procedures
Abaqus includes a full range of modal superposition procedures. Modal superposition procedures can be
run using a high-performance linear dynamics software architecture called SIM. The SIM architecture
offers advantages over the traditional linear dynamics architecture for some large-scale analyses, as
discussed below in “Using the SIM architecture for modal superposition dynamic analyses.”
Prior to any modal superposition procedure, the natural frequencies of a system must be extracted
using the eigenvalue analysis procedure (“Natural frequency extraction,” Section 6.3.5). Frequency
extraction can be performed using the SIM architecture.
The following modal superposition procedures are available in Abaqus:
•
•
•
A steady-state dynamic analysis
based on the natural modes of the system can be used to calculate a system’s linearized response to
harmonic excitation (“Mode-based steady-state dynamic analysis,” Section 6.3.8). This mode-based
method is typically less expensive than the direct method. The solution is given as in-phase (real)
and out-of-phase (imaginary) components of the solution variables (displacement, stress, etc.) as
functions of frequency. Mode-based steady-state harmonic analysis can be performed using the
SIM architecture.
Subspace-based steady-state harmonic response analysis: In this type of
Abaqus/Standard analysis the steady-state dynamic equations are written in terms of a vector
space spanned by a number of eigenvectors (“Subspace-based steady-state dynamic analysis,”
Section 6.3.9). The eigenmodes of the system extracted in a frequency extraction step are used as
the global basis vectors. The method is attractive because it allows frequency-dependent effects to
be modeled and is much cheaper than the direct analysis method (“Direct-solution steady-state
dynamic analysis,” Section 6.3.4). Subspace-based steady-state harmonic response analysis can be
used if the stiffness is nonsymmetric and can be performed using the SIM architecture.
Mode-based transient response analysis: The modal dynamic procedure (“Transient modal
dynamic analysis,” Section 6.3.7) provides transient response for linear problems using modal
superposition. Mode-based transient analysis can be performed using the SIM architecture.
Mode-based steady-state harmonic response analysis:
6.3.1–3
Abaqus Version 5.8 ID:
Printed on:
DYNAMIC ANALYSIS OVERVIEW
•
A linear response spectrum analysis (“Response spectrum
analysis,” Section 6.3.10) is often used to obtain an approximate upper bound of the peak significant
response of a system to a user-supplied input spectrum (such as earthquake data) as a function of
frequency. The method has a very low computational cost and provides useful information about
the spectral behavior of a system. Response spectrum analysis can be performed using the SIM
architecture.
Response spectrum analysis:
•
Random response analysis: The linearized response of a model to random excitation can be
calculated based on the natural modes of the system (“Random response analysis,” Section 6.3.11).
This procedure is used when the structure is excited continuously and the loading can be expressed
statistically in terms of a “Power Spectral Density” (PSD) function. The response is calculated in
terms of statistical quantities such as the mean value and the standard deviation of nodal and element
variables. Random response analysis can be performed using the SIM architecture.
•
Complex eigenvalue extraction: The complex eigenvalue extraction procedure performs
eigenvalue extraction to calculate the complex eigenvalues and the corresponding complex mode
shapes of a system (“Complex eigenvalue extraction,” Section 6.3.6). The eigenmodes of the
system extracted in a frequency extraction step are used as the global basis vectors. The complex
eigenvalue extraction can be performed using the SIM architecture.
Using the SIM architecture for modal superposition dynamic analyses
SIM is a high-performance software architecture available in Abaqus that can be used to perform modal
superposition dynamic analyses. The SIM architecture is much more efficient than the traditional
architecture for large-scale linear dynamic analyses (both model size and number of modes) with
minimal output requests.
SIM-based analyses can be used to efficiently handle nondiagonal damping generated from element
or material contributions, as discussed below in “Damping in a mode-based steady-state and transient
linear dynamic analysis using the SIM architecture.” Therefore, SIM-based procedures are an efficient
alternative to subspace-based linear dynamic procedures for models with element damping or frequencyindependent materials.
Activating the SIM architecture
To use the SIM architecture for a modal superposition dynamic analysis, activate SIM for the initial
frequency extraction procedure. SIM-based frequency extraction procedures write the mode shapes and
other modal system information to a special linear dynamics data (.sim) file. By default, this data file
is written to the scratch directory and deleted upon job completion; however, if restart is requested, the
file is saved in the user directory. All subsequent mode-based steady-state or transient dynamic steps in
an analysis automatically use this linear dynamics data file (and by extension the SIM architecture). If
you restart an analysis that uses the SIM architecture, you must include the linear dynamics data file.
For more information about frequency extraction procedures, see “Natural frequency extraction,”
Section 6.3.5.
Input File Usage:
*FREQUENCY, SIM
6.3.1–4
Abaqus Version 5.8 ID:
Printed on:
DYNAMIC ANALYSIS OVERVIEW
Abaqus/CAE Usage:
Step module: Step→Create: Frequency: Use SIM-based
linear dynamics procedures
Example
The SIM architecture will be used for the entire linear dynamic analysis in the following input file
template:
*STEP
*FREQUENCY, EIGENSOLVER=LANCZOS or AMS, SIM
Data line to control eigenvalue extraction
*END STEP
**
*STEP
*MODAL DYNAMIC
Data line to control time incrementation
*SELECT EIGENMODES
Data lines to define the applicable mode ranges
*END STEP
**
*STEP
*STEADY STATE DYNAMICS
Data lines to specify frequency ranges and bias parameters
*SELECT EIGENMODES
Data lines to define the applicable mode ranges
*END STEP
**
*STEP
*STEADY STATE DYNAMICS, SUBSPACE PROJECTION
Data lines to specify frequency ranges and bias parameters
*SELECT EIGENMODES
Data lines to define the applicable mode ranges
*END STEP
Output in a SIM-based analysis
Output is a fundamental factor in the performance of a linear dynamic analysis. Since it is difficult to
predict the desired output quantities for a linear dynamic analysis, no output is written to the output
database (.odb) file by default during a SIM-based linear dynamic analysis; output requests must be
requested explicitly. Preselected output requests are ignored in SIM-based dynamic analysis procedures.
There are several restrictions on available output requests that apply specifically to SIM-based
analyses:
•
You cannot request output to the results (.fil) file.
6.3.1–5
Abaqus Version 5.8 ID:
Printed on:
DYNAMIC ANALYSIS OVERVIEW
•
Element variables cannot be output to the printed data (.dat) file except for random response
analysis.
•
Output of “base motion” is not supported except for random response analysis.
Limitations of the SIM architecture
The SIM architecture cannot be used with frequency extractions using the subspace iteration eigensolver.
Fully coupled structural-acoustic frequency extractions cannot be performed using the
SIM architecture. However, projected coupling operators can be used to perform fully coupled
structural-acoustic steady-state response analyses (see “Structural-acoustic coupling” in “Natural
frequency extraction,” Section 6.3.5).
The cyclic symmetry modeling feature cannot be used in SIM-based analyses.
Nonphysical material properties in dynamic analyses
Abaqus relies on user-supplied model data and assumes that the material’s physical properties reflect
experimental results. Examples of meaningful material properties are a positive mass density per volume,
a positive Young’s modulus, and a positive value for any available damping coefficients. However, in
special cases you may want to “adjust” a value of density, mass, stiffness, or damping in a region or
a part of the model to bring the overall mass, stiffness, or damping to the expected required levels.
Certain material options in Abaqus allow you to introduce nonphysical material properties to achieve
this adjustment.
For example, to adjust the mass of the model, you can define a nonstructural mass with a negative
mass value, use mass elements with a negative mass over a region of nodes, or introduce additional
elements with negative density. Similarly, to adjust damping levels, you can use negative damping
coefficients or introduce dashpot elements with a negative dashpot constant to reduce the overall damping
levels. Springs with negative stiffness can be defined to adjust the model stiffness.
If you specify nonphysical but allowed material properties, Abaqus issues a warning message.
However, if you specify nonphysical material properties that are not allowed, Abaqus issues an error
message. When introducing nonphysical material properties, you must be aware that the overall
behavior should be “physical”; for example, the mass values at all nodes must be positive in an
eigenvalue extraction procedure.
There are consequences of using nonphysical material properties that are easy to check and interpret,
and there are others beyond the control of Abaqus. Therefore, you should fully understand the stated
problem and the consequences of using nonphysical material properties before you specify the properties.
This is particularly important in Abaqus/Explicit analyses, where the size of the time increment depends
on material properties. For example, distributed mass-dependent loads are calculated based on the overall
mass density (positive and negative) provided.
Damping in dynamic analysis
Every nonconservative system exhibits some energy loss that is attributed to material nonlinearity,
internal material friction, or to external (mostly joint) frictional behavior. Conventional engineering
materials like steel and high strength aluminum alloys provide small amounts of internal material
6.3.1–6
Abaqus Version 5.8 ID:
Printed on:
DYNAMIC ANALYSIS OVERVIEW
damping, not enough to prevent large amplification at or near resonant frequencies. Damping properties
increase in modern composite fiber-reinforced materials, where the energy loss occurs through plastic or
viscoelastic phenomena as well as from friction at the interfaces between the matrix and reinforcement.
Still larger material damping is exhibited by thermoplastics. Mechanical dampers may be added to
models to introduce damping forces to the system. In general, it is difficult to quantify the source of a
system’s damping. It usually comes from several sources simultaneously; e.g., from energy loss during
hysteretic loading, viscoelastic material properties, and external joint friction.
Users that work with a specific system know the source of the energy loss from experience. A
variety of methods are available in Abaqus to specify damping that accurately models the energy loss in
a dynamic system.
Sources of damping
Abaqus has four categories of damping sources: material and element damping, global damping, modal
damping, and damping associated with time integration. If necessary, you can include multiple damping
sources and combine different damping sources in a model.
Material and element damping
Damping may be specified as part of a material definition that is assigned to a model (see “Material
damping,” Section 26.1.1). In addition, Abaqus has elements such as dashpots, springs with their
complex stiffness matrix, and connectors that serve as dampers, all with viscous and structural damping
factors. Viscous damping can be included in mass, beam, pipe, and shell elements with general
section properties; and it can also be used in substructure elements (see “Defining substructures,”
Section 10.1.2). In direct steady-state dynamic analysis you can define the viscous and structural
damping due to the interaction between the contacting surfaces by using user subroutine UINTER (see
“UINTER,” Section 1.1.38 of the Abaqus User Subroutines Reference Manual). Contact damping is
not applicable for linear perturbation procedures.
In acoustic elements, velocity proportional viscous damping is implemented using the volumetric
drag parameter (see “Acoustic medium,” Section 26.3.1). Acoustic infinite elements and impedance
conditions also add damping to a model.
Global damping
In situations where material or element damping is not appropriate or sufficient, you can apply abstract
damping factors to an entire model. Abaqus allows you to specify global damping factors for both viscous
(Rayleigh damping) and structural damping (imaginary stiffness matrix).
Modal damping
Modal damping applies only to mode-based linear dynamic analyses. This technique allows you to apply
damping directly to the modes of the system. By definition, modal damping contributes only diagonal
entries to the modal system of equations and can be defined several different ways.
6.3.1–7
Abaqus Version 5.8 ID:
Printed on:
DYNAMIC ANALYSIS OVERVIEW
Damping associated with time integration
Marching through a simulation with a finite time increment size causes some damping. This type of
damping applies only to analyses using direct time integration. See “Implicit dynamic analysis using
direct integration,” Section 6.3.2, for further discussion of this source of damping.
Damping in a linear dynamic analysis
Damping can be applied to a linear dynamic system in two forms:
•
•
velocity proportional viscous damping; and
displacement proportional structural damping, which is for use in frequency domain dynamics.
The exception is SIM-based transient modal dynamic analysis, where the structural damping is
converted to the equivalent diagonal viscous damping (see “Modal dynamic analysis,” Section 2.5.5
of the Abaqus Theory Manual).
An additional type of damping known as composite damping serves as a means to calculate a model
average critical damping with the material density as the weight factor and is intended for use in modebased dynamics (excluding subspace projection steady-state analysis and SIM-based dynamic analyses).
For additional information, see “Damping options for modal dynamics,” Section 2.5.4 of the Abaqus
Theory Manual.
The types of damping available for linear dynamic analyses depend on the procedure type
and the architecture (traditional or SIM) used to perform the analysis, as outlined in Table 6.3.1–1
and Table 6.3.1–2. For completeness, Table 6.3.1–1 also includes the damping options for a direct
steady-state dynamic analysis. In addition to directly specified modal damping, global damping can be
used in all linear dynamic procedures. Material and element damping can be used in subspace-based
and SIM-based linear dynamic procedures.
Table 6.3.1–1
Damping sources for traditional architecture.
Damping Source
Traditional Architecture
Modal
Mode-based steady-state dynamics
Subspace-based steady-state dynamics
Transient modal dynamics
Random response analysis
Complex frequency
Response spectrum
Direct steady-state dynamics
6.3.1–8
Abaqus Version 5.8 ID:
Printed on:
Global
Material and Element
DYNAMIC ANALYSIS OVERVIEW
Table 6.3.1–2
Damping sources for SIM architecture.
Damping Source
SIM Architecture
Modal
Global
Material and Element
Mode-based steady-state dynamics
Subspace-based steady-state dynamics
Transient modal dynamics
Random response analysis
Complex frequency
Response spectrum
In a subspace-based or SIM-based linear dynamic analysis, material and element damping operators
must first be projected onto the basis of mode shapes. This projection results in a full modal damping
matrix for both viscous and structural damping; therefore, a modal steady-state response analysis requires
the solution of a system of linear equations at each frequency point. The size of this system is equal to
the number of modes used in the response calculation. In a mode-based transient analysis, the projected
damping operator is treated explicitly in time by including it on the right-hand side of the system of
equations.
Frequency-dependent damping is supported only for the subspace-based and direct-integration
steady-state dynamic procedures.
Material and element damping is not supported for the response spectrum or the random response
procedures. In these procedures, only modal and global damping are allowed, and material or element
damping is ignored.
Damping in a mode-based steady-state and transient linear dynamic analysis using the SIM architecture
SIM-based linear dynamic analyses may include material and element damping contributions that
introduce both diagonal and nondiagonal terms in the modal system of equations. The projection of
material and element damping operators onto the basis of mode shapes is performed during the natural
frequency extraction procedure, which enables a high-performance projection operation to be performed
when used with the AMS eigensolver. If the damping operators depend on frequency, they will be
evaluated at the frequency specified for property evaluation during the frequency extraction procedure.
When the structural and viscous damping operators are projected onto the mode shapes, the full
modal damping matrix is stored in the linear dynamics data (.sim) file. The full modal damping matrix
is combined with any diagonal contributions from global damping or traditional modal damping. The
combined damping operator matrix is included in subsequent mode-based transient or steady-state
dynamics steps. If there are nondiagonal (i.e., projected) damping contributions and a large number of
modes are included, performance of the linear dynamics calculations will be impacted since a direct
solve must be performed at each frequency point.
6.3.1–9
Abaqus Version 5.8 ID:
Printed on:
DYNAMIC ANALYSIS OVERVIEW
Acoustic damping due to impedance conditions is projected onto the subspace of acoustic
eigenvectors. These contributions are taken into account in a subspace-based steady-state dynamics
analysis that uses the SIM architecture.
The default behavior for a SIM-based frequency extraction step is to project any element and
material damping onto the mode shapes. You can turn off this damping projection if it is not desired;
however, in this case only diagonal damping is available for subsequent modal superposition steps.
If the projected damping matrices are not desired in a particular mode-based linear dynamic step
for performance reasons, they can be deactivated in that step using the damping control techniques
discussed above in “Damping in dynamic analysis.”
Input File Usage:
Use the following option to project material and element damping operators in
a SIM-based analysis:
*FREQUENCY, SIM, DAMPING PROJECTION=ON (default)
Use the following option to turn off damping projection in a SIM-based
analysis:
Abaqus/CAE Usage:
*FREQUENCY, SIM, DAMPING PROJECTION=OFF
To control the projection of element and material damping in a SIM-based
frequency extraction step that uses the Lanczos eigensolver:
Step module: Step→Create: Frequency: Eigensolver: Lanczos,
Use SIM-based linear dynamics procedures, toggle Project
damping operators
To control the projection of element and material damping in a frequency
extraction step that uses the AMS eigensolver:
Step module: Step→Create: Frequency: Eigensolver: AMS,
toggle Project damping operators
Defining viscous damping
Abaqus allows you to choose a particular source of viscous damping, to add several sources, or to exclude
viscous damping effects.
Defining material/element viscous damping
You can choose to model the viscous damping matrix,
, by using material damping properties
and/or damping elements (such as dashpot or mass elements). The viscous, mass, and/or stiffness
proportional damping matrix will include the material Rayleigh damping factors,
and
, as
well as the element-oriented damping factor,
(e.g., for mass elements). The material/element-based
viscous damping matrix can be written as
6.3.1–10
Abaqus Version 5.8 ID:
Printed on:
DYNAMIC ANALYSIS OVERVIEW
where
represents the viscous damping matrix for elements such as dashpots. In mode-based
procedures projection of
into the eigenmodes results in a non-diagonal matrix.
Input File Usage:
Use the following option to specify material viscous damping for elements with
mechanical degrees of freedom:
, BETA=
*DAMPING, ALPHA=
Use the following option to specify material viscous damping for acoustic
elements:
Abaqus/CAE Usage:
*ACOUSTIC MEDIUM, VOLUMETRIC DRAG
Property module: material editor: Mechanical→Damping:
Alpha:
or Beta:
Property module: material editor: Other→Acoustic Medium:
Volumetric Drag
Defining global viscous damping
You can supply global mass and stiffness proportional viscous damping factors,
and
respectively, to create the global damping matrix using the global model mass and stiffness matrices,
and , respectively:
,
These parameters can be specified for the entire model (default), for the mechanical degree of freedom
field (displacements and rotations) only, or for the acoustic field only.
Input File Usage:
Use the following option to specify global viscous damping:
Abaqus/CAE Usage:
, BETA=
*GLOBAL DAMPING, ALPHA=
Global viscous damping is not supported in Abaqus/CAE.
Defining viscous modal damping
Rayleigh damping introduces a damping matrix,
where
is the mass matrix of the model,
factors that you define.
, defined as
is the stiffness matrix of the model, and
6.3.1–11
Abaqus Version 5.8 ID:
Printed on:
and
are
DYNAMIC ANALYSIS OVERVIEW
In Abaqus/Standard you can define
becomes
and
independently for each mode, so that the above equation
(no sum on M)
where the subscript M refers to the mode number and
stiffness terms associated with the Mth mode.
Input File Usage:
,
, and
are the damping, mass, and
Use the following option to define Rayleigh damping by specifying mode
numbers:
*MODAL DAMPING, RAYLEIGH, DEFINITION=MODE NUMBERS
Use the following option to define Rayleigh damping by specifying a frequency
range:
Abaqus/CAE Usage:
*MODAL DAMPING, RAYLEIGH, DEFINITION=FREQUENCY RANGE
Use the following input to define Rayleigh damping by specifying mode
numbers:
Step module: Create Step: Linear perturbation: any valid step
type: Damping: Specify damping over ranges of: Modes,
Rayleigh: Use Rayleigh damping data
Use the following input to define Rayleigh damping by specifying frequency
ranges:
Step module: Create Step: Linear perturbation: any valid step
type: Damping: Specify damping over ranges of: Frequencies,
Rayleigh: Use Rayleigh damping data
Defining viscous modal damping as a fraction of the critical damping
You can also specify the damping in each eigenmode in the model or for the specified frequency as a
fraction of the critical damping. Critical damping is defined as
where m is the mass of the system and k is the stiffness of the system. Typical values of the fraction
of critical damping, , are from 1% to 10% of critical damping,
; but Abaqus/Standard accepts any
positive value. The critical damping factors can be changed from step to step.
Input File Usage:
Use the following option to define the fraction of critical damping by specifying
mode numbers:
*MODAL DAMPING, MODAL=DIRECT,
DEFINITION=MODE NUMBERS
Use the following option to define the fraction of critical damping by specifying
a frequency range:
6.3.1–12
Abaqus Version 5.8 ID:
Printed on:
DYNAMIC ANALYSIS OVERVIEW
*MODAL DAMPING, MODAL=DIRECT,
DEFINITION=FREQUENCY RANGE
Abaqus/CAE Usage:
Use the following input to define the fraction of critical damping by specifying
mode numbers:
Step module: Create Step: Linear perturbation: any valid step
type: Damping: Specify damping over ranges of: Modes,
Direct modal: Use direct damping data
Use the following input to define the fraction of critical damping by specifying
frequency ranges:
Step module: Create Step: Linear perturbation: any valid step
type: Damping: Specify damping over ranges of: Frequencies,
Direct modal: Use direct damping data
Viscous modal damping for uncoupled structural-acoustic frequency extractions
For uncoupled structural-acoustic frequency extractions performed using the AMS eigensolver, you can
apply different damping to the structural and acoustic modes. This technique can be used only when
damping is specified for a range of frequencies.
Input File Usage:
Use the following option to apply the specified damping to only the structural
modes:
*MODAL DAMPING, MODAL=DIRECT,
DEFINITION=FREQUENCY RANGE, FIELD=MECHANICAL
Use the following option to apply the specified damping to only the acoustic
modes:
*MODAL DAMPING, MODAL=DIRECT,
DEFINITION=FREQUENCY RANGE, FIELD=ACOUSTIC
Use the following option to apply the specified damping to both structural and
acoustic modes (default):
*MODAL DAMPING, MODAL=DIRECT,
DEFINITION=FREQUENCY RANGE, FIELD=ALL
Abaqus/CAE Usage:
The ability to specify different damping for structural and acoustic modes is not
supported in Abaqus/CAE.
Controlling the sources of viscous damping
The material/element and global viscous damping sources can be controlled at the step level; controls
are not available for modal damping. If both the material/element and global viscous damping matrices
are supplied, both will be used as a combined damping matrix unless you request that only the element
or global damping factor be used. The combined material/element and global viscous damping is
6.3.1–13
Abaqus Version 5.8 ID:
Printed on:
DYNAMIC ANALYSIS OVERVIEW
Input File Usage:
Use the following option to activate only the material/element viscous damping
matrix:
*DAMPING CONTROLS, VISCOUS=ELEMENT
Use the following option to activate only the global viscous damping matrix:
*DAMPING CONTROLS, VISCOUS=FACTOR
Use the following option to activate the combined material/element and global
viscous damping matrix:
Abaqus/CAE Usage:
*DAMPING CONTROLS, VISCOUS=COMBINED
Damping controls are not supported in Abaqus/CAE.
Excluding viscous damping effects
You can choose to exclude the effects of viscous damping altogether at the step level.
Input File Usage:
Use the following option to exclude the viscous damping matrix:
Abaqus/CAE Usage:
*DAMPING CONTROLS, VISCOUS=NONE
Damping controls are not supported in Abaqus/CAE.
Defining structural damping
Abaqus allows you to choose a particular source of structural damping, to add several sources, or to
exclude structural damping effects.
Defining material/element structural damping
The material/element structural damping matrix (that represents the imaginary stiffness and is
proportional to forces or displacements) is defined as
where represents the material structural damping,
represents the structural damping coefficient for
elements such as springs with complex stiffnesses and connectors, and
is the real element stiffness
matrix. In mode-based procedures the projection of
onto the mode shapes results in a full modal
damping matrix. When using SIM-based modal procedures, the projected material and element damping
matrix may be combined with global and modal damping (see “Defining and using both global and modal
diagonal damping,” below). Material/element structural damping is not available for acoustic elements.
Input File Usage:
Use the following option to specify material structural damping:
Abaqus/CAE Usage:
*DAMPING, STRUCTURAL=
Property module: material editor: Mechanical→Damping: Structural:
6.3.1–14
Abaqus Version 5.8 ID:
Printed on:
DYNAMIC ANALYSIS OVERVIEW
Defining global structural damping
You can define the global structural damping factor,
, to get
Global structural damping can be specified for the entire model (default), for the mechanical degree of
freedom field (displacements and rotations) only, or for the acoustic field only.
Input File Usage:
Use the following option to specify global structural damping:
Abaqus/CAE Usage:
*GLOBAL DAMPING, STRUCTURAL=
Global structural damping is not supported in Abaqus/CAE.
Defining structural modal damping
Structural damping assumes that the damping forces are proportional to the forces caused by stressing
of the structure and are opposed to the velocity (see “Structural damping” in “Material damping,”
Section 26.1.1, for more information). This form of damping can be used only when the displacement
and velocity are exactly 90° out of phase, as in steady-state and random response analyses where the
excitation is purely sinusoidal.
Structural damping can be defined as diagonal modal damping for mode-based steady-state dynamic
and random response analyses.
Input File Usage:
Use the following option to define structural damping by specifying mode
numbers:
*MODAL DAMPING, STRUCTURAL, DEFINITION=MODE NUMBERS
Use the following option to define structural damping by specifying a frequency
range:
*MODAL DAMPING, STRUCTURAL,
DEFINITION=FREQUENCY RANGE
Abaqus/CAE Usage:
Use the following input to define structural damping by specifying mode
numbers:
Step module: Create Step: Linear perturbation: any valid step
type: Damping: Specify damping over ranges of: Modes,
Structural: Use structural damping data
Use the following input to define structural damping by specifying frequency
ranges:
Step module: Create Step: Linear perturbation: any valid step
type: Damping: Specify damping over ranges of: Frequencies,
Structural: Use structural damping data
6.3.1–15
Abaqus Version 5.8 ID:
Printed on:
DYNAMIC ANALYSIS OVERVIEW
Controlling the sources of structural damping
The material/element and global structural damping sources can be controlled at the step level; controls
are not available for modal damping. If both the material/element and global structural damping matrices
are supplied, both will be combined unless you request that only the element or global damping factor
be used. The combined structural damping matrix is
Input File Usage:
Use the following option to activate only the material/element structural
damping matrix:
*DAMPING CONTROLS, STRUCTURAL=ELEMENT
Use the following option to activate only the global structural damping matrix:
*DAMPING CONTROLS, STRUCTURAL=FACTOR
Use the following option to activate the combined material/element and global
structural damping matrix:
Abaqus/CAE Usage:
*DAMPING CONTROLS, STRUCTURAL=COMBINED
Damping controls are not supported in Abaqus/CAE.
Excluding structural damping effects
You can choose to exclude the effects of structural damping altogether at the step level.
Input File Usage:
Use the following option to exclude structural damping matrix:
Abaqus/CAE Usage:
*DAMPING CONTROLS, STRUCTURAL=NONE
Damping controls are not supported in Abaqus/CAE.
Defining both viscous and structural damping
The imaginary contribution to the frequency domain dynamics equation, which represents the effect of
damping, may include both viscous and structural damping and can be written as
where
is the forcing frequency.
Defining composite modal damping
Composite modal damping allows you to define a damping factor for each material in the model as a
fraction of critical damping. These factors are then combined into a damping factor for each mode as
weighted averages of the mass matrix associated with each material:
6.3.1–16
Abaqus Version 5.8 ID:
Printed on:
DYNAMIC ANALYSIS OVERVIEW
(no sum over )
where
is the critical damping fraction used in mode ,
is the critical damping fraction defined for
material m,
is the mass matrix associated with material m,
is the eigenvector of mode , and
is the generalized mass associated with mode :
(no sum on )
If you specify composite modal damping, Abaqus calculates the damping coefficients
in
the eigenfrequency extraction step from the damping factors
that you defined for each material.
Composite modal damping can be defined only by specifying mode numbers; it cannot be defined by
specifying a frequency range.
Input File Usage:
Use both of the following options:
Abaqus/CAE Usage:
*DAMPING, COMPOSITE=
*MODAL DAMPING, MODAL=COMPOSITE
Property module: material editor: Mechanical→Damping: Composite:
Step module: Create Step: Linear perturbation: any valid step type:
Damping: Composite modal: Use composite damping data
Defining global damping for acoustic fields
If your model contains acoustic elements, Abaqus applies any specified global damping to both the
acoustic fields and the structural fields in the model by default. If desired, you can specify that a global
damping definition applies only to the acoustic fields or only to the displacement and rotation fields.
Input File Usage:
Use the following option to apply global damping to all of the displacement,
rotation, and acoustic fields in a model:
*GLOBAL DAMPING, FIELD=ALL (default)
Use the following option to apply global damping only to the acoustic fields in
a model:
*GLOBAL DAMPING, FIELD=ACOUSTIC
Use the following option to apply global damping only to the displacement and
rotation fields in a model:
Abaqus/CAE Usage:
*GLOBAL DAMPING, FIELD=MECHANICAL
Global damping is not supported in Abaqus/CAE.
Defining and using both global and modal diagonal damping
Mode-based procedures—such as steady-state dynamics, transient modal dynamic, response spectrum,
and random response analyses—can also use a step-dependent, modal damping definition that is specified
per eigenmode. When multiple modal damping definitions are used with different damping types, the
6.3.1–17
Abaqus Version 5.8 ID:
Printed on:
DYNAMIC ANALYSIS OVERVIEW
damping is additive. If the same damping type is specified more than once, the last specification is used.
If modal damping is used with global damping, both types of damping will contribute to the damping
matrix.
Damping controls have no effect on modal damping. If damping controls are used to exclude certain
global damping effects in a step, all modal damping effects are still included in the step. To exclude modal
damping, the damping definition must be specifically removed from the step definition.
6.3.1–18
Abaqus Version 5.8 ID:
Printed on:
IMPLICIT DYNAMIC ANALYSIS
6.3.2
IMPLICIT DYNAMIC ANALYSIS USING DIRECT INTEGRATION
Products: Abaqus/Standard
Abaqus/CAE
References
•
•
•
•
“Defining an analysis,” Section 6.1.2
“Dynamic analysis procedures: overview,” Section 6.3.1
*DYNAMIC
“Configuring a dynamic, implicit procedure” in “Configuring general analysis procedures,”
Section 14.11.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual
Overview
A direct-integration dynamic analysis in Abaqus/Standard:
•
•
•
must be used when nonlinear dynamic response is being studied;
can be fully nonlinear (general dynamic analysis) or can be based on the modes of the linear system
(subspace projection method); and
can be used to study a variety of applications, including:
– dynamic responses requiring transient fidelity and involving minimal energy dissipation;
– dynamic responses involving nonlinearity, contact, and moderate energy dissipation; and
– quasi-static responses in which considerable energy dissipation provides stability and improved
convergence behavior for determining an essentially static solution.
General dynamic analysis
General nonlinear dynamic analysis in Abaqus/Standard uses implicit time integration to calculate the
transient dynamic or quasi-static response of a system. The procedure can be applied to a broad range of
applications calling for varying numerical solution strategies, such as the amount of numerical damping
required to obtain convergence and the way in which the automatic time incrementation algorithm
proceeds through the solution. Typical dynamic applications fall into three categories:
•
•
Transient fidelity applications, such as an analysis of satellite systems, require minimal energy
dissipation. In these applications small time increments are taken to accurately resolve the
vibrational response of the structure, and numerical energy dissipation is kept at a minimum. These
stringent requirements tend to degrade convergence behavior for simulations involving contact or
nonlinearities.
Moderate dissipation applications encompass a more general range of dynamic events in which a
moderate amount of energy is dissipated by plasticity, viscous damping, or other effects. Typical
applications include various insertion, impact, and forming analyses. The response of these
structures can be either monotonic or nonmonotonic. Accurate resolution of high-frequency
6.3.2–1
Abaqus Version 5.8 ID:
Printed on:
IMPLICIT DYNAMIC ANALYSIS
•
vibrations is usually not of interest in these applications. Some numerical energy dissipation
tends to reduce solution noise and improve convergence behavior in these applications without
significantly degrading solution accuracy.
Quasi-static applications are primarily interested in determining a final static response. These
problems typically show monotonic behavior, and inertia effects are introduced primarily to
regularize unstable behavior. For example, the statically unstable behavior may be due to
temporarily unconstrained rigid body modes or “snap-through” phenomena. Large time increments
are taken when possible to obtain the final solution at minimal computational cost. Considerable
numerical dissipation may be required to obtain convergence during certain stages of the loading
history.
An example of a transient fidelity application is available in “Modeling of an automobile
suspension,” Section 2.1.7 of the Abaqus Example Problems Manual. An analysis that includes both
a moderate dissipation step and a quasi-static step is described in “Impact analysis of a pawl-ratchet
device,” Section 2.1.17 of the Abaqus Example Problems Manual.
Specifying the application type
Based on the classifications listed above, you should indicate the type of application you are studying
when performing a general dynamic analysis. Abaqus/Standard assigns numerical settings based on
your classification of the application type, and this classification can significantly affect a simulation. In
some cases accurate results can be obtained with more than one application-type setting, in which case
analysis efficiency should be considered. A general trend is that—among the three classifications—the
high-dissipation quasi-static classification tends to result in the best convergence behavior and the lowdissipation transient fidelity classification tends to have the highest likelihood of convergence difficulty.
Input File Usage:
Use the following option for transient fidelity applications:
*DYNAMIC, APPLICATION=TRANSIENT FIDELITY (default
for models without contact)
Use the following option for moderate dissipation applications:
*DYNAMIC, APPLICATION=MODERATE DISSIPATION
(default for models with contact)
Use the following option for quasi-static applications:
Abaqus/CAE Usage:
*DYNAMIC, APPLICATION=QUASI-STATIC
Step module: Create Step: General: Dynamic, Implicit
The application type is specified in the Edit Step dialog box:
Basic: Application: Transient fidelity, Moderate dissipation,
Quasi-static, or Analysis product default
Diagnostics for modeling errors associated with mass properties
Accurate representation of inertia properties is necessary for accurate dynamic analyses. In some cases
Abaqus/Standard provides diagnostic messages when it detects likely modeling errors associated with the
6.3.2–2
Abaqus Version 5.8 ID:
Printed on:
IMPLICIT DYNAMIC ANALYSIS
specification of inertia properties. The most common way of specifying inertia properties is with material
densities. Abaqus/Standard issues a warning message to the data (.dat) file if a material density is
omitted in a dynamic analysis (this warning is not issued if the density is zero only for certain values of
temperature or field variables). Other methods of specifying inertia properties include:
•
•
point mass and rotary inertia definitions, and
constraining nodes without inertia themselves to nodes having inertia properties defined.
In some circumstances Abaqus/Standard attempts to solve systems of equations involving effective
inversion of the global mass matrix to directly adjust velocities and accelerations during a general
dynamic analysis as described in “Initial conditions” and “Intermittent contact/impact” below. These
additional velocity and acceleration adjustments occur by default only for transient fidelity application
types as defined above. If the global mass matrix is found to be singular, Abaqus/Standard issues an
error message by default, because singular mass is an indication that the mass properties are not realistic
due to a modeling error.
Diagnostic feedback specific to the global mass matrix being singular is typically not provided for
quasi-static and moderate dissipation application types, although warnings typically are issued regarding
the lack of material density. Singular mass is not necessarily detrimental to a quasi-static analysis. For
example, it would be reasonable to only define inertia properties (such as density) in components or
regions with temporary static instabilities (such as initially unconstrained rigid body modes that become
constrained once contact occurs) in a quasi-static analysis.
You can control the course of action Abaqus/Standard takes upon detecting a singular global mass
matrix.
Input File Usage:
Use the following default option to issue an error message and stop execution
if a singular global mass matrix is detected when calculating velocity and
acceleration adjustments:
*DYNAMIC, SINGULAR MASS=ERROR
Use the following option to issue a warning message and avoid velocity and
acceleration adjustments (i.e., continue time integration using current velocities
and accelerations) if a singular global mass matrix is detected:
*DYNAMIC, SINGULAR MASS=WARNING
Use the following option to adjust velocities and accelerations even if a singular
mass matrix is detected. This setting can result in large, non-physical velocity
and/or acceleration adjustments, which can, in turn, cause poor time integration
solutions and artificial convergence difficulties. This approach is not generally
recommended; it should be used only in special cases when the analyst has a
thorough understanding of how to interpret results obtained in this way.
Abaqus/CAE Usage:
*DYNAMIC, SINGULAR MASS=MAKE ADJUSTMENTS
The default singular mass setting cannot be modified in Abaqus/CAE.
6.3.2–3
Abaqus Version 5.8 ID:
Printed on:
IMPLICIT DYNAMIC ANALYSIS
Numerical details
The effect of the application-type classification on numerical aspects of general dynamic analyses
is described below. In most cases the settings determined by the application type are sufficient to
successfully perform an analysis. However, detailed user controls are provided to override settings on
an individual basis.
Time integration methods
Abaqus/Standard uses the Hilber-Hughes-Taylor time integration by default unless you specify that the
application type is quasi-static. The Hilber-Hughes-Taylor operator is an extension of the Newmark
-method. Numerical parameters associated with the Hilber-Hughes-Taylor operator are tuned
differently for moderate dissipation and transient fidelity applications (as discussed later in this section).
The backward Euler operator is used by default if the application classification is quasi-static.
These time integration operators are implicit, which means that the operator matrix must be
inverted and a set of simultaneous nonlinear dynamic equilibrium equations must be solved at each time
increment. This solution is done iteratively using Newton’s method. The principal advantage of these
operators is that they are unconditionally stable for linear systems; there is no mathematical limit on
the size of the time increment that can be used to integrate a linear system. An unconditionally stable
integration operator is of great value when studying structural systems because a conditionally stable
integration operator (such as that used in the explicit method) can lead to impractically small time steps
and, therefore, a computationally expensive analysis.
Marching through a simulation with a finite time increment size generally introduces some
degree of numerical damping. This damping differs from the material damping discussed in “Material
damping,” Section 26.1.1 (and in many cases these two forms of damping will work well together).
The amount of damping associated with the time integration varies among the operator types (for
example, the backward Euler operator tends to be more dissipative than the Hilber-Hughes-Taylor
operator) and in many cases (such as with the Hilber-Hughes-Taylor operator) depends on settings
of numerical parameters associated with the operator. The ability of the operator to effectively treat
contact conditions is often of considerable importance with respect to their usefulness. For example,
some changes in contact conditions can result in “negative damping” (nonphysical energy source) for
many time integrators, which can be very undesirable.
It is possible to override the time integrator implied by the application-type classification; for
example, you can perform a moderate dissipation dynamic analysis using the backward Euler integrator.
Changing the default integrator is not generally recommended but may be useful in special cases.
Input File Usage:
Use the following option to use the Hilber-Hughes-Taylor integrator with
default integrator parameter settings corresponding to those for transient
fidelity applications:
*DYNAMIC, TIME INTEGRATOR=HHT-TF
Use the following option to use the Hilber-Hughes-Taylor integrator with
default integrator parameter settings corresponding to those for moderate
dissipation applications:
*DYNAMIC, TIME INTEGRATOR=HHT-MD
6.3.2–4
Abaqus Version 5.8 ID:
Printed on:
IMPLICIT DYNAMIC ANALYSIS
Use the following option to use the backward Euler integrator:
Abaqus/CAE Usage:
*DYNAMIC, TIME INTEGRATOR=BWE
The default time integrator cannot be modified in Abaqus/CAE.
Additional control over integrator parameters
Additional user controls enable modifications to settings of numerical parameters associated with the
Hilber-Hughes-Taylor operator (see Hilber, Hughes, and Taylor (1977) for descriptions of the numerical
parameters). The default parameter settings depend on the specified application type, as indicated in
Table 6.3.2–1 (see Czekanski, El-Abbasi, and Meguid (2001) for the basis of these settings).
Default parameters for the Hilber-Hughes-Taylor integrator.
Table 6.3.2–1
Application
Parameter
Transient Fidelity
Moderate Dissipation
–0.05
–0.41421
0.275625
0.5
0.55
0.91421
These parameters can be adjusted or modified individually if the Hilber-Hughes-Taylor operator is
being used. If the default settings of these parameters correspond to the transient fidelity settings shown
in Table 6.3.2–1 and you explicitly modify the parameter alone, the other parameters will be adjusted
automatically to
and
. This relation provides control of the numerical
damping associated with the time integrator while preserving desirable characteristics of the integrator.
The numerical damping grows with the ratio of the time increment to the period of vibration of a mode.
Negative values of provide damping; whereas
results in no damping (energy preserving) and
is exactly the trapezoidal rule (sometimes called the Newmark -method, with
and
).
The setting
provides the maximum numerical damping. It gives a damping ratio of about 6%
when the time increment is 40% of the period of oscillation of the mode being studied. Allowable values
of , , and are:
,
,
.
Input File Usage:
Abaqus/CAE Usage:
*DYNAMIC, ALPHA= , BETA= , GAMMA=
Only the parameter can be modified in Abaqus/CAE:
Step module: Create Step: General: Dynamic, Implicit:
Other: Alpha: Specify:
Default incrementation schemes
Automatic time incrementation is used by default for nonlinear dynamic procedures. The main
factors used to control adjustments to the time increment size for an implicit dynamic procedure are
the convergence behavior of the Newton iterations and the accuracy of the time integration. The
6.3.2–5
Abaqus Version 5.8 ID:
Printed on:
IMPLICIT DYNAMIC ANALYSIS
time increment size may vary considerably during an analysis. Details of the time increment control
algorithm depend on the type of dynamic application you are studying.
The following factors are considered by default in the time increment control algorithm if you
specify a quasi-static–type application (the same factors control the time increment size for purely static
analyses):
•
•
The time increment size is reduced if an increment appears to be diverging or if the convergence
rate is slow.
The time increment size is fairly aggressively increased if rapid convergence occurs in previous
increments.
Analyses for moderate dissipation-type applications also use these same factors, as well as a default
upper bound on the time increment size equal to one-tenth of the step duration.
The following factors are considered by default in the time increment control algorithm if you
specify a transient fidelity–type application:
•
•
•
•
•
The time increment size is reduced if an increment appears to be diverging or if the convergence
rate is slow.
The time increment size is reduced if changes in contact status are detected during the first
attempt of processing an increment. The new increment size is set such that the end of the
increment corresponds to the average time of the contact status changes that were detected with the
previous increment size. (In such cases an additional very small time increment is used to enforce
compatibility of velocities and accelerations across active contact interfaces.)
The time increment size is reduced if the half-increment residual (out-of-balance force) halfway
through a time increment exceeds the half-increment residual tolerance, which is 10,000 times the
time average force for a contact analysis or 1000 times the time average force for an analysis without
contact.
The time increment is gradually increased if rapid convergence occurs in previous increments.
The upper bound for the time increment size is equal to 1/100 of the step duration.
Intermittent contact/impact
The second and third factors described in the preceding list often result in very small time increment sizes
for contact simulations that are performed as a transient fidelity application (and the time increment size
tends to remain small due to the fourth factor). This problem can be avoided by specifying a different
application type or by using more detailed user controls, as discussed below.
General settings for the time increment controls
A high level user control over which factors are considered by the time increment control algorithm can
be used to override the defaults implied by the specified application type for the analysis. Regardless of
the application type you have specified, you can enforce time increment controls associated with either
quasi-static applications or transient fidelity applications.
Input File Usage:
Use the following option to obtain the aggressive time increment control
settings associated with quasi-static applications:
6.3.2–6
Abaqus Version 5.8 ID:
Printed on:
IMPLICIT DYNAMIC ANALYSIS
*DYNAMIC, INCREMENTATION=AGGRESSIVE
Use the following option to obtain the more conservative time increment control
settings associated with transient fidelity applications:
Abaqus/CAE Usage:
*DYNAMIC, INCREMENTATION=CONSERVATIVE
The default time incrementation control settings cannot be modified in
Abaqus/CAE.
Controlling the half-increment residual
Controls associated with the half-increment residual tolerance are provided for tuning the time
incrementation. These controls are intended for advanced users and typically do not need to be
modified.
Input File Usage:
Use the following option to specify that no check of the half-increment residual
should be performed:
*DYNAMIC, NOHAF
Use the following option to specify the half-increment residual tolerance as a
scale factor of the time average force (moment):
*DYNAMIC, HALFINC SCALE FACTOR=scale factor
Use the following option to directly specify the half-increment residual force
tolerance (the half-increment residual moment tolerance is the half-increment
residual force tolerance times the characteristic element length automatically
calculated):
Abaqus/CAE Usage:
*DYNAMIC, HAFTOL=tolerance
Use the following option to specify that no check of the half-increment residual
should be performed:
Step module: Create Step: General: Dynamic, Implicit: Incrementation:
toggle on Suppress half-increment residual calculation
Use the following option to specify the half-increment residual tolerance as a
scale factor of the time average force (moment):
Step module: Create Step: General: Dynamic, Implicit: Incrementation:
Half-increment Residual: Specify scale factor: scale factor
Use the following option to specify the half-increment residual force tolerance
directly:
Step module: Create Step: General: Dynamic, Implicit: Incrementation:
Half-increment Residual: Specify value: tolerance
Controlling incrementation involving contact
By default, specifying a transient fidelity application typically results in reduced time increment sizes
upon changes in contact status. An extra time increment with a very small size is subsequently performed
6.3.2–7
Abaqus Version 5.8 ID:
Printed on:
IMPLICIT DYNAMIC ANALYSIS
to enforce compatibility of velocities and accelerations across active contact interfaces. Direct user
control over these incrementation aspects is available.
Input File Usage:
Use the following option to avoid automatically cutting back the increment size
and enforcing velocity and acceleration compatibility in the contact region upon
changes in contact status:
*DYNAMIC, IMPACT=NO
Use the following option to automatically cut back the increment size and
enforce velocity and acceleration compatibility in the contact region upon
changes in contact status:
*DYNAMIC, IMPACT=AVERAGE TIME
Use the following option to enforce velocity and acceleration compatibility in
the contact region without automatically cutting back the increment size upon
changes in contact status:
Abaqus/CAE Usage:
*DYNAMIC, IMPACT=CURRENT TIME
The default contact incrementation scheme cannot be modified in Abaqus/CAE.
Direct time incrementation
You may directly specify the time increment size to be used. This approach is not generally recommended
but may be useful in special cases. The analysis will terminate if convergence tolerances are not satisfied
within the maximum number of iterations allowed.
It is possible to ignore convergence tolerances: the solution to an increment is accepted after
the specified maximum number of iterations allowed even if convergence tolerances are not satisfied.
Ignoring convergence tolerances can result in highly nonphysical results and is not recommended
except by analysts with a thorough understanding of how to interpret results obtained this way.
Input File Usage:
Use the following option to directly specify the time increment:
*DYNAMIC, DIRECT
Use the following option to ignore convergence tolerances after the maximum
number of iterations is reached:
Abaqus/CAE Usage:
*DYNAMIC, DIRECT=NO STOP
Use the following option to specify the time increment directly:
Step module: Create Step: General: Dynamic, Implicit:
Incrementation: Fixed
Use the following option to ignore convergence tolerances after the maximum
number of iterations is reached:
Step module: Create Step: General: Dynamic, Implicit: Other: Accept
solution after reaching maximum number of iterations
6.3.2–8
Abaqus Version 5.8 ID:
Printed on:
IMPLICIT DYNAMIC ANALYSIS
Default amplitude for loads
Loads such as applied forces or pressures are ramped on by default if you have selected the quasi-static
application classification; such ramping tends to enhance robustness because the load increment size is
proportional to the time increment size. For example, if the Newton iterations are not able to converge
for a particular time increment size, the automatic time incrementation algorithm will reduce the time
increment size and restart the Newton iterations with a smaller load incremental considered.
For the other application classifications the dynamic procedure applies loads with a step function by
default such that the full load is applied in the first increment of the step (regardless of the time increment
size) and the load magnitude remains constant over each step. Thus, if the first increment is unable to
converge with the original time increment size, reducing the time increment will not reduce the load
increment by default. In some cases the convergence behavior will still improve upon reducing the time
increment because the regularizing effect of inertia on the integration operators is inversely proportional
to the square of the time increment size. See “Defining an analysis,” Section 6.1.2, for more information
on default amplitude types for the various procedures and how to override the default.
The “subspace projection” method
The alternative approach provided in Abaqus/Standard for nonlinear dynamic problems is the “subspace
projection” method. See “Subspace dynamics,” Section 2.4.3 of the Abaqus Theory Manual, for
the theory behind this method. In this method the modes of the linear system are extracted in an
eigenfrequency extraction step (“Natural frequency extraction,” Section 6.3.5) prior to the dynamic
analysis and are used as a small set of global basis vectors to develop the solution. These modes will
include eigenmodes and, if activated in the eigenfrequency extraction step, residual modes. The method
works well when the system exhibits mildly nonlinear behavior, such as small regions of plastic yielding
or rotations that are not small but not too large.
This method can be very effective. As with the other direct integration methods, it is more expensive
in terms of computer time than the modal methods of purely linear dynamic analysis, but it is often
significantly less expensive than the direct integration of all of the equations of motion of the model.
However, since the subspace projection method is based on the modes of the system, it will not be
accurate if there is extreme nonlinear response that cannot be modeled well by the modes that form the
basis of the solution.
Input File Usage:
Abaqus/CAE Usage:
*DYNAMIC, SUBSPACE
Step module: Create Step: General: Dynamic, Subspace
Selecting the modes on which to project
You can select the modes of the system on which the subspace projection will be performed. The mode
numbers can be listed individually, or they can be generated automatically. If you choose not to select
the modes, all modes extracted in the prior frequency extraction step, including residual modes if they
were activated, are used in the subspace projection.
6.3.2–9
Abaqus Version 5.8 ID:
Printed on:
IMPLICIT DYNAMIC ANALYSIS
Input File Usage:
Abaqus/CAE Usage:
Use one of the following options:
*SELECT EIGENMODES
*SELECT EIGENMODES, GENERATE
Step module: Create Step: General: Dynamic, Subspace: Basic:
Number of modes to use: All or Specify
Numerical implementation
The subspace projection method is implemented in Abaqus/Standard using the explicit (central
difference) operator to integrate the equations of motion written in terms of the modes of the linear
system. This integration method is particularly effective here because the modes are orthogonal with
respect to the mass matrix so that the projected system always has a diagonal mass matrix.
A fixed time increment is used: this increment is the smaller of the time increment that you specify
or 80% of the stable time increment, which is
for the linear system, where
is the highest
circular frequency of the modes that are used as the basis of the solution. The 80% factor is intended as
a safety factor so that any increase in this highest frequency caused by nonlinear effects is less likely
to cause the integration to become unstable. The 80% is rather arbitrary; in some cases it may be
nonconservative. You must monitor the response—for example, the energy balance—to ensure that
the time increment is not causing instability. Instability is a concern if the nonlinearities can stiffen
the system significantly, although in many practical cases such stiffening effects are more prominent in
increasing the lower frequencies of the system than in affecting the highest frequencies that are likely to
be retained to represent the dynamic behavior accurately.
Accuracy of the subspace projection method
The effectiveness of the subspace projection method depends on the value of the modes of the linear
system as a set of global interpolation functions for the problem, which is a matter of judgment on your
part—the same sort of judgment as required when deciding if a particular mesh of finite elements is
sufficient. The method is valuable for mildly nonlinear systems and for cases where it is easy to extract
enough modes that you can be confident that they describe the system adequately.
If nonlinear geometric effects are considered in the subspace dynamics step, it is possible to perform
a dynamic simulation for some time, reextract the modes on the current stressed geometry by using
another frequency extraction step, and then continue the analysis with the new modes as the subspace
basis system. This procedure can improve the accuracy of the method in some cases.
Material damping
You can introduce Rayleigh damping, as explained in “Material damping,” Section 26.1.1. This damping
will act in addition to numerical damping associated with the time integrator (discussed previously).
Input File Usage:
Abaqus/CAE Usage:
*DAMPING, ALPHA= , BETA=
Property module: material editor: Mechanical→Damping: Alpha and Beta
6.3.2–10
Abaqus Version 5.8 ID:
Printed on:
IMPLICIT DYNAMIC ANALYSIS
Initial conditions
“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1, describes all of the
available initial conditions. Initial velocities must be defined in global directions regardless of the use
of nodal transformations (see “Transformed coordinate systems,” Section 2.1.5).
If initial velocities are specified at nodes for which displacement boundary conditions are also
specified, the initial velocities will be ignored at these nodes. However, if a displacement boundary
condition refers to an amplitude curve with an analytically defined time variation (i.e., excluding the
piecewise linear tabular and equally spaced definitions), Abaqus/Standard will compute the initial
velocity for the nodes involved in the boundary condition as the time derivative (evaluated at time zero)
of the analytic variation.
When initial velocities are specified for dynamic analysis, they should be consistent with all of
the constraints on the model, especially time-dependent boundary conditions. Abaqus/Standard will
ensure that initial velocities are consistent with boundary conditions and with multi-point and equation
constraints but will not check for consistency with internal constraints such as incompressibility of the
material. In case of a conflict, boundary conditions and multi-point constraints take precedence over
initial conditions.
Specified initial velocities are used in a dynamic step only if it is the first dynamic step in an analysis.
If a dynamic step is not the first dynamic step and there is an immediately preceding dynamic step, the
velocities from the end of the preceding step are used as the initial velocities for the current step. If a
dynamic step is not the first dynamic step and the immediately preceding step is not a dynamic step, zero
initial velocities are assumed for the current step.
Controlling calculation of accelerations at the beginning of a dynamic step
By default, Abaqus/Standard will calculate accelerations at the beginning of the dynamic step for
transient fidelity applications. You can choose to bypass these acceleration calculations, in which
case Abaqus/Standard will assume that initial accelerations for the current step are zero unless there
is an immediately preceding dynamic step. If the immediately preceding step is also a dynamic step,
bypassing the acceleration calculations will cause Abaqus/Standard to use the accelerations from the end
of the previous step to continue the new step. It is appropriate to bypass the acceleration calculations if
the loading has not changed suddenly at the start of the dynamic step, but it is not correct if the loading
at the beginning of the first increment is significantly different from that at the end of the previous
step. In cases where large loads are applied suddenly, high-frequency noise due to the bypass of the
acceleration calculations may greatly increase the half-increment residual.
Input File Usage:
Abaqus/CAE Usage:
*DYNAMIC, INITIAL=NO
Step module: Create Step: General: Dynamic, Implicit: Other: Initial
acceleration calculations at beginning of step: Bypass
Boundary conditions
Boundary conditions can be applied to any of the displacement or rotation degrees of freedom (1–6), to
warping degree of freedom 7 in open-section beam elements, to fluid pressure degree of freedom 8 for
6.3.2–11
Abaqus Version 5.8 ID:
Printed on:
IMPLICIT DYNAMIC ANALYSIS
hydrostatic fluid elements, or to acoustic pressure degree of freedom 8 for acoustic elements (“Boundary
conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1).
Amplitude references can be used to prescribe time-varying boundary conditions in a
direct-integration dynamic step. Default amplitude variations are described in “Defining an analysis,”
Section 6.1.2.
In direct time integration dynamic analysis, when a node with a prescribed motion is used in an
equation constraint or a multi-point constraint to control the motion of another node, the equation or
multi-point constraint will be imposed correctly for the displacement and velocity of the dependent node.
However, the acceleration will not be rigorously transmitted to the dependent node, which may cause
some high-frequency noise.
In the subspace projection method it is not currently possible to specify nonzero boundary
conditions directly. Instead, acceleration boundary conditions can be approximated by using appropriate
combinations of large point masses and concentrated loads. At the node where such a boundary
condition is desired, attach a large point mass that is approximatively 105 –106 times larger than the
mass of the original model. In addition, a concentrated load of magnitude equal to the product between
the large point mass and the desired acceleration must be specified in the direction of the approximated
boundary condition. Since the point mass is significantly larger than the mass of the model, the big
mass–concentrated load combination will approximate the desired acceleration in the specified direction
accurately. Boundary conditions other than accelerations must be converted into acceleration histories
before they can be approximated.
Loads
The following loads can be prescribed in a dynamic analysis:
•
•
•
Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6); see
“Concentrated loads,” Section 33.4.2.
Distributed pressure forces or body forces can be applied; see “Distributed loads,” Section 33.4.3.
The distributed load types available with particular elements are described in Part VI, “Elements.”
Distributed pressure or volumetric accelerations (on acoustic elements) can be applied; these are
described in “Acoustic, shock, and coupled acoustic-structural analysis,” Section 6.10.1.
Predefined fields
The following predefined fields can be specified in a dynamic analysis, as described in “Predefined
fields,” Section 33.6.1:
•
•
Although temperature is not a degree of freedom in stress/displacement elements, nodal
temperatures can be specified as a predefined field. Any difference between the applied and
initial temperatures will cause thermal strain if a thermal expansion coefficient is given for
the material (“Thermal expansion,” Section 26.1.2). The specified temperature also affects
temperature-dependent material properties, if any.
The values of user-defined field variables can be specified. These values only affect field-variabledependent material properties, if any.
6.3.2–12
Abaqus Version 5.8 ID:
Printed on:
IMPLICIT DYNAMIC ANALYSIS
Material options
Most material models that describe mechanical behavior are available for use in a dynamic analysis.
The following material properties are not active during a dynamic analysis: thermal properties (except
for thermal expansion), mass diffusion properties, electrical conductivity properties, and pore fluid flow
properties.
Rate-dependent material properties (“Time domain viscoelasticity,” Section 22.7.1; “Hysteresis in
elastomers,” Section 22.8.1; “Rate-dependent yield,” Section 23.2.3; and “Two-layer viscoplasticity,”
Section 23.2.11) can be included in a dynamic analysis.
Elements
Other than generalized axisymmetric elements with twist, any of the stress/displacement elements
in Abaqus/Standard (including those with temperature, pressure, and electrical potential degrees of
freedom) can be used in a dynamic analysis. Inertia effects are ignored in hydrostatic fluid elements,
and the inertia of the fluid in pore pressure elements is not taken into account.
Output
In addition to the usual output variables available in Abaqus/Standard (see “Abaqus/Standard output
variable identifiers,” Section 4.2.1), the following variables are provided specifically for implicit dynamic
analysis:
Variables for a specified element set or for the entire model:
XC
XCn
Current coordinates of the center of mass.
Coordinate n of the center of mass (
UC
UCn
URCn
VC
VCn
VRCn
HC
HCn
HO
HOn
RI
RIij
MASS
VOL
Displacement of the center of mass.
Displacement component n of the center of mass (
).
Rotation component n of the center of mass.
Equivalent rigid body velocity components.
).
Component n of the equivalent rigid body velocity (
Component n of the equivalent rigid body angular velocity (
Angular momentum about the center of mass.
Component n of the angular momentum about the center of mass (
Angular momentum about the origin.
Component n of the angular momentum about the origin (
Rotary inertia about the origin.
-component of the rotary inertia about the origin (
).
Mass.
Current volume.
6.3.2–13
Abaqus Version 5.8 ID:
Printed on:
).
).
).
).
IMPLICIT DYNAMIC ANALYSIS
Input file template
*HEADING
…
*BOUNDARY
Data lines to specify zero-valued boundary conditions
*INITIAL CONDITIONS
Data lines to specify initial conditions
*AMPLITUDE, NAME=name
Data lines to define amplitude variations
**
*STEP (,NLGEOM)
Once NLGEOM is specified, it will be active in all subsequent steps.
*DYNAMIC
Data line to control automatic time incrementation
*BOUNDARY
Data lines to describe zero-valued or nonzero boundary conditions
*CLOAD and/or *DLOAD and/or *INCIDENT WAVE
Data lines to specify loads
*TEMPERATURE and/or *FIELD
Data lines to prescribe predefined fields
*CECHARGE and/or *DECHARGE (if electrical potential degrees of
freedom are active)
Data lines to specify charges
*END STEP
Additional references
•
Czekanski, A., N. El-Abbasi, and S. A. Meguid, “Optimal Time Integration Parameters for
Elastodynamic Contact Problems,” Communications in Numerical Methods in Engineering,
vol. 17, pp. 379–384, 2001.
•
Hilber, H. M., T. J. R. Hughes, and R. L. Taylor, “Improved Numerical Dissipation for Time
Integration Algorithms in Structural Dynamics,” Earthquake Engineering and Structural Dynamics,
vol. 5, pp. 283–292, 1977.
6.3.2–14
Abaqus Version 5.8 ID:
Printed on:
EXPLICIT DYNAMIC ANALYSIS
6.3.3
EXPLICIT DYNAMIC ANALYSIS
Products: Abaqus/Explicit
Abaqus/CAE
References
•
•
•
“Defining an analysis,” Section 6.1.2
*DYNAMIC
“Configuring a dynamic, explicit procedure” in “Configuring general analysis procedures,”
Section 14.11.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual
Overview
An explicit dynamic analysis:
•
is computationally efficient for the analysis of large models with relatively short dynamic response
times and for the analysis of extremely discontinuous events or processes;
•
allows for the definition of very general contact conditions (“Contact interaction analysis:
overview,” Section 35.1.1);
•
uses a consistent, large-deformation theory—models can undergo large rotations and large
deformation;
•
can use a geometrically linear deformation theory—strains and rotations are assumed to be small
(see “Defining an analysis,” Section 6.1.2);
•
can be used to perform an adiabatic stress analysis if inelastic dissipation is expected to generate
heat in the material (see “Adiabatic analysis,” Section 6.5.4);
•
•
can be used to perform quasi-static analyses with complicated contact conditions; and
allows for either automatic or fixed time incrementation to be used—by default, Abaqus/Explicit
uses automatic time incrementation with the global time estimator.
Explicit dynamic analysis
The explicit dynamics procedure performs a large number of small time increments efficiently. An
explicit central-difference time integration rule is used; each increment is relatively inexpensive
(compared to the direct-integration dynamic analysis procedure available in Abaqus/Standard) because
there is no solution for a set of simultaneous equations. The explicit central-difference operator satisfies
the dynamic equilibrium equations at the beginning of the increment, t; the accelerations calculated at
time t are used to advance the velocity solution to time
and the displacement solution to time
.
Input File Usage:
Abaqus/CAE Usage:
*DYNAMIC, EXPLICIT
Step module: Create Step: General: Dynamic, Explicit
6.3.3–1
Abaqus Version 5.8 ID:
Printed on:
EXPLICIT DYNAMIC ANALYSIS
Numerical implementation
The explicit dynamics analysis procedure is based upon the implementation of an explicit integration
rule together with the use of diagonal (“lumped”) element mass matrices. The equations of motion for
the body are integrated using the explicit central-difference integration rule
where
is a degree of freedom (a displacement or rotation component) and the subscript i refers to the
increment number in an explicit dynamics step. The central-difference integration operator is explicit in
the sense that the kinematic state is advanced using known values of
and
from the previous
increment.
The explicit integration rule is quite simple but by itself does not provide the computational
efficiency associated with the explicit dynamics procedure. The key to the computational efficiency
of the explicit procedure is the use of diagonal element mass matrices because the accelerations at the
beginning of the increment are computed by
where
is the mass matrix,
is the applied load vector, and
is the internal force vector. A
lumped mass matrix is used because its inverse is simple to compute and because the vector multiplication
of the mass inverse by the inertial force requires only n operations, where n is the number of degrees
of freedom in the model. The explicit procedure requires no iterations and no tangent stiffness matrix.
The internal force vector, , is assembled from contributions from the individual elements such that a
global stiffness matrix need not be formed.
Nodal mass and inertia
The explicit integration scheme in Abaqus/Explicit requires nodal mass or inertia to exist at all activated
degrees of freedom (see “Conventions,” Section 1.2.2) unless constraints are applied using boundary
conditions. More precisely, a nonzero nodal mass must exist unless all activated translational degrees
of freedom are constrained and nonzero rotary inertia must exist unless all activated rotational degrees
of freedom are constrained. Nodes that are part of a rigid body do not require mass, but the entire rigid
body must possess mass and inertia unless constraints are used. Nodes that belong to Eulerian elements
also do not require mass, since the surrounding Eulerian elements may be void at some time during the
simulation.
When degrees of freedom at a node are activated by elements with a nonzero mass density (e.g.,
solid, shell, beam) or mass and inertia elements, a nonzero nodal mass or inertia occurs naturally from
the assemblage of lumped mass contributions.
6.3.3–2
Abaqus Version 5.8 ID:
Printed on:
EXPLICIT DYNAMIC ANALYSIS
When degrees of freedom at a node are activated by elements with no mass (e.g., spring, dashpot,
or connector elements), care must be taken either to constrain the node or to add mass and inertia as
appropriate.
Stability
The explicit procedure integrates through time by using many small time increments. The centraldifference operator is conditionally stable, and the stability limit for the operator (with no damping)
is given in terms of the highest frequency of the system as
With damping, the stable time increment is given by
where
is the fraction of critical damping in the mode with the highest frequency. Contrary to our
usual engineering intuition, introducing damping to the solution reduces the stable time increment. In
Abaqus/Explicit a small amount of damping is introduced in the form of bulk viscosity to control high
frequency oscillations. Physical forms of damping, such as dashpots or material damping, can also be
introduced. Bulk viscosity and material damping are discussed below.
Estimating the stable time increment size
An approximation to the stability limit is often written as the smallest transit time of a dilatational wave
across any of the elements in the mesh
where
is the smallest element dimension in the mesh and is the dilatational wave speed in terms
of
and , defined below.
In general, for beams, conventional shells, and membranes the element thickness or cross-sectional
dimensions are not considered in determining the smallest element dimension; the stability limit is based
upon the midplane or membrane dimensions only. When the transverse shear stiffness is defined for shell
elements (see “Shell section behavior,” Section 29.6.4), the stable time increment will also be based on
the transverse shear behavior.
This estimate for
is only approximate and in most cases is not a conservative (safe) estimate. In
general, the actual stable time increment chosen by Abaqus/Explicit will be less than this estimate by a
factor between
and 1 in a two-dimensional model and between
and 1 in a three-dimensional
model. The time increment chosen by Abaqus/Explicit also accounts for any stiffness behavior in a
model associated with penalty contact. For further discussion, see “Computational cost” below.
6.3.3–3
Abaqus Version 5.8 ID:
Printed on:
EXPLICIT DYNAMIC ANALYSIS
Stable time increment report
Abaqus/Explicit writes a report to the status (.sta) file during the data check phase of the analysis that
contains an estimate of the minimum stable time increment and a listing of the elements with the smallest
stable time increments and their values. The initial stable time increments listed do not include damping
(bulk viscosity), mass scaling, or penalty contact effects.
This listing is provided because often a few elements have much smaller stability limits than the
rest of the elements in the mesh. The stable time increment can be increased by modifying the mesh to
increase the size of the controlling element or by using appropriate mass scaling.
Dilatational wave speed
The current dilatational wave speed, , is determined in Abaqus/Explicit by calculating the effective
hypoelastic material moduli from the material’s constitutive response. Effective Lamé’s constants,
and
, are determined in the following manner. Define
as the increment in the mean stress,
as the increment in the deviatoric stress,
as the increment of volumetric strain, and
as the
deviatoric strain increment. We assume a hypoelastic stress-strain rule of the form
The effective moduli can then be computed as
For shell elements defined by a shell cross-section that requires numerical integration (see “Using a
shell section integrated during the analysis to define the section behavior,” Section 29.6.5), the effective
moduli for the section are computed by integrating the effective moduli at the section points through the
thickness. These effective moduli represent the element stiffness and determine the current dilatational
wave speed in the element as
where
is the density of the material.
6.3.3–4
Abaqus Version 5.8 ID:
Printed on:
EXPLICIT DYNAMIC ANALYSIS
In an isotropic, elastic material the effective Lamé’s constants can be defined in terms of Young’s
modulus, E, and Poisson’s ratio, , by
and
Time incrementation
The time increment used in an analysis must be smaller than the stability limit of the central-difference
operator. Failure to use a small enough time increment will result in an unstable solution. When the
solution becomes unstable, the time history response of solution variables such as displacements will
usually oscillate with increasing amplitudes. The total energy balance will also change significantly.
If the model contains only one material type, the initial time increment is directly proportional to
the size of the smallest element in the mesh. If the mesh contains uniform size elements but contains
multiple material descriptions, the element with the highest wave speed will determine the initial time
increment.
In nonlinear problems—those with large deformations and/or nonlinear material response—the
highest frequency of the model will continually change, which consequently changes the stability limit.
Abaqus/Explicit has two strategies for time incrementation control: fully automatic time incrementation
(where the code accounts for changes in the stability limit) and fixed time incrementation.
Scaling the time increment
To reduce the chance of a solution going unstable, you can adjust the stable time increment computed
by Abaqus/Explicit by a constant scaling factor. This factor can be used to scale the default global time
estimate, the element-by-element estimate, or the fixed time increment based on the initial element-byelement estimate; it cannot be used to scale a fixed time increment specified directly by you.
Input File Usage:
Use the following option to scale the stable time increment based on the global
time estimate:
*DYNAMIC, EXPLICIT, SCALE FACTOR=f
Use the following option to scale the stable time increment based on the
element-by-element estimate:
*DYNAMIC, EXPLICIT, ELEMENT BY ELEMENT, SCALE FACTOR=f
Use the following option to scale the stable time increment based on the fixed
time increment on the initial element-by-element estimate:
*DYNAMIC, EXPLICIT, FIXED TIME INCREMENTATION,
SCALE FACTOR=f
6.3.3–5
Abaqus Version 5.8 ID:
Printed on:
EXPLICIT DYNAMIC ANALYSIS
Abaqus/CAE Usage:
Step module: Create Step: General: Dynamic, Explicit:
Incrementation: Time scaling factor: f
Automatic time incrementation
The default time incrementation scheme in Abaqus/Explicit is fully automatic and requires no user
intervention. Two types of estimates are used to determine the stability limit: element by element and
global. An analysis always starts by using the element-by-element estimation method and may switch
to the global estimation method under certain circumstances, as explained below.
Element-by-element estimation
In an analysis Abaqus/Explicit initially uses a stability limit based on the highest element frequency in
the whole model. This element-by-element estimate is determined using the current dilatational wave
speed in each element.
The element-by-element estimate is conservative; it will give a smaller stable time increment
than the true stability limit that is based upon the maximum frequency of the entire model. In general,
constraints such as boundary conditions and kinematic contact have the effect of compressing the
eigenvalue spectrum, and the element-by-element estimates do not take this into account.
The concept of the stable time increment as the time required to propagate a dilatational wave
across the smallest element dimension is useful for interpreting how the explicit procedure chooses the
time increment when element-by-element stability estimation controls the time increment. As the step
proceeds, the global stability estimate, if used, will make the time increment less sensitive to element
size.
Input File Usage:
Abaqus/CAE Usage:
*DYNAMIC, EXPLICIT, ELEMENT BY ELEMENT
Step module: Create Step: General: Dynamic, Explicit: Incrementation:
Stable increment estimator: Element-by-element
Global estimation
The stability limit will be determined by the global estimator as the step proceeds unless the element-byelement estimation method is specified, fixed time incrementation is specified, or one of the conditions
explained below prevents the use of global estimation. The switch to the global estimation method occurs
once the algorithm determines that the accuracy of the global estimation method is acceptable.
The adaptive, global estimation algorithm determines the maximum frequency of the entire model
using the current dilatational wave speed. This algorithm continuously updates the estimate for the
maximum frequency. The global estimator will usually allow time increments that exceed the elementby-element values.
Abaqus/Explicit monitors the effectiveness of the global estimation algorithm. If the cost for
computing the global time estimate is more than its benefit, the code will turn off the global estimation
algorithm and simply use the element-by-element estimates to save computation time.
6.3.3–6
Abaqus Version 5.8 ID:
Printed on:
EXPLICIT DYNAMIC ANALYSIS
Conditions that will prevent the use of the global time estimator
The global estimation algorithm will not be used when any of the following capabilities are included in
the model:
•
•
•
•
•
•
•
•
•
•
•
Fluid elements
Infinite elements
Dashpots
Thick shells (thickness to characteristic length ratio larger than 0.92)
Thick beams (thickness to length ratio larger than 1.0)
The JWL equation of state
Material damping
Nonisotropic elastic materials with temperature and field variable dependency
Distortion control
Adaptive meshing
Subcycling
“Improved” stable time increment for three-dimensional continuum elements and elements with plane
stress formulations
For three-dimensional continuum elements and elements with plane stress formulations (shell,
membrane, and two-dimensional plane stress elements) an “improved” estimate of the element
characteristic length is used by default. This “improved” method usually results in a larger element
stable time increment than a more traditional method. For analyses using variable mass scaling, the
total mass added to achieve a given stable time increment will be less with the improved estimate.
Input File Usage:
Use the following option to activate the “improved” element time estimation
method:
*DYNAMIC, EXPLICIT, IMPROVED DT METHOD=YES
Use the following option to deactivate the “improved” element time estimation
method:
Abaqus/CAE Usage:
*DYNAMIC, EXPLICIT, IMPROVED DT METHOD=NO
The ability to deactivate the “improved” element time estimation method is not
supported in Abaqus/CAE.
Fixed time incrementation
A fixed time incrementation scheme is also available in Abaqus/Explicit. The fixed time increment size
is determined either by the initial element-by-element stability estimate for the step or by a user-specified
time increment.
Fixed time incrementation may be useful when a more accurate representation of the higher mode
response of a problem is required. In this case a time increment size smaller than the element-by-element
6.3.3–7
Abaqus Version 5.8 ID:
Printed on:
EXPLICIT DYNAMIC ANALYSIS
estimates may be used. The element-by-element estimate can be obtained simply by running a data check
analysis (see “Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution,” Section 3.2.2).
When fixed time incrementation is used, Abaqus/Explicit will not check that the computed response
is stable during the step. You should ensure that a valid response has been obtained by carefully checking
the energy history and other response variables.
Basing the fixed time increment size on the initial element-by-element stability limit
You can use time increments the size of the initial element-by-element stability limit throughout a step.
The dilatational wave speed in each element at the beginning of the step is used to compute the fixed
time increment size.
Input File Usage:
Abaqus/CAE Usage:
*DYNAMIC, EXPLICIT, FIXED TIME INCREMENTATION
Step module: Create Step: General: Dynamic, Explicit: Incrementation:
Type: Fixed: Use element-by-element time increment estimator
Specifying the fixed time increment size directly
Alternatively, you can specify a time increment size directly.
Input File Usage:
Abaqus/CAE Usage:
*DYNAMIC, EXPLICIT, DIRECT USER CONTROL
Step module: Create Step: General: Dynamic, Explicit: Incrementation:
Type: Fixed: User-defined time increment
Advantages of the explicit method
The use of small increments (dictated by the stability limit) is advantageous because it allows the solution
to proceed without iterations and without requiring tangent stiffness matrices to be formed. It also
simplifies the treatment of contact.
The explicit dynamics procedure is ideally suited for analyzing high-speed dynamic events, but
many of the advantages of the explicit procedure also apply to the analysis of slower (quasi-static)
processes. A good example is sheet metal forming, where contact dominates the solution and local
instabilities may form due to wrinkling of the sheet.
The results in an explicit dynamics analysis are not automatically checked for accuracy as they are in
Abaqus/Standard (Abaqus/Standard uses the half-increment residual). In most cases this is not of concern
because the stability condition imposes a small time increment such that the solution changes only slightly
in any one time increment, which simplifies the incremental calculations. While the analysis may take
an extremely large number of increments, each increment is relatively inexpensive, often resulting in an
economical solution. It is not uncommon for Abaqus/Explicit to take over 105 increments for an analysis.
The method is, therefore, computationally attractive for problems where the total dynamic response time
that must be modeled is only a few orders of magnitude longer than the stability limit; for example, wave
propagation studies or some “event and response” applications.
6.3.3–8
Abaqus Version 5.8 ID:
Printed on:
EXPLICIT DYNAMIC ANALYSIS
Computational cost
The computer time involved in running a simulation using explicit time integration with a given mesh
is proportional to the time period of the event. The time increment based on the element-by-element
stability estimate can be rewritten (ignoring damping) in the form
where the minimum is taken over all elements in the mesh,
is a characteristic length associated with an
element (see “Explicit dynamic analysis,” Section 2.4.5 of the Abaqus Theory Manual), is the density
of the material in the element, and and are the effective Lamé’s constants for the material in the
element (defined above).
The time increment from the global stability estimate may be somewhat larger, but for this
discussion we will assume that the above inequality always holds (when the inequality does not hold,
the solution time will be somewhat faster).
For linear, nonisotropic elastic materials this stability limit is further scaled down by the square
root of the ratio of the effective material stiffness to the maximum material stiffness in one particular
direction. Since this effectively means that the time increment can be no larger than the time required to
propagate a stress wave across an element, the computer time involved in running a quasi-static analysis
can be very large: the cost of the simulation is directly proportional to the number of time increments
required.
The number of increments, n, required is
if
remains constant, where T is the
time period of the event being simulated. (Even the element-by-element approximation of
will not
remain constant in general, since element distortion will change
and nonlinear material response will
change the effective Lamé constants. But the assumption is sufficiently accurate for the purposes of this
discussion.) Thus,
In a two-dimensional analysis refining the mesh by a factor of two in each direction will increase
the run time in the explicit procedure by a factor of eight—four times as many elements and half the
original time increment size. Similarly, in a three-dimensional analysis refining the mesh by a factor of
two in each direction will increase the run time by a factor of sixteen.
In a quasi-static analysis it is expedient to reduce the computational cost by either speeding up the
simulation or by scaling the mass. In either case the kinetic energy should be monitored to ensure that
the ratio of kinetic energy to internal energy does not get too large—typically less than 10%.
Reducing the computational cost by speeding up the simulation
To reduce the number of increments required, n, we can speed up the simulation compared to the time of
the actual process—that is, we can artificially reduce the time period of the event, T. This will introduce
6.3.3–9
Abaqus Version 5.8 ID:
Printed on:
EXPLICIT DYNAMIC ANALYSIS
two possible errors. If the simulation speed is increased too much, the increased inertia forces will change
the predicted response (in an extreme case the problem will exhibit wave propagation response). The
only way to avoid this error is to choose a speed-up that is not too large.
The other error is that some aspects of the problem other than inertia forces—for example, material
behavior—may also be rate dependent. In this case the actual time period of the event being modeled
cannot be changed.
Reducing the computational cost by using mass scaling
Artificially increasing the material density, , by a factor
reduces n to
, just like decreasing T
to
. This concept, called “mass scaling,” reduces the ratio of the event time to the time for wave
propagation across an element while leaving the event time fixed, which allows rate-dependent behavior
to be included in the analysis. Mass scaling has exactly the same effect on inertia forces as speeding up
the time of simulation.
Mass scaling is attractive because it can be used in rate-dependent problems, but it must be used with
care to ensure that the inertia forces do not dominate and change the solution. Either fixed or variable
mass scaling can be invoked (see “Mass scaling,” Section 11.6.1).
Mass scaling can also be accomplished by altering the density; however, the fixed and variable mass
scaling capabilities provide more versatile methods of scaling the mass of the entire model or specific
element sets in the model.
Reducing the computational cost by using selective subcycling
One disadvantage in an explicit dynamic analysis is that a few very small elements will force the entire
model to be integrated with a small time increment. You can use mixed time integration or “subcycling”
methods to reduce this problem. In these methods the equations of motion for the body are still integrated
using the explicit central-difference integration rule as shown above, but the different time increments are
allowed for different groups of nodes in the finite element model. If most nodes are integrated with a large
stable time increment and only a few nodes are integrated with a small time increment, the computational
cost may be reduced significantly.
Selective subcycling can be invoked by defining the subcycling zones. See “Selective subcycling,”
Section 11.7.1 for details.
Bulk viscosity
Bulk viscosity introduces damping associated with volumetric straining. Its purpose is to improve the
modeling of high-speed dynamic events (see “Stability” above for a discussion of the effect of damping
on the stable time increment). Abaqus/Explicit contains two forms of bulk viscosity: linear and quadratic.
Linear bulk viscosity is included by default in an Abaqus/Explicit analysis.
The bulk viscosity parameters and defined below can be redefined and can be changed from
step to step. If the default values are changed in a step, the new values will be used in subsequent steps
until they are redefined. Bulk viscosities defined this way apply to the whole model. For an individual
element set the linear and quadratic bulk viscosities can be scaled by a factor by defining section controls
(see “Section controls,” Section 27.1.4).
6.3.3–10
Abaqus Version 5.8 ID:
Printed on:
EXPLICIT DYNAMIC ANALYSIS
Input File Usage:
Use the following option to define bulk viscosity for the entire model:
*BULK VISCOSITY
Use the following options to define bulk viscosity for an individual element set:
Abaqus/CAE Usage:
*BULK VISCOSITY
*SECTION CONTROLS
Use the following option to define bulk viscosity for the entire model:
Step module: Create Step: General: Dynamic, Explicit: Other: Linear
bulk viscosity parameter and Quadratic bulk viscosity parameter
Defining bulk viscosity for an individual element set is not supported in
Abaqus/CAE.
Linear bulk viscosity
Linear bulk viscosity is found in all elements and is introduced to damp “ringing” in the highest element
frequency. This damping is sometimes referred to as truncation frequency damping. It generates a bulk
viscosity pressure that is linear in the volumetric strain rate
where
is a damping coefficient (default=.06), is the current material density,
is the current
dilatational wave speed,
is an element characteristic length, and
is the volumetric strain rate.
For acoustic elements, the bulk viscosity pressure can be obtained from the above equation by
using the relationship of the fluid particle velocity and the pressure rate (see “Coupled acoustic-structural
medium analysis,” Section 2.9.1 of the Abaqus Theory Manual) as
where
and c are the pressure rate and the speed of sound in the fluid, respectively.
Quadratic bulk viscosity
The second form of bulk viscosity pressure is found only in solid continuum elements (except the plane
stress element CPS4R). This form is quadratic in the volumetric strain rate
where is a damping coefficient (default=1.2) and all other quantities are as defined for the linear bulk
viscosity. Quadratic bulk viscosity is applied only if the volumetric strain rate is compressive.
The quadratic bulk viscosity pressure will smear a shock front across several elements and is
introduced to prevent elements from collapsing under extremely high velocity gradients. Consider a
simple one-element problem in which the nodes on one side of the element are fixed and the nodes on
the other side have an initial velocity in the direction of the fixed nodes. If the initial velocity is equal
to the dilatational wave speed of the material, without the quadratic bulk viscosity, the element would
6.3.3–11
Abaqus Version 5.8 ID:
Printed on:
EXPLICIT DYNAMIC ANALYSIS
collapse to zero volume in one time increment (because the stable time increment size is precisely
the transit time of a dilatational wave across the element). The quadratic bulk viscosity pressure will
introduce a resisting pressure that will prevent the element from collapsing.
Fraction of critical damping due to bulk viscosity
The bulk viscosity pressure is not included in the material point stresses because it is intended as a
numerical effect only—it is not considered part of the material’s constitutive response. The bulk viscosity
pressures are based upon the dilatational mode of each element. The fraction of critical damping in the
dilatational mode of each element is given by
Rotational bulk viscosity for shell elements
For the displacement degrees of freedom, bulk viscosity introduces damping associated with volumetric
straining. Linear bulk viscosity or truncation frequency damping is used to damp the high frequency
ringing that leads to unwanted noise in the solution or spurious overshoot in the response amplitude. For
the same reason, in shells the high frequency ringing in the rotational degrees of freedom is damped with
linear bulk viscosity acting on the mean curvature strain rate. This damping generates a bulk viscosity
“pressure moment,” m, which is linear in the mean curvature strain rate
where is a damping coefficient (default = 0.06),
is the original thickness, is the mass density,
is the current dilatational wave speed, L is the characteristic length used for rotary inertia and transverse
shear stiffness scaling (see “Finite-strain shell element formulation,” Section 3.6.5 of the Abaqus Theory
Manual), and
is twice the mean curvature strain rate. The resultant pressure moment
,
where h is the current thickness, is added to the direct components of the moment resultant.
Material damping
Defining inelastic material behavior, dashpots, etc. will introduce energy dissipation into a model. In
addition to these mechanisms, general (“Rayleigh”) material damping can be introduced (see “Material
damping,” Section 26.1.1). Adding damping to a model, especially stiffness proportional damping, ,
may significantly reduce the stable time increment.
Input File Usage:
Abaqus/CAE Usage:
*DAMPING, ALPHA= , BETA=
Property module: material editor: Mechanical→Damping: Alpha and Beta
6.3.3–12
Abaqus Version 5.8 ID:
Printed on:
EXPLICIT DYNAMIC ANALYSIS
Obtaining diagnostic information about critical elements
Abaqus/Explicit writes critical elements (elements with the smallest stable time increments) and their
stable time increment values to the output database at each summary increment for visualization in
Abaqus/CAE. By default, the number of critical elements written to the output database is 10.
Input File Usage:
Abaqus/CAE Usage:
*DIAGNOSTICS, CRITICAL ELEMENTS=value
The ability to control the number of critical elements written to the output
database is not supported in Abaqus/CAE.
Obtaining diagnostic information about the deformation speed
The deformation speed in an element is defined as the largest absolute value of all the deformation
rate components of an element times the element characteristic length, . You can request diagnostic
information about the deformation speed within a step definition, as described below. In a multistep
analysis diagnostic requests remain in effect until they are explicitly redefined.
Deformation speed warnings
By default, Abaqus/Explicit will check for a relatively large deformation speed in all the elements since
too high a value may cause the element to deform or collapse unrealistically. A warning message is
issued if the ratio of deformation speed versus dilatational wave speed in an element reaches the value
specified for the “warning ratio.” By default, the warning ratio is 0.3. You can redefine this limit.
The first occurrence of the warning message is written to the status (.sta) file; subsequent
occurrences are written to the message (.msg) file. See “Output,” Section 4.1.1, for a description of
these output files.
Generally when the ratio of deformation speed to dilatational wave speed is greater than 0.3, it is
an indication that the purely mechanical material constitutive relationship is no longer valid and that a
thermo-mechanical equation of state material is required.
Input File Usage:
Abaqus/CAE Usage:
*DIAGNOSTICS, WARNING RATIO=ratio
The ability to redefine the warning ratio limit is not supported in Abaqus/CAE.
Deformation speed errors
An error message is issued and the analysis is terminated when the maximum ratio of deformation speed
versus current dilatational wave speed for any element is greater than the “cutoff ratio.” By default, the
cutoff ratio is 1.0. You can redefine this limit.
The check for this cutoff ratio is not applied to any model that has an equation of state material (see
“Equation of state,” Section 25.2.1) or a user-defined material (see “User-defined mechanical material
behavior,” Section 26.7.1).
Input File Usage:
Abaqus/CAE Usage:
*DIAGNOSTICS, CUTOFF RATIO=ratio
The ability to redefine the cutoff ratio limit is not supported in Abaqus/CAE.
6.3.3–13
Abaqus Version 5.8 ID:
Printed on:
EXPLICIT DYNAMIC ANALYSIS
Obtaining a summary of the deformation speed information
You can request summary diagnostic information to obtain warning and error messages for only the
element with the largest ratio of deformation speed to dilatational wave speed.
Input File Usage:
Abaqus/CAE Usage:
*DIAGNOSTICS, DEFORMATION SPEED CHECK=SUMMARY
A summary of the deformation speed diagnostic information is output by
default in Abaqus/CAE.
Obtaining detailed deformation speed information
You can request detailed diagnostic information to obtain warning and error messages for all elements
with large deformation speed to dilatational wave speed ratios.
Input File Usage:
Abaqus/CAE Usage:
*DIAGNOSTICS, DEFORMATION SPEED CHECK=DETAIL
You cannot output detailed diagnostic information about the deformation speed
in Abaqus/CAE.
Disabling deformation speed checks
You can choose to completely bypass the checks for large deformation speed.
Input File Usage:
Abaqus/CAE Usage:
*DIAGNOSTICS, DEFORMATION SPEED CHECK=OFF
You cannot disable the deformation speed checks in Abaqus/CAE.
Monitoring output variables for extreme values
There are some analyses in which it is useful to monitor the value of a variable at every increment. For
example, in a force-driven analysis such as hydro-forming, the simulation time that is sufficient to model
the completion of the physical process may depend on the magnitude of the displacement of a node or a
group of nodes in the model. Another example is a drop test simulation where the postfailure response is
not of interest. Monitoring the values of critical variables and halting the analysis when those variables
exceed a given criterion can reduce computational expense and turnaround time.
For such problems Abaqus/Explicit allows output variables to be monitored during an analysis
to verify whether or not their values have exceeded or fallen below user-specified values in specified
element or node sets. Comparisons of specified element integration point variables, element section
variables, or nodal variables with user-specified values are performed at every increment. At the first
occurrence of a variable exceeding the user-specified bounds, the variable name, the associated element
or node number, and the increment number are written to the status (.sta) file. In addition, you can
request that the analysis be stopped and/or the output state be written in the increment following the one
in which the variable has exceeded the user-specified bound. At the end of each step in which variables
are monitored, the maximum, minimum, or absolute maximum value that each variable attains during the
course of the analysis, along with the number of the element or node where the extreme value occurred,
will be written to the status file.
6.3.3–14
Abaqus Version 5.8 ID:
Printed on:
EXPLICIT DYNAMIC ANALYSIS
Defining the element and nodal variables to be monitored
The element output variables that can be monitored include all the element integration point variables
and element section point variables that are available for history-type output to the output database.
Similarly, the nodal output variables that can be monitored include all the nodal variables that are
available for history output to the output database. The keys identifying the output variables are defined
in “Abaqus/Explicit output variable identifiers,” Section 4.2.2.
Input File Usage:
Use the first option with one or both of the following options in the history
portion of the input file:
*EXTREME VALUE
*EXTREME ELEMENT VALUE, ELSET=element_set_name
*EXTREME NODE VALUE, NSET=nset_set_name
The *EXTREME VALUE option can be repeated in the same step, and the
*EXTREME ELEMENT VALUE and *EXTREME NODE VALUE options
can be repeated as many times as necessary.
Abaqus/CAE Usage:
Extreme value output monitoring is not supported in Abaqus/CAE.
Halting the analysis when the extreme value criterion is met
You can choose to halt the analysis when the extreme value criterion is met. The analysis will stop at the
end of the increment following the one in which any of the specified element or nodal variables exceeded
the prescribed bounds.
Input File Usage:
Use the following options:
Abaqus/CAE Usage:
*EXTREME VALUE, HALT=YES
*EXTREME ELEMENT VALUE and/or *EXTREME NODE VALUE
Extreme value output monitoring is not supported in Abaqus/CAE.
Obtaining output when the extreme value criterion is met
You can obtain field-type output to the output database and an additional restart state when any of the
selected variables fall outside the specified bounds for the first time during the analysis. The output will
be written in the increment following the one in which such an occurrence took place. Since output is
automatically written when the analysis terminates, this request has an effect only if you have not chosen
to halt the analysis when the extreme value criterion is met as described above.
Input File Usage:
Use either or both of the following options in conjunction with the *EXTREME
VALUE option:
*EXTREME ELEMENT VALUE, ELSET=element_set_name,
OUTPUT=YES
*EXTREME NODE VALUE, NSET=node_set_name, OUTPUT=YES
Abaqus/CAE Usage:
Extreme value output monitoring is not supported in Abaqus/CAE.
6.3.3–15
Abaqus Version 5.8 ID:
Printed on:
EXPLICIT DYNAMIC ANALYSIS
Monitoring variables in a multistep analysis
In a multistep analysis the monitoring requests you specify remain in effect until they are redefined. You
must redefine all requests to add or change any variables, element or node sets, or maxima or minima.
Stopping the monitoring of variables in a new step
You can stop monitoring variables in a new step.
Input File Usage:
Use the *EXTREME VALUE option without the *EXTREME ELEMENT
VALUE and *EXTREME NODE VALUE options.
Abaqus/CAE Usage:
Extreme value output monitoring is not supported in Abaqus/CAE.
Initial conditions
“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1, describes all of the initial
conditions that are available for an explicit dynamic analysis.
Boundary conditions
Boundary conditions can be defined as explained in “Boundary conditions in Abaqus/Standard and
Abaqus/Explicit,” Section 33.3.1. Boundary conditions applied during an explicit dynamic response
step should use appropriate amplitude references (“Amplitude curves,” Section 33.1.2). If boundary
conditions are specified for the step without amplitude references, they are applied instantaneously at
the beginning of the step. Since Abaqus/Explicit does not admit jumps in displacement, the value of
a nonzero displacement boundary condition that is specified without an amplitude reference will be
ignored, and a zero velocity boundary condition will be enforced.
Loads
The loading types available for an explicit dynamic analysis are explained in “Applying loads: overview,”
Section 33.4.1. Concentrated nodal forces or moments can be applied to the displacement or rotation
degrees of freedom (1–6). Distributed pressure forces or body forces can also be applied; the distributed
load types available with particular elements are described in Part VI, “Elements.”
As with boundary conditions, loads applied during a dynamic response step should use appropriate
amplitude references (“Amplitude curves,” Section 33.1.2). If loads are specified for the step without
amplitude references, they are applied instantaneously at the beginning of the step.
Predefined fields
The following predefined fields can be specified, as described in “Predefined fields,” Section 33.6.1:
•
Although temperature is not a degree of freedom in explicit dynamic analysis, nodal temperatures
can be specified. Any difference between the applied and initial temperatures will cause
thermal strain if a thermal expansion coefficient is given for the material (“Thermal expansion,”
6.3.3–16
Abaqus Version 5.8 ID:
Printed on:
EXPLICIT DYNAMIC ANALYSIS
•
Section 26.1.2). The specified temperature also affects temperature-dependent material properties,
if any.
The values of user-defined field variables can be specified. These values affect only field-variabledependent material properties, if any.
Material options
Any of the material models in Abaqus/Explicit can be used in a general explicit dynamic analysis (see
“Combining material behaviors,” Section 21.1.3).
Elements
All of the elements available in Abaqus/Explicit can be used in an explicit dynamic analysis. The
elements are listed in Part VI, “Elements.”
If coupled temperature-displacement elements are used in an explicit dynamic analysis, the
temperature degrees of freedom will be ignored.
Output
The element output available for a dynamic analysis includes stress; strain; energies; and the values of
state, field, and user-defined variables. The nodal output available includes displacements, velocities,
accelerations, reaction forces, and coordinates. All of the output variable identifiers are outlined in
“Abaqus/Explicit output variable identifiers,” Section 4.2.2. The types of output available are described
in “Output,” Section 4.1.1.
When an Abaqus/Explicit analysis encounters a fatal error, the preselected variables applicable to
the current procedure are added automatically to the output database as field data for the last increment.
Energy output is particularly important in checking the accuracy of the solution in an explicit
dynamic analysis. In general, the total energy (ETOTAL) should be a constant or close to a constant; the
“artificial” energies, such as the artificial strain energy (ALLAE), the damping dissipation (ALLVD),
and the mass scaling work (ALLMW) should be negligible compared to “real” energies such as the
strain energy (ALLSE) and the kinetic energy (ALLKE).
In a quasi-static analysis the value of the kinetic energy (ALLKE) should not exceed a small fraction
of the value of the strain energy (ALLIE).
It is a good practice to output the constraint penalty work (ALLCW) and the contact penalty work
(ALLPW) in analyses involving constraints (such as ties and fasteners) and contact. The value of these
energies should be close to zero.
Input file template
*HEADING
…
*MATERIAL, NAME=name
*ELASTIC
…
6.3.3–17
Abaqus Version 5.8 ID:
Printed on:
EXPLICIT DYNAMIC ANALYSIS
*DENSITY
Data lines to define density
*DAMPING, ALPHA = , BETA=
Data lines to define Rayleigh damping
…
*BOUNDARY
Data lines to specify zero-valued boundary conditions
*INITIAL CONDITIONS, TYPE=type
Data lines to specify initial conditions
*AMPLITUDE, NAME=name
Data lines to define amplitude variations
*************************
*STEP
*DYNAMIC, EXPLICIT
Data line to specify the time period of the step
*DIAGNOSTICS, DEFORMATION SPEED CHECK=SUMMARY
*BOUNDARY, AMPLITUDE=name
Data lines to describe zero-valued or nonzero boundary conditions
*CLOAD and/or *DLOAD
Data lines to specify loading
*TEMPERATURE and/or *FIELD
Data lines to specify predefined fields
*FILE OUTPUT, NUMBER INTERVAL=n
*EL FILE
Data line specifying element output variables
*NODE FILE
Data line specifying node output variables
*ENERGY FILE
*OUTPUT, FIELD, NUMBER INTERVAL=n
*ELEMENT OUTPUT
Data line specifying element output variables
*NODE OUTPUT
Data line specifying node output variables
*OUTPUT, HISTORY, TIME INTERVAL=t
*ELEMENT OUTPUT, ELSET=element set name
Data line specifying element output variables
*NODE OUTPUT, NSET=node set name
Data line specifying node output variables
*ENERGY OUTPUT
Data line specifying energy output variables
*END STEP
*************************
6.3.3–18
Abaqus Version 5.8 ID:
Printed on:
EXPLICIT DYNAMIC ANALYSIS
*STEP
*DYNAMIC, EXPLICIT, ELEMENT BY ELEMENT
…
*BULK VISCOSITY
Data line to define linear and/or quadratic bulk viscosity in this step
…
*END STEP
6.3.3–19
Abaqus Version 5.8 ID:
Printed on:
DIRECT-SOLUTION STEADY-STATE DYNAMICS
6.3.4
DIRECT-SOLUTION STEADY-STATE DYNAMIC ANALYSIS
Products: Abaqus/Standard
Abaqus/CAE
References
•
•
•
•
•
•
•
•
“Dynamic analysis procedures: overview,” Section 6.3.1
“Mode-based steady-state dynamic analysis,” Section 6.3.8
“Subspace-based steady-state dynamic analysis,” Section 6.3.9
“Defining an analysis,” Section 6.1.2
“General and linear perturbation procedures,” Section 6.1.3
*STEADY STATE DYNAMICS
“Configuring a direct-solution steady-state dynamic procedure” in “Configuring linear perturbation
analysis procedures,” Section 14.11.2 of the Abaqus/CAE User’s Manual, in the online HTML
version of this manual
“Creating and modifying prescribed conditions,” Section 16.4 of the Abaqus/CAE User’s Manual
Overview
A direct-solution steady-state dynamic analysis:
•
•
•
•
•
•
•
is used to calculate the steady-state dynamic linearized response of a system to harmonic excitation;
is a linear perturbation procedure;
calculates the response directly in terms of the physical degrees of freedom of the model;
is an alternative to mode-based steady-state dynamic analysis, in which the response of the system
is calculated on the basis of the eigenmodes;
is more expensive computationally than mode-based or subspace-based steady-state dynamics;
is more accurate than mode-based or subspace-based steady-state dynamics, in particular if
significant frequency-dependent material damping or viscoelastic material behavior is present in
the structure; and
is able to bias the excitation frequencies toward the approximate values that generate a response
peak.
Introduction
Steady-state dynamic analysis provides the steady-state amplitude and phase of the response of a system
due to harmonic excitation at a given frequency. Usually such analysis is done as a frequency sweep by
applying the loading at a series of different frequencies and recording the response; in Abaqus/Standard
the direct-solution steady-state dynamic procedure conducts this frequency sweep. In a direct-solution
steady-state analysis the steady-state harmonic response is calculated directly in terms of the physical
degrees of freedom of the model using the mass, damping, and stiffness matrices of the system.
6.3.4–1
Abaqus Version 5.8 ID:
Printed on:
DIRECT-SOLUTION STEADY-STATE DYNAMICS
When defining a direct-solution steady-state dynamic step, you specify the frequency ranges
of interest and the number of frequencies at which results are required in each range (including the
bounding frequencies of the range). In addition, you can specify the type of frequency spacing (linear or
logarithmic) to be used, as described below (“Selecting the frequency spacing”). Logarithmic frequency
spacing is the default. Frequencies are given in cycles/time.
Those frequency points for which results are required can be spaced equally along the frequency axis
(on a linear or a logarithmic scale), or they can be biased toward the ends of the user-defined frequency
range by introducing a bias parameter (described below).
The direct-solution steady-state analysis procedure can be used in the following cases for which the
eigenvalues cannot be extracted (and, thus, the mode-based steady-state dynamics procedures are not
applicable):
•
•
•
for nonsymmetric stiffness;
when any form of damping other than modal damping must be included; and
when viscoelastic material properties must be taken into account.
While the response in this procedure is linear, the prior response can be nonlinear. Initial stress
effects (stress stiffening) as well as load stiffness effects will be included in the steady-state dynamics
response if nonlinear geometric effects (“General and linear perturbation procedures,” Section 6.1.3)
were included in any general analysis step prior to the direct-solution steady-state dynamic procedure.
Input File Usage:
Abaqus/CAE Usage:
*STEADY STATE DYNAMICS, DIRECT
Step module: Create Step: Linear perturbation: Steady-state
dynamics, Direct
Ignoring damping
If damping terms can be ignored, you can specify that a real, rather than a complex, system matrix be
factored, which can significantly reduce computational time. Damping is discussed below.
Input File Usage:
Abaqus/CAE Usage:
*STEADY STATE DYNAMICS, DIRECT, REAL ONLY
Step module: Create Step: Linear perturbation: Steady-state
dynamics, Direct: Compute real response only
Selecting the type of frequency interval for which output is requested
Three types of frequency intervals are permitted for output from a direct-solution steady-state dynamic
step. If an eigenvalue extraction step precedes the direct-solution steady-state dynamic step, you can
select either the range or the eigenfrequency type of frequency interval; otherwise, only the range type
can be used.
Dividing the specified frequency range using the user-defined number of points and the optional bias
function
For the range type of frequency interval (the default), the specified frequency range of interest is divided
using the user-defined number of points and the optional bias function.
6.3.4–2
Abaqus Version 5.8 ID:
Printed on:
DIRECT-SOLUTION STEADY-STATE DYNAMICS
Input File Usage:
Abaqus/CAE Usage:
*STEADY STATE DYNAMICS, DIRECT, INTERVAL=RANGE
Step module: Create Step: Linear perturbation: Steady-state
dynamics, Direct: toggle off Use eigenfrequencies to
subdivide each frequency range
Specifying the frequency ranges by using the system’s eigenfrequencies
If the direct-solution steady-state dynamic analysis is preceded by an eigenfrequency extraction step,
you can select the eigenfrequency type of frequency interval. The following intervals then exist in each
frequency range:
•
•
•
First interval: extends from the lower limit of the frequency range given to the first eigenfrequency
in the range.
Intermediate intervals: extend from eigenfrequency to eigenfrequency.
Last interval: extends from the highest eigenfrequency in the range to the upper limit of the
frequency range.
For each of these intervals the frequencies at which results are calculated are determined using the userdefined number of points (which includes the bounding frequencies for the interval) and the optional bias
function. Figure 6.3.4–1 illustrates the division of the frequency range for 5 calculation points and a bias
parameter equal to 1.
Input File Usage:
*STEADY STATE DYNAMICS, DIRECT,
INTERVAL=EIGENFREQUENCY
Abaqus/CAE Usage:
Step module: Create Step: Linear perturbation: Steady-state dynamics,
Direct: Use eigenfrequencies to subdivide each frequency range
frequency points
lower end
of the range
mode n
mode n +1
mode n + 2
upper end
of the range
Figure 6.3.4–1 Division of range for the eigenfrequency
type of interval and 5 calculation points.
Specifying the frequency ranges by the frequency spread
If the direct-solution steady-state dynamic analysis is preceded by an eigenfrequency extraction
step, you can select the spread type of frequency interval. In this case intervals exist around each
6.3.4–3
Abaqus Version 5.8 ID:
Printed on:
DIRECT-SOLUTION STEADY-STATE DYNAMICS
eigenfrequency in the frequency range. For each of the intervals the equally spaced frequencies at
which results are calculated are determined using the user-defined number of points (which includes
the bounding frequencies for the interval). The minimum number of frequency points is 3. If the
user-defined value is less than 3 (or omitted), the default value of 3 points is assumed. Figure 6.3.4–2
illustrates the division of the frequency range for 5 calculation points.
The bias parameter is not supported with the spread type of frequency interval.
Frequency points
Frequency points
fn
(1 – spread) · fn
fn + 1
(1 + spread) · fn
(1 – spread) · fn + 1
(1 + spread) · fn + 1
Figure 6.3.4–2 Division of range for the spread type of interval and 5 calculation
and
are eigenfrequencies of the system.
points.
Input File Usage:
*STEADY STATE DYNAMICS, DIRECT, INTERVAL=SPREAD
lwr_freq, upr_freq, numpts, bias_param, freq_scale_factor, spread
Abaqus/CAE Usage:
You cannot specify frequency ranges by frequency spread in Abaqus/CAE.
Selecting the frequency spacing
Two types of frequency spacing are permitted for a direct-solution steady-state dynamic step. For the
logarithmic frequency spacing (the default), the specified frequency ranges of interest are divided using
a logarithmic scale. Alternatively, a linear frequency spacing can be used if a linear scale is desired.
Input File Usage:
Use either of the following options:
*STEADY STATE DYNAMICS, DIRECT,
FREQUENCY SCALE=LOGARITHMIC
*STEADY STATE DYNAMICS, DIRECT, FREQUENCY SCALE=LINEAR
Abaqus/CAE Usage:
Step module: Create Step: Linear perturbation: Steady-state
dynamics, Direct: Scale: Logarithmic or Linear
Requesting multiple frequency ranges
You can request multiple frequency ranges or multiple single frequency points for a direct-solution
steady-state dynamic step.
6.3.4–4
Abaqus Version 5.8 ID:
Printed on:
DIRECT-SOLUTION STEADY-STATE DYNAMICS
Input File Usage:
*STEADY STATE DYNAMICS, DIRECT
lwr_freq1, upr_freq1, numpts1, bias_param1, freq_scale_factor1
lwr_freq2, upr_freq2, numpts2, bias_param2, freq_scale_factor2
...
single_freq1
single_freq2
...
Repeat the data lines as often as necessary.
Abaqus/CAE Usage:
Step module: Create Step: Linear perturbation: Steady-state dynamics,
Direct: Data: enter data in table, and add rows as necessary
The bias parameter
The bias parameter can be used to provide closer spacing of the results points either toward the middle
or toward the ends of each frequency interval. Figure 6.3.4–3 shows a few examples of the effect of the
bias parameter on the frequency spacing.
frequency points
Bias parameter = 1
f1
f2
Bias parameter = 2
Bias parameter = 3
Bias parameter = 5
Figure 6.3.4–3 Effect of the bias parameter on the frequency
.
spacing for a number of points
The bias formula used in direct-solution steady-state dynamics is
6.3.4–5
Abaqus Version 5.8 ID:
Printed on:
DIRECT-SOLUTION STEADY-STATE DYNAMICS
where
;
is the number of frequency points at which results are to be given;
);
is one such frequency point (
is the lower limit of the frequency range;
is the upper limit of the range;
is the frequency at which the kth results are given;
is the bias parameter value; and
is the frequency or the logarithm of the frequency, depending on the value chosen for the
frequency scale.
y
n
k
p
A bias parameter, p, that is greater than 1.0 provides closer spacing of the results points toward the ends
of the frequency interval, while values of p that are less than 1.0 provide closer spacing toward the middle
of the frequency interval. The default bias parameter is 1.0 for a range frequency interval and 3.0 for an
eigenfrequency interval.
The frequency scale factor
The frequency scale factor can be used to scale frequency points. All the frequency points, except the
lower and upper limit of the frequency range, are multiplied by this factor. This scale factor can be used
only when the frequency interval is specified by using the system’s eigenfrequencies (see “Specifying
the frequency ranges by using the system’s eigenfrequencies,” above).
Damping
If damping is absent, the response of a structure will be unbounded if the forcing frequency is equal
to an eigenfrequency of the structure. To get quantitatively accurate results, especially near natural
frequencies, accurate specification of damping properties is essential. The various damping options
available are discussed in “Material damping,” Section 26.1.1.
In direct-solution steady-state dynamics damping can be created by the following:
•
•
•
•
•
dashpots (see “Dashpots,” Section 32.2.1),
“Rayleigh” damping associated with materials and elements (see “Material damping,”
Section 26.1.1),
damping associated with acoustic elements (see “Acoustic medium,” Section 26.3.1; “Infinite
elements,” Section 28.3.1; and “Acoustic and shock loads,” Section 33.4.6),
structural damping (see “Damping in dynamic analysis” in “Dynamic analysis procedures:
overview,” Section 6.3.1), and
viscoelasticity included in the material definitions (see “Frequency domain viscoelasticity,”
Section 22.7.2).
When a real-only system matrix is factored, all forms of damping are ignored, including quiet
boundaries on infinite elements and nonreflecting boundaries on acoustic elements.
6.3.4–6
Abaqus Version 5.8 ID:
Printed on:
DIRECT-SOLUTION STEADY-STATE DYNAMICS
Contact conditions with sliding friction
Abaqus/Standard automatically detects the contact nodes that are slipping due to velocity differences
imposed by the motion of the reference frame or the transport velocity in prior steps. At those nodes the
tangential degrees of freedom are not constrained and the effect of friction results in an unsymmetric
contribution to the stiffness matrix. At other contact nodes the tangential degrees of freedom are
constrained.
Friction at contact nodes at which a velocity differential is imposed can give rise to damping terms.
There are two kinds of friction-induced damping effects. The first effect is caused by the friction forces
stabilizing the vibrations in the direction perpendicular to the slip direction. This effect exists only in
three-dimensional analysis. The second effect is caused by a velocity-dependent friction coefficient.
If the friction coefficient decreases with velocity (which is usually the case), the effect is destabilizing
and is also known as “negative damping.” For more details, see “Coulomb friction,” Section 5.2.3 of
the Abaqus Theory Manual. Direct-solution steady-state dynamics analysis allows you to include these
friction-induced contributions to the damping matrix.
Input File Usage:
Abaqus/CAE Usage:
*STEADY STATE DYNAMICS, DIRECT, FRICTION DAMPING=YES
Step module: Create Step: Linear perturbation: Steady-state dynamics,
Direct: Include friction-induced damping effects
Initial conditions
The base state is the current state of the model at the end of the last general analysis step prior to the
steady-state dynamic step. If the first step of an analysis is a perturbation step, the base state is determined
from the initial conditions (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1).
Initial condition definitions that directly define solution variables, such as velocity, cannot be used in a
steady-state dynamic analysis.
Boundary conditions
In a steady-state dynamic analysis the real and imaginary parts of any degree of freedom are either
restrained or unrestrained simultaneously; it is physically impossible to have one part restrained and the
other part unrestrained. Abaqus/Standard will automatically restrain both the real and imaginary parts of
a degree of freedom even if only one part is prescribed specifically. The unspecified part will be assumed
to have a perturbation magnitude of zero.
Boundary conditions can be applied to any of the displacement or rotation degrees of freedom
(1–6) in a direct-solution steady-state analysis. See “Boundary conditions in Abaqus/Standard and
Abaqus/Explicit,” Section 33.3.1. These boundary conditions will vary sinusoidally with time. You
specify the real (in-phase) part of a boundary condition and the imaginary (out-of-phase) part of a
boundary condition separately.
Input File Usage:
Use either of the following options to define the real (in-phase) part of the
boundary condition:
*BOUNDARY
*BOUNDARY, REAL
6.3.4–7
Abaqus Version 5.8 ID:
Printed on:
DIRECT-SOLUTION STEADY-STATE DYNAMICS
Use the following option to define the imaginary (out-of-phase) part of the
boundary condition:
Abaqus/CAE Usage:
*BOUNDARY, IMAGINARY
Load module: boundary condition editor: real (in-phase) part + imaginary
(out-of-phase) part i
Frequency-dependent boundary conditions
An amplitude definition can be used to specify the amplitude of a boundary condition as a function of
frequency (“Amplitude curves,” Section 33.1.2).
Input File Usage:
Use both of the following options:
Abaqus/CAE Usage:
*AMPLITUDE, NAME=name
*BOUNDARY, REAL or IMAGINARY, AMPLITUDE=name
Load or Interaction module: Create Amplitude: Name: name
Load module: boundary condition editor: real (in-phase) part + imaginary
(out-of-phase) part i: Amplitude: name
Loads
The following loads can be prescribed in a steady-state dynamic analysis:
•
•
•
Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6); see
“Concentrated loads,” Section 33.4.2.
Distributed pressure forces or body forces can be applied; see “Distributed loads,” Section 33.4.3.
The distributed load types available with particular elements are described in Part VI, “Elements.”
Incident wave loads can be applied; see “Acoustic and shock loads,” Section 33.4.6.
These loads are assumed to vary sinusoidally with time over a user-specified range of frequencies. Loads
are given in terms of their real and imaginary components.
Coriolis distributed loading adds an imaginary antisymmetric contribution to the overall system of
equations. This contribution is currently accounted for in solid and truss elements only and is activated
by using the unsymmetric matrix storage and solution scheme for the step (“Defining an analysis,”
Section 6.1.2).
Incident wave loads can be used to model sound waves from distinct planar or spherical sources or
from diffuse fields.
Fluid flux loading cannot be used in a steady-state dynamic analysis.
Input File Usage:
Use any of the following options to define the real (in-phase) part of the load:
*CLOAD or *DLOAD
*CLOAD or *DLOAD, REAL
Use either of the following options to define the imaginary (out-of-phase) part
of the load:
*CLOAD or *DLOAD, IMAGINARY
6.3.4–8
Abaqus Version 5.8 ID:
Printed on:
DIRECT-SOLUTION STEADY-STATE DYNAMICS
Abaqus/CAE Usage:
Load module: load editor: real (in-phase) part + imaginary (out-of-phase)
part i
Frequency-dependent loading
An amplitude definition can be used to specify the amplitude of a load as a function of frequency
(“Amplitude curves,” Section 33.1.2).
Input File Usage:
Use both of the following options:
Abaqus/CAE Usage:
*AMPLITUDE, NAME=name
*CLOAD or *DLOAD, REAL or IMAGINARY, AMPLITUDE=name
Load or Interaction module: Create Amplitude: Name: name
Load module: load editor: real (in-phase) part + imaginary (out-of-phase)
part i: Amplitude: name
Predefined fields
Predefined temperature fields can be specified in direct-solution steady-state dynamic analysis (see
“Predefined fields,” Section 33.6.1) and will produce harmonically varying thermal strains if thermal
expansion is included in the material definition (“Thermal expansion,” Section 26.1.2). Other predefined
fields are ignored.
Material options
As in any dynamic analysis procedure, mass or density (“Density,” Section 21.2.1) must be assigned
to some regions of any separate parts of the model where dynamic response is required. If an analysis
is desired in which the inertia effects are neglected, the density should be set to a very small number.
The following material properties are not active during steady-state dynamic analyses: plasticity and
other inelastic effects, thermal properties (except for thermal expansion), mass diffusion properties,
electrical properties (except for the electrical potential, , in piezoelectric analysis), and pore fluid flow
properties—see “General and linear perturbation procedures,” Section 6.1.3.
Viscoelastic effects can be included in direct-solution steady-state harmonic response analysis.
The linearized viscoelastic response is considered to be a perturbation about a nonlinear preloaded
state, which is computed on the basis of purely elastic behavior (long-term response) in the viscoelastic
components. Therefore, the vibration amplitude must be sufficiently small so that the material response
in the dynamic phase of the problem can be treated as a linear perturbation about the predeformed
state. Viscoelastic frequency domain response is described in “Frequency domain viscoelasticity,”
Section 22.7.2.
Elements
Any of the following elements available in Abaqus/Standard can be used in a steady-state dynamic
procedure:
•
stress/displacement elements (other than generalized axisymmetric elements with twist);
6.3.4–9
Abaqus Version 5.8 ID:
Printed on:
DIRECT-SOLUTION STEADY-STATE DYNAMICS
•
•
•
acoustic elements;
piezoelectric elements; or
hydrostatic fluid elements.
See “Choosing the appropriate element for an analysis type,” Section 27.1.3.
Output
In direct-solution steady-state dynamic analysis the value of an output variable such as strain (E) or stress
(S) is a complex number with real and imaginary components. In the case of data file output the first
printed line gives the real components while the second lists the imaginary components. Results and
data file output variables are also provided to obtain the magnitude and phase of many variables (see
“Abaqus/Standard output variable identifiers,” Section 4.2.1). In the case of data file output the first
printed line gives the magnitudes while the second lists the phase angle.
The following variables are provided specifically for steady-state dynamic analysis:
Element integration point variables:
PHS
PHE
PHEPG
PHEFL
PHMFL
PHMFT
Magnitude and phase angle of all stress components.
Magnitude and phase angle of all strain components.
Magnitude and phase angles of the electrical potential gradient vector.
Magnitude and phase angles of the electrical flux vector.
Magnitude and phase angle of the mass flow rate in fluid link elements.
Magnitude and phase angle of the total mass flow in fluid link elements.
For connector elements, the following element output variables are available:
PHCTF
PHCEF
PHCVF
PHCRF
PHCSF
PHCU
PHCCU
PHCV
PHCA
Magnitude and phase angle of connector total forces.
Magnitude and phase angle of connector elastic forces.
Magnitude and phase angle of connector viscous forces.
Magnitude and phase angle of connector reaction forces.
Magnitude and phase angle of connector friction forces.
Magnitude and phase angle of connector relative displacements.
Magnitude and phase angle of connector constitutive displacements.
Magnitude and phase angle of connector relative velocities.
Magnitude and phase angle of connector relative accelerations.
Nodal variables:
PU
PPOR
PHPOT
PRF
PHCHG
Magnitude and phase angle of all displacement/rotation components at a node.
Magnitude and phase angle of the fluid, pore, or acoustic pressure at a node.
Magnitude and phase angle of the electrical potential at a node.
Magnitude and phase angle of all reaction forces/moments at a node.
Magnitude and phase angle of the reactive charge at a node.
6.3.4–10
Abaqus Version 5.8 ID:
Printed on:
DIRECT-SOLUTION STEADY-STATE DYNAMICS
Element energy densities (such as the elastic strain energy density, SENER) and whole element
energies (such as the total kinetic energy of an element, ELKE) are not available for output in a directsolution steady-state dynamic analysis.
Whole model variables such as ALLIE (total strain energy) are available for direct-solution steadystate dynamic analysis by requesting energy output to the data, results, or output database files (see
“Output to the data and results files,” Section 4.1.2, and “Output to the output database,” Section 4.1.3).
Input file template
*HEADING
…
*AMPLITUDE, NAME=loadamp
Data lines to define an amplitude curve as a function of frequency (cycles/time)
**
*STEP, NLGEOM
Include the NLGEOM parameter so that stress stiffening effects will
be included in the steady-state dynamic step
*STATIC
**Any general analysis procedure can be used to preload the structure
…
*CLOAD and/or *DLOAD
Data lines to prescribe preloads
*TEMPERATURE and/or *FIELD
Data lines to define values of predefined fields for preloading the structure
*BOUNDARY
Data lines to specify boundary conditions to preload the structure
…
*END STEP
**
*STEP
*STEADY STATE DYNAMICS, DIRECT
Data lines to specify frequency ranges and bias parameters
*BOUNDARY, REAL
Data lines to specify real (in-phase) boundary conditions
*BOUNDARY, IMAGINARY
Data lines to specify imaginary (out-of-phase) boundary conditions
*CLOAD, AMPLITUDE=loadamp
Data lines to specify sinusoidally varying, frequency-dependent, concentrated loads
*CLOAD and/or *DLOAD
Data lines to specify sinusoidally varying loads
…
*END STEP
6.3.4–11
Abaqus Version 5.8 ID:
Printed on:
NATURAL FREQUENCY EXTRACTION
6.3.5
NATURAL FREQUENCY EXTRACTION
Products: Abaqus/Standard
Abaqus/CAE
Abaqus/AMS
References
•
•
•
•
•
“Defining an analysis,” Section 6.1.2
“General and linear perturbation procedures,” Section 6.1.3
“Dynamic analysis procedures: overview,” Section 6.3.1
*FREQUENCY
“Configuring a frequency procedure” in “Configuring linear perturbation analysis procedures,”
Section 14.11.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual
Overview
The frequency extraction procedure:
•
•
•
•
•
•
performs eigenvalue extraction to calculate the natural frequencies and the corresponding mode
shapes of a system;
will include initial stress and load stiffness effects due to preloads and initial conditions if geometric
nonlinearity is accounted for in the base state, so that small vibrations of a preloaded structure can
be modeled;
will compute residual modes if requested;
is a linear perturbation procedure;
can be performed using the traditional Abaqus software architecture or, if appropriate, the highperformance SIM architecture (see “Using the SIM architecture for modal superposition dynamic
analyses” in “Dynamic analysis procedures: overview,” Section 6.3.1); and
solves the eigenfrequency problem only for symmetric mass and stiffness matrices; the complex
eigenfrequency solver must be used if unsymmetric contributions, such as the load stiffness, are
needed.
Eigenvalue extraction
The eigenvalue problem for the natural frequencies of an undamped finite element model is
where
is the mass matrix (which is symmetric and positive definite);
6.3.5–1
Abaqus Version 5.8 ID:
Printed on:
NATURAL FREQUENCY EXTRACTION
is the stiffness matrix (which includes initial stiffness effects if the base state
included the effects of nonlinear geometry);
is the eigenvector (the mode of vibration); and
are degrees of freedom.
M and N
is positive definite, all eigenvalues are positive. Rigid body modes and instabilities
When
cause
to be indefinite. Rigid body modes produce zero eigenvalues. Instabilities produce
negative eigenvalues and occur when you include initial stress effects. Abaqus/Standard solves the
eigenfrequency problem only for symmetric matrices.
Selecting the eigenvalue extraction method
Abaqus/Standard provides three eigenvalue extraction methods:
•
•
•
Lanczos
Automatic multi-level substructuring (AMS), an add-on analysis capability for Abaqus/Standard
Subspace iteration
In addition, you must consider the software architecture that will be used for the subsequent modal
superposition procedures. The choice of architecture has minimal impact on the frequency extraction
procedure, but the SIM architecture can offer significant performance improvements over the traditional
architecture for subsequent mode-based steady-state or transient dynamic procedures (see “Using
the SIM architecture for modal superposition dynamic analyses” in “Dynamic analysis procedures:
overview,” Section 6.3.1). The architecture that you use for the frequency extraction procedure is used
for all subsequent mode-based linear dynamic procedures; you cannot switch architectures during an
analysis. The software architectures used by the different eigensolvers are outlined in Table 6.3.5–1.
Table 6.3.5–1
Software architectures available with different eigensolvers.
Software
Architecture
Eigensolver
Lanczos
AMS
Subspace
Iteration
Traditional
SIM
The Lanczos solver with the traditional architecture is the default eigenvalue extraction method
because it has the most general capabilities. However, the Lanczos method is generally slower than the
AMS method. The increased speed of the AMS eigensolver is particularly evident when you require a
large number of eigenmodes for a system with many degrees of freedom. However, the AMS method
has the following limitations:
•
All restrictions imposed on SIM-based linear dynamic procedures also apply to mode-based linear
dynamic analyses based on mode shapes computed by the AMS eigensolver. See “Using the
6.3.5–2
Abaqus Version 5.8 ID:
Printed on:
NATURAL FREQUENCY EXTRACTION
SIM architecture for modal superposition dynamic analyses” in “Dynamic analysis procedures:
overview,” Section 6.3.1, for details.
•
The AMS eigensolver does not compute composite modal damping factors, participation factors,
or modal effective masses. However, if participation factors are needed for primary base motions,
they will be computed but are not written to the printed data (.dat) file.
•
•
You cannot use the AMS eigensolver in an analysis that contains piezoelectric elements.
You cannot request output to the results (.fil) file in an AMS frequency extraction step.
If your model has many degrees of freedom and these limitations are acceptable, you should use the
AMS eigensolver. Otherwise, you should use the Lanczos eigensolver. The Lanczos eigensolver and the
subspace iteration method are described in “Eigenvalue extraction,” Section 2.5.1 of the Abaqus Theory
Manual.
Lanczos eigensolver
For the Lanczos method you need to provide the maximum frequency of interest or the number of
eigenvalues required; Abaqus/Standard will determine a suitable block size (although you can override
this choice, if needed). If you specify both the maximum frequency of interest and the number of
eigenvalues required and the actual number of eigenvalues is underestimated, Abaqus/Standard will issue
a corresponding warning message; the remaining eigenmodes can be found by restarting the frequency
extraction.
You can also specify the minimum frequencies of interest; Abaqus/Standard will extract
eigenvalues until either the requested number of eigenvalues has been extracted in the given range or
all the frequencies in the given range have been extracted.
See “Using the SIM architecture for modal superposition dynamic analyses” in “Dynamic analysis
procedures: overview,” Section 6.3.1, for information on using the SIM architecture with the Lanczos
eigensolver.
Input File Usage:
Abaqus/CAE Usage:
*FREQUENCY, EIGENSOLVER=LANCZOS
Step module: Step→Create: Frequency: Basic: Eigensolver: Lanczos
Choosing a block size for the Lanczos method
In general, the block size for the Lanczos method should be as large as the largest expected multiplicity of
eigenvalues (that is, the largest number of modes with the same frequency). A block size larger than 10
is not recommended. If the number of eigenvalues requested is n, the default block size is the minimum
of (7, n). The choice of 7 for block size proves to be efficient for problems with rigid body modes. The
number of block Lanczos steps within each Lanczos run is usually determined by Abaqus/Standard but
can be changed by you. In general, if a particular type of eigenproblem converges slowly, providing more
block Lanczos steps will reduce the analysis cost. On the other hand, if you know that a particular type
of problem converges quickly, providing fewer block Lanczos steps will reduce the amount of in-core
memory used. The default values are
6.3.5–3
Abaqus Version 5.8 ID:
Printed on:
NATURAL FREQUENCY EXTRACTION
Block size
Maximum number of
block Lanczos steps
1
80
2
50
3
45
≥ 4
35
Automatic multi-level substructuring (AMS) eigensolver
For the AMS method you need only specify the maximum frequency of interest (the global frequency),
and Abaqus/Standard will extract all the modes up to this frequency. You can also specify the minimum
frequencies of interest and/or the number of requested modes. However, specifying these values will not
affect the number of modes extracted by the eigensolver; it will affect only the number of modes that are
stored for output or for a subsequent modal analysis.
The execution of the AMS eigensolver can be controlled by specifying three parameters:
,
, and
. These three parameters multiplied by the maximum
frequency of interest define three cutoff frequencies.
(default value of 5) controls the cutoff
frequency for substructure eigenproblems in the reduction phase, while
and
(default values of 1.7 and 1.1, respectively) control the cutoff frequencies used to define a starting
subspace in the reduced eigensolution phase. Generally, increasing the value of
and
improves the accuracy of the results but may affect the performance of the analysis.
Requesting eigenvectors at all nodes
By default, the AMS eigensolver computes eigenvectors at every node of the model.
Input File Usage:
Abaqus/CAE Usage:
*FREQUENCY, EIGENSOLVER=AMS
Step module: Step→Create: Frequency: Basic: Eigensolver: AMS
Requesting eigenvectors only at specified nodes
Alternatively, you can specify a node set, and eigenvectors will be computed and stored only at the
nodes that belong to that node set. The node set that you specify must include all nodes at which loads
are applied or output is requested in any subsequent modal analysis (this includes any restarted analysis).
If element output is requested or element-based loading is applied, the nodes attached to the associated
elements must also be included in this node set. Computing eigenvectors at only selected nodes improves
performance and reduces the amount of stored data. Therefore, it is recommended that you use this option
for large problems.
Input File Usage:
Abaqus/CAE Usage:
*FREQUENCY, EIGENSOLVER=AMS, NSET=name
Step module: Step→Create: Frequency: Basic: Eigensolver:
AMS: Limit region of saved eigenvectors
6.3.5–4
Abaqus Version 5.8 ID:
Printed on:
NATURAL FREQUENCY EXTRACTION
Controlling the AMS eigensolver
The AMS method consists of the following three phases:
•
Reduction phase: In this phase Abaqus/Standard uses a multi-level substructuring technique to
reduce the full system in a way that allows a very efficient eigensolution of the reduced system. The
approach combines a sparse factorization based on a multi-level supernode elimination tree and a
local eigensolution at each supernode.
Starting from the lowest level supernodes, we use a Craig-Bampton substructure reduction
technique to successively reduce the size of the system as we progress upward in the elimination
tree. At each supernode a local eigensolution is obtained based on fixing the degrees of freedom
connected to the next higher level supernode (these are the local retained or “fixed-interface” degrees
of freedom). At the end of the reduction phase the full system has been reduced such that the reduced
stiffness matrix is diagonal and the reduced mass matrix has unit diagonal values but contains
off-diagonal blocks of nonzero values representing the coupling between the supernodes.
The cost of the reduction phase depends on the system size and the number of eigenvalues
extracted (the number of eigenvalues extracted is controlled indirectly by specifying the highest
eigenfrequency desired). You can make trade-offs between cost and accuracy during the reduction
phase through the
parameter. This parameter multiplied by the highest eigenfrequency
specified for the full model yields the highest eigenfrequency that is extracted in the local supernode
eigensolutions. Increasing the value of
increases the accuracy of the reduction since
more local eigenmodes are retained. However, increasing the number of retained modes also
increases the cost of the reduced eigensolution phase, which is discussed next.
•
Reduced eigensolution phase: In this phase Abaqus/Standard computes the eigensolution of
the reduced system that comes from the previous phase. Although the reduced system typically is
two orders of magnitude smaller in size than the original system, generally it still is too large to
solve directly. Thus, the system is further reduced mainly by truncating the retained eigenmodes
and then solved using a single subspace iteration step. The two AMS parameters,
and
, define a starting subspace of the subspace iteration step. The default values of these
parameters are carefully chosen and provide accurate results in most cases. When a more accurate
solution is needed, the recommended procedure is to increase both parameters proportionally from
their respective default values.
•
Recovery phase: In this phase the eigenvectors of the original system are recovered using
eigenvectors of the reduced problem and local substructure modes. If you request recovery at
specified nodes, the eigenvectors are computed only at those nodes.
Subspace iteration method
For the subspace iteration procedure you need only specify the number of eigenvalues required;
Abaqus/Standard chooses a suitable number of vectors for the iteration. If the subspace iteration
technique is requested, you can also specify the maximum frequency of interest; Abaqus/Standard
extracts eigenvalues until either the requested number of eigenvalues has been extracted or the last
frequency extracted exceeds the maximum frequency of interest.
6.3.5–5
Abaqus Version 5.8 ID:
Printed on:
NATURAL FREQUENCY EXTRACTION
Input File Usage:
Abaqus/CAE Usage:
*FREQUENCY, EIGENSOLVER=SUBSPACE
Step module: Step→Create: Frequency: Basic: Eigensolver: Subspace
Structural-acoustic coupling
Structural-acoustic coupling affects the natural frequency response of systems. In Abaqus only the
Lanczos eigensolver fully includes this effect. In Abaqus/AMS and the subspace eigensolver the effect
of coupling is neglected for the purpose of computing the modes and frequencies; these are computed
using natural boundary conditions at the structural-acoustic coupling surface. An intermediate degree of
consideration of the structural-acoustic coupling operator is the default in Abaqus/AMS and the Lanczos
eigensolver, which is based on the SIM architecture: the coupling is projected onto the modal space and
stored for later use.
Structural-acoustic coupling using the Lanczos eigensolver without the SIM architecture
If structural-acoustic coupling is present in the model and the Lanczos method not based on the SIM
architecture is used, Abaqus/Standard extracts the coupled modes by default. Because these modes
fully account for coupling, they represent the mathematically optimal basis for subsequent modal
procedures. The effect is most noticeable in strongly coupled systems such as steel shells and water.
However, coupled structural-acoustic modes cannot be used in subsequent random response or response
spectrum analyses. You can define the coupling using either acoustic-structural interaction elements
(see “Acoustic interface elements,” Section 32.13.1) or the surface-based tie constraint (see “Acoustic,
shock, and coupled acoustic-structural analysis,” Section 6.10.1). It is possible to ignore coupling when
extracting acoustic and structural modes; in this case the coupling boundary is treated as traction-free
on the structural side and rigid on the acoustic side.
Input File Usage:
Use the following option to account for structural-acoustic coupling during the
frequency extraction:
*FREQUENCY, EIGENSOLVER=LANCZOS,
ACOUSTIC COUPLING=ON (default if the SIM architecture is not used)
Use the following option to ignore structural-acoustic coupling during the
frequency extraction:
*FREQUENCY, EIGENSOLVER=LANCZOS,
ACOUSTIC COUPLING=OFF
Abaqus/CAE Usage:
Step module: Step→Create: Frequency: Basic: Eigensolver: Lanczos,
toggle Include acoustic-structural coupling where applicable
Structural-acoustic coupling using the AMS and Lanczos eigensolver based on the SIM
architecture
For frequency extractions that use the AMS eigensolver or the Lanczos eigensolver based on the SIM
architecture, the modes are computed using traction-free boundary conditions on the structural side of
the coupling boundary and rigid boundary conditions on the acoustic side. Structural-acoustic coupling
operators (see “Acoustic, shock, and coupled acoustic-structural analysis,” Section 6.10.1) are projected
6.3.5–6
Abaqus Version 5.8 ID:
Printed on:
NATURAL FREQUENCY EXTRACTION
by default onto the subspace of eigenvectors. Contributions to these global operators, which come from
surface-based tie constraints defined between structural and acoustic surfaces, are assembled into global
matrices that are projected onto the mode shapes and used in subsequent SIM-based modal dynamic
procedures.
User-defined acoustic-structural interaction elements (see “Acoustic interface elements,”
Section 32.13.1) cannot be used in an AMS eigenvalue extraction analysis.
Input File Usage:
Use either of the following options to project structural-acoustic coupling
operators onto the subspace of eigenvectors:
*FREQUENCY, EIGENSOLVER=AMS,
ACOUSTIC COUPLING=PROJECTION (default for the AMS eigensolver)
or
*FREQUENCY, EIGENSOLVER=LANCZOS, SIM,
ACOUSTIC COUPLING=PROJECTION (default in SIM-based analysis)
Use the following option to disable the projection of structural-acoustic
coupling operators:
Abaqus/CAE Usage:
*FREQUENCY, ACOUSTIC COUPLING=OFF
Use the following option to project structural-acoustic coupling operators onto
the subspace of eigenvectors:
Step module: Step→Create: Frequency: Basic: Eigensolver: AMS,
toggle on Project acoustic-structural coupling where applicable
Use the following option to disable the projection of structural-acoustic
coupling operators:
Step module: Step→Create: Frequency: Basic: Eigensolver: AMS,
toggle off Project acoustic-structural coupling where applicable
Projection of structural-acoustic coupling operators using the Lanczos
eigensolver based on the SIM architecture is not supported in Abaqus/CAE.
Specifying a frequency range for the acoustic modes
Because structural-acoustic coupling is ignored during the AMS and SIM-based Lanczos eigenanalysis,
the computed resonances will, in principle, be higher than those of the fully coupled system. This may
be understood as a consequence of neglecting the mass of the fluid in the structural phase and vice versa.
For the common metal and air case, the structural resonances may be relatively unaffected; however,
some acoustic modes that are significant in the coupled response may be omitted due to the air’s upward
frequency shift during eigenanalysis. Therefore, Abaqus allows you to specify a multiplier, so that the
maximum acoustic frequency in the analysis is taken to be higher than the structural maximum.
Input File Usage:
Use either of the following options:
*FREQUENCY, EIGENSOLVER=AMS
, , , , , , acoustic range factor
6.3.5–7
Abaqus Version 5.8 ID:
Printed on:
NATURAL FREQUENCY EXTRACTION
or
*FREQUENCY, EIGENSOLVER=LANCZOS, SIM
, , , , , , acoustic range factor
Abaqus/CAE Usage:
Step module: Step→Create: Frequency: Basic: Eigensolver: AMS,
Acoustic range factor: acoustic range factor
Specifying a frequency range for the acoustic modes when using the SIM-based
Lanczos eigenanalysis is not supported in Abaqus/CAE.
Effects of fluid motion on natural frequency analysis of acoustic systems
To extract natural frequencies from an acoustic-only or coupled structural-acoustic system in which
fluid motion is prescribed using an acoustic flow velocity, either the Lanczos method or the complex
eigenvalue extraction procedure can be used. In the former case Abaqus extracts real-only eigenvalues
and considers the fluid motion’s effects only on the acoustic stiffness matrix. Thus, these results are of
primary interest as a basis for subsequent linear perturbation procedures. When the complex eigenvalue
extraction procedure is used, the fluid motion effects are included in their entirety; that is, the acoustic
stiffness and damping matrices are included in the analysis.
Frequency shift
For the Lanczos and subspace iteration eigensolvers you can specify a positive or negative shifted
squared frequency, S. This feature is useful when a particular frequency is of concern or when the
natural frequencies of an unrestrained structure or a structure that uses secondary base motions (large
mass approach) are needed. In the latter case a shift from zero (the frequency of the rigid body modes)
will avoid singularity problems or round-off errors for the large mass approach; a negative frequency
shift is normally used. The default is no shift.
If the Lanczos eigensolver is in use and the user-specified shift is outside the requested frequency
range, the shift will be adjusted automatically to a value close to the requested range.
Normalization
For the Lanczos and subspace iteration eigensolvers both displacement and mass eigenvector
normalization are available. Displacement normalization is the default. Mass normalization is the only
option available for SIM-based natural frequency extraction.
The choice of eigenvector normalization type has no influence on the results of subsequent modal
dynamic steps (see “Linear analysis of a rod under dynamic loading,” Section 1.4.9 of the Abaqus
Benchmarks Manual). The normalization type determines only the manner in which the eigenvectors
are represented.
In addition to extracting the natural frequencies and mode shapes, the Lanczos and subspace
iteration eigensolvers automatically calculate the generalized mass, the participation factor, the effective
mass, and the composite modal damping for each mode; therefore, these variables are available for use
in subsequent linear dynamic analyses. The AMS eigensolver computes only the generalized mass.
6.3.5–8
Abaqus Version 5.8 ID:
Printed on:
NATURAL FREQUENCY EXTRACTION
Displacement normalization
If displacement normalization is selected, the eigenvectors are normalized so that the largest displacement
entry in each vector is unity. If the displacements are negligible, as in a torsional mode, the eigenvectors
are normalized so that the largest rotation entry in each vector is unity. In a coupled acoustic-structural
extraction, if the displacements and rotations in a particular eigenvector are small when compared to the
acoustic pressures, the eigenvector is normalized so that the largest acoustic pressure in the eigenvector
is unity. The normalization is done before the recovery of dependent degrees of freedom that have been
previously eliminated with multi-point constraints or equation constraints. Therefore, it is possible that
such degrees of freedom may have values greater than unity.
Input File Usage:
Abaqus/CAE Usage:
*FREQUENCY, NORMALIZATION=DISPLACEMENT
Step module: Step→Create: Frequency: Other: Normalize
eigenvectors by: Displacement
Mass normalization
Alternatively, the eigenvectors can be normalized so that the generalized mass for each vector is unity.
The “generalized mass” associated with mode is
(no sum on )
where
is the structure’s mass matrix and
is the eigenvector for mode . The superscripts N
and M refer to degrees of freedom of the finite element model.
If the eigenvectors are normalized with respect to mass, all the eigenvectors are scaled so that
=1.
For coupled acoustic-structural analyses, an acoustic contribution fraction to the generalized mass is
computed as well.
Input File Usage:
Abaqus/CAE Usage:
*FREQUENCY, NORMALIZATION=MASS
Step module: Step→Create: Frequency: Other: Normalize
eigenvectors by: Mass
Modal participation factors
The participation factor for mode in direction i,
, is a variable that indicates how strongly motion
in the global x-, y-, or z-direction or rigid body rotation about one of these axes is represented in the
eigenvector of that mode. The six possible rigid body motions are indicated by
, 2,
, 6. The
participation factor is defined as
(no sum on )
where
defines the magnitude of the rigid body response of degree of freedom N in the model to
imposed rigid body motion (displacement or infinitesimal rotation) of type i. For example, at a node
with three displacement and three rotation components,
is
6.3.5–9
Abaqus Version 5.8 ID:
Printed on:
NATURAL FREQUENCY EXTRACTION
where is unity and all other
are zero; x, y, and z are the coordinates of the node; and , , and
represent the coordinates of the center of rotation. The participation factors are, thus, defined for the
translational degrees of freedom and for rotation around the center of rotation. For coupled acousticstructural eigenfrequency analysis, an additional acoustic participation factor is computed as outlined in
“Coupled acoustic-structural medium analysis,” Section 2.9.1 of the Abaqus Theory Manual.
Modal effective mass
The effective mass for mode
associated with kinematic direction i (
, 2,
, 6) is defined as
(no sum on )
If the effective masses of all modes are added in any global translational direction, the sum should give
the total mass of the model (except for mass at kinematically restrained degrees of freedom). Thus, if
the effective masses of the modes used in the analysis add up to a value that is significantly less than
the model’s total mass, this result suggests that modes that have significant participation in a certain
excitation direction have not been extracted.
For coupled acoustic-structural eigenfrequency analysis, an additional acoustic effective mass is
computed as outlined in “Coupled acoustic-structural medium analysis,” Section 2.9.1 of the Abaqus
Theory Manual.
Composite modal damping
You can define composite damping factors for each material (“Material damping,” Section 26.1.1), which
are assembled into fractions of critical damping values for each mode,
, according to
(no sum on )
where
is the critical damping fraction given for material a and
is the part of the structure’s
mass matrix made of material a.
A composite damping value will be calculated for each mode. These values are weighted damping
values based on each material’s participation in each mode.
Input File Usage:
Abaqus/CAE Usage:
*DAMPING, COMPOSITE
Property module: Material→Create: Mechanical→Damping: Composite
6.3.5–10
Abaqus Version 5.8 ID:
Printed on:
NATURAL FREQUENCY EXTRACTION
Obtaining residual modes for use in mode-based procedures
Several analysis types in Abaqus/Standard are based on the eigenmodes and eigenvalues of the system.
For example, in a mode-based steady-state dynamic analysis the mass and stiffness matrices and load
vector of the physical system are projected onto a set of eigenmodes resulting in a diagonal system in
terms of modal amplitudes (or generalized degrees of freedom). The solution to the physical system is
obtained by scaling each eigenmode by its corresponding modal amplitude and superimposing the results
(for more information, see “Linear dynamic analysis using modal superposition,” Section 2.5.3 of the
Abaqus Theory Manual).
Due to cost, usually only a small subset of the total possible eigenmodes of the system are
extracted, with the subset consisting of eigenmodes corresponding to eigenfrequencies that are close to
the excitation frequency. Since excitation frequencies typically fall in the range of the lower modes,
it is usually the higher frequency modes that are left out. Depending on the nature of the loading,
the accuracy of the modal solution may suffer if too few higher frequency modes are used. Thus, a
trade-off exists between accuracy and cost. To minimize the number of modes required for a sufficient
degree of accuracy, the set of eigenmodes used in the projection and superposition can be augmented
with additional modes known as residual modes. The residual modes help correct for errors introduced
by mode truncation. In Abaqus/Standard a residual mode, R, represents the static response of the
structure subjected to a nominal (or unit) load, P, corresponding to the actual load that will be used in
the mode-based analysis orthogonalized against the extracted eigenmodes,
followed by an orthogonalization of the residual modes against each other.
This orthogonalization is required to retain the orthogonality properties of the modes (residual and
eigen) with respect to mass and stiffness. As a consequence of the mass and stiffness matrices being
available, the orthogonalization can be done efficiently during the frequency extraction. Hence, if you
wish to include residual modes in subsequent mode-based procedures, you must activate the residual
mode calculations in the frequency extraction step. If the static responses are linearly dependent on each
other or on the extracted eigenmodes, Abaqus/Standard automatically eliminates the redundant responses
for the purpose of computing the residual modes.
For the Lanczos eigensolver you must ensure that the static perturbation response of the load that
will be applied in the subsequent mode-based analysis (i.e.,
) is available by specifying that load in
a static perturbation step immediately preceding the frequency extraction step. If multiple load cases are
specified in this static perturbation analysis, one residual mode is calculated for each load case; otherwise,
it is assumed that all loads are part of a single load case, and only one residual mode will be calculated.
When residual modes are requested, the boundary conditions applied in the frequency extraction step
must match those applied in the preceding static perturbation step. In addition, in the immediately
preceding static perturbation step Abaqus/Standard requires that (1) if multiple load cases are used,
the boundary conditions applied in each load case must be identical, and (2) the boundary condition
magnitudes are zero. When generating dynamic substructures (see “Generating a reduced structural
damping matrix for a substructure” in “Defining substructures,” Section 10.1.2), residual modes usually
6.3.5–11
Abaqus Version 5.8 ID:
Printed on:
NATURAL FREQUENCY EXTRACTION
will provide the most benefit if the loading patterns defined in each of the load cases in the preceding
static perturbation step match the loading patterns defined under the corresponding substructure load
cases in the substructure generation step.
If you use the AMS eigensolver, you do not need to specify the loads in a preceding static
perturbation step. Residual modes are computed at all degrees of freedom at which a concentrated
load is applied in the following mode-based procedure. You can request additional residual modes by
specifying degrees of freedom. One residual mode is computed for every requested degree of freedom.
As an outcome of the orthogonalization process, a pseudo-eigenvalue corresponding to each residual
mode, , is computed and given by
(no sum on )
Henceforth, and in other Abaqus/Standard documentation, the term eigenvalue is used generally to refer
to actual eigenvalues and pseudo-eigenvalues. All data (e.g., participation factors, etc.; see “Output”)
associated with the modes (eigenmodes and residual modes) are ordered by increasing eigenvalue.
Therefore, both eigenmodes and residual modes are assigned mode numbers. In the printed output file
Abaqus/Standard clearly identifies which modes are eigenmodes and which modes are residual modes
so that you can easily distinguish between them. By default, if you activate residual modes, all the
calculated eigenmodes and residual modes will be used in subsequent mode-based procedures, unless:
•
•
You choose to obtain a new set of eigenmodes and residual modes in a new frequency extraction
step.
You choose to select a subset of the available eigenmodes and residual modes in the mode-based
procedure (selection of modes is described in each of the mode-based analysis type sections).
Residual modes cannot be calculated if the cyclic symmetric modeling capability is used. In addition,
the Lanczos or AMS eigensolver must be used if you wish to activate residual mode calculations.
Input File Usage:
Abaqus/CAE Usage:
*FREQUENCY, RESIDUAL MODES
Step module: Step→Create: Frequency: Basic: Include residual modes
Evaluating frequency-dependent material properties
When frequency-dependent material properties are specified, Abaqus/Standard offers the option of
choosing the frequency at which these properties are evaluated for use in the frequency extraction
procedure. This evaluation is necessary because the stiffness cannot be modified during the eigenvalue
extraction procedure. If you do not choose the frequency, Abaqus/Standard evaluates the stiffness
associated with frequency-dependent springs and dashpots at zero frequency and does not consider the
stiffness contributions from frequency domain viscoelasticity. If you do specify a frequency, only the
real part of the stiffness contributions from frequency domain viscoelasticity is considered.
Evaluating the properties at a specified frequency is particularly useful in analyses in which the
eigenfrequency extraction step is followed by a subspace projection steady-state dynamic step (see
“Subspace-based steady-state dynamic analysis,” Section 6.3.9). In these analyses the eigenmodes
extracted in the frequency extraction step are used as global basis functions to compute the steady-state
6.3.5–12
Abaqus Version 5.8 ID:
Printed on:
NATURAL FREQUENCY EXTRACTION
dynamic response of a system subjected to harmonic excitation at a number of output frequencies. The
accuracy of the results in the subspace projection steady-state dynamic step is improved if you choose
to evaluate the material properties at a frequency in the vicinity of the center of the range spanned by
the frequencies specified for the steady-state dynamic step.
Input File Usage:
Abaqus/CAE Usage:
*FREQUENCY, PROPERTY EVALUATION=frequency
Step module: Step→Create: Frequency: Other: Evaluate
dependent properties at frequency
Initial conditions
If the frequency extraction procedure is the first step in an analysis, the initial conditions form the base
state for the procedure (except for initial stresses, which cannot be included in the frequency extraction if
it is the first step). Otherwise, the base state is the current state of the model at the end of the last general
analysis step (“General and linear perturbation procedures,” Section 6.1.3). Initial stress stiffness effects
(specified either through defining initial stresses or through loading in a general analysis step) will be
included in the eigenvalue extraction only if geometric nonlinearity is considered in a general analysis
procedure prior to the frequency extraction procedure.
If initial stresses must be included in the frequency extraction and there is not a general nonlinear
step prior to the frequency extraction step, a “dummy” static step—which includes geometric
nonlinearity and which maintains the initial stresses with appropriate boundary conditions and
loads—must be included before the frequency extraction step.
“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1, describes all of the
available initial conditions.
Boundary conditions
Nonzero magnitudes of boundary conditions in a frequency extraction step will be ignored; the degrees
of freedom specified will be fixed (“Boundary conditions in Abaqus/Standard and Abaqus/Explicit,”
Section 33.3.1).
Boundary conditions defined in a frequency extraction step will not be used in subsequent general
analysis steps (unless they are respecified).
In a frequency extraction step involving piezoelectric elements, the electric potential degree of
freedom must be constrained at least at one node to remove numerical singularities arising from the
dielectric part of the element operator.
Defining primary and secondary bases for modal superposition procedures
If displacements or rotations are to be prescribed in subsequent dynamic modal superposition
procedures, boundary conditions must be applied in the frequency extraction step; these degrees
of freedom are grouped into “bases.” The bases are then used for prescribing motion in the modal
superposition procedure—see “Transient modal dynamic analysis,” Section 6.3.7.
Boundary conditions defined in the frequency extraction step supersede boundary conditions defined
in previous steps. Hence, degrees of freedom that were fixed prior to the frequency extraction step will
6.3.5–13
Abaqus Version 5.8 ID:
Printed on:
NATURAL FREQUENCY EXTRACTION
be associated with a specific base if they are redefined with reference to such a base in the frequency
extraction step.
The primary base
By default, all degrees of freedom listed for a boundary condition will be assigned to an unnamed
“primary” base. If the same motion will be prescribed at all fixed points, the boundary condition is
defined only once; and all prescribed degrees of freedom belong to the primary base.
Unless removed in the frequency extraction step, boundary conditions from the last general analysis
step become fixed boundary conditions for the frequency step and belong to the primary base.
If all rigid body motions are not suppressed by the boundary conditions that make up the primary
base, you must apply a suitable frequency shift to avoid numerical problems.
Input File Usage:
*BOUNDARY
The *BOUNDARY option without the BASE NAME parameter can appear
only once in a frequency extraction step.
Abaqus/CAE Usage:
Load module: Create Boundary Condition
Secondary bases
If the modal superposition procedure will have more than one independent base motion, the driven
nodes must be grouped together into “secondary” bases in addition to the primary base. The secondary
bases must be named. (See “Base motions in modal-based procedures,” Section 2.5.9 of the Abaqus
Theory Manual.) Secondary bases are used only in modal dynamic and steady-state dynamic (not direct)
procedures.
The degrees of freedom associated with secondary bases are not suppressed; instead, a “big” mass
is added to each of them. To provide six digits of numerical accuracy, Abaqus/Standard sets each “big”
mass equal to 106 times the total mass of the structure and each “big” rotary inertia equal to 106 times
the total moment of inertia of the structure. Hence, an artificial low frequency mode is introduced for
every degree of freedom in a secondary base. To keep the requested range of frequencies unchanged,
Abaqus/Standard automatically increases the number of eigenvalues extracted. Consequently, the cost
of the eigenvalue extraction step will increase as more degrees of freedom are included in the secondary
bases. To reduce the analysis cost, keep the number of degrees of freedom associated with secondary
bases to a minimum. This can sometimes be done by reducing several secondary bases that all have the
same prescribed motion to a single node by using BEAM type MPCs (“General multi-point constraints,”
Section 34.2.2).
For the Lanczos and subspace iteration methods a negative shift must be used with either the rigid
body modes or secondary bases.
The “big” masses are not included in the model statistics, and the total mass of the structure and the
printed messages about masses and inertia for the entire model are not affected. However, the presence
of the masses will be noticeable in the output tables printed for the eigenvalue extraction step, as well as
in the information for the generalized masses and effective masses. See “Double cantilever subjected to
multiple base motions,” Section 1.4.12 of the Abaqus Benchmarks Manual, for an example of the use of
the base motion feature.
6.3.5–14
Abaqus Version 5.8 ID:
Printed on:
NATURAL FREQUENCY EXTRACTION
More than one secondary base can be defined by repeating the boundary condition definition and
assigning different base names.
Input File Usage:
Abaqus/CAE Usage:
*BOUNDARY, BASE NAME=name
Load module; Create Boundary Condition; Step: frequency_step;
Category: Mechanical; Types for Selected Step: Secondary
base; Constrained degrees-of-freedom: Region: select region,
U1, U2, U3, UR1, UR2, and/or UR3
Loads
Applied loads (“Applying loads: overview,” Section 33.4.1) are ignored during a frequency extraction
analysis. If loads were applied in a previous general analysis step and geometric nonlinearity
was considered for that prior step, the load stiffness determined at the end of the previous general
analysis step is included in the eigenvalue extraction (“General and linear perturbation procedures,”
Section 6.1.3).
Predefined fields
Predefined fields cannot be prescribed during natural frequency extraction.
Material options
The density of the material must be defined (“Density,” Section 21.2.1). The following material
properties are not active during a frequency extraction: plasticity and other inelastic effects,
rate-dependent material properties, thermal properties, mass diffusion properties, electrical properties
(although piezoelectric materials are active), and pore fluid flow properties—see “General and linear
perturbation procedures,” Section 6.1.3.
Elements
Other than generalized axisymmetric elements with twist, any of the stress/displacement or acoustic
elements in Abaqus/Standard (including those with temperature, pressure, or electrical degrees of
freedom) can be used in a frequency extraction procedure.
Output
The eigenvalues (EIGVAL), eigenfrequencies in cycles/time (EIGFREQ), generalized masses (GM),
composite modal damping factors (CD), participation factors for displacement degrees of freedom 1–6
(PF1–PF6) and acoustic pressure (PF7), and modal effective masses for displacement degrees of freedom
1–6 (EM1–EM6) and acoustic pressure (EM7) are written automatically to the output database as history
data. Output variables such as stress, strain, and displacement (which represent mode shapes) are also
available for each eigenvalue; these quantities are perturbation values and represent mode shapes, not
absolute values.
6.3.5–15
Abaqus Version 5.8 ID:
Printed on:
NATURAL FREQUENCY EXTRACTION
The eigenvalues and corresponding frequencies (in both radians/time and cycles/time) will also
be automatically listed in the printed output file, along with the generalized masses, composite modal
damping factors, participation factors, and modal effective masses.
The only energy density available in eigenvalue extraction procedures is the elastic strain energy
density, SENER. All of the output variable identifiers are outlined in “Abaqus/Standard output variable
identifiers,” Section 4.2.1.
The AMS eigensolver does not compute composite modal damping factors, participation factors,
or modal effective masses. In addition, you cannot request output to the results (.fil) file.
You can restrict output to the results, data, and output database files by selecting the modes for
which output is desired (see “Output to the data and results files,” Section 4.1.2, and “Output to the
output database,” Section 4.1.3).
Input File Usage:
Use one of the following options:
*EL FILE, MODE, LAST MODE
*EL PRINT, MODE, LAST MODE
*OUTPUT, MODE LIST
Abaqus/CAE Usage:
Step module: Output→Field Output Requests→Create:
Frequency: Specify modes
Input file template
*HEADING
…
*BOUNDARY
Data lines to specify zero-valued boundary conditions
*INITIAL CONDITIONS
Data lines to specify initial conditions
**
*STEP (,NLGEOM)
If NLGEOM is used, initial stress and preload stiffness effects
will be included in the frequency extraction step
*STATIC
…
*CLOAD and/or *DLOAD
Data lines to specify loads
*TEMPERATURE and/or *FIELD
Data lines to specify values of predefined fields
*BOUNDARY
Data lines to specify zero-valued or nonzero boundary conditions
*END STEP
**
*STEP, PERTURBATION
*STATIC
6.3.5–16
Abaqus Version 5.8 ID:
Printed on:
NATURAL FREQUENCY EXTRACTION
…
*LOAD CASE, NAME=load case name
Keywords and data lines to define loading for this load case
*END LOAD CASE
…
*END STEP**
*STEP
*FREQUENCY, EIGENSOLVER=LANCZOS, RESIDUAL MODES
Data line to control eigenvalue extraction
*BOUNDARY
*BOUNDARY, BASE NAME=name
Data lines to assign degrees of freedom to a secondary base
*END STEP
6.3.5–17
Abaqus Version 5.8 ID:
Printed on:
COMPLEX EIGENVALUE EXTRACTION
6.3.6
COMPLEX EIGENVALUE EXTRACTION
Products: Abaqus/Standard
Abaqus/CAE
References
•
•
•
•
“Defining an analysis,” Section 6.1.2
“General and linear perturbation procedures,” Section 6.1.3
*COMPLEX FREQUENCY
“Configuring a complex frequency procedure” in “Configuring linear perturbation analysis
procedures,” Section 14.11.2 of the Abaqus/CAE User’s Manual, in the online HTML version of
this manual
Overview
The complex eigenvalue extraction procedure:
•
performs eigenvalue extraction to calculate the complex eigenvalues and the corresponding complex
mode shapes of a system;
•
•
is a linear perturbation procedure;
•
can use the high-performance SIM software architecture (see “Using the SIM architecture for modal
superposition dynamic analyses” in “Dynamic analysis procedures: overview,” Section 6.3.1);
•
will include initial stress and load stiffness effects due to preloads and initial conditions if nonlinear
geometric effects are included in the base state step definition (“General and linear perturbation
procedures,” Section 6.1.3);
•
•
can include friction, damping, and unsymmetric load stiffness contributions;
•
requires that an eigenfrequency extraction procedure (“Natural frequency extraction,” Section 6.3.5)
be performed prior to the complex eigenvalue extraction;
can include unsymmetric damping and stiffness contributions in acoustic finite elements due to
underlying mean flow (“Acoustic, shock, and coupled acoustic-structural analysis,” Section 6.10.1);
and
cannot be used in a model defined as a cyclic symmetric structure (“Analysis of models that exhibit
cyclic symmetry,” Section 10.4.3).
Complex eigenvalue extraction
The complex eigenvalue extraction procedure uses a projection method to extract the complex
eigenvalues of the current system. The eigenvalue problem of the finite element model is formulated in
the following manner:
6.3.6–1
Abaqus Version 5.8 ID:
Printed on:
COMPLEX EIGENVALUE EXTRACTION
where
M and N
is the mass matrix (which is symmetric and, in general, is semi-positive definite);
is the damping matrix;
is the stiffness matrix (which can include initial stress stiffness and friction effects
and, therefore, in general is unsymmetric);
is the complex eigenvalue;
is the complex eigenvector (the mode of vibration); and
are degrees of freedom.
The complex eigenvalue extraction procedure in Abaqus/Standard uses a subspace projection
method; thus, the eigenmodes of the undamped system with the symmetrized stiffness matrix must be
extracted using the eigenfrequency extraction procedure prior to the complex eigenvalue extraction step.
By default, the entire subspace is used as the base vector; this subspace can be reduced as described
below. Abaqus/Standard always computes all the complex eigenmodes available in the projection
subspace (taking into account any user-specified modifications to the subspace). The user-specified
number of requested eigenmodes and frequency range for the complex eigenvalue extraction procedure
do not influence the number of computed complex eigenmodes. It determines only the number of
reported modes, which cannot be higher than the dimension of the projected subspace. To modify the
number of computed eigenmodes, reduce the projection subspace as described below or change the
number of eigenmodes extracted in the prior natural frequency extraction step accordingly. If you do
not specify the number of requested complex modes or the frequency range, all the computed modes
will be reported.
To take into account the unsymmetric effects, the unsymmetric matrix solution and storage scheme
is used automatically for a complex eigenvalue extraction step. The unsymmetric effects will be
disregarded if you specify that the symmetric solution and storage scheme should be used (see “Defining
an analysis,” Section 6.1.2).
Input File Usage:
*COMPLEX FREQUENCY
number of complex eigenmodes, frequency_min, frequency_max
Abaqus/CAE Usage:
Step module: Create Step: Linear perturbation: Complex
frequency: Number of eigenvalues requested: All or Value,
Minimum frequency of interest (cycles/time): value, Maximum
frequency of interest (cycles/time): value
Shift point
You can specify a shift point, S, in cycles per time, for the complex eigenvalue extraction procedure
(S ≥ 0). Abaqus/Standard reports the complex eigenmodes, , in order of increasing
so
that the modes with the imaginary part closest to a given shift point are reported first. This feature is
useful when a particular frequency range is of concern. The default is no shift.
6.3.6–2
Abaqus Version 5.8 ID:
Printed on:
COMPLEX EIGENVALUE EXTRACTION
Input File Usage:
Abaqus/CAE Usage:
*COMPLEX FREQUENCY
, , , S
Step module: Create Step: Linear perturbation: Complex
frequency: Frequency shift (cycles/time): S
Selecting the eigenmodes on which to project
You can select eigenmodes of the undamped system with the symmetrized stiffness matrix on which
the subspace projection will be performed. You can select them by specifying the mode numbers
individually, by requesting that Abaqus/Standard generate the mode numbers automatically, or
by requesting the eigenmodes that belong to specified frequency ranges. If you do not select the
eigenmodes, all modes extracted in the prior eigenfrequency extraction step are used in the modal
superposition.
Input File Usage:
Use one of the following options to select the eigenmodes by specifying mode
numbers:
*SELECT EIGENMODES, DEFINITION=MODE NUMBERS
*SELECT EIGENMODES, GENERATE, DEFINITION=MODE NUMBERS
Use the following option to define the eigenmodes by specifying a frequency
range:
Abaqus/CAE Usage:
*SELECT EIGENMODES, DEFINITION=FREQUENCY RANGE
You cannot select the eigenmodes in Abaqus/CAE; all modes extracted are used
in the subspace projection.
Evaluating frequency-dependent material properties
When frequency-dependent material properties are specified, Abaqus/Standard offers the option of
choosing the frequency at which these properties are evaluated for use in the complex eigenvalue
extraction procedure. This evaluation is necessary because the operators cannot be modified during the
eigenvalue extraction procedure. If you do not choose the frequency, Abaqus/Standard evaluates the
stiffness and damping associated with frequency-dependent springs and dashpots at zero frequency and
does not consider the stiffness and damping contributions from frequency-domain viscoelasticity. If you
do specify a frequency, the stiffness and damping contributions from frequency-domain viscoelasticity
are considered.
Input File Usage:
Abaqus/CAE Usage:
*COMPLEX FREQUENCY, PROPERTY EVALUATION=frequency
Step module: Create Step: Complex Frequency: Other: Evaluate
dependent properties at frequency: value
Contact conditions with sliding friction
Abaqus/Standard automatically detects the contact nodes that are slipping due to velocity differences
imposed by the motion of the reference frame or the transport velocity in prior steps. At those nodes
the tangential degrees of freedom will not be constrained and the effect of friction will result in an
6.3.6–3
Abaqus Version 5.8 ID:
Printed on:
COMPLEX EIGENVALUE EXTRACTION
unsymmetric contribution to the stiffness matrix. At other nodes in contact the tangential degrees of
freedom will be constrained.
Friction at contact nodes at which a velocity differential is imposed can give rise to damping terms.
There are two kinds of friction-induced damping effects. The first effect is caused by the friction forces
stabilizing the vibrations in the direction perpendicular to the slip direction. This effect exists only in
three-dimensional analysis. The second effect is caused by a velocity-dependent friction coefficient. If
the friction coefficient decreases with velocity (which is usually the case), the effect is destabilizing and is
also known as “negative damping.” For more details, see “Coulomb friction,” Section 5.2.3 of the Abaqus
Theory Manual. The complex eigensolver allows you to include these friction-induced contributions to
the damping matrix.
Input File Usage:
Abaqus/CAE Usage:
*COMPLEX FREQUENCY, FRICTION DAMPING=YES
Step module: Create Step: Linear perturbation: Complex frequency:
Include friction-induced damping effects
Damping
In complex eigenvalue extraction analysis damping can be defined by dashpots (see “Dashpots,”
Section 32.2.1), by “Rayleigh” damping associated with materials and elements (see “Material
damping,” Section 26.1.1), and by quiet boundaries on infinite elements or acoustic elements. In
addition, as described in “Contact conditions with sliding friction” above, friction-induced damping
can be included.
Structural damping, damping contributions from frequency-domain viscoelasticity, and all types
of modal damping (except composite modal damping) are supported in complex eigenvalue extraction
using the high-performance SIM architecture.
Prescribing motion, transport velocity, and acoustic flow velocity
Motion, transport velocity, and acoustic flow velocity affect complex frequency analyses. Motion and
transport velocity must be specified in a preceding steady-state transport general step, and their effects
are included in the complex frequency step. The acoustic flow velocity has no effect in steady-state
transport steps, and acoustic flow velocities specified in a steady-state transport step are not propagated
to perturbation steps. The acoustic flow velocity must be specified in each linear perturbation step where
it is desired.
Initial conditions
Initial conditions cannot be specified for complex eigenvalue extraction.
Boundary conditions
Boundary conditions cannot be defined during complex eigenvalue extraction. The boundary conditions
will be the same as in the prior natural frequency extraction analysis.
6.3.6–4
Abaqus Version 5.8 ID:
Printed on:
COMPLEX EIGENVALUE EXTRACTION
Loads
Applied loads (“Applying loads: overview,” Section 33.4.1) are ignored during a complex eigenvalue
extraction. If loads were applied in a previous general analysis step in which nonlinear geometric effects
were included, the load stiffness determined at the end of the previous general analysis step is included
in the complex eigenvalue extraction (see “General and linear perturbation procedures,” Section 6.1.3).
Coriolis distributed loading adds an unsymmetric contribution to the damping operator, which is
currently accounted for only in solid and truss elements.
Predefined fields
Predefined fields cannot be prescribed during complex eigenvalue extraction.
Material options
The density of the material must be defined (see “Density,” Section 21.2.1). The following material
properties are not active during complex eigenvalue extraction:
•
•
plasticity and other inelastic effects;
•
•
•
•
thermal properties;
rate-dependent material properties, excluding friction, which can be rate dependent if the velocity
differential on the contact interface exists;
mass diffusion properties;
electrical properties (although piezoelectric materials are active); and
pore fluid flow properties.
Elements
Other than generalized axisymmetric elements with twist, any of the stress/displacement elements in
Abaqus/Standard (including those with temperature or pressure degrees of freedom) can be used in
complex eigenvalue extraction.
Output
The real (EIGREAL) and imaginary (EIGIMAG) parts of the eigenvalues, ( and ); frequencies
in cycles/time (EIGFREQ); and effective damping ratios (DAMPRATIO =
) are written
automatically to the data (.dat) file and to the output database (.odb) file as history data. In addition,
you can request that the generalized displacements (GU), which are the modes of the projected system,
be written to the output database file (see “Output to the output database,” Section 4.1.3). Output
variables such as stress, strain, and displacement (which represent mode shapes) are also available
for each eigenvalue; these quantities are perturbation values and represent mode shapes, not absolute
values.
6.3.6–5
Abaqus Version 5.8 ID:
Printed on:
COMPLEX EIGENVALUE EXTRACTION
The only energy density available in eigenvalue extraction procedures is the elastic strain energy
density, SENER. All of the output variable identifiers are outlined in “Abaqus/Standard output variable
identifiers,” Section 4.2.1.
You can restrict output to the data file and output database file by selecting the modes for which
output is desired (see “Output to the data and results files,” Section 4.1.2) or “Output to the output
database,” Section 4.1.3). Output to the results (.fil) file is not available for the complex eigenvalue
extraction procedure.
Setting the cutoff value for complex eigenmodes
You can also set the cutoff value for complex eigenmodes, so only complex modes with the real part
of the eigenvalue higher than the cutoff value are written to the output database file. The default cutoff
value is 0.0. If the cutoff value is not set, all complex modes are output.
Input File Usage:
Use one of the following options to select complex eigenmodes for output:
*COMPLEX FREQUENCY, UNSTABLE MODES ONLY
*COMPLEX FREQUENCY, UNSTABLE MODES ONLY=value
The SIM architecture
The complex eigenvalue extraction analysis can be performed using the SIM architecture. The
advantages of performing the complex eigenvalue extraction procedure using the SIM architecture are
as follows:
•
•
•
•
structural damping, including damping defined with viscoelastic material, is taken into account;
modal damping can be specified;
matrices representing the stiffness, mass, and damping can be defined (both symmetric and
unsymmetric matrices are supported); and
the AMS eigensolver can be used to generate the projection subspace for the complex eigenvalue
extraction.
When the AMS eigensolver is used for computing the projection subspace, you should increase the
accuracy of the AMS eigensolution by increasing the values of the AMS parameters and by increasing
the highest frequency of interest. The coupled structural-acoustic modes cannot be used in complex
eigenvalue extraction analysis based on the SIM architecture.
Input file template
*HEADING
…
*SURFACE INTERACTION
*FRICTION
Specify zero friction coefficient
*BOUNDARY
Data lines to specify zero-valued boundary conditions
*INITIAL CONDITIONS
6.3.6–6
Abaqus Version 5.8 ID:
Printed on:
COMPLEX EIGENVALUE EXTRACTION
Data lines to specify initial conditions
**
*STEP (,NLGEOM)
If NLGEOM is used, initial stress and preload stiffness effects
will be included in the eigenvalue extraction steps
*STATIC
…
*CLOAD and/or *DLOAD
Data lines to specify loads
*TEMPERATURE and/or *FIELD
Data lines to specify values of predefined fields
*BOUNDARY
Data lines to specify zero-valued or nonzero boundary conditions
*END STEP
**
*STEP(,NLGEOM)
*STATIC
Data line to define incrementation
*CHANGE FRICTION
*FRICTION
Data lines to redefine friction coefficient
*MOTION, ROTATION or TRANSLATION
Data lines to define the velocity differential
*END STEP
**
*STEP
*FREQUENCY
Data line to control eigenvalue extraction
*END STEP
**
*STEP
*COMPLEX FREQUENCY
Data line to control complex eigenvalue extraction
*SELECT EIGENMODES
Data lines to define applicable mode ranges
*END STEP
6.3.6–7
Abaqus Version 5.8 ID:
Printed on:
MODAL DYNAMIC ANALYSIS
6.3.7
TRANSIENT MODAL DYNAMIC ANALYSIS
Products: Abaqus/Standard
Abaqus/CAE
References
•
•
•
•
•
“Defining an analysis,” Section 6.1.2
“General and linear perturbation procedures,” Section 6.1.3
“Dynamic analysis procedures: overview,” Section 6.3.1
*MODAL DYNAMIC
“Configuring a modal dynamics procedure” in “Configuring linear perturbation analysis
procedures,” Section 14.11.2 of the Abaqus/CAE User’s Manual, in the online HTML version of
this manual
Overview
A modal dynamic analysis:
•
•
•
•
•
is used to analyze transient linear dynamic problems using modal superposition;
can be performed only after a frequency extraction procedure since it bases the structure’s response
on the modes of the system;
can use the high-performance SIM software architecture (see “Using the SIM architecture for modal
superposition dynamic analyses” in “Dynamic analysis procedures: overview,” Section 6.3.1);
can include nondiagonal damping effects (i.e., from material or element damping) only when using
the SIM architecture; and
is a linear perturbation procedure.
Modal dynamic analysis
Transient modal dynamic analysis gives the response of the model as a function of time based on a given
time-dependent loading. The structure’s response is based on a subset of the modes of the system, which
must first be extracted using an eigenfrequency extraction procedure (“Natural frequency extraction,”
Section 6.3.5). The modes will include eigenmodes and, if activated in the eigenfrequency extraction
step, residual modes. The number of modes extracted must be sufficient to model the dynamic response
of the system adequately, which is a matter of judgment on your part.
The modal amplitudes are integrated through time, and the response is synthesized from these modal
responses. For linear systems the modal dynamic procedure is much less expensive computationally than
the direct integration of the entire system of equations performed in the dynamic procedure (“Implicit
dynamic analysis using direct integration,” Section 6.3.2).
As long as the system is linear and is represented correctly by the modes being used (which are
generally only a small subset of the total modes of the finite element model), the method is also very
accurate because the integration operator used is exact whenever the forcing functions vary piecewise
6.3.7–1
Abaqus Version 5.8 ID:
Printed on:
MODAL DYNAMIC ANALYSIS
linearly with time. You should ensure that the forcing function definition and the choice of time increment
are consistent for this purpose. For example, if the forcing is a seismic record in which acceleration
values are given every millisecond and it is assumed that the acceleration varies linearly between these
values, the time increment used in the modal dynamic procedure should be a millisecond.
The user-specified maximum number of increments is ignored in a modal dynamic step. The number
of increments is based on both the time increment and the total time chosen for the step.
While the response in this procedure is for linear vibrations, the prior response can be nonlinear and
stress stiffening (initial stress) effects will be included in the response if nonlinear geometric effects were
included in the step definition for the base state of the eigenfrequency extraction procedure, as explained
in “Natural frequency extraction,” Section 6.3.5.
Selecting the modes and specifying damping
You can select the modes to be used in modal superposition and specify damping values for all selected
modes.
Selecting the modes
You can select modes by specifying the mode numbers individually, by requesting that Abaqus/Standard
generate the mode numbers automatically, or by requesting the modes that belong to specified frequency
ranges. If you do not select the modes, all modes extracted in the prior eigenfrequency extraction step,
including residual modes if they were activated, are used in the modal superposition.
Input File Usage:
Use one of the following options to select the modes by specifying mode
numbers:
*SELECT EIGENMODES, DEFINITION=MODE NUMBERS
*SELECT EIGENMODES, GENERATE, DEFINITION=MODE NUMBERS
Use the following option to select the modes by specifying a frequency range:
Abaqus/CAE Usage:
*SELECT EIGENMODES, DEFINITION=FREQUENCY RANGE
You cannot select the modes in Abaqus/CAE; all modes extracted are used in
the modal superposition.
Specifying modal damping
Damping is almost always specified for a mode-based procedure; see “Material damping,” Section 26.1.1.
You can define a damping coefficient for all or some of the modes used in the response calculation. The
damping coefficient can be given for a specified mode number or for a specified frequency range. When
damping is defined by specifying a frequency range, the damping coefficient for a mode is interpolated
linearly between the specified frequencies. The frequency range can be discontinuous; the average
damping value will be applied for an eigenfrequency at a discontinuity. The damping coefficients are
assumed to be constant outside the range of specified frequencies.
Input File Usage:
Use the following option to define damping by specifying mode numbers:
*MODAL DAMPING, DEFINITION=MODE NUMBERS
6.3.7–2
Abaqus Version 5.8 ID:
Printed on:
MODAL DYNAMIC ANALYSIS
Use the following option to define damping by specifying a frequency range:
Abaqus/CAE Usage:
*MODAL DAMPING, DEFINITION=FREQUENCY RANGE
Use the following input to define damping by specifying mode numbers:
Step module: Create Step: Linear perturbation: Modal dynamics:
Damping
Defining damping by specifying frequency ranges is not supported in
Abaqus/CAE.
Example of specifying damping
Figure 6.3.7–1 illustrates how the damping coefficients at different eigenfrequencies are determined for
the following input:
*MODAL DAMPING, DEFINITION=FREQUENCY RANGE
λi
fi
di
damping values
d=
x
f1
λ1
damping values
2
d3
d4
x
f2
frequencies
d2 + d3
d2 d3
d1
eigenfrequencies
f3
f4
x
λ3
frequency
λ2
Figure 6.3.7–1
Damping coefficients specified by frequency range.
Rules for selecting modes and specifying damping coefficients
The following rules apply for selecting modes and specifying modal damping coefficients:
•
No modal damping is included by default.
6.3.7–3
Abaqus Version 5.8 ID:
Printed on:
MODAL DYNAMIC ANALYSIS
•
Mode selection and modal damping must be specified in the same way, using either mode numbers
or a frequency range.
•
If you do not select any modes, all modes extracted in the prior frequency analysis, including residual
modes if they were activated, will be used in the superposition.
•
If you do not specify damping coefficients for modes that you have selected, zero damping values
will be used for these modes.
•
•
Damping is applied only to the modes that are selected.
Damping coefficients for selected modes that are beyond the specified frequency range are constant
and equal to the damping coefficient specified for the first or the last frequency (depending which
one is closer). This is consistent with the way Abaqus interprets amplitude definitions.
Specifying global damping
For convenience you can specify constant global damping factors for all selected eigenmodes for
mass and stiffness proportional viscous factors, as well as stiffness proportional structural damping.
Structural damping is a commonly used damping model that represents damping as complex stiffness.
This representation causes no difficulty for frequency domain analysis such as steady-state dynamics
for which the solution is already complex. However, the solution must remain real-valued in the time
domain. To allow users to apply their structural damping model in the time domain, a method has
been developed to convert structural damping to an equivalent viscous damping. This technique was
designed so that the viscous damping applied in the frequency domain is identical to the structural
damping if the projected damping matrix is diagonal. For further details, see “Modal dynamic analysis,”
Section 2.5.5 of the Abaqus Theory Manual.
Input File Usage:
*GLOBAL DAMPING, ALPHA=factor, BETA=factor,
STRUCTURAL=factor
Abaqus/CAE Usage:
Defining damping by global factors is not supported in Abaqus/CAE.
Material damping
Structural and viscous material damping (see “Material damping,” Section 26.1.1) is taken into account
in a SIM-based transient modal analysis. Since the projection of damping onto the mode shapes is
performed only one time during the frequency extraction step, significant performance advantages can
be achieved by using the SIM-based transient modal procedure (see “Using the SIM architecture for
modal superposition dynamic analyses” in “Dynamic analysis procedures: overview,” Section 6.3.1).
If the damping operators depend on frequency, they will be evaluated at the frequency specified for
property evaluation during the frequency extraction procedure.
You can deactivate the structural or viscous damping in a transient modal procedure if desired.
Input File Usage:
Abaqus/CAE Usage:
Use the following option to deactivate structural and viscous damping in a
specific transient modal dynamic step:
*DAMPING CONTROLS, STRUCTURAL=NONE, VISCOUS=NONE
Damping controls are not supported in Abaqus/CAE.
6.3.7–4
Abaqus Version 5.8 ID:
Printed on:
MODAL DYNAMIC ANALYSIS
Initial conditions
By default, the modal dynamic step will begin with zero initial displacements. If initial velocities have
been defined (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1), they will be
used; otherwise, the initial velocities will be zero.
Alternatively, you can force the modal dynamic step to carry over the initial conditions from the
immediately preceding step, which must be either another modal dynamic step or a static perturbation
step:
•
In most cases if the immediately preceding step is a modal dynamic step, both the displacements and
velocities are carried over from the end of that step and used as initial conditions for the current step.
For a SIM-based analysis, you should use secondary base motion instead of primary base motion
(see “Prescribed motions in modal superposition procedures”) to carry over the initial conditions;
Abaqus issues a warning message if primary base motion is used.
•
If the immediately preceding step is a static perturbation step, the displacements are carried over
from that step. If initial velocities have been defined (“Initial conditions in Abaqus/Standard and
Abaqus/Explicit,” Section 33.2.1), they will be used; otherwise, the initial velocities will be zero.
Input File Usage:
Use the following option to begin the modal dynamic step with zero initial
displacements:
*MODAL DYNAMIC, CONTINUE=NO
Use the following option to force the modal dynamic step to carry over the
initial conditions from the immediately preceding step:
Abaqus/CAE Usage:
*MODAL DYNAMIC, CONTINUE=YES
Use the following option to begin the modal dynamic step with zero initial
displacements:
Step module: Create Step: Linear perturbation: Modal dynamics:
Basic: Zero initial conditions
Use the following option to force the modal dynamic step to carry over the
initial conditions from the immediately preceding step:
Step module: Create Step: Linear perturbation: Modal dynamics:
Basic: Use initial conditions
Boundary conditions
It is not possible to prescribe nonzero displacements and rotations directly as boundary conditions
(“Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1) in mode-based
dynamic response procedures. In these procedures the motion for nodes can be specified only as base
motion, as described below. Nonzero displacement or acceleration history definitions given as boundary
conditions are ignored in modal superposition procedures, and any changes in the support conditions
from the eigenfrequency extraction step are flagged as errors.
6.3.7–5
Abaqus Version 5.8 ID:
Printed on:
MODAL DYNAMIC ANALYSIS
Prescribed motions in modal superposition procedures
Boundary conditions must be applied during the eigenfrequency extraction step to the degrees of freedom
that will be prescribed in the modal dynamic procedure. These degrees of freedom are grouped into one
or more “bases” (see “Natural frequency extraction,” Section 6.3.5). The unnamed base is called the
“primary” base. Named “secondary” bases must be defined by specifying boundary conditions in the
frequency extraction step. A different motion can be prescribed for each base.
Specifying the degree of freedom and the time history of the motion
The displacements and rotations that are associated with a base are prescribed during the modal dynamic
response procedure. The base motions are fully defined by at most three global translations and
three global rotations. Thus, at most one base motion can be defined for each translation and rotation
component. Base motions are always specified in global directions, regardless of the use of nodal
transformations. You specify the global direction (1–6) for which the base motion is being defined.
If a rotation is specified about an origin that is not the origin of the coordinates, you must specify the
center of rotation.
The time history of a motion must be defined by an amplitude curve (“Amplitude curves,”
Section 33.1.2).
Input File Usage:
Abaqus/CAE Usage:
*BASE MOTION, DOF=n, AMPLITUDE=name
Load module; Create Boundary Condition; Step: modal_dynamic_step;
Category: Mechanical; Types for Selected Step: Displacement
base motion or Velocity base motion or Acceleration base
motion; Basic tabbed page: Degree-of-freedom: U1, U2, U3,
UR1, UR2, or UR3; Amplitude: name
Scaling the amplitude of the base motion
The amplitude curve used to define the time history of the motion can be scaled. By default, the scaling
factor is 1.0.
Input File Usage:
Abaqus/CAE Usage:
*BASE MOTION, DOF=n, AMPLITUDE=name, SCALE=n
Load module; Create Boundary Condition; Step: modal_dynamic_step;
Category: Mechanical; Types for Selected Step: Displacement
base motion or Velocity base motion or Acceleration base motion;
Basic tabbed page: Degree-of-freedom: U1, U2, U3, UR1, UR2, or
UR3; Amplitude: name; Amplitude scale factor: n
Specifying the type of base motion
Base motions can be defined by a displacement, a velocity, or an acceleration history. If the prescribed
excitation record is given in the form of a displacement or velocity history, Abaqus/Standard
differentiates it to obtain the acceleration history. Furthermore, if the displacement or velocity histories
have nonzero initial values, Abaqus/Standard will make corrections to the initial accelerations as
6.3.7–6
Abaqus Version 5.8 ID:
Printed on:
MODAL DYNAMIC ANALYSIS
described in “Modal dynamic analysis,” Section 2.5.5 of the Abaqus Theory Manual. The default is to
give an acceleration history.
Input File Usage:
Abaqus/CAE Usage:
Use one of the following options:
*BASE MOTION, DOF=n, AMPLITUDE=name, TYPE=ACCELERATION
*BASE MOTION, DOF=n, AMPLITUDE=name, TYPE=VELOCITY
*BASE MOTION, DOF=n, AMPLITUDE=name, TYPE=DISPLACEMENT
Load module; Create Boundary Condition; Step: modal_dynamic_step;
Category: Mechanical; Types for Selected Step: Displacement base
motion or Velocity base motion or Acceleration base motion
Specifying secondary base motion
The primary base motion is specified by defining a base motion without referring to a base. If the
base motion is to be applied to a secondary base, it must refer to the name of the base defined in the
eigenfrequency extraction step.
Input File Usage:
*BASE MOTION, DOF=n, AMPLITUDE=name, BASE
NAME=secondary base
Abaqus/CAE Usage:
Load module; Create Boundary Condition; Step: modal_dynamic_step;
Category: Mechanical; Types for Selected Step: Displacement
base motion or Velocity base motion or Acceleration base motion;
toggle on Secondary base: boundary_condition_name
Example
To illustrate the concept of primary and secondary bases, consider a single-bay frame with supports at
nodes 1 and 4. If the input prior to the eigenfrequency extraction step includes the following boundary
conditions:
•
•
•
degrees of freedom 1 through 6 constrained at node 1
degree of freedom 1 constrained at node 4
degrees of freedom 3 through 6 constrained at node 4
and different base motions are assigned to degree of freedom 2 at nodes 1 and 4, the following step
definitions could be used:
•
an eigenfrequency extraction step that includes a boundary condition associated with BASE2
constraining degree of freedom 2 at node 4; and
•
a modal dynamic step that includes two base motion definitions: the primary base motion assigned
to degree of freedom 2 that does not refer to a base and the secondary base motion assigned to
degree of freedom 2 that refers to BASE2.
If boundary conditions were not given prior to the eigenfrequency extraction step, you would have to
define them in the eigenfrequency extraction step. Again, the secondary base would be defined by a
boundary condition with a base name.
6.3.7–7
Abaqus Version 5.8 ID:
Printed on:
MODAL DYNAMIC ANALYSIS
Calculating the response of the structure
The degrees of freedom associated with the primary base are set to zero in the eigenfrequency extraction
step, and primary base motions are introduced by multiplying the base acceleration with the modal
participation factors. Hence, Abaqus/Standard calculates the response of the structure with respect to the
primary base. If the rotational degrees of freedom are references in the primary base motion definition,
the rotation is defined, as default, about the origin of the coordinate system unless you provide the center
of rotation.
The degrees of freedom associated with the secondary bases are not set to zero in the eigenfrequency
extraction step; instead, a “big” mass is added to each of them. Any degree of freedom in a secondary
base that was constrained by a regular boundary condition in a previous general step will be released,
and a big mass will be added to that degree of freedom. Secondary base motions are introduced by nodal
forces, obtained by multiplying the base acceleration with the big mass. Although the secondary base
motions are defined in absolute terms, the response calculated at the secondary bases is relative to the
motion of the primary base for the translational degrees of freedom. The rotational secondary bases are
defined about the nodes included in the node sets specified in the base name definition. Therefore, you
cannot change the center of rotation for secondary bases.
For a more detailed description of the base motion procedure, see “Base motions in modal-based
procedures,” Section 2.5.9 of the Abaqus Theory Manual.
Loads
The following loads can be prescribed in modal dynamic analysis, as described in “Concentrated loads,”
Section 33.4.2:
•
•
Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6).
Distributed pressure forces or body forces can be applied; the distributed load types available with
particular elements are described in Part VI, “Elements.”
Predefined fields
Predefined temperature fields are not allowed in transient modal dynamic analysis. Other predefined
fields are ignored.
Material options
The density of the material must be defined (“Density,” Section 21.2.1). The following material
properties are not active during a modal dynamic analysis: plasticity and other inelastic effects,
rate-dependent material properties, thermal properties, mass diffusion properties, electrical properties
(except for the electrical potential, , in piezoelectric analysis), and pore fluid flow properties. See
“General and linear perturbation procedures,” Section 6.1.3.
6.3.7–8
Abaqus Version 5.8 ID:
Printed on:
MODAL DYNAMIC ANALYSIS
Elements
Other than generalized axisymmetric elements with twist, any of the stress/displacement elements in
Abaqus/Standard (including those with temperature and pressure degrees of freedom) can be used in a
modal dynamic analysis.
Output
All the output variables in Abaqus/Standard are listed in “Abaqus/Standard output variable identifiers,”
Section 4.2.1. The values of nodal solution variables U, V, and A in modal dynamics in the time domain
are relative to the motion of the primary base. Hence, the sum of the relative motion and the base motion
of the primary base yields the total motion; this total motion is available by requesting output variables
TU, TV, and TA. In the absence of primary base motions, the relative and total motions are identical.
The following modal variables can be output to the data or results files (see “Output to the data and
results files,” Section 4.1.2):
GU
GV
GA
SNE
KE
T
BM
Generalized displacements for all modes.
Generalized velocities for all modes.
Generalized accelerations for all modes.
Elastic strain energy for the entire model per each mode.
Kinetic energy for the entire model per each mode.
External work for the entire model per each mode.
Base motion.
Neither element energy densities (such as the elastic strain energy density, SENER) nor whole
element energies (such as the total kinetic energy of an element, ELKE) are available for output in modal
dynamic analysis. However, whole model variables such as ALLIE (total strain energy) are available for
mode-based procedures as output to the data or results files (see “Output to the data and results files,”
Section 4.1.2).
The computational expense of a modal dynamic analysis can be decreased significantly by reducing
the amount of output requested.
Input file template
*HEADING
…
*AMPLITUDE, NAME=amplitude
Data lines to define amplitude variations
**
*STEP
*FREQUENCY
Data line to specify the number of modes to be extracted
*BOUNDARY
6.3.7–9
Abaqus Version 5.8 ID:
Printed on:
MODAL DYNAMIC ANALYSIS
Data lines to assign degrees of freedom to the primary base
*BOUNDARY, BASE NAME=base
Data lines to assign degrees of freedom to a secondary base
*END STEP
**
*STEP
*MODAL DYNAMIC
Data line to control time incrementation
*SELECT EIGENMODES
Data lines to define the applicable mode ranges
*MODAL DAMPING
Data line to define modal damping
*BASE MOTION, DOF=dof, AMPLITUDE=amplitude
*BASE MOTION, DOF=dof, AMPLITUDE=amplitude, BASE NAME=base
*END STEP
6.3.7–10
Abaqus Version 5.8 ID:
Printed on:
MODE-BASED STEADY-STATE DYNAMICS
6.3.8
MODE-BASED STEADY-STATE DYNAMIC ANALYSIS
Products: Abaqus/Standard
Abaqus/CAE
References
•
•
•
•
•
•
•
•
“Defining an analysis,” Section 6.1.2
“General and linear perturbation procedures,” Section 6.1.3
“Dynamic analysis procedures: overview,” Section 6.3.1
“Direct-solution steady-state dynamic analysis,” Section 6.3.4
“Natural frequency extraction,” Section 6.3.5
“Subspace-based steady-state dynamic analysis,” Section 6.3.9
*STEADY STATE DYNAMICS
“Configuring a mode-based steady-state dynamic analysis” in “Configuring linear perturbation
analysis procedures,” Section 14.11.2 of the Abaqus/CAE User’s Manual, in the online HTML
version of this manual
Overview
A mode-based steady-state dynamic analysis:
•
•
•
•
is used to calculate the steady-state dynamic linearized response of a system to harmonic excitation;
is a linear perturbation procedure;
calculates the response based on the system’s eigenfrequencies and modes;
requires that an eigenfrequency extraction procedure be performed prior to the steady-state dynamic
analysis;
•
can use the high-performance SIM software architecture (see “Using the SIM architecture for modal
superposition dynamic analyses” in “Dynamic analysis procedures: overview,” Section 6.3.1);
•
can include nondiagonal damping effects (i.e., from material or element damping) only when using
the SIM architecture;
•
is an alternative to direct-solution steady-state dynamic analysis, in which the system’s response is
calculated in terms of the physical degrees of freedom of the model;
•
•
is computationally cheaper than direct-solution or subspace-based steady-state dynamics;
•
is able to bias the excitation frequencies toward the values that generate a response peak.
is less accurate than direct-solution or subspace-based steady-state analysis, in particular if
significant material damping is present, and
6.3.8–1
Abaqus Version 5.8 ID:
Printed on:
MODE-BASED STEADY-STATE DYNAMICS
Introduction
Steady-state dynamic analysis provides the steady-state amplitude and phase of the response of a system
due to harmonic excitation at a given frequency. Usually such analysis is done as a frequency sweep by
applying the loading at a series of different frequencies and recording the response; in Abaqus/Standard
the steady-state dynamic analysis procedure is used to conduct the frequency sweep.
In a mode-based steady-state dynamic analysis the response is based on modal superposition
techniques; the modes of the system must first be extracted using the eigenfrequency extraction
procedure. The modes will include eigenmodes and, if activated in the eigenfrequency extraction step,
residual modes. The number of modes extracted must be sufficient to model the dynamic response of
the system adequately, which is a matter of judgment on your part.
When defining a mode-based steady-state dynamic step, you specify the frequency ranges of
interest and the number of frequencies at which results are required in each range (including the
bounding frequencies of the range). In addition, you can specify the type of frequency spacing (linear or
logarithmic) to be used, as described below (“Selecting the frequency spacing”). Logarithmic frequency
spacing is the default. Frequencies are given in cycles/time.
These frequency points for which results are required can be spaced equally along the frequency axis
(on a linear or a logarithmic scale), or they can be biased toward the ends of the user-defined frequency
range by introducing a bias parameter (see “The bias parameter,” below).
While the response in this procedure is for linear vibrations, the prior response can be nonlinear.
Initial stress effects (stress stiffening) will be included in the steady-state dynamics response if nonlinear
geometric effects (“General and linear perturbation procedures,” Section 6.1.3) were included in any
general analysis step prior to the eigenfrequency extraction step preceding the steady-state dynamic
procedure.
Input File Usage:
*STEADY STATE DYNAMICS
The DIRECT and SUBSPACE PROJECTION parameters must be omitted
from the *STEADY STATE DYNAMICS option to conduct a mode-based
steady-state dynamic analysis.
Abaqus/CAE Usage:
Step module: Create Step: Linear perturbation: Steady-state
dynamics, Modal
Selecting the type of frequency interval for which output is requested
Three types of frequency intervals are permitted for output from a mode-based steady-state dynamic step.
Specifying the frequency ranges by using the system’s eigenfrequencies
By default, the eigenfrequency type of frequency interval is used; in this case the following intervals
exist in each frequency range:
•
•
First interval: extends from the lower limit of the frequency range given to the first eigenfrequency
in the range.
Intermediate intervals: extend from eigenfrequency to eigenfrequency.
6.3.8–2
Abaqus Version 5.8 ID:
Printed on:
MODE-BASED STEADY-STATE DYNAMICS
•
Last interval: extends from the highest eigenfrequency in the range to the upper limit of the
frequency range.
For each of these intervals the frequencies at which results are calculated are determined using the userdefined number of points (which includes the bounding frequencies for the interval) and the optional bias
function (which is discussed below and allows the sampling points on the frequency scale to be spaced
closer together at eigenfrequencies in the frequency range). Thus, detailed definition of the response
close to resonance frequencies is allowed. Figure 6.3.8–1 illustrates the division of the frequency range
for 5 calculation points and a bias parameter equal to 1.
Input File Usage:
Abaqus/CAE Usage:
*STEADY STATE DYNAMICS, INTERVAL=EIGENFREQUENCY
Step module: Create Step: Linear perturbation: Steady-state
dynamics, Modal: Use eigenfrequencies to subdivide
each frequency range
frequency points
lower end
of the range
Figure 6.3.8–1
mode n
mode n +1
mode n + 2
upper end
of the range
Division of range for the eigenfrequency type of interval and 5 calculation points.
Specifying the frequency ranges by the frequency spread
If the spread type of frequency interval is selected, intervals exist around each eigenfrequency in the
frequency range. For each of the intervals the equally spaced frequencies at which results are calculated
are determined using the user-defined number of points (which includes the bounding frequencies for
the interval). The minimum number of frequency points is 3. If the user-defined value is less than 3 (or
omitted), the default value of 3 points is assumed. Figure 6.3.8–2 illustrates the division of the frequency
range for 5 calculation points.
The bias parameter is not supported with the spread type of frequency interval.
Input File Usage:
*STEADY STATE DYNAMICS, INTERVAL=SPREAD
lwr_freq, upr_freq, numpts, bias_param, freq_scale_factor, spread
Abaqus/CAE Usage:
You cannot specify frequency ranges by frequency spread in Abaqus/CAE.
Specifying the frequency ranges directly
If the alternative range type of frequency interval is chosen, there is only one interval in the specified
frequency range spanning from the lower to the upper limit of the range. This interval is divided using
6.3.8–3
Abaqus Version 5.8 ID:
Printed on:
MODE-BASED STEADY-STATE DYNAMICS
Frequency points
Frequency points
fn
(1 – spread) · fn
fn + 1
(1 + spread) · fn
(1 – spread) · fn + 1
(1 + spread) · fn + 1
Figure 6.3.8–2 Division of range for the spread type of interval and 5 calculation
and
are eigenfrequencies of the system.
points.
the user-defined number of points and the optional bias function, which can be used to space the sampling
frequency points closer to the range limits. For the range type of frequency interval, the peak responses
around the system’s eigenfrequencies may be missed since the sampling frequencies at which output will
be reported will not be biased toward the eigenfrequencies.
Input File Usage:
Abaqus/CAE Usage:
*STEADY STATE DYNAMICS, INTERVAL=RANGE
Step module: Create Step: Linear perturbation: Steady-state
dynamics, Modal: toggle off Use eigenfrequencies to
subdivide each frequency range
Selecting the frequency spacing
Two types of frequency spacing are permitted for a mode-based steady-state dynamic step. For the
logarithmic frequency spacing (the default), the specified frequency ranges of interest are divided using
a logarithmic scale. Alternatively, a linear frequency spacing can be used if a linear scale is desired.
Input File Usage:
Abaqus/CAE Usage:
Use either of the following options:
*STEADY STATE DYNAMICS, FREQUENCY SCALE=LOGARITHMIC
*STEADY STATE DYNAMICS, FREQUENCY SCALE=LINEAR
Step module: Create Step: Linear perturbation: Steady-state
dynamics, Modal: Scale: Logarithmic or Linear
Requesting multiple frequency ranges
You can request multiple frequency ranges or multiple single frequency points for a mode-based steadystate dynamic step.
Input File Usage:
*STEADY STATE DYNAMICS
lwr_freq1, upr_freq1, numpts1, bias_param1, freq_scale_factor1
lwr_freq2, upr_freq2, numpts2, bias_param2, freq_scale_factor2
...
6.3.8–4
Abaqus Version 5.8 ID:
Printed on:
MODE-BASED STEADY-STATE DYNAMICS
single_freq1
single_freq2
...
Repeat the data lines as often as necessary.
Abaqus/CAE Usage:
Step module: Create Step: Linear perturbation: Steady-state dynamics,
Modal: Data: enter data in table, and add rows as necessary
The bias parameter
The bias parameter can be used to provide closer spacing of the results points either toward the middle
or toward the ends of each frequency interval. Figure 6.3.8–3 shows a few examples of the effect of the
bias parameter on the frequency spacing.
frequency points
Bias parameter = 1
f1
f2
Bias parameter = 2
Bias parameter = 3
Bias parameter = 5
Figure 6.3.8–3 Effect of the bias parameter on the frequency
.
spacing for a number of points
The bias formula used to calculate the frequency at which results are presented is as follows:
where
y
n
k
;
is the number of frequency points at which results are to be given within a frequency interval
(discussed above);
is one such frequency point (
);
is the lower limit of the frequency interval;
is the upper limit of the frequency interval;
is the frequency at which the kth results are given;
6.3.8–5
Abaqus Version 5.8 ID:
Printed on:
MODE-BASED STEADY-STATE DYNAMICS
p
is the bias parameter value; and
is the frequency or the logarithm of the frequency, depending on the value used for the
frequency scale parameter.
A bias parameter, p, that is greater than 1.0 provides closer spacing of the results points toward the ends
of the frequency interval, while values of p that are less than 1.0 provide closer spacing toward the middle
of the frequency interval. The default bias parameter is 3.0 for an eigenfrequency interval and 1.0 for a
range frequency interval.
The frequency scale factor
The frequency scale factor can be used to scale frequency points. All the frequency points, except the
lower and upper limit of the frequency range, are multiplied by this factor. This scale factor can be used
only when the frequency interval is specified by using the system’s eigenfrequencies (see “Specifying
the frequency ranges by using the system’s eigenfrequencies,” above).
Selecting the modes and specifying damping
You can select the modes to be used in modal superposition and specify damping values for all selected
modes.
Selecting the modes
You can select modes by specifying the mode numbers individually, by requesting that Abaqus/Standard
generate the mode numbers automatically, or by requesting the modes that belong to specified frequency
ranges. If you do not select the modes, all modes extracted in the prior eigenfrequency extraction step,
including residual modes if they were activated, are used in the modal superposition.
Input File Usage:
Use one of the following options to select the modes by specifying mode
numbers:
*SELECT EIGENMODES, DEFINITION=MODE NUMBERS
*SELECT EIGENMODES, GENERATE, DEFINITION=MODE NUMBERS
Use the following option to select the modes by specifying a frequency range:
Abaqus/CAE Usage:
*SELECT EIGENMODES, DEFINITION=FREQUENCY RANGE
You cannot select the modes in Abaqus/CAE; all modes extracted are used in
the modal superposition.
Specifying modal damping
Damping is almost always specified for a steady-state analysis (see “Material damping,” Section 26.1.1).
If damping is absent, the response of a structure will be unbounded if the forcing frequency is equal
to an eigenfrequency of the structure. To get quantitatively accurate results, especially near natural
frequencies, accurate specification of damping properties is essential. The various damping options
available are discussed in “Material damping,” Section 26.1.1. You can define a damping coefficient for
all or some of the modes used in the response calculation. The damping coefficient can be given for
a specified mode number or for a specified frequency range. When damping is defined by specifying
6.3.8–6
Abaqus Version 5.8 ID:
Printed on:
MODE-BASED STEADY-STATE DYNAMICS
a frequency range, the damping coefficient for a mode is interpolated linearly between the specified
frequencies. The frequency range can be discontinuous; the average damping value will be applied for
an eigenfrequency at a discontinuity. The damping coefficients are assumed to be constant outside the
range of specified frequencies.
Input File Usage:
Use the following option to define damping by specifying mode numbers:
*MODAL DAMPING, DEFINITION=MODE NUMBERS
Use the following option to define damping by specifying a frequency range:
*MODAL DAMPING, DEFINITION=FREQUENCY RANGE
Use the following option to define damping by global factors:
Abaqus/CAE Usage:
Use the following input to define damping by specifying mode numbers:
Step module: Create Step: Linear perturbation:
Steady-state dynamics, Modal: Damping
Defining damping by specifying frequency ranges is not supported in
Abaqus/CAE.
Example of specifying damping
Figure 6.3.8–4 illustrates how the damping coefficients at different eigenfrequencies are determined for
the following input:
*MODAL DAMPING, DEFINITION=FREQUENCY RANGE
Rules for selecting modes and specifying damping coefficients
The following rules apply for selecting modes and specifying modal damping coefficients:
•
•
•
•
•
•
No modal damping is included by default.
Mode selection and modal damping must be specified in the same way, using either mode numbers
or a frequency range.
If you do not select any modes, all modes extracted in the prior frequency analysis, including residual
modes if they were activated, will be used in the superposition.
If you do not specify damping coefficients for modes that you have selected, zero damping values
will be used for these modes.
Damping is applied only to the modes that are selected.
Damping coefficients for selected modes that are beyond the specified frequency range are constant
and equal to the damping coefficient specified for the first or the last frequency (depending which
one is closer). This is consistent with the way Abaqus interprets amplitude definitions.
6.3.8–7
Abaqus Version 5.8 ID:
Printed on:
MODE-BASED STEADY-STATE DYNAMICS
λi
fi
di
damping values
d=
d2 d3
d1
x
λ1
f1
frequencies
damping values
d2 + d3
2
d3
d4
x
f2
eigenfrequencies
f3
f4
x
λ3
frequency
λ2
Figure 6.3.8–4
Damping values specified by frequency range.
Specifying global damping
For convenience you can specify constant global damping factors for all selected eigenmodes for mass
and stiffness proportional viscous factors, as well as stiffness proportional structural damping. For further
details, see “Damping in dynamic analysis” in “Dynamic analysis procedures: overview,” Section 6.3.1.
Input File Usage:
*GLOBAL DAMPING, ALPHA=factor, BETA=factor,
STRUCTURAL=factor
Abaqus/CAE Usage:
Defining damping by global factors is not supported in Abaqus/CAE.
Material damping
Structural and viscous material damping (see “Material damping,” Section 26.1.1) is taken into account
in a SIM-based steady-state dynamic analysis. Since the projection of damping onto the mode shapes is
performed only one time during the frequency extraction step, significant performance advantages can
be achieved by using the SIM-based steady-state dynamic procedure (see “Using the SIM architecture
for modal superposition dynamic analyses” in “Dynamic analysis procedures: overview,” Section 6.3.1).
If the damping operators depend on frequency, they will be evaluated at the frequency specified for
property evaluation during the frequency extraction procedure.
You can deactivate the structural or viscous damping in a mode-based steady-state dynamic
procedure if desired.
Input File Usage:
Abaqus/CAE Usage:
Use the following option to deactivate structural and viscous damping in a
specific steady-state dynamic step:
*DAMPING CONTROLS, STRUCTURAL=NONE, VISCOUS=NONE
Damping controls are not supported in Abaqus/CAE.
6.3.8–8
Abaqus Version 5.8 ID:
Printed on:
MODE-BASED STEADY-STATE DYNAMICS
Initial conditions
The base state is the current state of the model at the end of the last general analysis step prior to the
steady-state dynamic step. If the first step of an analysis is a perturbation step, the base state is determined
from the initial conditions (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1).
Initial condition definitions that directly define solution variables, such as velocity, cannot be used in a
steady-state dynamic analysis.
Boundary conditions
In a mode-based steady-state dynamic analysis both the real and imaginary parts of any degree of freedom
are either restrained or unrestrained; it is physically impossible to have one part restrained and the other
part unrestrained. Abaqus/Standard will automatically restrain both the real and imaginary parts of a
degree of freedom even if only one part is restrained.
Base motion
It is not possible to prescribe nonzero displacements and rotations directly as boundary conditions
(“Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1) in mode-based
dynamic response procedures. Therefore, in a mode-based steady-state dynamic analysis, the motion of
nodes can be specified only as base motion; nonzero displacement or acceleration history definitions
given as boundary conditions are ignored, and any changes in the support conditions from the
eigenfrequency extraction step are flagged as errors. The method for prescribing base motion in modal
superposition procedures is described in “Transient modal dynamic analysis,” Section 6.3.7.
When secondary bases are used, low frequency eigenmodes will be extracted for each “big” mass
applied in the model. Use care when choosing the frequency lower limit range in such cases. The
“big” mass modes are important in the modal superposition; however, the response at zero or arbitrarily
low frequency level should not be requested since it forces Abaqus/Standard to calculate responses at
frequencies between these “big” mass eigenfrequencies, which is not desirable.
Frequency-dependent base motion
An amplitude definition can be used to specify the amplitude of a base motion as a function of frequency
(“Amplitude curves,” Section 33.1.2).
Input File Usage:
Use both of the following options:
Abaqus/CAE Usage:
*AMPLITUDE, NAME=name
*BASE MOTION, REAL or IMAGINARY, AMPLITUDE=name
Load module; Create Boundary Condition; Step: step_name; Category:
Mechanical; Types for Selected Step: Displacement base motion or
Velocity base motion or Acceleration base motion; Basic tabbed page:
Degree-of-freedom: U1, U2, U3, UR1, UR2, or UR3; Amplitude: name
6.3.8–9
Abaqus Version 5.8 ID:
Printed on:
MODE-BASED STEADY-STATE DYNAMICS
Loads
The following loads can be prescribed in a mode-based steady-state dynamic analysis, as described in
“Concentrated loads,” Section 33.4.2:
•
•
Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6).
Distributed pressure forces or body forces can be applied; the distributed load types available with
particular elements are described in Part VI, “Elements.”
These loads are assumed to vary sinusoidally with time over a user-specified range of frequencies. Loads
are given in terms of their real and imaginary components.
Fluid flux loading cannot be used in a steady-state dynamic analysis.
Input File Usage:
Use either of the following input lines to define the real (in-phase) part of the
load:
*CLOAD or *DLOAD
*CLOAD or *DLOAD, REAL
Use the following input line to define the imaginary (out-of-phase) part of the
load:
Abaqus/CAE Usage:
*CLOAD or *DLOAD, IMAGINARY
Load module: load editor: real (in-phase) part + imaginary (out-of-phase)
part i
Frequency-dependent loading
An amplitude definition can be used to specify the amplitude of a load as a function of frequency
(“Amplitude curves,” Section 33.1.2).
Input File Usage:
Use both of the following options:
Abaqus/CAE Usage:
*AMPLITUDE, NAME=name
*CLOAD or *DLOAD, REAL or IMAGINARY, AMPLITUDE=name
Load or Interaction module: Create Amplitude: Name: name
Load module: load editor: real (in-phase) part + imaginary (out-of-phase)
part i: Amplitude: name
Predefined fields
Predefined temperature fields are not allowed in mode-based steady-state dynamic analysis. Other
predefined fields are ignored.
Material options
As in any dynamic analysis procedure, mass or density (“Density,” Section 21.2.1) must be assigned to
some regions of any separate parts of the model where dynamic response is required. The following
material properties are not active during mode-based steady-state dynamic analyses: plasticity and other
6.3.8–10
Abaqus Version 5.8 ID:
Printed on:
MODE-BASED STEADY-STATE DYNAMICS
inelastic effects, viscoelastic effects, thermal properties, mass diffusion properties, electrical properties
(except for the electrical potential, , in piezoelectric analysis), and pore fluid flow properties—see
“General and linear perturbation procedures,” Section 6.1.3.
Elements
Any of the following elements available in Abaqus/Standard can be used in a steady-state dynamics
procedure:
•
•
•
•
stress/displacement elements (other than generalized axisymmetric elements with twist);
acoustic elements;
piezoelectric elements; or
hydrostatic fluid elements.
See “Choosing the appropriate element for an analysis type,” Section 27.1.3.
Output
In mode-based steady-state dynamic analysis the value of an output variable such as strain (E) or stress
(S) is a complex number with real and imaginary components. In the case of data file output the first
printed line gives the real components while the second lists the imaginary components. Results and
data file output variables are also provided to obtain the magnitude and phase of many variables (see
“Abaqus/Standard output variable identifiers,” Section 4.2.1). In this case the first printed line in the
data file gives the magnitude while the second gives the phase angle.
The following variables are provided specifically for steady-state dynamic analysis:
Element integration point variables:
PHS
PHE
PHEPG
PHEFL
PHMFL
PHMFT
Magnitude and phase angle of all stress components.
Magnitude and phase angle of all strain components.
Magnitude and phase angles of the electrical potential gradient vector.
Magnitude and phase angles of the electrical flux vector.
Magnitude and phase angle of the mass flow rate in fluid link elements.
Magnitude and phase angle of the total mass flow in fluid link elements.
For connector elements, the following element output variables are available:
PHCTF
PHCEF
PHCVF
PHCRF
PHCSF
PHCU
PHCCU
Magnitude and phase angle of connector total forces.
Magnitude and phase angle of connector elastic forces.
Magnitude and phase angle of connector viscous forces.
Magnitude and phase angle of connector reaction forces.
Magnitude and phase angle of connector friction forces.
Magnitude and phase angle of connector relative displacements.
Magnitude and phase angle of connector constitutive displacements.
6.3.8–11
Abaqus Version 5.8 ID:
Printed on:
MODE-BASED STEADY-STATE DYNAMICS
Nodal variables:
PU
PPOR
PHPOT
PRF
PHCHG
Magnitude and phase angle of all displacement/rotation components at a node.
Magnitude and phase angle of the fluid or acoustic pressure at a node.
Magnitude and phase angle of the electrical potential at a node.
Magnitude and phase angle of all reaction forces/moments at a node.
Magnitude and phase angle of the reactive charge at a node.
Element energy densities (such as the elastic strain energy density, SENER) and whole element
energies (such as the total kinetic energy of an element, ELKE) are not available for output in a modebased steady-state dynamic analysis.
The standard output variables U, V, A, and the variable PU listed above correspond to motions
relative to the motion of the primary base in a mode-based analysis. Total values, which include the
motion of the primary base, are also available:
TU
TV
TA
PTU
Magnitude of all components of total displacement/rotation at a node.
Magnitude of all components of total velocity at a node.
Magnitude of all components of total acceleration at a node.
Magnitude and phase angle of all total displacement/rotation components at a node.
The following modal variables are also available for mode-based steady-state dynamic analysis and
can be output to the data, results, and/or output database files (see “Output to the data and results files,”
Section 4.1.2, and “Output to the output database,” Section 4.1.3):
GU
GV
GA
GPU
GPV
GPA
SNE
KE
T
BM
Generalized displacements for all modes.
Generalized velocities for all modes.
Generalized accelerations for all modes.
Phase angle of generalized displacements for all modes.
Phase angle of generalized velocities for all modes.
Phase angle of generalized acceleration for all modes.
Elastic strain energy for the entire model per mode.
Kinetic energy for the entire model per mode.
External work for the entire model per mode.
Base motion.
Whole model variables such as ALLIE (total strain energy) are available for mode-based steadystate dynamics as output to the data, results, and/or output database files (see “Output to the data and
results files,” Section 4.1.2).
Input file template
*HEADING
…
6.3.8–12
Abaqus Version 5.8 ID:
Printed on:
MODE-BASED STEADY-STATE DYNAMICS
*AMPLITUDE, NAME=loadamp
Data lines to define an amplitude curve as a function of frequency (cycles/time)
*AMPLITUDE, NAME=base
Data lines to define an amplitude curve to be used to prescribe base motion
**
*STEP, NLGEOM
Include the NLGEOM parameter so that stress stiffening effects will
be included in the steady-state dynamics step
*STATIC
**Any general analysis procedure can be used to preload the structure
…
*CLOAD and/or *DLOAD
Data lines to prescribe preloads
*TEMPERATURE and/or *FIELD
Data lines to define values of predefined fields for preloading the structure
*BOUNDARY
Data lines to specify boundary conditions to preload the structure
*END STEP
**
*STEP
*FREQUENCY
Data line to control eigenvalue extraction
*BOUNDARY
Data lines to assign degrees of freedom to the primary base
*BOUNDARY, BASE NAME=base2
Data lines to assign degrees of freedom to a secondary base
*END STEP
**
*STEP
*STEADY STATE DYNAMICS
Data lines to specify frequency ranges and bias parameters
*SELECT EIGENMODES
Data lines to define the applicable mode ranges
*MODAL DAMPING
Data lines to define the modal damping factors
*BASE MOTION, DOF=dof, AMPLITUDE=base
*BASE MOTION, DOF=dof, AMPLITUDE=base, BASE NAME=base2
*CLOAD and/or *DLOAD, AMPLITUDE=loadamp
Data lines to specify sinusoidally varying, frequency-dependent loads
…
*END STEP
6.3.8–13
Abaqus Version 5.8 ID:
Printed on:
SUBSPACE-BASED STEADY-STATE DYNAMICS
6.3.9
SUBSPACE-BASED STEADY-STATE DYNAMIC ANALYSIS
Products: Abaqus/Standard
Abaqus/CAE
References
•
•
•
•
•
•
•
•
“Defining an analysis,” Section 6.1.2
“General and linear perturbation procedures,” Section 6.1.3
“Dynamic analysis procedures: overview,” Section 6.3.1
“Direct-solution steady-state dynamic analysis,” Section 6.3.4
“Natural frequency extraction,” Section 6.3.5
“Mode-based steady-state dynamic analysis,” Section 6.3.8
*STEADY STATE DYNAMICS
“Configuring a subspace-based steady-state dynamic analysis” in “Configuring linear perturbation
analysis procedures,” Section 14.11.2 of the Abaqus/CAE User’s Manual, in the online HTML
version of this manual
Overview
A subspace-based steady-state dynamic analysis:
•
•
•
•
•
•
•
•
•
•
•
is used to calculate the steady-state dynamic linearized response of a system to harmonic excitation;
is based on projection of the steady-state dynamic equations on a subspace of selected modes of the
undamped system;
is a linear perturbation procedure;
provides a cost-effective way to include frequency-dependent effects (such as frequency-dependent
damping and viscoelastic effects) in the model;
allows for nonsymmetric stiffness;
requires that an eigenfrequency extraction procedure be performed prior to the steady-state dynamic
analysis;
can use the high-performance SIM software architecture (see “Using the SIM architecture for modal
superposition dynamic analyses” in “Dynamic analysis procedures: overview,” Section 6.3.1);
is an alternative to direct-solution steady-state dynamic analysis, in which the system’s response is
calculated in terms of the physical degrees of freedom of the model;
is computationally cheaper than direct-solution steady-state dynamics but more expensive than
mode-based steady-state dynamics;
is less accurate than direct-solution steady-state analysis, in particular if significant material
damping or viscoelasticity with a high loss modulus is present; and
is able to bias the excitation frequencies toward the values that generate a response peak.
6.3.9–1
Abaqus Version 5.8 ID:
Printed on:
SUBSPACE-BASED STEADY-STATE DYNAMICS
Introduction
Steady-state dynamic analysis provides the steady-state amplitude and phase of the response of a system
subjected to harmonic excitation at a given frequency. Usually such analysis is done as a frequency
sweep, by applying the loading at a series of different frequencies and recording the response. In
Abaqus/Standard the subspace-based steady-state dynamic analysis procedure is used to conduct the
frequency sweep.
In a subspace-based steady-state dynamic analysis the response is based on direct solution of the
steady-state dynamic equations projected onto a subspace of modes. The modes of the undamped,
symmetric system must first be extracted using the eigenfrequency extraction procedure. The modes
will include eigenmodes and, if activated in the eigenfrequency extraction step, residual modes. The
procedure is based on the assumption that the forced steady-state vibration can be represented accurately
by a number of modes of the undamped system that are in the range of the excitation frequencies of
interest. The number of modes extracted must be sufficient to model the dynamic response of the system
adequately, which is a matter of judgment on your part. The projection of the dynamic equilibrium
equations onto a subspace of selected modes leads to a small system of complex equations that is solved
for modal amplitudes, which are then used to compute nodal displacements, stresses, etc.
When defining a subspace-based steady-state dynamic step, you specify the frequency ranges
of interest and the number of frequencies at which results are required in each range (including the
bounding frequencies of the range). In addition, you can specify the type of frequency spacing (linear or
logarithmic) to be used, as described below (“Selecting the frequency spacing”). Logarithmic frequency
spacing is the default if the frequency ranges are specified directly or by eigenfrequencies. If the
frequency ranges are specified by the frequency spread, only linear spacing can be used. Frequencies
should be given in cycles/time.
The frequency points for which results are required can be spaced equally along the frequency axis
(on a linear or a logarithmic scale), or they can be biased toward the ends of the user-defined frequency
range by introducing a bias parameter (see “The bias parameter” below).
The subspace-based steady-state dynamic analysis procedure can be used:
•
•
•
for nonsymmetric stiffness;
when any form of damping (except modal damping) is included; and
when viscoelastic material properties must be taken into account.
While the response in this procedure is for linear vibrations, the prior response can be nonlinear.
Initial stress effects (stress stiffening) will be included in the steady-state dynamic response if nonlinear
geometric effects (“General and linear perturbation procedures,” Section 6.1.3) were included in any
general analysis step prior to the eigenfrequency extraction step preceding the subspace-based steadystate dynamic procedure.
Input File Usage:
Abaqus/CAE Usage:
*STEADY STATE DYNAMICS, SUBSPACE PROJECTION
Step module: Create Step: Linear perturbation: Steady-state
dynamics, Subspace
6.3.9–2
Abaqus Version 5.8 ID:
Printed on:
SUBSPACE-BASED STEADY-STATE DYNAMICS
Ignoring damping
If damping terms can be ignored, you can specify that a real, rather than a complex, system matrix be
generated and projected, which can significantly reduce computational time, at the cost of ignoring the
damping effects.
Input File Usage:
Abaqus/CAE Usage:
*STEADY STATE DYNAMICS, SUBSPACE PROJECTION, REAL ONLY
Step module: Create Step: Linear perturbation: Steady-state
dynamics, Subspace: Compute real response only
Selecting the type of frequency interval for which output is requested
Three types of frequency intervals are permitted for output from a subspace-based steady-state dynamic
step.
Specifying the frequency ranges by using the system’s eigenfrequencies
By default, the eigenfrequency type of frequency interval is used; in this case the following intervals
exist in each frequency range:
•
First interval: extends from the lower limit of the frequency range given to the first eigenfrequency
in the range.
•
•
Intermediate intervals: extend from eigenfrequency to eigenfrequency.
Last interval: extends from the highest eigenfrequency in the range to the upper limit of the
frequency range.
For each of these intervals the frequencies at which results are calculated are determined using the userdefined number of points (which includes the bounding frequencies for the interval) and the optional bias
function (which is discussed below and allows the sampling points on the frequency scale to be spaced
closer together at eigenfrequencies in the frequency range). Thus, detailed definition of the response
close to resonance frequencies is allowed. Figure 6.3.9–1 illustrates the division of the frequency range
for 5 calculation points and a bias parameter equal to 1.
frequency points
lower end
of the range
Figure 6.3.9–1
mode n
mode n +1
mode n + 2
upper end
of the range
Division of range for the eigenfrequency type of interval and 5 calculation points.
6.3.9–3
Abaqus Version 5.8 ID:
Printed on:
SUBSPACE-BASED STEADY-STATE DYNAMICS
Input File Usage:
*STEADY STATE DYNAMICS, SUBSPACE PROJECTION,
INTERVAL=EIGENFREQUENCY
Abaqus/CAE Usage:
Step module: Create Step: Linear perturbation: Steady-state
dynamics, Subspace: Use eigenfrequencies to subdivide
each frequency range
Specifying the frequency ranges by the frequency spread
If the spread type of frequency interval is selected, intervals exist around each eigenfrequency in the
frequency range. For each of the intervals the equally spaced frequencies at which results are calculated
are determined using the user-defined number of points (which includes the bounding frequencies for
the interval). The minimum number of frequency points is 3. If the user-defined value is less than 3 (or
omitted), the default value of 3 points is assumed. Figure 6.3.9–2 illustrates the division of the frequency
range for 5 calculation points.
The bias parameter is not supported with the spread type of frequency interval.
Frequency points
Frequency points
fn
(1 – spread) · fn
fn + 1
(1 + spread) · fn
(1 – spread) · fn + 1
(1 + spread) · fn + 1
Figure 6.3.9–2 Division of range for the spread type of interval and 5 calculation
and
are eigenfrequencies of the system.
points.
Input File Usage:
*STEADY STATE DYNAMICS, SUBSPACE PROJECTION,
INTERVAL=SPREAD
lwr_freq, upr_freq, numpts, bias_param, freq_scale_factor, spread
Abaqus/CAE Usage:
You cannot specify frequency ranges by frequency spread in Abaqus/CAE.
Specifying the frequency ranges directly
If the alternative range type of frequency interval is chosen, there is only one interval in the specified
frequency range spanning from the lower to the upper limit of the range. This interval is divided using
the user-defined number of points and the optional bias function, which can be used to space the sampling
frequency points closer to the range limits. For the range type of frequency interval, the peak responses
6.3.9–4
Abaqus Version 5.8 ID:
Printed on:
SUBSPACE-BASED STEADY-STATE DYNAMICS
around the system’s eigenfrequencies may be missed since the sampling frequencies at which output will
be reported will not be biased toward the eigenfrequencies.
Input File Usage:
*STEADY STATE DYNAMICS, SUBSPACE PROJECTION,
INTERVAL=RANGE
Abaqus/CAE Usage:
Step module: Create Step: Linear perturbation: Steady-state
dynamics, Subspace: toggle off Use eigenfrequencies to
subdivide each frequency range
Selecting the frequency spacing
Two types of frequency spacing are permitted for a subspace-based steady-state dynamic step. For the
logarithmic frequency spacing (the default), the specified frequency ranges of interest are divided using
a logarithmic scale. Alternatively, a linear frequency spacing can be used if a linear scale is desired.
Input File Usage:
Use the following option to specify logarithmic frequency spacing:
*STEADY STATE DYNAMICS, SUBSPACE PROJECTION,
FREQUENCY SCALE=LOGARITHMIC (default)
Use the following option to specify linear frequency spacing:
*STEADY STATE DYNAMICS, SUBSPACE PROJECTION,
FREQUENCY SCALE=LINEAR
Abaqus/CAE Usage:
Step module: Create Step: Linear perturbation: Steady-state
dynamics, Subspace: Scale: Logarithmic or Linear
Requesting multiple frequency ranges
You can request multiple frequency ranges for a subspace-based steady-state dynamic step. When both
frequency ranges and additional single frequency points are requested, the frequency ranges must be
specified first.
Input File Usage:
Repeat the data lines as often as necessary to request multiple frequency ranges
or multiple single frequency points:
*STEADY STATE DYNAMICS, SUBSPACE PROJECTION
lwr_freq1, upr_freq1, numpts1, bias_param1, freq_scale_factor1
lwr_freq2, upr_freq2, numpts2, bias_param2, freq_scale_factor2
...
single_freq1
single_freq2
...
Abaqus/CAE Usage:
Step module: Create Step: Linear perturbation: Steady-state dynamics,
Subspace: Data: enter data in table, and add rows as necessary
The bias parameter
The bias parameter can be used to provide closer spacing of the results points either toward the middle
or toward the ends of each frequency interval. Figure 6.3.9–3 shows a few examples of the effect of the
bias parameter on the frequency spacing.
6.3.9–5
Abaqus Version 5.8 ID:
Printed on:
SUBSPACE-BASED STEADY-STATE DYNAMICS
frequency points
Bias parameter = 1
f1
f2
Bias parameter = 2
Bias parameter = 3
Bias parameter = 5
Figure 6.3.9–3 Effect of the bias parameter on the frequency
.
spacing for a number of points
The bias formula used in subspace-based steady-state dynamics is
where
;
y
n
is the number of frequency points at which results are to be given within a frequency interval
(discussed above);
k
is one such frequency point (
);
is the lower limit of the frequency interval;
is the upper limit of the frequency interval;
is the frequency at which the kth results are given;
p
is the bias parameter value; and
is the frequency or the logarithm of the frequency, depending on the value chosen for the
frequency scale.
A bias parameter, p, that is greater than 1.0 provides closer spacing of the results points toward the ends
of the frequency interval, while values of p that are less than 1.0 provide closer spacing toward the middle
of the frequency interval. The default bias parameter is 3.0 for an eigenfrequency interval and 1.0 for a
range frequency interval.
6.3.9–6
Abaqus Version 5.8 ID:
Printed on:
SUBSPACE-BASED STEADY-STATE DYNAMICS
The frequency scale factor
The frequency scale factor can be used to scale frequency points. All the frequency points, except the
lower and upper limit of the frequency range, are multiplied by this factor. This scale factor can be used
only when the frequency interval is specified by using the system’s eigenfrequencies (see “Specifying
the frequency ranges by using the system’s eigenfrequencies,” above).
Damping
If damping is absent, the response of a structure will be unbounded if the forcing frequency is equal
to an eigenfrequency of the structure. To get quantitatively accurate results, especially near natural
frequencies, accurate specification of damping properties is essential. The various damping options
available are discussed in “Material damping,” Section 26.1.1.
In subspace-based steady-state dynamic analysis damping can be created by the following:
•
•
•
•
•
•
dashpots (see “Dashpots,” Section 32.2.1),
“Rayleigh” damping associated with materials and elements (see “Material damping,”
Section 26.1.1),
structural damping (see “Damping in dynamic analysis” in “Dynamic analysis procedures:
overview,” Section 6.3.1),
viscoelasticity included in the material definitions (see “Frequency domain viscoelasticity,”
Section 22.7.2),
contributions from infinite elements (see “Infinite elements,” Section 28.3.1) or defined impedance
conditions (see “Acoustic and shock loads,” Section 33.4.6) on acoustic elements, and
“volumetric drag” (viscous Rayleigh damping) in acoustic elements (see “Acoustic medium,”
Section 26.3.1).
If you specify that a real-only system matrix be generated and projected (see “Ignoring damping”
above), all forms of damping are ignored, including quiet boundaries on infinite elements and
nonreflecting boundaries on acoustic elements.
Contact conditions with sliding friction
Abaqus/Standard automatically detects the contact nodes that are slipping due to velocity differences
imposed by the motion of the reference frame or the transport velocity in prior steps. At those nodes the
tangential degrees of freedom are not constrained and the effect of friction results in an unsymmetric
contribution to the stiffness matrix. At other contact nodes the tangential degrees of freedom are
constrained.
Friction at contact nodes at which a velocity differential is imposed can give rise to damping terms.
There are two kinds of friction-induced damping effects. The first effect is caused by the friction forces
stabilizing the vibrations in the direction perpendicular to the slip direction. This effect exists only in
three-dimensional analysis. The second effect is caused by a velocity-dependent friction coefficient. If
the friction coefficient decreases with velocity (which is usually the case), the effect is destabilizing and
6.3.9–7
Abaqus Version 5.8 ID:
Printed on:
SUBSPACE-BASED STEADY-STATE DYNAMICS
is also known as “negative damping.” For more details, see “Coulomb friction,” Section 5.2.3 of the
Abaqus Theory Manual. Subspace-based steady-state dynamics analysis allows you to include these
friction-induced contributions to the damping matrix.
Input File Usage:
*STEADY STATE DYNAMICS, SUBSPACE PROJECTION,
FRICTION DAMPING=YES
Abaqus/CAE Usage:
Step module: Create Step: Linear perturbation: Steady-state dynamics,
Subspace: Include friction-induced damping effects
Selecting the modes on which to project
You can select modes by specifying the mode numbers individually, by requesting that Abaqus/Standard
generate the mode numbers automatically, or by requesting the modes that belong to specified frequency
ranges. If you do not select the modes, all modes extracted in the prior eigenfrequency extraction step,
including residual modes if they were activated, are used in the modal superposition.
Input File Usage:
Use the following option to select the modes by specifying mode numbers
individually:
*SELECT EIGENMODES, DEFINITION=MODE NUMBERS
Use the following option to request that Abaqus/Standard generate the mode
numbers automatically:
*SELECT EIGENMODES, GENERATE, DEFINITION=MODE NUMBERS
Use the following option to select the modes by specifying a frequency range:
Abaqus/CAE Usage:
*SELECT EIGENMODES, DEFINITION=FREQUENCY RANGE
You cannot select the modes in Abaqus/CAE; all modes extracted are used in
the modal superposition.
Selecting the subspace projection frequency
You can control the frequency of the subspace projections. By default, the dynamic equations are
projected onto the subspace at each frequency you request. However, considerable computational
savings can be obtained if the projection onto the subspace is performed only at selected frequency
points.
Projecting the subspace at each frequency requested
By default, the dynamic equations are projected onto the subspace at each frequency you requested. This
is the most computationally expensive method. If coupled acoustic-structural modes are extracted in the
preceding eigenfrequency extraction step, this is the only method allowed.
Input File Usage:
Use either of the following options:
*STEADY STATE DYNAMICS, SUBSPACE PROJECTION
*STEADY STATE DYNAMICS,
SUBSPACE PROJECTION=ALL FREQUENCIES
6.3.9–8
Abaqus Version 5.8 ID:
Printed on:
SUBSPACE-BASED STEADY-STATE DYNAMICS
Abaqus/CAE Usage:
Step module: Create Step: Linear perturbation: Steady-state dynamics,
Subspace: Projection: Evaluate at each frequency
Projecting the subspace using model properties at the center frequency of all ranges
You can perform only one projection using model properties evaluated at the center frequency of all
ranges and individual frequency points specified. The center frequency is determined on a logarithmic
or linear scale depending on the spacing requested.
This method is the least expensive. However, it should be chosen only when the material properties
do not depend strongly on frequency.
Input File Usage:
Abaqus/CAE Usage:
*STEADY STATE DYNAMICS, SUBSPACE PROJECTION=CONSTANT
Step module: Create Step: Linear perturbation: Steady-state
dynamics, Subspace: Projection: Constant
Projecting the subspace at each extracted eigenfrequency
You can perform the projections at each extracted eigenfrequency in the requested frequency range and
at eigenfrequencies immediately outside the range. The projected mass, stiffness, and damping matrices
are then interpolated at each frequency point requested. The interpolation is performed on a linear or
logarithmic scale depending on the spacing requested.
Input File Usage:
*STEADY STATE DYNAMICS,
SUBSPACE PROJECTION=EIGENFREQUENCY
Abaqus/CAE Usage:
Step module: Create Step: Linear perturbation: Steady-state dynamics,
Subspace: Projection: Interpolate at eigenfrequencies
Projecting the subspace based on material property changes as a function of frequency
You can select how often subspace projections are performed based on material property changes as
a function of frequency. You specify the relative change in material stiffness and damping properties
allowed before a new projection is performed. In the beginning of the subspace-based steady-state
dynamic step Abaqus/Standard computes a table of relative changes in material stiffness and damping
properties, and projections are performed based on the strictest of the two criteria. The projections
are then interpolated at each requested frequency point as described above. The default value for the
allowable stiffness or damping change is 0.1.
Input File Usage:
*STEADY STATE DYNAMICS,
SUBSPACE PROJECTION=PROPERTY CHANGE,
DAMPING CHANGE=percentage, STIFFNESS CHANGE=percentage
Abaqus/CAE Usage:
Step module: Create Step: Linear perturbation: Steady-state dynamics,
Subspace: Projection: As a function of property changes, Max.
damping change: percentage, Max. stiffness change: percentage
6.3.9–9
Abaqus Version 5.8 ID:
Printed on:
SUBSPACE-BASED STEADY-STATE DYNAMICS
Projecting the subspace at the limits of each frequency range
You can select how often subspace projections are performed based on the limits of each frequency range.
The projections onto the modal subspace of the dynamic equations are performed at the lower limit of
each frequency range and at the upper limit of the last frequency range. The interpolation of the projected
mass, stiffness, and damping matrices is performed on a linear scale. This method can be used only with
the SIM architecture.
This method should be chosen when the frequency dependence of material properties is close to
linear within a frequency range.
Input File Usage:
Abaqus/CAE Usage:
*STEADY STATE DYNAMICS, SUBSPACE PROJECTION=RANGE
Step module: Create Step: Linear perturbation: Steady-state dynamics,
Subspace: Projection: Interpolate at lower and upper frequency limits
Initial conditions
The base state is the current state of the model at the end of the last general analysis step prior to the
steady-state dynamic step. If the first step of an analysis is a perturbation step, the base state is determined
from the initial conditions (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1).
Initial condition definitions that directly define solution variables, such as velocity, cannot be used in a
steady-state dynamic analysis.
Boundary conditions
In a subspace-based steady-state dynamic analysis both the real and imaginary parts of any degree of
freedom are either restrained or unrestrained; it is physically impossible to have one part restrained and
the other part unrestrained. Abaqus/Standard will restrain both the real and imaginary parts of a degree
of freedom automatically even if only one part is restrained.
Base motion
It is not possible to prescribe nonzero displacements and rotations directly as boundary conditions
(“Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1) in subspace-based
steady-state dynamic analysis. Instead, prescribed motion can be specified as base motion; nonzero
displacement or acceleration history definitions given as boundary conditions are ignored, and any
changes in the support conditions from the eigenfrequency extraction step are flagged as errors. The
method for prescribing base motion in modal superposition procedures is described in “Transient modal
dynamic analysis,” Section 6.3.7.
Frequency-dependent base motion
An amplitude definition can be used to specify the amplitude of a base motion as a function of frequency
(“Amplitude curves,” Section 33.1.2).
Input File Usage:
Use both of the following options:
*AMPLITUDE, NAME=name
*BASE MOTION, REAL or IMAGINARY, AMPLITUDE=name
6.3.9–10
Abaqus Version 5.8 ID:
Printed on:
SUBSPACE-BASED STEADY-STATE DYNAMICS
Abaqus/CAE Usage:
Load module; Create Boundary Condition; Step: step_name; Category:
Mechanical; Types for Selected Step: Displacement base motion or
Velocity base motion or Acceleration base motion; Basic tabbed page:
Degree-of-freedom: U1, U2, U3, UR1, UR2, or UR3; Amplitude: name
Loads
The following loads can be prescribed in a subspace-based steady-state dynamic analysis, as described
in “Concentrated loads,” Section 33.4.2:
•
•
Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6).
•
Incident wave loads can be applied; see “Acoustic and shock loads,” Section 33.4.6. Incident wave
loads can be used to model sound waves from distinct planar or spherical sources or from diffuse
fields.
Distributed pressure forces or body forces can be applied; the distributed load types available with
particular elements are described in Part VI, “Elements.”
These loads are assumed to vary sinusoidally with time over a user-specified range of frequencies. Loads
are given in terms of their real and imaginary components.
Input File Usage:
Use either of the following input lines to define the real (in-phase) part of the
load:
*CLOAD or *DLOAD
*CLOAD or *DLOAD, REAL
Use the following input line to define the imaginary (out-of-phase) part of the
load:
Abaqus/CAE Usage:
*CLOAD or *DLOAD, IMAGINARY
You can only define the real (in phase) part of the load in Abaqus/CAE.
Load module: load editor: real (in-phase) part
Frequency-dependent loading
An amplitude definition can be used to specify the amplitude of a load as a function of frequency
(“Amplitude curves,” Section 33.1.2).
Input File Usage:
Use both of the following options:
Abaqus/CAE Usage:
*AMPLITUDE, NAME=name
*CLOAD or *DLOAD, REAL or IMAGINARY, AMPLITUDE=name
Load or Interaction module: Create Amplitude: Name: name
Load module: load editor: Amplitude: name
6.3.9–11
Abaqus Version 5.8 ID:
Printed on:
SUBSPACE-BASED STEADY-STATE DYNAMICS
Loading limitations
Coriolis distributed loading adds an imaginary antisymmetric contribution to the overall system of
equations. This contribution is currently accounted for in solid and truss elements only and is activated
by requesting the unsymmetric matrix storage and solution scheme for the step.
Fluid flux loading cannot be used in subspace-based steady-state dynamic analysis.
Predefined fields
Predefined temperature fields can be specified in subspace-based steady-state dynamic analysis (see
“Predefined fields,” Section 33.6.1) and will produce harmonically varying thermal strains if thermal
expansion is included in the material definition (“Thermal expansion,” Section 26.1.2). Other predefined
fields are ignored.
Material options
As in any dynamic analysis procedure, mass or density (“Density,” Section 21.2.1) must be assigned
to some regions of any separate parts of the model where dynamic response is required. If an analysis
is desired in which the inertia effects are neglected, the density should be set to a very small number.
Natural damping, as well as individual dashpots, can be included in this procedure.
Viscoelastic effects can be included in subspace-based steady-state dynamic analysis. The
linearized viscoelastic response is considered to be a perturbation about a nonlinear preloaded state,
which is computed on the basis of purely elastic behavior (long-term response) in the viscoelastic
components. Therefore, the vibration amplitude must be sufficiently small so that the material response
in the dynamic phase of the problem can be treated as a linear perturbation about the predeformed
state. Viscoelastic frequency domain response is described in “Frequency domain viscoelasticity,”
Section 22.7.2.
The following material properties are not active during subspace-based steady-state dynamic
analyses: plasticity and other inelastic effects, thermal properties (except for thermal expansion), mass
diffusion properties, electrical properties (except for the electrical potential, , in piezoelectric analysis),
and pore fluid flow properties—see “General and linear perturbation procedures,” Section 6.1.3.
Numerical investigations show that in general the accuracy of the results in the subspace-based
steady-state dynamic step is improved if in the previous eigenfrequency extraction step the material
properties are evaluated at a frequency in the vicinity of the center of the range spanned by
the frequencies specified for the steady-state dynamic step (see “Natural frequency extraction,”
Section 6.3.5). In this case the modes extracted in the previous eigenfrequency extraction step for the
undamped system will reflect most accurately the modes of the damped system at frequencies located in
the proximity of the frequency at which the material properties are evaluated. Thus, if the steady-state
dynamic response is sought for a large span of frequencies and the specified material properties vary
significantly over this span, the results will be more accurate if the range is divided into smaller ranges
and several separate analyses are run over these smaller ranges with the material properties evaluated
at appropriate frequencies.
6.3.9–12
Abaqus Version 5.8 ID:
Printed on:
SUBSPACE-BASED STEADY-STATE DYNAMICS
Elements
Any of the following elements available in Abaqus/Standard can be used in a subspace-based steady-state
dynamic analysis:
•
•
•
•
stress/displacement elements (other than generalized axisymmetric elements with twist);
acoustic elements;
piezoelectric elements; and
hydrostatic fluid elements.
See “Choosing the appropriate element for an analysis type,” Section 27.1.3.
Output
In subspace-based steady-state dynamic analysis the value of an output variable such as strain (E) or
stress (S) is a complex number with real and imaginary components. In the case of data file output the
first printed line gives the real components while the second lists the imaginary components. Results
and data file output variables are also provided to obtain the magnitude and phase of many variables (see
“Abaqus/Standard output variable identifiers,” Section 4.2.1). In this case the first printed line in the data
file gives the magnitude while the second gives the phase angle.
The following variables are provided specifically for subspace-based steady-state dynamic analysis:
Element integration point variables:
PHS
PHE
PHEPG
PHEFL
PHMFL
PHMFT
Magnitude and phase angle of all stress components.
Magnitude and phase angle of all strain components.
Magnitude and phase angles of the electrical potential gradient vector.
Magnitude and phase angles of the electrical flux vector.
Magnitude and phase angle of the mass flow rate in fluid link elements.
Magnitude and phase angle of the total mass flow in fluid link elements.
For connector elements, the following element output variables are available:
PHCTF
PHCEF
PHCVF
PHCRF
PHCSF
PHCU
PHCCU
PHCV
PHCA
Magnitude and phase angle of connector total forces.
Magnitude and phase angle of connector elastic forces.
Magnitude and phase angle of connector viscous forces.
Magnitude and phase angle of connector reaction forces.
Magnitude and phase angle of connector friction forces.
Magnitude and phase angle of connector relative displacements.
Magnitude and phase angle of connector constitutive displacements.
Magnitude and phase angle of connector relative velocities.
Magnitude and phase angle of connector relative accelerations.
6.3.9–13
Abaqus Version 5.8 ID:
Printed on:
SUBSPACE-BASED STEADY-STATE DYNAMICS
Nodal variables:
PU
PPOR
PHPOT
PRF
PHCHG
Magnitude and phase angle of all displacement/rotation components at a node.
Magnitude and phase angle of the fluid or acoustic pressure at a node.
Magnitude and phase angle of the electrical potential at a node.
Magnitude and phase angle of all reaction forces/moments at a node.
Magnitude and phase angle of the reactive charge at a node.
Neither element energy densities (such as the elastic strain energy density, SENER) nor whole
element energies (such as the total kinetic energy of an element, ELKE) are available for output in a
subspace-based steady-state dynamic analysis.
The standard output variables U, V, A, and the variable PU listed above correspond to motions
relative to the motion of the primary base in a subspace-based steady-state dynamic analysis. Total
values, which include the motion of the primary base, are also available:
TU
TV
TA
PTU
Components of total displacement/rotation at a node.
Components of total velocity at a node.
Components of total acceleration at a node.
Magnitude and phase angle of all total displacement/rotation components at a node.
The specified base motion is available for subspace-based steady-state dynamic analysis and can
be output to the data, results, and/or output database files (see “Output to the data and results files,”
Section 4.1.2, and “Output to the output database,” Section 4.1.3).
BM
Base motion.
Whole model variables such as ALLIE (total strain energy) are available for subspace-based steadystate dynamic analysis as output to the data, results, and/or output database files (see “Output to the data
and results files,” Section 4.1.2, and “Output to the output database,” Section 4.1.3).
Input file template
*HEADING
…
*AMPLITUDE, NAME=loadamp
Data lines to define an amplitude curve as a function of frequency (cycles/time)
*AMPLITUDE, NAME=base
Data lines to define an amplitude curve to be used to prescribe base motion
**
*STEP, NLGEOM
Include the NLGEOM parameter so that stress stiffening effects will
be included in the steady-state dynamics step
*STATIC
**Any general analysis procedure can be used to preload the structure
6.3.9–14
Abaqus Version 5.8 ID:
Printed on:
SUBSPACE-BASED STEADY-STATE DYNAMICS
…
*CLOAD and/or *DLOAD
Data lines to prescribe preloads
*TEMPERATURE and/or *FIELD
Data lines to define values of predefined fields for preloading the structure
*BOUNDARY
Data lines to specify boundary conditions to preload the structure
*END STEP
**
*STEP
*FREQUENCY
Data line to control eigenvalue extraction
*BOUNDARY
Data lines to assign degrees of freedom to the primary base
*BOUNDARY, BASE NAME=base2
Data lines to assign degrees of freedom to a secondary base
*END STEP
**
*STEP
*STEADY STATE DYNAMICS, SUBSPACE PROJECTION
Data lines to specify frequency ranges and bias parameters
*SELECT EIGENMODES
Data lines to define the applicable mode ranges
*BASE MOTION, DOF=dof, AMPLITUDE=base
*BASE MOTION, DOF=dof, AMPLITUDE=base, BASE NAME=base2
*CLOAD and/or *DLOAD, AMPLITUDE=loadamp
Data lines to specify sinusoidally varying, frequency-dependent loads
…
*END STEP
6.3.9–15
Abaqus Version 5.8 ID:
Printed on:
RESPONSE SPECTRUM ANALYSIS
6.3.10
RESPONSE SPECTRUM ANALYSIS
Products: Abaqus/Standard
Abaqus/CAE
References
•
•
•
•
•
•
“Dynamic analysis procedures: overview,” Section 6.3.1
•
“Defining a spectrum,” Section 57.11 of the Abaqus/CAE User’s Manual, in the online HTML
version of this manual
“Defining an analysis,” Section 6.1.2
“General and linear perturbation procedures,” Section 6.1.3
*RESPONSE SPECTRUM
*SPECTRUM
“Configuring a response spectrum procedure” in “Configuring linear perturbation analysis
procedures,” Section 14.11.2 of the Abaqus/CAE User’s Manual, in the online HTML version of
this manual
Overview
A response spectrum analysis:
•
provides an estimate of the peak linear response of a structure to dynamic motion of fixed points
(“base motion”) or dynamic force;
•
•
is typically used to analyze response to a seismic event;
•
can use the high-performance SIM software architecture (see “Using the SIM architecture for modal
superposition dynamic analyses” in “Dynamic analysis procedures: overview,” Section 6.3.1); and
•
is a linear perturbation procedure and is, therefore, not appropriate if the excitation is so severe that
nonlinear effects in the system are important.
assumes that the system’s response is linear so that it can be analyzed in the frequency domain using
its natural modes, which must be extracted in a previous eigenfrequency extraction step (“Natural
frequency extraction,” Section 6.3.5);
Response spectrum analysis
Response spectrum analysis can be used to estimate the peak response (displacement, stress, etc.) of a
structure to a particular base motion or force. The method is only approximate, but it is often a useful,
inexpensive method for preliminary design studies.
The response spectrum procedure is based on using a subset of the modes of the system, which must
first be extracted by using the eigenfrequency extraction procedure. The modes will include eigenmodes
and, if activated in the eigenfrequency extraction step, residual modes. The number of modes extracted
6.3.10–1
Abaqus Version 5.8 ID:
Printed on:
RESPONSE SPECTRUM ANALYSIS
must be sufficient to model the dynamic response of the system adequately, which is a matter of judgment
on your part.
In cases with repeated eigenvalues and eigenvectors, the modal summation results must be
interpreted with care. You should add insignificant mass to the structure or perturb the symmetric
geometry such that the eigenvalues become unique.
While the response in the response spectrum procedure is for linear vibrations, the prior response
may be nonlinear. Initial stress effects (stress stiffening) will be included in the response spectrum
analysis if nonlinear geometric effects (“General and linear perturbation procedures,” Section 6.1.3) were
included in a general analysis step prior to the eigenfrequency extraction step.
The problem to be solved can be stated as follows: given a set of base motions,
(
),
), estimate the peak value
specified in orthogonal directions defined by direction cosines (
over all time of the response of any variable in a finite element model that is simultaneously subjected
to these multiple base motions. The peak response is first computed independently for each direction
of excitation for each natural mode of the system as a function of frequency and damping. These
independent responses are then combined to create an estimate of the actual peak response of any
variable chosen for output, as a function of frequency and damping.
The acceleration history (base motion) is not given directly in a response spectrum analysis; it must
first be converted into a spectrum.
Specifying a spectrum
The response spectrum method is based on first finding the peak response to each base motion excitation
of a one degree of freedom system that has a natural frequency equal to the frequency of interest.
The single degree of freedom system is characterized by its undamped natural frequency,
, and the
fraction of critical damping present in the system, , at each mode . The equations of motion of the
system are integrated through time to find peak values of relative displacement, relative velocity, and
relative or absolute acceleration for the linear, one degree of freedom system. This process is repeated
for all frequency and damping values in the range of interest. Plots of these responses are known
as displacement, velocity, and acceleration spectra:
,
, and
. The
response spectrum can be obtained directly from measured data, as described in “Defining a spectrum
using values of S as a function of frequency and damping,” below. You can also use a FORTRAN
program to define a spectrum; an example of defining a spectrum from an acceleration record in this way
is provided in “Analysis of a cantilever subject to earthquake motion,” Section 1.4.13 of the Abaqus
Benchmarks Manual.
Alternatively, you can create the required spectrum by specifying an amplitude (time history
record), the frequency range, and the damping values for which the spectrum will be built, as described
in “Creating a spectrum from a given time history record,” below. The spectrum can be used in the
subsequent response spectrum analysis, or it can be written to a file for future use.
For each damping value the magnitude of the response spectrum must be given over the entire
range of frequencies needed, in ascending value of frequency. Abaqus/Standard interpolates linearly
between the values given on a log-log scale. Outside the extremes of the frequency range given,
the magnitude is assumed to be constant, corresponding to the end value given. (See “Material data
definition,” Section 21.1.2, for an explanation of data interpolation.)
6.3.10–2
Abaqus Version 5.8 ID:
Printed on:
RESPONSE SPECTRUM ANALYSIS
Any number of spectra can be defined, and each spectrum must be named. The response spectrum
procedure allows up to three spectra to be applied simultaneously to the model in orthogonal physical
directions defined by their direction cosines.
Defining a spectrum using values of S as a function of frequency and damping
You can define a spectrum by specifying values for the magnitude of the spectrum; frequency, in cycles
per time, at which the magnitude is used; and associated damping, given as a ratio of critical damping.
Input File Usage:
To define the spectrum on the data lines:
*SPECTRUM, NAME=spectrum name
Repeat this option to define multiple spectra for an analysis.
Abaqus/CAE Usage:
To define a spectrum, do the following:
Step, Interaction, or Load module: Tools→Amplitude→Create;
Name: spectrum name, Type: Spectrum
To apply a spectrum to the model, do the following:
Step module: Create Step: Linear perturbation: Response
spectrum: Use response spectrum: select spectrum name for each
physical direction in which it should be applied
Specifying the type of spectrum
You can indicate whether a displacement, velocity, or acceleration spectrum is given. The default is an
acceleration spectrum.
Alternatively, an acceleration spectrum can be given in g-units. In this case you must also specify
the value of the acceleration of gravity.
Input File Usage:
Use one of the following options to define a displacement, velocity, or
acceleration spectrum:
*SPECTRUM, NAME=name, TYPE=DISPLACEMENT
*SPECTRUM, NAME=name, TYPE=VELOCITY
*SPECTRUM, NAME=name, TYPE=ACCELERATION
Use the following option to define an acceleration spectrum given in g-units:
Abaqus/CAE Usage:
*SPECTRUM, NAME=name, TYPE=G, G=g
Use one of the following options to define a displacement, velocity, or
acceleration spectrum:
Step, Interaction, or Load module: Tools→Amplitude→Create; Type:
Spectrum; Specification units: Displacement, Velocity, or Acceleration
Use the following option to define an acceleration spectrum given in g-units:
Step, Interaction, or Load module: Tools→Amplitude→Create; Type:
Spectrum; Specification units: Gravity, Gravity: g
6.3.10–3
Abaqus Version 5.8 ID:
Printed on:
RESPONSE SPECTRUM ANALYSIS
Reading the data defining the spectrum from an alternate input file
The data for the spectrum can be specified in an alternate input file and read into the Abaqus/Standard
input file.
Input File Usage:
Abaqus/CAE Usage:
*SPECTRUM, NAME=name, INPUT=file name
Step, Interaction, or Load module: Tools→Amplitude→Create;
Type: Spectrum; click mouse button 3 while holding the cursor
over the data table, and select Read from File
Creating a spectrum from a given time history record
If you have a time history of a dynamic event (e.g., acceleration, velocity, displacement), you can build
your own spectrum by specifying the record type and the amplitude name that this record represents. If
the amplitude record is given with an arbitrarily changing time increment, linear interpolation will be
needed for the implicit integration scheme for the dynamic equation of motion for a single degree of
freedom system subjected to this record. You can specify the frequency range for the integration scheme
and the frequency increment. You can build a spectrum for every fraction of critical damping indicated
in the list of damping values.
Input File Usage:
*SPECTRUM, CREATE, AMPLITUDE=amplitude name,
NAME=spectrum name, TIME INCREMENT=dt
Abaqus/CAE Usage:
Creating a spectrum from a given time history record is not supported in
Abaqus/CAE.
Specifying the type of spectrum to be created
You can indicate whether a displacement, velocity, or acceleration spectrum is to be created. The default
is an acceleration spectrum.
Alternatively, an acceleration spectrum can be created in g-units. In this case you must also specify
the value of the acceleration of gravity.
Input File Usage:
Use one of the following options to create a displacement, velocity, or
acceleration spectrum:
*SPECTRUM, CREATE, TYPE=DISPLACEMENT
*SPECTRUM, CREATE, TYPE=VELOCITY
*SPECTRUM, CREATE, TYPE=ACCELERATION
Use the following option to create an acceleration spectrum in g-units:
Abaqus/CAE Usage:
*SPECTRUM, CREATE, TYPE=G, G=g
Creating a spectrum from a given time history record is not supported in
Abaqus/CAE.
6.3.10–4
Abaqus Version 5.8 ID:
Printed on:
RESPONSE SPECTRUM ANALYSIS
Specifying the record type that the time history represents
You can indicate whether a displacement, velocity, or acceleration amplitude is specified. The default is
an acceleration amplitude.
Alternatively, an acceleration amplitude can be given in g-units. In this case you must also specify
the value of the acceleration of gravity.
Input File Usage:
Use one of the following options to indicate that the amplitude is defined in
displacement, velocity, or acceleration units:
*SPECTRUM, CREATE, EVENT TYPE=DISPLACEMENT
*SPECTRUM, CREATE, EVENT TYPE=VELOCITY
*SPECTRUM, CREATE, EVENT TYPE=ACCELERATION
Use the following option to indicate that an acceleration amplitude is given in
g-units:
Abaqus/CAE Usage:
*SPECTRUM, CREATE, EVENT TYPE=G, G=g
Creating a spectrum from a given time history record is not supported in
Abaqus/CAE.
Creating an absolute or relative acceleration spectrum
When you create an acceleration spectrum from a given time history record, you can create an absolute
or relative response spectrum. The default is an absolute spectrum.
Input File Usage:
Abaqus/CAE Usage:
*SPECTRUM, CREATE, TYPE=ACCELERATION, ABSOLUTE
*SPECTRUM, CREATE, TYPE=ACCELERATION, RELATIVE
Creating a spectrum from a given time history record is not supported in
Abaqus/CAE.
Generating the list of damping values for the fraction of critical damping
You must provide a list of damping values for the fraction of critical damping to create a spectrum.
However, if the damping is evenly spaced between its lower and upper bound, you can automatically
generate the list of damping values by providing the start value, end value, and increment for the fraction
of critical damping.
Input File Usage:
Abaqus/CAE Usage:
*SPECTRUM, CREATE, DAMPING GENERATE
Creating a spectrum from a given time history record is not supported in
Abaqus/CAE.
Writing the generated spectra to an independent file
You can write the generated spectra to an independent file. Otherwise, the generated spectra can be used
only within the currently submitted job in subsequent response spectra procedures. You can inspect the
generated spectra if you request that model definition data be printed to the data file (see “Model and
history definition summaries” in “Output,” Section 4.1.1).
6.3.10–5
Abaqus Version 5.8 ID:
Printed on:
RESPONSE SPECTRUM ANALYSIS
Input File Usage:
Abaqus/CAE Usage:
*SPECTRUM, CREATE, FILE=file name
Creating a spectrum from a given time history record is not supported in
Abaqus/CAE.
Estimating the peak values of the modal responses
Since the response spectrum procedure uses modal methods to define a model’s response, the value of any
physical variable is defined from the amplitudes of the modal responses (the “generalized coordinates”),
. The first stage in the response spectrum procedure is to estimate the peak values of these modal
responses. For mode and spectrum k this is
where
is the modal amplitude for mode ;
is a scaling parameter introduced as part of the response spectrum procedure
definition for spectrum
;
is the user-defined value of the spectrum (see “Specifying a spectrum”) in
direction k interpolated, if necessary, at natural frequency
and the fraction of
critical damping
in mode ;
is the jth direction cosine for the kth spectrum; and
is the participation factor for mode
in direction j (see “Natural frequency
extraction,” Section 6.3.5).
Similar expressions for
and
acceleration spectra in the above equation.
can be obtained by substituting velocity or
Combining the individual peak responses
The individual peak responses to the excitations in different directions will occur at different times and,
therefore, must be combined into an overall peak response. Two combinations must be performed, and
both introduce approximations into the results:
1. The multidirectional excitations must be combined into one overall response. This combination
is controlled by the directional summation method, as described below in “Directional summation
methods.”
2. The peak modal responses must be combined to estimate the peak physical response. This
combination is controlled by the modal summation method, as described below in “Modal
summation methods.”
Depending on the type of base excitation, either modal responses or directional responses are combined
first.
6.3.10–6
Abaqus Version 5.8 ID:
Printed on:
RESPONSE SPECTRUM ANALYSIS
Directional summation methods
You choose the method for combining the multidirectional excitations depending on the nature of the
excitations.
The algebraic method
If the input spectra in the different directions are components of a base excitation that is approximately
in a single direction in space, then for each mode the peak responses in the different spatial directions
are summed algebraically by
After this summation is performed, the modal responses are summed. (Choosing the method used for
modal summation is described below in “Modal summation methods.”) Since the directional components
are summed first, the subscript k is not relevant and can be ignored in the modal summation equations
that follow.
Input File Usage:
Abaqus/CAE Usage:
*RESPONSE SPECTRUM, COMP=ALGEBRAIC, SUM=sum
Step module: Create Step: Linear perturbation: Response spectrum:
Excitations: Single direction or Multiple direction absolute sum
The square root of the sum of the squares directional summation method
If the spectra in different directions represent independent excitations, the modal summation is performed
first, as explained below in “Modal summation methods.” Then, the responses in different excitation
directions are combined by
Input File Usage:
Abaqus/CAE Usage:
*RESPONSE SPECTRUM, COMP=SRSS, SUM=sum
Step module: Create Step: Linear perturbation: Response spectrum:
Excitations: Multiple direction square root of the sum of squares
The forty-percent method
If the spectra in different directions represent independent excitations, the modal summation is performed
first, as explained below in “Modal summation methods.” Then, the responses in different excitation
directions are combined by the 40% rule recommended by the ASCE 4–98 standard for Seismic Analysis
of Safety-Related Nuclear Structures and Commentary, Section 3.2.7.1.2. This method combines the
response for all possible combinations of the three components, including variations in sign (plus/minus),
assuming that when the maximum response from one component occurs, the response from the other two
components is 40% of their maximum value, using one of the following:
6.3.10–7
Abaqus Version 5.8 ID:
Printed on:
RESPONSE SPECTRUM ANALYSIS
Input File Usage:
Abaqus/CAE Usage:
*RESPONSE SPECTRUM, COMP=R40, SUM=sum
Step module: Create Step: Linear perturbation: Response spectrum:
Excitations: Multiple direction forty percent rule
The thirty-percent method
If the spectra in different directions represent independent excitations, the modal summation is performed
first, as explained below in “Modal summation methods.” Then, the responses in different excitation
directions are combined by the 30% rule recommended by the ASCE 4–98 standard for Seismic Analysis
of Safety-Related Nuclear Structures and Commentary, Section 3.2.7.1.2. This method combines the
response for all possible combinations of the three components, including variations in sign (plus/minus),
assuming that when the maximum response from one component occurs, the response from the other two
components is 30% of their maximum value, using one of the following:
Input File Usage:
Abaqus/CAE Usage:
*RESPONSE SPECTRUM, COMP=R30, SUM=sum
Step module: Create Step: Linear perturbation: Response spectrum:
Excitations: Multiple direction thirty percent rule
Modal summation methods
The peak response of some physical variable
(a component i of displacement, stress, section force,
reaction force, etc.) caused by the motion in the th natural mode excited by the given response spectra
in direction k at frequency
with damping
is given by
6.3.10–8
Abaqus Version 5.8 ID:
Printed on:
RESPONSE SPECTRUM ANALYSIS
where
is the ith component of mode , and there is no sum on . (In the case of algebraic summation
the subscript k is not relevant and can be ignored in this equation and in those that follow.)
There are several methods for combining these peak physical responses in the individual modes,
, into estimates of the total peak response,
. Most of the methods implemented in
Abaqus/Standard follow the ASCE 4–98 standard for Seismic Analysis of Safety Related Nuclear
Structures and Commentary. The updated documents, “Reevaluation of Regulatory Guidance on
Modal Response Combination Methods for Seismic Response Spectrum Analysis” issued in 1999
(NUREG/CR-6645, BNL-NUREG-52276) and “Draft Regulatory Guide” (DG-1127) issued in 2005
contain new recommendations. You are advised to read the new recommendations before choosing a
modal summation method from among those described below.
The absolute value method
The absolute value method is the most conservative method for combining the modal responses. It is
obtained by summing the absolute values resulting from each mode:
This method implies that all of the responses peak simultaneously. It will overpredict the peak response
of most systems; therefore, it may be too conservative to help in design.
Input File Usage:
Abaqus/CAE Usage:
*RESPONSE SPECTRUM, COMP=comp, SUM=ABS
Step module: Create Step: Linear perturbation: Response
spectrum: Summations: Absolute values
The square root of the sum of the squares modal summation method
The square root of the sum of the squares method is less conservative than the absolute value method.
It is also usually more accurate if the natural frequencies of the system are well separated. It uses the
square root of the sum of the squares to combine the modal responses:
Input File Usage:
Abaqus/CAE Usage:
*RESPONSE SPECTRUM, COMP=comp, SUM=SRSS
Step module: Create Step: Linear perturbation: Response spectrum:
Summations: Square root of the sum of squares
The Naval Research Laboratory method
The absolute value and square root of the sum of the squares methods can be combined to yield the
Naval Research Laboratory method. It distinguishes the mode, , in which the physical variable has its
maximum response and adds the square root of the sum of squares of the peak responses in all other
modes to the absolute value of the peak response of that mode. This method gives the estimate:
6.3.10–9
Abaqus Version 5.8 ID:
Printed on:
RESPONSE SPECTRUM ANALYSIS
Input File Usage:
Abaqus/CAE Usage:
*RESPONSE SPECTRUM, COMP=comp, SUM=NRL
Step module: Create Step: Linear perturbation: Response spectrum:
Summations: Naval Research Laboratory
The ten-percent method
The ten-percent method recommended by Regulatory Guide 1.92 (1976) is no longer recommended
according to the “Reevaluation of Regulatory Guidance on Modal Response Combination Methods
for Seismic Response Spectrum Analysis” document issued in 1999. It is retained here because of its
extensive prior use. The ten-percent method modifies the square root of the sum of the squares method
by adding a contribution from all pairs of modes and whose frequencies are within 10% of each
other, giving the estimate:
The frequencies of modes
and
are considered to be within 10% of each other whenever
The ten-percent method reduces to the square root of the sum of the squares method if the modes
are well separated with no coupling between them.
Input File Usage:
Abaqus/CAE Usage:
*RESPONSE SPECTRUM, COMP=comp, SUM=TENP
Step module: Create Step: Linear perturbation: Response
spectrum: Summations: Ten percent
The complete quadratic combination method
Like the ten-percent method, the complete quadratic combination method improves the estimation for
structures with closely spaced eigenvalues. The complete quadratic combination method combines the
modal response with the formula
where
are cross-correlation coefficients between modes
frequencies and modal damping between the two modes:
6.3.10–10
Abaqus Version 5.8 ID:
Printed on:
and
, which depend on the ratio of
RESPONSE SPECTRUM ANALYSIS
where
.
If the modes are well spaced, their cross-correlation coefficient will be small (
) and the
method will give the same results as the square root of the sum of the squares method.
This method is usually recommended for asymmetrical building systems since, in such cases, other
methods can underestimate the response in the direction of motion and overestimate the response in the
transverse direction.
Input File Usage:
Abaqus/CAE Usage:
*RESPONSE SPECTRUM, COMP=comp, SUM=CQC
Step module: Create Step: Linear perturbation: Response spectrum:
Summations: Complete quadratic combination
The grouping method
This method, also known as the NRC grouping method, improves the response estimation for structures
with closely spaced eigenvalues. The modal responses are grouped such that the lowest and highest
frequency modes in a group are within 10% and no mode is in more than one group. The modal responses
are summed absolutely within groups before performing a SRSS combination of the groups. Within the
group responses are summed as
for “n” frequencies within any “gr” group and then performing
The above expression includes all the groups; in addition, the group can consist of just one frequency
response if this frequency does not have another member that is within the 10% limit.
The ten-percent method will always produce results higher in value than the grouping method.
Input File Usage:
Abaqus/CAE Usage:
*RESPONSE SPECTRUM, COMP=comp, SUM=GRP
Step module: Create Step: Linear perturbation: Response
spectrum: Summations: Grouping method
Double sum combination
This method, also known as Rosenblueth’s double sum combination (Rosenblueth and Elorduy, 1969),
is the first attempt to evaluate modal correlation based on random vibration theory. It utilizes the time
duration
of strong earthquake motion. The mode correlation coefficients
, which depend also on
the frequencies and damping coefficient , lead to the following mode combination:
6.3.10–11
Abaqus Version 5.8 ID:
Printed on:
RESPONSE SPECTRUM ANALYSIS
where
where
Input File Usage:
Abaqus/CAE Usage:
*RESPONSE SPECTRUM, COMP=comp, SUM=DSC
Step module: Create Step: Linear perturbation: Response spectrum:
Summations: Double sum combination
Selecting the modes and specifying damping
You can select the modes to be used in modal superposition and specify damping values for all selected
modes.
Selecting the modes
You can select modes by specifying the mode numbers individually, by requesting that Abaqus/Standard
generate the mode numbers automatically, or by requesting the modes that belong to specified frequency
ranges. If you do not select the modes, all modes extracted in the prior eigenfrequency extraction step,
including residual modes if they were activated, are used in the modal superposition.
Input File Usage:
Use one of the following options to select the modes by specifying mode
numbers:
*SELECT EIGENMODES, DEFINITION=MODE NUMBERS
*SELECT EIGENMODES, GENERATE, DEFINITION=MODE NUMBERS
Use the following option to select the modes by specifying a frequency range:
Abaqus/CAE Usage:
*SELECT EIGENMODES, DEFINITION=FREQUENCY RANGE
You cannot select the modes in Abaqus/CAE; all modes extracted are used in
the modal superposition.
6.3.10–12
Abaqus Version 5.8 ID:
Printed on:
RESPONSE SPECTRUM ANALYSIS
Specifying damping
Damping is almost always specified for a mode-based procedure; see “Material damping,” Section 26.1.1.
You can define a damping coefficient for all or some of the modes used in the response calculation. The
damping coefficient can be given for a specified mode number or for a specified frequency range. When
damping is defined by specifying a frequency range, the damping coefficient for an mode is interpolated
linearly between the specified frequencies. The frequency range can be discontinuous; the average
damping value will be applied for an eigenfrequency at a discontinuity. The damping coefficients are
assumed to be constant outside the range of specified frequencies.
Input File Usage:
Use the following option to define damping by specifying mode numbers:
*MODAL DAMPING, DEFINITION=MODE NUMBERS
Use the following option to define damping by specifying a frequency range:
Abaqus/CAE Usage:
*MODAL DAMPING, DEFINITION=FREQUENCY RANGE
Use the following input to define damping by specifying mode numbers:
Step module: Create Step: Linear perturbation: Response spectrum:
Damping: Specify damping over ranges of: Modes
Use the following input to define damping by specifying a frequency range:
Step module: Create Step: Linear perturbation: Response spectrum:
Damping: Specify damping over ranges of: Frequencies
Example of specifying damping
Figure 6.3.10–1 illustrates how the damping coefficients at different eigenfrequencies are determined for
the following input:
*MODAL DAMPING, DEFINITION=FREQUENCY RANGE
Rules for selecting modes and specifying damping coefficients
The following rules apply for selecting modes and specifying modal damping coefficients:
•
•
•
•
No modal damping is included by default.
Mode selection and modal damping must be specified in the same way, using either mode numbers
or a frequency range.
If you do not select any modes, all modes extracted in the prior frequency analysis, including residual
modes if they were activated, will be used in the superposition.
If you do not specify damping coefficients for modes that you have selected, zero damping values
will be used for these modes.
6.3.10–13
Abaqus Version 5.8 ID:
Printed on:
RESPONSE SPECTRUM ANALYSIS
λi
fi
di
damping values
d=
d2 d3
d1
x
λ1
f1
frequencies
damping values
d2 + d3
2
d3
d4
x
f2
eigenfrequencies
f3
f4
x
λ3
frequency
λ2
Figure 6.3.10–1
•
•
Damping values specified by frequency range.
Damping is applied only to the modes that are selected.
Damping coefficients for selected modes that are beyond the specified frequency range are constant
and equal to the damping coefficient specified for the first or the last frequency (depending which
one is closer). This is consistent with the way Abaqus interprets amplitude definitions.
Initial conditions
It is not appropriate to specify initial conditions in a response spectrum analysis.
Boundary conditions
All points constrained by boundary conditions and the ground nodes of connector elements are assumed
to move in phase in any one direction. This base motion can use a different input spectrum in each of
three orthogonal directions (two directions in a two-dimensional model). You define the input spectra,
, as functions of frequency, , for different values of critical damping, , as described earlier in
“Specifying a spectrum.” Secondary bases cannot be used in a response spectrum analysis.
Loads
The only “loading” that can be defined in a response spectrum analysis is that defined by the input spectra,
as described earlier. No other loads can be prescribed in a response spectrum analysis.
Predefined fields
Predefined fields, including temperature, cannot be used in response spectrum analysis.
6.3.10–14
Abaqus Version 5.8 ID:
Printed on:
RESPONSE SPECTRUM ANALYSIS
Material options
The density of the material must be defined (“Density,” Section 21.2.1). The following material
properties are not active during a response spectrum analysis: plasticity and other inelastic effects,
rate-dependent material properties, thermal properties, mass diffusion properties, electrical properties,
and pore fluid flow properties—see “General and linear perturbation procedures,” Section 6.1.3.
Elements
Other than generalized axisymmetric elements with twist, any of the stress/displacement elements in
Abaqus/Standard can be used in a response spectrum analysis—see “Choosing the appropriate element
for an analysis type,” Section 27.1.3.
Output
All the output variables in Abaqus/Standard are listed in “Abaqus/Standard output variable identifiers,”
Section 4.2.1. The value of an output variable such as strain, E; stress, S; or displacement, U, is its peak
magnitude.
In addition to the usual output variables available, the following modal variables are available for
response spectrum analysis and can be output to the data and/or results files (see “Output to the data and
results files,” Section 4.1.2):
GU
GV
GA
SNE
KE
T
Generalized displacements for all modes.
Generalized velocities for all modes.
Generalized accelerations for all modes.
Elastic strain energy for the entire model per each mode.
Kinetic energy for the entire model per each mode.
External work for the entire model per each mode.
Neither element energy densities (such as the elastic strain energy density, SENER) nor whole
element energies (such as the total kinetic energy of an element, ELKE) are available for output in
response spectrum analysis. However, whole model variables such as ALLIE (total strain energy) are
available for modal-based procedures as output to the data and/or results files (see “Output to the data
and results files,” Section 4.1.2).
Reaction force output is not supported for response spectrum analysis using eigenmodes extracted
using a SIM-based frequency extraction procedure with either the AMS or Lanczos eigensolver.
Reaction force output in response spectrum analysis using eigenmodes extracted with the default
Lanczos eigensolver provides directional combinations of so-called, modal reaction forces weighted
with maximal absolute values of corresponding generalized displacements. Directional and modal
combination rules used for the reaction force calculation are the same as for other nodal output variables.
Modal reaction forces are calculated in the frequency extraction procedure. They represent static
reaction forces calculated for the normal mode shapes. Generally, they cannot adequately represent
reaction force in dynamic analysis. For models with diagonal mass and diagonal damping matrices the
6.3.10–15
Abaqus Version 5.8 ID:
Printed on:
RESPONSE SPECTRUM ANALYSIS
superposition of the modal reaction forces can provide a reasonable approximation of a nodal reaction
force in mode-based analyses other than response spectrum analysis. In response spectrum analysis the
model response can be better represented by requesting section stresses and section forces in structural
elements containing supported nodes.
Input file template
*HEADING
…
*BOUNDARY
Data lines to define points to be excited by the base motion controlled by the input spectra
*SPECTRUM, NAME=name1, TYPE=type
Data lines to define spectrum “name1” as a function of frequency, , and
fraction of critical damping,
*SPECTRUM, NAME=name2, TYPE=type
Data lines to define spectrum “name2” as a function of frequency, , and
fraction of critical damping,
**
*STEP
*FREQUENCY
Data line to specify number of modes to be extracted
*END STEP
**
*STEP
*RESPONSE SPECTRUM, COMP=comp, SUM=sum
Data lines referring to response spectra and defining direction cosines
*SELECT EIGENMODES
Data lines to define the applicable mode ranges
*MODAL DAMPING
Data lines to define modal damping
*END STEP
Additional reference
•
Rosenblueth, E., and J. Elorduy, “Response of Linear Systems to Certain Transient Disturbances,”
Proceedings of the Fourth World Conference on Earthquake Engineering, Santiago, Chile, 1969.
6.3.10–16
Abaqus Version 5.8 ID:
Printed on:
RANDOM RESPONSE ANALYSIS
6.3.11
RANDOM RESPONSE ANALYSIS
Products: Abaqus/Standard
Abaqus/CAE
References
•
•
•
•
•
•
•
“Defining an analysis,” Section 6.1.2
“General and linear perturbation procedures,” Section 6.1.3
“Dynamic analysis procedures: overview,” Section 6.3.1
*RANDOM RESPONSE
*PSD-DEFINITION
*CORRELATION
“Configuring a random response procedure” in “Configuring linear perturbation analysis
procedures,” Section 14.11.2 of the Abaqus/CAE User’s Manual, in the online HTML version of
this manual
Overview
A random response analysis:
•
•
is a linear perturbation procedure that gives the linearized dynamic response of a model to userdefined random excitation; and
uses the set of modes extracted in a previous eigenfrequency extraction step to calculate the power
spectral densities of response variables (stresses, strains, displacements, etc.) and the corresponding
root mean square (RMS) values of these same variables.
Random response analysis
Random response analysis predicts the response of a system that is subjected to a nondeterministic
continuous excitation that is expressed in a statistical sense by a cross-spectral density matrix. Since the
loading is nondeterministic, it can be characterized only in a statistical sense; Abaqus/Standard assumes
that the excitation is stationary and ergodic. These statistical measures are explained in detail in “Random
response analysis,” Section 2.5.8 of the Abaqus Theory Manual. The random response procedure can,
for example, be used to determine the response of an airplane to turbulence, the response of a car to
road surface imperfections, the response of a structure to jet noise, or the response of a building to an
earthquake.
In the most general case the excitation is defined as a frequency-dependent cross-spectral density
(CSD) matrix. Except in cases involving moving noise or user subroutine UCORR, it is assumed that for
a given load case the CSD matrix can be separated into a product of a frequency-dependent, complexvalued scalar function and a frequency-independent, complex-valued, spatial correlation matrix. This
assumption helps reduce both the computational time and the amount of required user input but implies
that each element of the CSD matrix in a given load case has the same frequency dependence. You can
6.3.11–1
Abaqus Version 5.8 ID:
Printed on:
RANDOM RESPONSE ANALYSIS
define a different frequency dependence for each load case, but the loads in one load case will not be
correlated with loads in another. Consequently, the system CSD matrix is assembled by simply summing
(superimposing) the CSD matrices of the individual load cases.
The frequency-dependent scalar function can be composed of a weighted sum of user-defined,
complex-valued, frequency functions. These user-defined frequency functions are specified in units of
power spectral density. You assign weights to each frequency function as well as specify properties of
the spatial correlation matrix that defines the correlation between excitations at different locations and in
different directions for a particular load case. Frequency functions and correlations are discussed below;
see “Defining the frequency functions,” and “Defining the correlation.”
The loads can be defined as concentrated point loads, as distributed loads, as connector element
loads, or as base motion excitations, as described below in “Boundary conditions,” and “Loads.”
Multiple, uncorrelated load cases can be defined for concentrated point loads, connector loads, and
base motions. Load case 1 is reserved for all distributed loads defined in a particular step. In these
steps load case 1 cannot be used for any concentrated point load, connector load, or base motion. Thus,
there cannot be any correlation between distributed loads and any other load. Moreover, base motion
excitations are assumed to be statistically independent (no correlation) with any other load type even
when the same load case number is used. The concentrated point and connector element loads are
assumed to be correlated if the same load case number is used.
The random response procedure is based on using a subset of the modes of the system, which must
first be extracted by using the eigenfrequency extraction procedure. The modes will include eigenmodes
and, if activated in the eigenfrequency extraction step, residual modes. The number of modes extracted
must be sufficient to model the dynamic response of the system adequately, which is a matter of judgment
on your part. The model can be preloaded prior to the eigenfrequency extraction. Initial stress effects are
included in the stiffness used in the eigenfrequency extraction if geometric nonlinearities are included in
the general analysis procedure used to apply the preloads (“General and linear perturbation procedures,”
Section 6.1.3).
The random response of the model is expressed as power spectral density values of nodal and
element variables, as well as their root mean square values.
Defining the frequency range
You specify the frequency range of interest for the random response procedure. The response is calculated
at multiple points between the lowest frequency of interest and the first eigenfrequency in the range,
between each eigenfrequency in the range, and between the last eigenfrequency in the range and the
highest frequency in the range as illustrated in Figure 6.3.11–1. The default number of calculation points
in each interval is 20; you can change this number when you define the step. Accurate RMS values can
be obtained only if enough points are used so that Abaqus/Standard can integrate accurately over the
frequency range. The bias function allows the points on the frequency scale to be spaced closer together
at the eigenfrequencies, thus allowing detailed definition of the response close to resonant frequencies
and more accurate integration.
Input File Usage:
*RANDOM RESPONSE
lower_freq_limit, upper_freq_limit, num_calc_pts, bias_parameter, freq_scale
6.3.11–2
Abaqus Version 5.8 ID:
Printed on:
RANDOM RESPONSE ANALYSIS
frequency points
lower end
of the range
mode n
Figure 6.3.11–1
Abaqus/CAE Usage:
mode n +1
mode n + 2
upper end
of the range
Division of range using modes and 5 calculation points.
Step module: Create Step: Linear perturbation: Random response
The bias parameter
The bias parameter can be used to provide closer spacing of the result points either toward the middle or
toward the ends of each frequency interval. Figure 6.3.11–2 shows a few examples of the effect of the
bias parameter on the frequency spacing.
frequency points
Bias parameter = 1
f1
f2
Bias parameter = 2
Bias parameter = 3
Bias parameter = 5
Figure 6.3.11–2 Effect of the bias parameter on the frequency
spacing for a number of points
.
The bias formula used to calculate the frequency at which results are presented is as follows:
where
6.3.11–3
Abaqus Version 5.8 ID:
Printed on:
RANDOM RESPONSE ANALYSIS
y
n
k
p
;
is the number of frequency points at which results are to be given;
is one such frequency point (
);
is the lower limit of the frequency interval;
is the upper limit of the interval;
is the frequency at which the kth results are given;
is the bias parameter value; and
is the frequency or the logarithm of the frequency, depending on the chosen frequency scale.
A bias parameter, p, that is greater than 1.0 provides closer spacing of the results points toward the ends of
each frequency interval (as shown in the examples above), while values of p that are less than 1.0 provide
closer spacing toward the middle of each frequency interval. The default value of the bias parameter for
random response analysis is 3.0.
Defining the frequency functions
To define the random loading, you specify a frequency function and a cross-correlation definition that
refers to the frequency function. The frequency functions are defined as model data (i.e., they are step
independent) and must be named. A log-log scale is used in interpolating between the given values.
The type of units in the CSD matrix of the excitation are specified as part of the frequency function
definition. The default type is power units. If the CSD matrix of the excitation is due to base motion,
the units must be in g units and you should define the acceleration of gravity. Alternatively, decibel units
can be specified; this type of units is explained below.
Input File Usage:
Abaqus/CAE Usage:
Use one of the following options to define the frequency function:
*PSD-DEFINITION, NAME=name, TYPE=FORCE (default; power units)
*PSD-DEFINITION, NAME=name, TYPE=BASE, G=g
*PSD-DEFINITION, NAME=name, TYPE=DB, DB REFERENCE=
Load module: Create Amplitude; Type: PSD Definition; Specification
units: Power, Decibel, or Gravity
Defining the cross-spectral density matrix in decibel units
In Abaqus/Standard the decibel value
full octave band conversion formula:
is related to the frequency function
by the following
where
is the user-specified reference power and is the midband frequency (see Table 6.3.11–1).
Hence, the frequency function follows from the function defined in decibel units as
6.3.11–4
Abaqus Version 5.8 ID:
Printed on:
RANDOM RESPONSE ANALYSIS
Standard octave bands.
Table 6.3.11–1
Band
number
Band center
(frequency, Hz)
1
1.0
2
2.0
3
4.0
4
8.0
5
16.0
6
31.5
7
63.0
8
125.0
9
250.0
10
500.0
11
1000.0
12
2000.0
13
4000.0
14
8000.0
15
16000.0
If you have data in terms of an alternative frequency scale (e.g., one-third octave band), an equivalent
full octave band power reference value can be obtained as described in “Random response analysis,”
Section 2.5.8 of the Abaqus Theory Manual.
in decibels must be specified as a function of the frequency band; the associated midband
frequencies are given in Table 6.3.11–1.
Alternate methods for defining frequency functions
You can define a frequency function in an external file or in a user subroutine.
Defining the frequency function in an external file
The data to define a frequency function can be contained in an external file.
Input File Usage:
Abaqus/CAE Usage:
*PSD-DEFINITION, NAME=name, TYPE=type, INPUT=file name
Load module: Create Amplitude; Type: PSD Definition; Specification
units: Power, Decibel, or Gravity; Real, Imaginary, Frequency
6.3.11–5
Abaqus Version 5.8 ID:
Printed on:
RANDOM RESPONSE ANALYSIS
Defining the frequency function in a user subroutine
Complicated frequency functions can be more easily defined by user subroutine UPSD than by entering
data directly.
Input File Usage:
*PSD-DEFINITION, NAME=name, TYPE=type, USER
Any data lines given will be ignored if the USER parameter is specified.
Abaqus/CAE Usage:
Load module: Create Amplitude; Type: PSD Definition;
Specification units: Power or Gravity; toggle on Specify
data in an external user subroutine
Defining the correlation
You define the cross-correlation between the applied nodal loads or base motions. You can also assign
scaling (weight) factors to the frequency functions through the cross-correlation definition. Distributed
loads are converted to equivalent nodal loads, which are treated as individual point loads with respect
to the cross-correlation. The cross-correlation is defined in the random response step and references a
particular load case number and frequency function.
Three types of correlation can be defined: correlated, uncorrelated, and moving noise. As many
correlations as needed to define the random loading can be specified unless the moving noise type is
chosen, in which case only one correlation can appear in the step definition.
•
•
•
For the correlated type all terms in the cross-spectral density matrix are considered, which implies
that the loads on all degrees of freedom within the load case are fully correlated (statistically
dependent on each other).
For the uncorrelated type only diagonal terms in the cross-spectral density matrix are considered,
which implies that no correlation exists between the load on one degree of freedom and the load on
another. You should exercise caution when choosing the uncorrelated type with distributed loads
since the equivalent nodal forces would be uncorrelated with each other (statistically independent).
For the moving noise type the terms in the correlation matrix depend on the relative position of the
points where the loads are applied. This type can be used only in conjunction with concentrated point
loads and distributed loads. In addition, the moving noise formulation assumes that the frequency
function referenced by the cross-correlation defines a reference power spectral density function of
the noise source. (It is a reference power spectral density because it can later be scaled by the
magnitude of the loadings specified as distributed, concentrated point, or connector element loads.)
Since the power spectral density is real-valued for real-valued variables, the frequency function
must not contain imaginary terms when used with the moving noise type of cross-correlation.
Input File Usage:
Use one of the following options to define the correlation:
*CORRELATION, TYPE=CORRELATED, PSD=name
*CORRELATION, TYPE=UNCORRELATED, PSD=name
*CORRELATION, TYPE=MOVING NOISE
For the moving noise type the reference to the power spectral density function
must be given on each data line.
6.3.11–6
Abaqus Version 5.8 ID:
Printed on:
RANDOM RESPONSE ANALYSIS
Abaqus/CAE Usage:
Load module; Create Boundary Condition; Step: random_response_step;
Category: Mechanical; Types for Selected Step: Displacement
base motion or Velocity base motion or Acceleration base motion;
Correlation tabbed page: toggle on Specify correlation; Approach:
Correlated or Uncorrelated; PSD: psd_amplitude_name
Specifying whether the correlation matrix is complex
For correlated or uncorrelated cross-correlations you can specify whether or not both real and imaginary
terms will be included in the spatial correlation matrix. This specification does not affect the imaginary
terms given for the power spectral density frequency function.
Input File Usage:
Use one of the following options:
*CORRELATION, TYPE=CORRELATED, COMPLEX=YES or NO,
PSD=name
*CORRELATION, TYPE=UNCORRELATED, COMPLEX=YES or NO,
PSD=name
Abaqus/CAE Usage:
Load module; Create Boundary Condition; Step: random_response_step;
Category: Mechanical; Types for Selected Step: Displacement
base motion or Velocity base motion or Acceleration base motion;
Correlation tabbed page: toggle on Specify correlation; Approach:
Correlated or Uncorrelated; PSD: psd_amplitude_name; Real; Imaginary
Alternate methods for defining a correlation
You can define a correlation in an external input file or in a user subroutine.
Defining the correlation in an external input file
The data to define a correlation can be contained in an external input file.
Input File Usage:
Abaqus/CAE Usage:
*CORRELATION, TYPE=type, PSD=name, INPUT=file_name
You cannot define a correlation in an external file in Abaqus/CAE.
Defining the correlation in a user subroutine
Simple excitations, such as uncorrelated white noise, are easily defined. Excitations involving more
complicated correlations, including cases where the elements of the CSD matrix have different frequency
dependencies, can be defined through user subroutine UCORR. If the user subroutine is specified, only
the load case number must be entered as part of the correlation definition. A user subroutine cannot be
used to define a moving noise correlation.
For uncorrelated cross-correlations only the diagonal terms of the correlation matrix specified in
UCORR will be used. The combination of the cross-correlation with the various kinds of applied loads is
discussed in more detail below.
Input File Usage:
Use one of the following options:
6.3.11–7
Abaqus Version 5.8 ID:
Printed on:
RANDOM RESPONSE ANALYSIS
*CORRELATION, TYPE=CORRELATED, USER, COMPLEX=YES
or NO, PSD=name
*CORRELATION, TYPE=UNCORRELATED, USER, PSD=name
Abaqus/CAE Usage:
Load module; Create Boundary Condition; Step: random_response_step;
Category: Mechanical; Types for Selected Step: Displacement
base motion or Velocity base motion or Acceleration base motion;
Correlation tabbed page: toggle on Specify correlation; Approach: User
Selecting the modes and specifying damping
You can select the modes to be used in modal superposition and specify damping values for all selected
modes.
Selecting the modes
You can select modes by specifying the mode numbers individually, by requesting that Abaqus/Standard
generate the mode numbers automatically, or by requesting the modes that belong to specified frequency
ranges. If you do not select the modes, all modes extracted in the prior eigenfrequency extraction step,
including residual modes if they were activated, are used in the modal superposition.
Input File Usage:
Use one of the following options to select the modes by specifying mode
numbers:
*SELECT EIGENMODES, DEFINITION=MODE NUMBERS
*SELECT EIGENMODES, GENERATE, DEFINITION=MODE NUMBERS
Use the following option to select the modes by specifying a frequency range:
Abaqus/CAE Usage:
*SELECT EIGENMODES, DEFINITION=FREQUENCY RANGE
You cannot select the modes in Abaqus/CAE; all modes extracted are used in
the modal superposition.
Specifying damping
Damping is almost always specified for a random response analysis (see “Material damping,”
Section 26.1.1). If damping is absent, the response of a structure will be unbounded if the forcing
frequency is equal to an eigenfrequency of the structure. To get quantitatively accurate results,
especially near natural frequencies, accurate specification of damping properties is essential. The
various damping options available are discussed in “Material damping,” Section 26.1.1. You can define
a damping coefficient for all or some of the modes used in the response calculation. The damping
coefficient can be given for a specified mode number or for a specified frequency range. When damping
is defined by specifying a frequency range, the damping coefficient for a mode is interpolated linearly
between the specified frequencies. The frequency range can be discontinuous; the average damping
value will be applied for an eigenfrequency at a discontinuity. The damping coefficients are assumed to
be constant outside the range of specified frequencies.
Input File Usage:
Use the following option to define damping by specifying mode numbers:
6.3.11–8
Abaqus Version 5.8 ID:
Printed on:
RANDOM RESPONSE ANALYSIS
*MODAL DAMPING, DEFINITION=MODE NUMBERS
Use the following option to define damping by specifying a frequency range:
Abaqus/CAE Usage:
*MODAL DAMPING, DEFINITION=FREQUENCY RANGE
Use the following input to define damping by specifying mode numbers:
Step module: Create Step: Linear perturbation: Random response:
Damping
Defining damping by specifying frequency ranges is not supported in
Abaqus/CAE.
Example of specifying damping
Figure 6.3.11–3 illustrates how the damping coefficients at different eigenfrequencies are determined for
the following input:
*MODAL DAMPING, DEFINITION=FREQUENCY RANGE
λi
fi
di
damping values
d=
d2 d3
d1
x
f1
λ1
frequencies
damping values
d2 + d3
2
d3
d4
x
f2
eigenfrequencies
f3
f4
x
λ3
frequency
λ2
Figure 6.3.11–3
Damping values specified by frequency range.
Rules for selecting modes and specifying damping coefficients
The following rules apply for selecting modes and specifying modal damping coefficients:
6.3.11–9
Abaqus Version 5.8 ID:
Printed on:
RANDOM RESPONSE ANALYSIS
•
•
•
•
•
•
No modal damping is included by default.
Mode selection and modal damping must be specified in the same way, using either mode numbers
or a frequency range.
If you do not select any modes, all modes extracted in the prior frequency analysis, including residual
modes if they were activated, will be used in the superposition.
If you do not specify damping coefficients for modes that you have selected, zero damping values
will be used for these modes.
Damping is applied only to the modes that are selected.
Damping coefficients for selected modes that are beyond the specified frequency range are constant
and equal to the damping coefficient specified for the first or the last frequency (depending which
one is closer). This is consistent with the way Abaqus interprets amplitude definitions.
Initial conditions
It is not appropriate to specify initial conditions in a random response analysis.
Boundary conditions
It is not possible to prescribe nonzero displacements and rotations directly as boundary conditions
(“Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1) in mode-based
dynamic response procedures. Therefore, in a random response analysis the motion of nodes can be
specified only as base motion; nonzero displacement, velocity, or acceleration history definitions given
as boundary conditions are ignored, and any changes in the support conditions from the eigenfrequency
extraction step are flagged as errors. In addition, any amplitude definitions are ignored in a random
response analysis.
The method for prescribing motion in modal superposition procedures is described in “Transient
modal dynamic analysis,” Section 6.3.7. In random response analysis only a single (primary) base can
be defined.
Defining multiple load cases
The excitation defined by the base motion is assigned to numbered load cases. These load cases are then
referenced in the cross-correlation definition. The load cases are associated with frequency functions
through the reference in the cross-correlation definition. Any number of load cases can be defined, but
load case number 1 cannot be used if distributed loads are defined in the same step.
Input File Usage:
Abaqus/CAE Usage:
*BASE MOTION, LOAD CASE=n
Base motions with load cases are not supported in Abaqus/CAE.
Converting base motion excitation to a cross-spectral density matrix
When the excitation is provided by a base motion, it is converted directly into a cross-spectral density
matrix projected onto the eigenspace through the modal participation factors (see “Natural frequency
extraction,” Section 6.3.5), giving
6.3.11–10
Abaqus Version 5.8 ID:
Printed on:
RANDOM RESPONSE ANALYSIS
Re
for
for
,
,
for
,
where the superscript * denotes complex conjugate and where
is the modal participation factor for mode
in excitation direction i (i=1–6);
is the frequency function referenced by the Jth cross-correlation and defined as a function
of the frequency f in g units;
is a matrix of weight factors indicating the fraction of
to be associated with the correlation
between base motion in directions i and j for load case I, as described below;
, 1, or 2, depending on whether the base motion corresponding to load case I is defined
in terms of an acceleration spectrum, a velocity spectrum, or a displacement spectrum (see
“Transient modal dynamic analysis,” Section 6.3.7); and
is the user-specified acceleration of gravity for the same power spectral density frequency
function that defines
.
If the cross-correlation is defined in user subroutine UCORR,
Otherwise,
for all
is defined in the user subroutine.
if the excitation is correlated or
if the excitation is uncorrelated,
is the (complex) value of the weight factor by which to scale the frequency function
where
in load case I.
used
Loads
The loading for random response analysis is defined in general terms by the cross-spectral density matrix
, where f is frequency in cycles per time and the subscripts
and
refer to
degree of freedom i at node N and degree of freedom j at node M, respectively. Distributed loads are
converted to equivalent nodal loads, which—for the formulation of the correlation matrix—are treated
in the same way as concentrated point loads. The units of
are (force)2 or (moment)2
per frequency. In addition, any amplitude references on the concentrated point, connector element, or
distributed load definitions are ignored in a random response analysis.
Defining multiple load cases
Distributed loads will be assigned automatically to load case number 1. You assign a concentrated point
load or connector element load to a numbered load case. Any number of concentrated point and connector
element load cases can be specified, but load case number 1 cannot be used for a concentrated point or
connector element load if a distributed load is present in the same step. The concentrated point, connector
6.3.11–11
Abaqus Version 5.8 ID:
Printed on:
RANDOM RESPONSE ANALYSIS
element, and distributed load cases are associated with frequency functions through the cross-correlation
definition.
Input File Usage:
Use one or more of the following options:
*CLOAD, LOAD CASE=n
*CONNECTOR LOAD, LOAD CASE=m
*DLOAD
Correlated and uncorrelated loading
For correlated or uncorrelated cross-correlations, the cross-spectral density matrix is defined as
Re
for
,
for
,
for
,
where the superscript * denotes complex conjugate and where
is the load magnitude applied to degree of freedom i at node N for load case I;
is the frequency function referenced by the Jth cross-correlation and defined as a
function of the frequency f in power (force) or decibel units; and
is a matrix of weight factors indicating the fraction of
to be associated with
the
cross-correlation term for load case I, as described below.
If the cross-correlation is defined in user subroutine UCORR,
Otherwise,
for all
is defined in the user subroutine.
if the excitation is correlated or
if the excitation is uncorrelated,
is the (complex) value of the weight factor by which to scale the frequency function
where
in load case I.
used
Moving noise loading
For moving noise cross-correlations, the cross-spectral density matrix is defined as
where
is the load magnitude applied to degree of freedom i at node N for load case I;
is the reference power spectral density function associated with load case I and defined as a
function of the frequency f in power (force) or decibel units;
is the velocity vector of noise propagation given for load case I; and
6.3.11–12
Abaqus Version 5.8 ID:
Printed on:
RANDOM RESPONSE ANALYSIS
are the coordinates of node N.
This definition of moving noise implies that the different noise sources have no cross-correlation.
Therefore, it is most generally used with only one noise source (
only). In addition, since
is the actual power spectral density of the moving noise source, it must be defined as a real-valued
function.
Predefined fields
Predefined fields, including temperature, cannot be used in random response analysis.
Material options
As in any dynamic analysis procedure, mass or density (“Density,” Section 21.2.1) must be assigned
to some regions of any separate parts of the model where dynamic response is required. The following
material properties are not active during a random response analysis: plasticity and other inelastic effects,
rate-dependent properties, thermal properties, mass diffusion properties, electrical properties, and pore
fluid flow properties (see “General and linear perturbation procedures,” Section 6.1.3).
Elements
Other than generalized axisymmetric elements with twist, any of the stress/displacement elements in
Abaqus/Standard can be used in a random response analysis (see “Choosing the appropriate element for
an analysis type,” Section 27.1.3).
Output
In random response analysis the value of a variable is its power spectral density; all of the output variables
in Abaqus/Standard are listed in “Abaqus/Standard output variable identifiers,” Section 4.2.1. Power
spectral density values are not available for concentrated and distributed loads and for SINV.
Options are also provided in random response analysis to obtain root mean square values for certain
variables, as listed below. Total values include base motion, while relative values are measured relative
to the base motion.
Element integration point variables:
RS
RE
Root mean square of all stress components.
Root mean square of all strain components.
Element nodal point variables:
MISES
RMISES
Mises equivalent stress..
Root mean square of Mises equivalent stress.
For connector elements, the following element output variables are available:
RCTF
Root mean square of connector total forces.
6.3.11–13
Abaqus Version 5.8 ID:
Printed on:
RANDOM RESPONSE ANALYSIS
RCEF
RCVF
RCRF
RCSF
RCU
RCCU
Root mean square of connector elastic forces.
Root mean square of connector viscous forces.
Root mean square of connector reaction forces.
Root mean square of connector friction forces.
Root mean square of connector relative displacements.
Root mean square of connector constitutive displacements.
Nodal variables:
RU
RTU
RV
RTV
RA
RTA
RRF
Root mean square values of all components of the relative displacement/rotation
at a node.
Root mean square values of all components of the total displacement/rotation at a
node.
Root mean square values of all components of the relative velocity at a node.
Root mean square values of all components of the total velocity at a node.
Root mean square values of all components of the relative acceleration at a node.
Root mean square values of all components of the total acceleration at a node.
Root mean square values of all components of reaction forces and reaction
moments at a node.
No energy values are available for a random response analysis.
To reduce the computational cost of random response analysis, you should request output only for
selected element and node sets. Abaqus/Standard will calculate the response for only the element and
nodal variables requested.
When MISES or RMISES output is requested, Abaqus/Standard stores the needed data in the
output database (.odb) file and Abaqus/Viewer does the actual computation of the responses. These
computations require element stress output in the frequency step preceding the random response step.
Note that specifying the name of the element set in the output request in the random response step has
no effect on these two output variables. If MISES or RMISES output for a selected set of elements is
desired, the name of that element set needs to be specified for the element stress output request in the
preceding frequency step. Unlike in other procedures, MISES and RMISES output for random response
analysis is computed at the element nodal points and not at the element integration points.
Input file template
*HEADING
…
*PSD-DEFINITION, NAME=name, TYPE=type
Data lines to define a frequency function (or PSD function for moving noise)
**
*STEP
*FREQUENCY
Data line to control eigenvalue extraction
6.3.11–14
Abaqus Version 5.8 ID:
Printed on:
RANDOM RESPONSE ANALYSIS
*BOUNDARY
Data lines to assign degrees of freedom to the primary base
*END STEP
*STEP
*RANDOM RESPONSE
Data line to specify frequency range of interest
*SELECT EIGENMODES
Data lines to define the applicable mode ranges
*MODAL DAMPING
Data line to define modal damping
*CORRELATION, PSD=name, TYPE=type
Data lines to specify correlation for various excitation load cases (n, p)
*DLOAD
Data lines to define distributed loads
*CLOAD, LOAD CASE=n
Data lines to define concentrated loads in load case n
*CONNECTOR LOAD, LOAD CASE=m
Data lines to define connector loads in load case m
*BASE MOTION, DOF=dof, LOAD CASE=p
Data lines to define base motion p
*END STEP
6.3.11–15
Abaqus Version 5.8 ID:
Printed on:
STEADY-STATE TRANSPORT ANALYSIS
6.4
Steady-state transport analysis
•
“Steady-state transport analysis,” Section 6.4.1
6.4–1
Abaqus Version 5.8 ID:
Printed on:
STEADY-STATE TRANSPORT ANALYSIS
6.4.1
STEADY-STATE TRANSPORT ANALYSIS
Product: Abaqus/Standard
References
•
•
•
•
•
•
•
“Defining an analysis,” Section 6.1.2
“Symmetric model generation,” Section 10.4.1
*STEADY STATE TRANSPORT
*SYMMETRIC MODEL GENERATION
*MOTION
*TRANSPORT VELOCITY
*ACOUSTIC FLOW VELOCITY
Overview
A steady-state transport analysis:
•
•
•
•
•
•
•
•
•
allows for steady-state rolling and sliding solutions including frictional effects and inertia effects;
allows for steady-state solutions to be obtained directly or by using a quasi-steady-state (pass-bypass) technique;
is used to model the interaction between a deformable rolling object and one or more flat, convex,
or concave surfaces;
is based on a specialized analysis capability where the rigid body motion is described in a spatial or
Eulerian manner and the deformation in a material or Lagrangian manner;
allows for one element set in a model to be described in an Eulerian manner while the rest of the
elements in the model are treated in a classical Lagrangian manner;
can be preceded by a static stress analysis or followed by a natural frequency extraction or a complex
eigenvalue extraction step;
uses regular stress/displacement elements and special steady-state rolling and sliding contact pairs;
is currently available only for three-dimensional analysis with an axisymmetric geometry or a
periodic geometry; and
allows rate-independent, rate-dependent, or history-dependent material behavior.
Steady-state transport analysis
It is cumbersome to model rolling and sliding contact, such as a tire rolling along a rigid surface or a
disc rotating relative to a brake assembly, using a traditional Lagrangian formulation since the frame
of reference in which motion is described is attached to the material. An observer in this reference
frame views even steady-state rolling as a time-dependent process since each point undergoes a repeated
6.4.1–1
Abaqus Version 5.8 ID:
Printed on:
STEADY-STATE TRANSPORT ANALYSIS
history of deformation. Such an analysis is computationally expensive since a transient analysis must be
performed and fine meshing is required along the entire surface of the cylinder.
The steady-state transport analysis capability in Abaqus/Standard uses a reference frame that is
attached to the axle of the rotating cylinder. An observer in this frame sees the cylinder as points that
are not moving, although the material of which the cylinder is made is moving through those points.
This removes the explicit time dependence from the problem—the observer sees a fixed point anywhere,
with material moving through it. Thus, the finite element mesh describing the cylinder in this frame of
reference does not undergo the large rigid body spinning motion. This means that a fine mesh is required
only near the contact zone.
This description can be viewed as a mixed Lagrangian/Eulerian method, where rigid body rotation
is described in a spatial or Eulerian manner, and deformation, which is now measured relative to the
rotating rigid body, is described in a material or Lagrangian manner. It is this kinematic description that
converts the steady-state moving contact problem into a purely spatially dependent simulation.
The steady-state rolling and sliding analysis capability provides solutions that include frictional
effects, inertia effects, and material convection for most rate-independent, rate-dependent, and historydependent material models.
The theory is described in detail in “Steady-state transport analysis,” Section 2.7.1 of the Abaqus
Theory Manual.
Input File Usage:
*STEADY STATE TRANSPORT
Pass-by-pass analysis technique
By default, the steady-state transport analysis procedure in Abaqus/Standard solves for a steady-state
rolling and sliding solution directly as a series of increments, with iterations to obtain equilibrium within
each increment. The solution in each increment is a steady-state solution corresponding to the loads
acting on the structure at that instant. The steady-state transport analysis procedure also provides an
alternative technique to obtain a quasi-steady-state rolling and sliding solution as a series of increments,
with iterations to obtain equilibrium within each increment. However, the solution in each increment
is usually not a steady-state solution corresponding to the loads acting on the structure at that instant.
A steady-state solution is generally obtained in several increments, with each increment corresponding
to a loading pass through the structure. Each loading pass through the structure can have a different
magnitude.
The pass-by-pass analysis technique is relevant only when used with plasticity/creep models. It has
no effect on a viscoelastic material model.
Input File Usage:
*STEADY STATE TRANSPORT, PASS BY PASS
Unstable problems
Local instabilities (e.g., surface wrinkling, material instability, or local buckling), can occur in a steadystate transport analysis. Abaqus/Standard offers the option to stabilize this class of problems by applying
damping throughout the model in such a way that the viscous forces introduced are sufficiently large to
prevent instantaneous buckling or collapse but small enough not to affect the behavior significantly while
6.4.1–2
Abaqus Version 5.8 ID:
Printed on:
STEADY-STATE TRANSPORT ANALYSIS
the problem is stable. The available automatic stabilization schemes are described in detail in “Automatic
stabilization of unstable problems” in “Solving nonlinear problems,” Section 7.1.1.
Defining the model
A steady-state transport analysis requires the definition of streamlines. The streamlines are the
trajectories that the material follows during transport through the mesh. To meet this requirement, the
mesh must be generated using the symmetric model generation capability, which is described in detail in
“Symmetric model generation,” Section 10.4.1. The three-dimensional model can be created either by
revolving an axisymmetric model about its axis of revolution or by revolving a single three-dimensional
repetitive sector about its axis of symmetry.
Revolving an axisymmetric cross-section to create a three-dimensional model
You can generate a three-dimensional mesh by revolving a two-dimensional cross-section about
a symmetry axis, so that the streamlines follow the mesh lines. In this case the symmetric model
generation capability requires a two-dimensional cross-section of the body as a starting point. The
cross-section, which must be discretized with axisymmetric finite elements, is defined in a separate
input file. A data check analysis must be performed to write the model information to a restart file. The
restart file is read in a subsequent run, and a three-dimensional model is generated by Abaqus/Standard
by revolving the cross-section about the symmetry axis, starting at a reference plane. Both the symmetry
axis and reference plane of the new three-dimensional model can be oriented in any direction in the
global coordinate system. The symmetry axis also defines the axis of the spinning body. A nonuniform
discretization in the circumferential direction can be specified to allow a finer mesh in the contact region
than elsewhere in the model.
Input File Usage:
*SYMMETRIC MODEL GENERATION, REVOLVE
Revolving a single three-dimensional sector to create a periodic model
Alternatively, you can generate a periodic three-dimensional mesh by revolving a single
three-dimensional sector about its axis of symmetry. To accurately account for the material
convection when the streamline integration is performed, the segment angle for the repetitive
three-dimensional sector must be chosen small enough.
In this case the symmetric model generation capability requires a single three-dimensional sector
as a starting point. The original three-dimensional sector is defined in a separate input file. A data check
analysis must be performed to write the model information to a restart file. The restart file is read in a
subsequent run, and a three-dimensional periodic model is generated by Abaqus/Standard by revolving
the original three-dimensional sector about the symmetry axis. Both the symmetry axis and the original
three-dimensional repetitive sector can be oriented in any direction in the global coordinate system. The
symmetry axis also defines the axis of the spinning body. There is no restriction that the meshes on the
two symmetry surfaces of the repetitive sector match in any way. If the surface meshes on either side of
the original sector are not matched completely, constraints will be generated automatically to couple the
opposing neighboring surfaces when revolving the original sector to create a periodic model.
Input File Usage:
*SYMMETRIC MODEL GENERATION, PERIODIC
6.4.1–3
Abaqus Version 5.8 ID:
Printed on:
STEADY-STATE TRANSPORT ANALYSIS
Identifying the elements being treated in an Eulerian manner
By default, the rigid body motion in the whole model will be described in a spatial or Eulerian manner.
In some cases you may want only part of the model to be treated with the Eulerian method while the rest
should be treated with the classical Lagrangian method. One typical example is a disc brake where the
disc itself can be treated with the Eulerian method while the brake assembly (brake pads and caliper) is
treated with the Lagrangian method. In this case you can specify the name of an element set for which
the rigid body motion will be described in an Eulerian manner. The elements that are not included in
the element set will be treated with the classical Lagrangian method. Only one Eulerian element set can
be specified in the whole model. In a new steady-state transport step or upon restart (see “Restarting an
analysis,” Section 9.1.1) you can respecify a set of elements to be treated with the Eulerian method even
after it has previously been treated with the Lagrangian method and vice versa. Elements treated with the
Eulerian method and elements treated with the Lagrangian method cannot be mixed along a streamline.
Input File Usage:
*STEADY STATE TRANSPORT, ELSET=name
Defining reference frame motions
The deformable and rigid bodies can each be defined in their own moving reference frame in a steadystate rolling and sliding analysis. The motion of these reference frames can be defined quite generally
and provides modeling of a spinning deformable body traveling along a straight line, or “cornering”
or “precessing” around an axis. It is also possible to define reference frame motions for rigid bodies,
including translations and rotations. The rigid body can be flat, convex, or concave, which allows for
modeling of a deformable body in contact with a rotating drum, such as a tire rolling on a drum, or for
modeling a tire mounted on a rigid rim.
When defining different reference frame motions for bodies that interact, you must make sure that
the interactions are indeed steady. For example, for a planar rigid surface the relative reference frame
motion must be tangential to the rigid surface, and for a body of revolution the relative reference frame
motion must be rotation around its axis.
Spinning motion
The spinning motion of the deformable body around its own axis is described by a user-specified angular
velocity, . This angular velocity defines the transport of material through the mesh; you define the
magnitude of the spinning rotation, . The axis of revolution is the symmetry axis used for generating
the mesh as described in “Defining the model.” The transport velocity must be defined for all nodes
on the spinning body. The magnitude of the angular velocity can also be defined with user subroutine
UMOTION.
The transport velocity can also be applied to a rigid body based on a three-dimensional surface of
revolution. In that case the velocity is applied to the rigid body reference node to describe the transport
of the (rigid) material relative to the reference node. Abaqus/Standard assumes that the rigid body spins
around the axis of revolution of the rigid body. This option can, for example, be applied to the rigid body
representing the rim on which a tire is mounted.
6.4.1–4
Abaqus Version 5.8 ID:
Printed on:
STEADY-STATE TRANSPORT ANALYSIS
Abaqus/Standard will automatically update the position and orientation of the rotation axis to the
current configuration in a large-displacement analysis, such as in the case where a prescribed load applied
to the reference node of a rotating rigid drum maintains the contact pressure between the tire and drum
or the case where a camber angle is applied to the axle of the deformable body.
Input File Usage:
Use either of the following options:
*TRANSPORT VELOCITY
*TRANSPORT VELOCITY, USER
Defining a reference frame for translational or rotational motion
The rotating deformable body is also associated with a reference frame. This reference frame can either
translate or rotate with respect to the fixed global reference frame. Similarly, each rigid body must be
defined in a reference frame that is either fixed, translates, or rotates. For example, to associate straight
line travel at ground velocity, , with a spinning deformable body, the deformable body can be defined in
a reference frame translating at velocity and the rigid surface can be defined in a fixed reference frame.
Alternatively, the deformable body can be defined in a reference frame that does not translate and the
rigid body can be defined in a frame translating at velocity
. Another example is a deformable body
precessing along a circular path. In such a case a rotating frame is associated with the deformable body
that defines the precession axis and angular velocity, while the rigid body is defined in a fixed reference
frame.
For this purpose you can apply a specified motion of the reference frame to all nodes of the
deformable body or to the reference node of a rigid body. A translating reference frame is defined by
specifying the components of the velocity vector, . A rotating reference frame is defined by specifying
the magnitude of an angular rotation velocity, , and the position and orientation of the axis of rotation
in the current configuration. The position and orientation of the axis are applied at the beginning of the
step and remain fixed during the step.
Input File Usage:
Use the following option to define the motion of a translating reference frame:
*MOTION, TRANSLATION
Use the following option to define the motion of a rotating reference frame:
*MOTION, ROTATION
Contact conditions
Abaqus/Standard provides contact between a rigid surface and deformable body moving with different
velocities, such as contact between a rolling tire and the ground, as well as contact between surfaces
moving with the same velocity, such as the contact between the bead and rim in a tire analysis.
Abaqus/Standard also provides contact between two deformable bodies moving with the same velocity,
such as the contact between the tread blocks on a tire surface, as well as contact between two deformable
bodies moving with different velocities, such as the contact between a disc and brake assembly.
6.4.1–5
Abaqus Version 5.8 ID:
Printed on:
STEADY-STATE TRANSPORT ANALYSIS
Contact between a rigid surface and a deformable body moving with different velocities
The rigid surface can be either an analytical surface or made from rigid elements. When the master and
slave surfaces move with different velocities, you will normally select to use a Coulomb friction law that
assumes that slip occurs if the frictional stress
is equal to the critical stress
, where and are the shear stresses on the contact plane, is
the friction coefficient, and p is the contact pressure. No slip occurs when
. For steady-state
transport the condition of no slip is approximated in Abaqus/Standard by stiff “viscous” behavior
where
are the tangential slip velocities that depend on deformation along a streamline and
is the “stick viscosity,” R is the radius of the cylinder, and
is a user-defined slip tolerance for which
the default is 0.005. Using a larger slip tolerance makes convergence of the solution more rapid at the
expense of solution accuracy. Using a smaller slip tolerance imposes the “no relative motion” constraint
more accurately but may slow convergence. The default value provides a conservative balance between
efficiency and accuracy for rolling contact problems.
Since this frictional model used for steady-state rolling is different from the frictional models used
with other analysis procedures in Abaqus/Standard, discontinuities may arise in the solutions between a
steady-state transport analysis and any other analysis procedure, such as a static footprint analysis. To
ensure a smooth transition in the solution, it is recommended that all analysis steps prior to a steadystate rolling analysis use a zero coefficient of friction. You can then modify the friction properties in
the steady-state transport analysis step to use the desired friction coefficient (see “Changing friction
properties during an Abaqus/Standard analysis” in “Frictional behavior,” Section 36.1.5).
This frictional model is more relevant in a tire analysis since the velocity of the rotating tire strongly
depends on the deformation gradients along a streamline on the contact surface. The solution state at a
material point depends on the solution of neighboring points, and convective effects must be considered.
However, since the deformation gradients along a streamline on the contact surface are small in a disc
brake analysis, a simplified frictional model, which ignores the convective effect on the contact surface,
can be used. Such a frictional model is discussed in the following section.
Contact between two deformable bodies moving with different velocities
When the slave and master surfaces rotate with different velocities, such as contact between a disc
and brake assembly, slip will develop between the two deformable surfaces. The transport velocity
(“Spinning motion”) and the motion of a reference frame (“Defining a reference frame for translational or
rotational motion”) can be defined in a steady-state transport analysis procedure to model the steady-state
6.4.1–6
Abaqus Version 5.8 ID:
Printed on:
STEADY-STATE TRANSPORT ANALYSIS
frictional sliding between two deformable bodies that are moving with different velocities. In this case
it is assumed that the slip rate simply follows from the difference in velocities specified by the transport
velocity and the motion of the reference frame and is independent of the deformation gradient along
a streamline or the nodal displacements on the contact surface. No convective effects are considered
between the contact surfaces, and the frictional stress does not depend on any history effects. Hence, the
frictional stress is given by
where is the friction coefficient, p is the contact pressure, are the slip directions, and
are the slip
velocities that are defined by the transport velocity and the motion of the reference frame. If no velocity or
the same velocity are defined at contact nodes with friction, sticking conditions are applied automatically.
The friction model is described in detail in “Coulomb friction,” Section 5.2.3 of the Abaqus Theory
Manual.
Such a simplified frictional model is relevant only in a disc brake analysis. It should be used with
care in a rolling tire analysis where deformation gradients on the contact surface are significant.
Since this frictional behavior is different from the frictional models used with other analysis
procedures in Abaqus/Standard, discontinuities may arise in the solutions between a steady-state
transport analysis and any other analysis procedure. An example is the discontinuity that occurs
between the initial preloading of the disc pads in a disc brake system and the subsequent braking
analysis where the disc spins with a prescribed rotation. To ensure a smooth transition in the solution,
it is recommended that all analysis steps prior to a steady-state analysis use a zero coefficient of
friction (see “Including friction properties in a contact property definition” in “Frictional behavior,”
Section 36.1.5). You can then increase the friction coefficient to the desired value in the steady-state
transport analysis (see “Changing friction properties during an Abaqus/Standard analysis” in “Frictional
behavior,” Section 36.1.5).
Contact between surfaces spinning with the same angular velocity
When the slave and master surfaces rotate with the same angular velocity, such as the surface between
the bead and rim in a tire analysis, no relative velocity develops between the surfaces. In such a
case, frictional stresses develop as a reaction between the bodies. Abaqus/Standard will automatically
determine that the slave and master surface rotate with the same speed and apply the standard Coulomb
friction model, which is described in detail in “Frictional behavior,” Section 36.1.5.
When the standard Coulomb friction model is used in a reference frame that implies flow of material
through the mesh, convective effects must be considered. However, Abaqus/Standard assumes that no
convective effects are present between surfaces during steady-state transport analysis. In other words,
Abaqus/Standard assumes that the frictional stress at a point depends on the history of deformation in the
Lagrangian reference frame and ignores any history effects that may occur as a result of the deformation
that the point experiences during the spinning motion. The assumption that the frictional stress does
not depend on history effects during rolling is valid for modeling contact between a tire bead and rim
where relative slip occurs only during rim mounting in a static analysis prior to the steady-state transport
analysis. When slip occurs during the steady-state transport analysis, the solution obtained is no longer
6.4.1–7
Abaqus Version 5.8 ID:
Printed on:
STEADY-STATE TRANSPORT ANALYSIS
the correct steady-state solution because convective effects are ignored. To ensure that no slip takes
place between the surfaces during steady-state rolling, it is recommended that you modify the friction
properties in the steady-state transport analysis step to activate rough friction (see “Changing friction
properties during an Abaqus/Standard analysis” in “Frictional behavior,” Section 36.1.5).
Incrementation
Abaqus/Standard uses Newton’s method to solve the nonlinear equilibrium equations. The nonlinearities
in a steady-state transport analysis arise from large-displacement effects, material nonlinearity, and
boundary nonlinearities such as contact and friction. If geometrically nonlinear behavior is expected
other than the large rigid body rotation associated with the steady-state motion, the step definition
should include nonlinear geometric effects.
The steady-state rolling and sliding solution must often be obtained as a series of increments, with
iterations to obtain equilibrium within each increment. If the direct steady-state solution technique is
used, the solution in each increment is a steady-state solution corresponding to the loads acting on the
structure at that instant. If the pass-by-pass steady-state solution technique is used, the solution in each
increment is usually not a steady-state solution corresponding to the loads acting on the structure at
that instant. In this case a steady-state solution is generally obtained in several increments, with each
increment corresponding to a loading pass through the structure.
Since Newton’s method has a finite radius of convergence, too large an increment in the applied
load can prevent any solution from being obtained because the current steady-state solution is too far
away from the new steady-state equilibrium solution that is being sought: it is outside the radius of
convergence. Thus, there is an algorithmic restriction on the increment size.
Automatic incrementation
In most cases the default automatic incrementation scheme is preferred because it will select increment
sizes based on computational efficiency.
Input File Usage:
*STEADY STATE TRANSPORT
Direct incrementation
Direct user control of the increment size is also provided because if you have considerable experience
with a particular problem, you may be able to select a more economical approach.
Input File Usage:
*STEADY STATE TRANSPORT, DIRECT
Using the maximum number of iterations to determine the increment size
The solution to an increment can be accepted after the maximum number of iterations allowed has been
completed (as defined in “Commonly used control parameters,” Section 7.2.2), even if the equilibrium
tolerances are not satisfied. This approach is not recommended; it should be used only in special cases
when you have a thorough understanding of how to interpret results obtained in this way. Very small
increments and a minimum of two iterations are usually necessary in this case.
Input File Usage:
*STEADY STATE TRANSPORT, DIRECT=NO STOP
6.4.1–8
Abaqus Version 5.8 ID:
Printed on:
STEADY-STATE TRANSPORT ANALYSIS
Convergence in a steady-state transport analysis
The steady-state transport procedure may experience convergence difficulties in certain situations that
are described below.
Convergence issues with friction
The frictional forces that develop on the contact surface as a result of steady-state rolling are functions
of the spinning angular velocity, , and the traveling straight line velocity, , or cornering velocity, .
When these frictional forces are large, convergence of Newton’s method becomes difficult. Convergence
problems in Abaqus/Standard are usually resolved by taking a smaller load increment. However, contact
forces due to steady-state rolling usually do not reduce when the magnitudes of the velocities are reduced.
For example, if a spinning object is prevented from moving (
), full slipping conditions will
develop over the entire contact zone for all values of spinning angular velocity
. Consequently,
the frictional force remains constant for all
(provided that the normal force remains constant),
so that smaller increments in the velocities (
) do not reduce the magnitude of the frictional forces
and, hence, do not overcome convergence difficulties.
To provide for convergence through the use of smaller increments in such cases, the friction
coefficient can be increased from zero to the desired value over the analysis step. This is accomplished
by setting the initial friction coefficient for the model to zero (see “Including friction properties in
a contact property definition” in “Frictional behavior,” Section 36.1.5), then increasing the friction
coefficient to its final value in the steady-state transport analysis step (see “Changing friction properties
during an Abaqus/Standard analysis” in “Frictional behavior,” Section 36.1.5).
Convergence issues with the Mullins effect material model
If the Mullins effect material model is included in the material definition (see “Mullins effect,”
Section 22.6.1), there could be a strong discontinuity in the response of a structure in transitioning from
a static (non-rolling) state to a steady-state rolling state. This discontinuity is due to the damage that
occurs during the transient response (such as the damage that occurs as the structure undergoes its first
revolution after static preloading). Since the transient response is not modeled during a steady-state
transport analysis, the resulting discontinuity in the response can lead to convergence problems. The
damage associated with the Mullins effect is independent of the angular speed of rotation: as a result,
time increment cutbacks do not resolve the convergence problems. The Mullins effect can be ramped
up over the time period of the step in these situations to obtain a converged solution. In such a case the
change in response due to damage is applied gradually over the step. The solution at the end of the step
corresponds to the fully damaged material; solutions during the step correspond to a partially damaged
material and are, therefore, physically meaningless. Thus, it is recommended that in going from a static
to a steady-state rolling solution, a do-nothing step at a low angular speed of rotation be first carried out
with the Mullins effect ramped on. This facilitates resolution of the discontinuity in a gradual manner.
The do-nothing step can then be followed by the regular steady-state transport step with the Mullins
effect applied instantaneously at the beginning of the step. This approach is illustrated in “Analysis of
6.4.1–9
Abaqus Version 5.8 ID:
Printed on:
STEADY-STATE TRANSPORT ANALYSIS
a solid disc with Mullins effect and permanent set,” Section 3.1.7 of the Abaqus Example Problems
Manual.
Input File Usage:
*STEADY STATE TRANSPORT, MULLINS=RAMP or STEP (default)
Convergence issues with streamline integration in plasticity/creep models
Although in principle any material point along a streamline can be used as a starting point for the
streamline integration when material convective calculations are performed, Abaqus/Standard always
uses the material points in the original sector or the material points in the original cross-section as
starting points for the streamline integration in a model with periodic geometry or axisymmetric
geometry, respectively.
If the pass-by-pass solution technique is used, after an increment has been performed for all the
streamlines, Abaqus/Standard will automatically use the state obtained at the end of the streamline as the
starting state for the streamline integration in the subsequent increment. This iterative process is repeated
for each increment until a steady-state solution is reached.
If the direct steady-state solution technique is used, several local iterations are usually required for
each streamline, with a local iteration corresponding to an integration over a closed loop streamline.
After a local iteration has been performed for a streamline, Abaqus/Standard will check to see if the
steady-state condition is satisfied for the streamline. This is best measured by ensuring the differences
between the stresses/strains at the starting point of the streamline obtained before and after the iteration
are sufficiently small. If the steady-state condition is not satisfied for the streamline, Abaqus/Standard
will automatically use the state obtained at the end of the previous local iteration as the starting state
for the streamline integration in the subsequent local iteration. This iterative process is repeated until a
steady-state solution is reached for all the streamlines.
To improve the rate of convergence, it is recommended that you apply loads on elements or nodes
away from the starting points of the streamlines.
Initial conditions
Initial values of stresses, temperatures, field variables, solution-dependent state variables, etc. can be
specified. “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1, describes all of
the available initial conditions.
Boundary conditions
Boundary conditions can be applied to any of the displacement or rotation degrees of freedom (1–6). (See
“Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1, for details of applying
boundary conditions to rotation degrees of freedom when large rotation will occur.) During the analysis
prescribed boundary conditions can be varied using an amplitude definition (see “Amplitude curves,”
Section 33.1.2).
6.4.1–10
Abaqus Version 5.8 ID:
Printed on:
STEADY-STATE TRANSPORT ANALYSIS
Loads
Loading in a steady-state transport analysis includes the motion of the structure, inertia (d’Alembert)
forces due to motion, concentrated loads, distributed pressures, and body forces.
Inertia effects
The motion of the deformable body gives rise to inertia (d’Alembert) forces that can be included. These
forces include centrifugal and Coriolis effects.
The density of the material must be defined in the material description. At higher rotational
velocities, inertia forces can give rise to instabilities in the form of standing waves, which are likely
to prevent convergence of the Newton algorithm.
Input File Usage:
Use the following option to include inertia forces:
*STEADY STATE TRANSPORT, INERTIA=YES
Inertia loads for tetrahedral elements
Inertia loads for tetrahedral elements C3D4, C3D10, C3D10I, and C3D10M are not taken into account
in a steady-state transport analysis. Tetrahedral elements will appear only in a periodic model created by
revolving a three-dimensional sector that contains tetrahedral elements. Tetrahedral elements will not
appear in an axisymmetric model created by revolving a two-dimensional cross-section about a symmetry
axis. See “Symmetric model generation,” Section 10.4.1, for details.
Other prescribed loads
The following loads can be prescribed in a steady-state transport analysis, as described in “Concentrated
loads,” Section 33.4.2:
•
•
Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6).
Distributed pressure forces or body forces can be applied; the distributed load types available with
particular elements are described in Part VI, “Elements.”
In most cases such loads should be applied around the whole circumference of the body; a load on a
single point or element corresponds to a spatially fixed load, which in most cases is not realistic.
Predefined fields
The following predefined fields can be specified in a steady-state transport analysis, as described in
“Predefined fields,” Section 33.6.1:
•
Although temperature is not a degree of freedom in a steady-state transport analysis, nodal
temperatures can be specified as a predefined field. Any difference between the applied and
initial temperatures will cause thermal strain if a thermal expansion coefficient is given for
the material (“Thermal expansion,” Section 26.1.2). The specified temperature also affects
temperature-dependent material properties, if any.
6.4.1–11
Abaqus Version 5.8 ID:
Printed on:
STEADY-STATE TRANSPORT ANALYSIS
•
The values of user-defined field variables can be specified. These values only affect field-variabledependent material properties, if any.
Material options
Since the steady-state transport capability uses a kinematic description that implies flow of material
through the mesh, convective effects must be considered for the material response. Most material
models that describe mechanical behavior (including user-defined materials) are available for use
in a steady-state transport analysis. In particular, history-dependent viscoelasticity (“Time domain
viscoelasticity,” Section 22.7.1), history-dependent Mullins effect (“Mullins effect,” Section 22.6.1),
classical metal plasticity (“Classical metal plasticity,” Section 23.2.1), rate-dependent yield
(“Rate-dependent yield,” Section 23.2.3), rate-dependent creep (“Rate-dependent plasticity: creep and
swelling,” Section 23.2.4), and two-layer viscoplasticity (“Two-layer viscoplasticity,” Section 23.2.11)
can all be used during a steady-state transport analysis.
The following material properties are not active during a steady-state transport analysis: thermal
properties (except for thermal expansion), mass diffusion properties, electrical properties, and pore fluid
flow properties.
Abaqus/Standard also provides the ability to obtain the fully relaxed long-term elastic or elasticplastic solution during a steady-state transport analysis if the material description includes viscoelastic
or viscoplastic material properties. If the material description includes viscoelastic material properties,
the long-term solution will ignore the material convection calculations. If the two-layer viscoplastic
material model is used, the long-term solution will include only the material convection calculations
based on the long-term response of the elastic-plastic network.
Input File Usage:
*STEADY STATE TRANSPORT, LONG TERM
Choosing an appropriate material model
Since material points in a spinning and sliding body undergo repeated loading/unloading cycles, an
appropriate material model must be chosen to characterize the response correctly under such loading
conditions. The use of plasticity material models with isotropic type hardening is generally not
recommended since they will continue to harden during cyclic loading, which may lead to a large
number of iterations until the steady-state solution is reached. Kinematic hardening plasticity models
should be used to model the inelastic behavior of materials that are subjected to repeated loading.
For rate-dependent creep, the two-layer viscoplasticity model is recommended (“Two-layer
viscoplasticity,” Section 23.2.11) for modeling the response of materials with significant time-dependent
behavior as well as plasticity at elevated temperatures.
For history-dependent viscoelasticity, it is more appropriate to use cyclic (frequency domain) test
data to calibrate the time-domain viscoelastic material model for steady-state transport analysis. The
cyclic experiments should be performed in the frequency range anticipated in the rolling simulation.
Abaqus/Standard internally converts the frequency domain storage and loss modulus data into a timedomain (Prony series) representation. This data conversion capability is described in detail in “Time
domain viscoelasticity,” Section 22.7.1.
6.4.1–12
Abaqus Version 5.8 ID:
Printed on:
STEADY-STATE TRANSPORT ANALYSIS
Analysis steps prior to a steady-state transport analysis
It is recommended that the solutions in any analysis step prior to a steady-state transport analysis, such
as a static footprint or preloading solution, be based on the long-term elastic moduli or the long-term
elastic-plastic response if viscoelastic or viscoplastic material properties are used (for example, see
“Static stress analysis,” Section 6.2.2). The long-term solution provides a smooth transition between a
static analysis and a slow rolling or sliding steady-state transport analysis.
Material convection in nonlinear analysis
When material convection is included in the steady-state transport solution, Abaqus/Standard uses
an approximate Jacobian matrix in the Newton solution of the nonlinear equilibrium equations. The
rate of convergence in such a case is no longer quadratic but depends strongly on the severity of the
nonlinearities. It is often necessary to adjust the default solution controls (“Commonly used control
parameters,” Section 7.2.2) to obtain a steady-state transport solution when material convection is
considered.
Elements
Most of the three-dimensional stress/displacement elements in Abaqus/Standard can be used
in a steady-state transport analysis (see “Choosing the appropriate element for an analysis type,”
Section 27.1.3). When the three-dimensional model is generated from an axisymmetric cross-section, the
element type used in the two-dimensional model determines the element type in the three-dimensional
model. The correspondence between the two-dimensional and three-dimensional element types
is described in “Symmetric model generation,” Section 10.4.1. If the three-dimensional periodic
model is generated from a single three-dimensional sector, any of the stress/displacement elements in
Abaqus/Standard can be used.
Output
The element output available for a steady-state transport analysis includes stress, strain, energies, and
the values of state, field, and user-defined variables. The nodal output available includes displacements,
velocities, reaction forces, and coordinates. The contact output variable CSLIP contains steady-state slip
rates for the steady-state transport procedure, unlike the usual definition of this variable. All of the output
variable identifiers are outlined in “Abaqus/Standard output variable identifiers,” Section 4.2.1.
Limitations
The steady-state transport analysis capability has several limitations.
•
The deformable structure must be a full 360° cylindrical body of revolution. Convective boundary
conditions are not available to model segments of a cylinder.
•
•
The capability is not available in two dimensions.
Only one deformable spinning body is permitted. The symmetric model generation capability must
be used to generate the deformable body (“Symmetric model generation,” Section 10.4.1).
6.4.1–13
Abaqus Version 5.8 ID:
Printed on:
STEADY-STATE TRANSPORT ANALYSIS
Input file template
*HEADING
…
*SYMMETRIC MODEL GENERATION, REVOLVE
Data lines to define model generation
*SURFACE INTERACTION
*FRICTION
Specify zero friction coefficient
**
*STEP
*STATIC
Data lines to define analysis steps prior to transport analysis
*END STEP
…
*STEP
*STEADY STATE TRANSPORT
Data line to define incrementation
*CHANGE FRICTION
*FRICTION
Data lines to redefine friction coefficient
*BOUNDARY
Data lines to define boundary conditions
*TRANSPORT VELOCITY
Data lines to define spinning angular velocity
*MOTION, TRANSLATION or ROTATION
Data lines to define traveling velocity or cornering rotational velocity
*EL PRINT and/or *NODE PRINT
Data lines to request output variables
*END STEP
6.4.1–14
Abaqus Version 5.8 ID:
Printed on:
HEAT TRANSFER AND THERMAL-STRESS ANALYSIS
6.5
Heat transfer and thermal-stress analysis
•
•
•
•
“Heat transfer analysis procedures: overview,” Section 6.5.1
“Uncoupled heat transfer analysis,” Section 6.5.2
“Fully coupled thermal-stress analysis,” Section 6.5.3
“Adiabatic analysis,” Section 6.5.4
6.5–1
Abaqus Version 5.8 ID:
Printed on:
HEAT TRANSFER ANALYSIS
6.5.1
HEAT TRANSFER ANALYSIS PROCEDURES: OVERVIEW
Abaqus can solve the following types of heat transfer problems:
•
•
Uncoupled heat transfer analysis: Heat transfer problems involving conduction, forced
convection, and boundary radiation can be analyzed in Abaqus/Standard. See “Uncoupled heat transfer
analysis,” Section 6.5.2. In these analyses the temperature field is calculated without knowledge of the
stress/deformation state or the electrical field in the bodies being studied. Pure heat transfer problems
can be transient or steady-state and linear or nonlinear.
If the stress/displacement solution is dependent on
a temperature field but there is no inverse dependency, a sequentially coupled thermal-stress analysis
can be conducted in Abaqus/Standard. Sequentially coupled thermal-stress analysis is performed by
first solving the pure heat transfer problem, then reading the temperature solution into a stress analysis
as a predefined field. See “Sequentially coupled thermal-stress analysis,” Section 16.1.2. In the stress
analysis the temperature can vary with time and position but is not changed by the stress analysis solution.
Abaqus allows for dissimilar meshes between the heat transfer analysis model and the thermal-stress
analysis model. Temperature values will be interpolated based on element interpolators evaluated at
nodes of the thermal-stress model.
Sequentially coupled thermal-stress analysis:
•
A coupled temperature-displacement procedure is used
to solve simultaneously for the stress/displacement and the temperature fields. A coupled analysis
is used when the thermal and mechanical solutions affect each other strongly. For example, in rapid
metalworking problems the inelastic deformation of the material causes heating, and in contact problems
the heat conducted across gaps may depend strongly on the gap clearance or pressure.
Both Abaqus/Standard and Abaqus/Explicit provide coupled temperature-displacement analysis
procedures, but the algorithms used by each program differ considerably. In Abaqus/Standard the heat
transfer equations are integrated using a backward-difference scheme, and the coupled system is solved
using Newton’s method. These problems can be transient or steady-state and linear or nonlinear. In
Abaqus/Explicit the heat transfer equations are integrated using an explicit forward-difference time
integration rule, and the mechanical solution response is obtained using an explicit central-difference
integration rule. Fully coupled thermal-stress analysis in Abaqus/Explicit is always transient. Cavity
radiation effects cannot be included in a fully coupled thermal-stress analysis. See “Fully coupled
thermal-stress analysis,” Section 6.5.3, for more details.
•
Fully coupled thermal-electrical-structural analysis: A coupled thermal-electrical-structural
procedure is used to solve simultaneously for the stress/displacement, the electrical potential, and the
temperature fields. A coupled analysis is used when the thermal, electrical, and mechanical solutions
affect each other strongly. An example of such a process is resistance spot welding, where two or more
metal parts are joined by fusion at discrete points at the material interface. The fusion is caused by heat
generated due to the current flow at the contact points, which depends on the pressure applied at these
points.
These problems can be transient or steady-state and linear or nonlinear. Cavity radiation effects
cannot be included in a fully coupled thermal-electrical-structural analysis. This procedure is available
Fully coupled thermal-stress analysis:
6.5.1–1
Abaqus Version 5.8 ID:
Printed on:
HEAT TRANSFER ANALYSIS
only in Abaqus/Standard. See “Fully coupled thermal-electrical-structural analysis,” Section 6.7.4, for
more details.
•
Adiabatic analysis: An adiabatic mechanical analysis can be used in cases where mechanical
deformation causes heating, but the event is so rapid that this heat has no time to diffuse through the
material. Adiabatic analysis can be performed in Abaqus/Standard or Abaqus/Explicit; see “Adiabatic
analysis,” Section 6.5.4. An adiabatic analysis can be static or dynamic and linear or nonlinear.
•
Coupled thermal-electrical analysis: A fully coupled thermal-electrical analysis capability is
provided in Abaqus/Standard for problems where heat is generated due to the flow of electrical current
through a conductor. See “Coupled thermal-electrical analysis,” Section 6.7.3.
•
Cavity radiation: In Abaqus/Standard cavity radiation effects can be included (in addition
to prescribed boundary radiation) in uncoupled heat transfer problems. See “Cavity radiation,”
Section 40.1.1. The cavities can be open or closed. Symmetries and blocking within cavities can
be modeled. Viewfactors are calculated automatically, and motion of objects bounding a cavity can
be prescribed during the analysis. Cavity radiation problems are nonlinear and can be transient or
steady-state.
6.5.1–2
Abaqus Version 5.8 ID:
Printed on:
UNCOUPLED HEAT TRANSFER ANALYSIS
6.5.2
UNCOUPLED HEAT TRANSFER ANALYSIS
Products: Abaqus/Standard
Abaqus/CAE
References
•
•
•
•
“Defining an analysis,” Section 6.1.2
•
“Configuring a heat transfer procedure” in “Configuring general analysis procedures,”
Section 14.11.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual
“Heat transfer analysis procedures: overview,” Section 6.5.1
*HEAT TRANSFER
“Including volumetric heat generation in heat transfer analyses,” Section 12.10.2 of the
Abaqus/CAE User’s Manual, in the online HTML version of this manual
Overview
Uncoupled heat transfer problems:
•
are those in which the temperature field is calculated without consideration of the stress/deformation
or the electrical field in the bodies being studied;
•
•
•
can include conduction, boundary convection, and boundary radiation;
•
can include thermal interactions such as gap radiation, conductance, and heat generation between
contact surfaces—see “Thermal contact properties,” Section 36.2.1;
•
can include thermal material behavior defined in user subroutine UMATHT—see “User-defined
thermal material behavior,” Section 26.7.2;
•
•
•
can be transient or steady-state;
can include cavity radiation effects—see “Cavity radiation,” Section 40.1.1;
can include forced convection through the mesh if forced convection/diffusion heat transfer
elements are used;
can be linear or nonlinear; and
require the use of heat transfer elements.
Heat transfer analysis
Uncoupled heat transfer analysis is used to model solid body heat conduction with general, temperaturedependent conductivity, internal energy (including latent heat effects), and quite general convection and
radiation boundary conditions, including cavity radiation. Forced convection of a fluid through the mesh
can be modeled by using forced convection/diffusion elements.
6.5.2–1
Abaqus Version 5.8 ID:
Printed on:
UNCOUPLED HEAT TRANSFER ANALYSIS
Sources of nonlinearity in a heat transfer analysis
Heat transfer problems can be nonlinear because the material properties are temperature dependent or
because the boundary conditions are nonlinear. Usually the nonlinearity associated with temperaturedependent material properties is mild because the properties do not change rapidly with temperature.
However, when latent heat effects are included, the analysis may be severely nonlinear (see “Latent
heat,” Section 26.2.4).
Boundary conditions are very often nonlinear; for example, film coefficients can be functions of
surface temperature. Again, the nonlinearities are often mild and cause little difficulty. An exception
is the “boiling” film condition, in which the film coefficient can change very rapidly because the
fluid adjacent to the surface boils. A rapidly changing film condition (within a step or from one step
to another) can be modeled easily using temperature-dependent and field-variable-dependent film
coefficients. Radiation effects always make heat transfer problems nonlinear. Nonlinearities in radiation
grow as temperatures increase.
Abaqus/Standard uses an iterative scheme to solve nonlinear heat transfer problems. The scheme
uses the Newton method with some modification to improve stability of the iteration process in the
presence of highly nonlinear latent heat effects.
Steady-state cases involving severe nonlinearities are sometimes more effectively solved as
transient cases because of the stabilizing influence of the heat capacity terms. The required steady-state
solution can be obtained as the very long transient time response; the transient will simply stabilize the
solution for that long time response.
Matrix storage and solution scheme
In heat transfer analyses involving cavity radiation or forced convection/diffusion elements, the system
of equations is unsymmetric. The nonsymmetric matrix storage and solution scheme is invoked
automatically in these cases (see “Defining an analysis,” Section 6.1.2).
Steady-state analysis
Steady-state analysis means that the internal energy term (the specific heat term) in the governing
heat transfer equation is omitted. The problem then has no intrinsic physically meaningful time scale.
Nevertheless, you can assign an initial time increment, a total time period, and maximum and minimum
allowed time increments to the analysis step, which is often convenient for output identification and for
specifying prescribed temperatures and fluxes with varying magnitudes.
Any fluxes or boundary condition changes to be applied during a steady-state heat transfer step
should be given within the step, using appropriate amplitude references to specify their “time” variations
(“Amplitude curves,” Section 33.1.2). If fluxes and boundary conditions are specified for the step
without amplitude references, they are assumed to change linearly with “time” during the step, from
their magnitudes at the end of the previous step (or zero, if this is the beginning of the analysis) to their
newly specified magnitudes at the end of the heat transfer step.
Input File Usage:
*HEAT TRANSFER, STEADY STATE
6.5.2–2
Abaqus Version 5.8 ID:
Printed on:
UNCOUPLED HEAT TRANSFER ANALYSIS
Abaqus/CAE Usage:
Step module: Create Step: General: Heat transfer: Response:
Steady state
Automatic incrementation
When steady-state analysis is chosen, you suggest an initial “time” increment and define a “time”
period for the step; Abaqus/Standard then increments through the step accordingly. By default,
Abaqus/Standard automatically determines a suitable increment size for each increment of the step.
Fixed incrementation
You can also use a fixed incrementation scheme, in which Abaqus/Standard uses the same increment size
for the duration of the step. The suggested initial “time” increment,
, defines the increment size.
Input File Usage:
Set the initial increment, minimum increment size, and maximum increment
size to the same value:
*HEAT TRANSFER, STEADY STATE
, ,
,
Abaqus/CAE Usage:
Step module: Create Step: General: Heat transfer: Response:
Steady-state: Incrementation: Type: Fixed: Increment size:
Transient analysis
Time integration in transient problems is done with the backward Euler method (sometimes also
referred to as the modified Crank-Nicholson operator) in the pure conduction elements. This method is
unconditionally stable for linear problems.
The forced convection/diffusion elements use the trapezoidal rule for time integration. They
include numerical diffusion control (the “upwinding” Petrov-Galerkin method) and, optionally,
numerical dispersion control. The elements with dispersion control offer improved solution accuracy
in cases where the transient response of the fluid is important. Artificial dispersion control introduces a
stability limit on the size of the time increment such that the local Courant number
must be less than 1, where
is the time increment,
is the magnitude of the velocity vector, and
is
a characteristic element length in the direction of flow; that is, heat cannot be convected across more than
one element length,
, in a single increment of time. In a uniform velocity field the smallest element
will dictate the stable time increment. Approximate calculation of the Courant number, C, is helpful
during the mesh design stages so that excessively small stable time increments can be avoided. The
elements without dispersion control have no such stability limit; therefore, it may be more economical
to use the elements without this feature in transient cases where transient effects in the fluid itself are not
a critical part of the solution (for example, when the important solution is the temperature field in the
solid bodies that are included in the model, and when characteristic transient times in the fluid are very
much shorter than characteristic transient times in the solids).
6.5.2–3
Abaqus Version 5.8 ID:
Printed on:
UNCOUPLED HEAT TRANSFER ANALYSIS
Time incrementation in a transient heat transfer analysis can be controlled directly by you or
automatically by Abaqus/Standard. Automatic time incrementation is generally preferred.
Automatic incrementation
The time increments can be selected automatically based on the user-prescribed maximum allowable
nodal temperature change in an increment,
. Abaqus/Standard will restrict the time increments to
ensure that this value is not exceeded at any node (except nodes with boundary conditions) during any
increment of the analysis (see “Time integration accuracy in transient problems,” Section 7.2.4).
Input File Usage:
Abaqus/CAE Usage:
*HEAT TRANSFER, DELTMX=
Step module: Create Step: General: Heat transfer: Response:
Transient: Incrementation: Type: Automatic: Max. allowable
temperature change per increment:
Fixed incrementation
If you select direct incrementation and do not specify
, fixed time increments equal to the userspecified initial time increment,
, will then be used throughout the analysis.
Input File Usage:
*HEAT TRANSFER
Abaqus/CAE Usage:
Step module: Create Step: General: Heat transfer: Response: Transient:
Incrementation: Type: Fixed: Increment size:
Spurious oscillations due to small time increments
In transient heat transfer analysis with second-order elements there is a relationship between the
minimum usable time increment and the element size. A simple guideline is
where
is the time increment, is the density, c is the specific heat, k is the thermal conductivity,
and
is a typical element dimension (such as the length of a side of an element). If time increments
smaller than this value are used in a mesh of second-order elements, spurious oscillations can appear
in the solution, in particular in the vicinity of boundaries with rapid temperature changes. These
oscillations are nonphysical and may cause problems if temperature-dependent material properties
are present. Abaqus/Standard provides no check on the user-defined initial time increment; you must
ensure that the given value does not violate the above criterion.
In transient analyses using first-order elements the heat capacity terms are lumped, which eliminates
such oscillations but can lead to locally inaccurate solutions especially in terms of the heat flux for small
time increments. If smaller time increments are required, a finer mesh should be used in regions where
the temperature changes occur.
Unless you specify a maximum allowable time increment size as part of the heat transfer
step definition, there is no upper limit on the time increment size (the integration procedure is
unconditionally stable, at least for linear problems). However, if forced convection/diffusion elements
6.5.2–4
Abaqus Version 5.8 ID:
Printed on:
UNCOUPLED HEAT TRANSFER ANALYSIS
including numerical dispersion control (element types DCCxxD) are included in the model, there is a
numerical stability limit on the allowable time increment. The requirement is that
, where
is the magnitude of the fluid velocity and
is a characteristic element length in the direction of
flow. Abaqus/Standard will adjust the time increment automatically to satisfy this stability limit.
Ending a transient analysis
A transient analysis can be terminated by completing a specified time period, or it can be continued until
steady-state conditions are reached. By default, the analysis will end when the given time period has
been completed. Alternatively, you can specify that the analysis will end when steady state is reached
or after the given time period, whichever comes first. Steady state is defined by the temperature change
rate: when the temperature at every temperature degree of freedom changes at a rate that is less than the
user-specified rate (given as part of the step definition), the analysis terminates.
Input File Usage:
Use the following option to end the analysis when the time period is reached:
*HEAT TRANSFER, END=PERIOD (default)
Use the following option to end the analysis based on the temperature change
rate:
Abaqus/CAE Usage:
*HEAT TRANSFER, END=SS
Step module: Create Step: General: Heat transfer: Response: Transient:
Incrementation: End step when temperature change is less than
Internal heat generation
Volumetric heat generation within a material can be defined either in user subroutine HETVAL or user
subroutine UMATHT. These user subroutines are mutually exclusive.
Defining internal heat generation in user subroutine HETVAL
If user subroutine HETVAL is used to define internal heat generation, heat generation must be included
in the material definition with the other thermal property definitions.
Heat generation might be associated with (relatively low) energy phase changes occurring during
the solution. Such heat generation usually depends on state variables (such as the fraction transformed),
which themselves evolve with the solution and are stored as solution-dependent state variables (see “User
subroutines: overview,” Section 18.1.1). The heat generation is computed in user subroutine HETVAL,
where any associated state variables can also be updated. The subroutine will be called at all material
calculation points for which the material definition includes heat generation.
Input File Usage:
Abaqus/CAE Usage:
*HEAT GENERATION
Property module: material editor: Thermal: Heat Generation
Defining internal heat generation in user subroutine UMATHT
If user subroutine UMATHT is used to define internal heat generation, all other thermal properties must
also be defined within the subroutine.
6.5.2–5
Abaqus Version 5.8 ID:
Printed on:
UNCOUPLED HEAT TRANSFER ANALYSIS
Input File Usage:
Abaqus/CAE Usage:
*USER MATERIAL
Property module: material editor: General: User Material:
User material type: Thermal
Forced convection through the mesh
The velocity of a fluid moving through the mesh can be prescribed if forced convection/diffusion heat
transfer elements are used. Conduction between the fluid and adjacent forced convection/diffusion heat
transfer elements will be affected by the mass flow rate of the fluid. For example, if a pipe is filled with
a fluid with an initial temperature profile that contains a temperature pulse, the initial temperature pulse
will not only diffuse (because of conduction in the fluid and the pipe), but it will also be transported (or
convected) down the pipe. Since the fluid velocity is prescribed, it is called forced convection.
Natural convection occurs when differences in fluid density created by thermal gradients cause
motion of the fluid (bouyancy-driven flow). The forced convection/diffusion elements are not designed
to handle this phenomenon; the flow must be prescribed.
You can specify the mass flow rates per unit area (or through the entire section for one-dimensional
elements) at the nodes. Abaqus/Standard interpolates the mass flow rates to the material points. The
numerical solution of the transient heat transfer equation including convection becomes increasingly
difficult as convection dominates diffusion. The Peclet number, , is a dimensionless parameter that
indicates the degree of convection dominance over diffusion:
where
is the magnitude of the velocity vector, is the density, c is the specific heat, k is the thermal
conductivity, and
is a characteristic element length in the direction of flow. Large values of indicate
that convection dominates over diffusion on the spatial scale defined by the element size, . In general,
Peclet numbers greater than about 1000 should not be used.
Petrov-Galerkin finite elements are used in Abaqus/Standard to model systems with high Peclet
numbers accurately; these elements use nonsymmetric, upwinded weighting functions to control
numerical diffusion and dispersion and, thus, stabilize results. The upwinding term is partly a function
of the element Peclet number, as described in “Convection/diffusion,” Section 2.11.3 of the Abaqus
Theory Manual.
If the fluid flows along a boundary along which a rapid change of temperature is prescribed, it is,
in fact, subjected to a thermal transient, even for steady-state analysis. This transient can give rise to
the same kind of spurious temperature oscillations that are observed in transient heat transfer analysis,
as discussed earlier in this section. Since Abaqus/Standard uses first-order elements for convective heat
transfer, the oscillation can be eliminated by lumping the heat capacity terms. However, the upwinded
weighting functions prevent lumping in the direction of the flow. Hence, spurious oscillations may still
occur, in particular if the flow is not precisely tangential to the boundary along which the temperature
change occurs.
Input File Usage:
Use the following option within the heat transfer step definition to prescribe the
fluid velocity:
*MASS FLOW RATE
6.5.2–6
Abaqus Version 5.8 ID:
Printed on:
UNCOUPLED HEAT TRANSFER ANALYSIS
Abaqus/CAE Usage:
Mass flow rate is not supported in Abaqus/CAE.
Modifying or removing mass flow rates
By default, the mass flow rates given are modifications of existing flow rates or are to be applied in
addition to any mass flow rates defined previously. You can remove all previously defined mass flow
rates and, optionally, specify new mass flow rates.
Input File Usage:
Use the following option to modify an existing flow rate or to specify an
additional flow rate:
*MASS FLOW RATE, OP=MOD (default)
Use the following option to release all previously applied flow rates and to
specify new flow rates:
Abaqus/CAE Usage:
*MASS FLOW RATE, OP=NEW
Mass flow rate is not supported in Abaqus/CAE.
Specifying time-dependent mass flow rates
Mass flow rates can be given in combination with an amplitude definition, if required, to control the
magnitude of the flow rate as a function of time (“Amplitude curves,” Section 33.1.2).
Input File Usage:
Use both of the following options to define a time-dependent mass flow rate:
Abaqus/CAE Usage:
*AMPLITUDE, NAME=name
*MASS FLOW RATE, AMPLITUDE=name
Mass flow rate is not supported in Abaqus/CAE.
Defining mass flow rates in a user subroutine
Mass flow rates can be defined by user subroutine UMASFL. UMASFL will be called for each specified
node. Any mass flow rate values given directly will be ignored.
Input File Usage:
Abaqus/CAE Usage:
*MASS FLOW RATE, USER
Mass flow rate is not supported in Abaqus/CAE.
Reading the mass flow rate data from an alternate file
The data for the mass flow rate can be contained in an alternate file. See “Input syntax rules,”
Section 1.2.1, for the syntax of the file name.
Input File Usage:
Abaqus/CAE Usage:
*MASS FLOW RATE, INPUT=file_name
Mass flow rate is not supported in Abaqus/CAE.
Cavity radiation
Cavity radiation can be activated in a heat transfer step. This feature involves interacting heat transfer
between all of the facets of the cavity surface, dependent on the facet temperatures, facet emissivities,
and the geometric viewfactors between each facet pair. When the thermal emissivity is a function of
6.5.2–7
Abaqus Version 5.8 ID:
Printed on:
UNCOUPLED HEAT TRANSFER ANALYSIS
temperature or field variables, you can specify the maximum allowable emissivity change during an
increment in addition to the maximum temperature change to control the time incrementation. See
“Cavity radiation,” Section 40.1.1, for more information.
Input File Usage:
Use the following option in the step definition to activate cavity radiation:
*RADIATION VIEWFACTOR
Use the following option to specify the maximum allowable emissivity change:
Abaqus/CAE Usage:
*HEAT TRANSFER, MXDEM=max_delta_emissivity
You can specify the maximum allowable emissivity change for a heat transfer
step.
Step module: Create Step: General: Heat transfer: Incrementation:
Max. allowable emissivity change per increment
Initial conditions
By default, the initial temperature of all nodes is zero. You can specify nonzero initial temperatures (see
“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1).
Forced convection through the mesh
In a heat transfer analysis involving forced convection through the mesh, you can define nonzero initial
mass flow rates at the nodes of the forced convection/diffusion heat transfer elements in the model, as
described in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1.
For element types DCC1D2 and DCC1D2D the mass flow rate is positive from the first to the second
node of the element. For two- and three-dimensional elements the direction of the mass flow rate is
defined by giving the components in the x-, y-, and z-directions.
Input File Usage:
Abaqus/CAE Usage:
*INITIAL CONDITIONS, TYPE=MASS FLOW RATE
Mass flow rate is not supported in Abaqus/CAE.
Boundary conditions
Boundary conditions can be used to prescribe temperatures (degree of freedom 11) at nodes in a heat
transfer analysis (see “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1).
Shell elements have additional temperature degrees of freedom 12, 13, etc. through the thickness (see
“Conventions,” Section 1.2.2). Boundary conditions can be specified as functions of time by referring
to amplitude curves (see “Amplitude curves,” Section 33.1.2).
For purely diffusive heat transfer elements a boundary without any prescribed boundary conditions
(natural boundary condition) corresponds to an insulated surface. For forced convection/diffusion
elements only the flux associated with conduction is zero; energy is free to convect across an
unconstrained surface. This natural boundary condition correctly models areas where fluid is crossing
a surface (as, for example, at the upstream and downstream boundaries of the mesh) and prevents
spurious reflections of energy back into the mesh.
6.5.2–8
Abaqus Version 5.8 ID:
Printed on:
UNCOUPLED HEAT TRANSFER ANALYSIS
Loads
The following types of loading can be prescribed in a heat transfer analysis, as described in “Thermal
loads,” Section 33.4.4:
•
•
•
•
Concentrated heat fluxes.
Body fluxes and distributed surface fluxes.
Average-temperature radiation conditions.
Convective film conditions and radiation conditions; film properties can be made a function of
temperature.
Cavity radiation effects can also be included, as described in “Cavity radiation,” Section 40.1.1.
Predefined fields
Predefined temperature fields are not allowed in heat transfer analyses. Boundary conditions should be
used instead to specify temperatures, as described earlier.
Other predefined field variables can be specified in a heat transfer analysis. These values will affect
field-variable-dependent material properties, if any. See “Predefined fields,” Section 33.6.1.
Material options
The thermal conductivity of the materials in a heat transfer analysis must be defined. The specific heat
and density of the materials must also be defined for transient heat transfer problems. Latent heat can
be defined for diffusive heat transfer elements if changes in internal energy due to phase changes are
important. Latent heat cannot be defined directly for forced convection/diffusion elements. See “Thermal
properties: overview,” Section 26.2.1, for details on defining thermal properties in Abaqus.
Alternatively, user subroutine UMATHT can be used to define the thermal constitutive behavior of
the material, including internal heat generation. For example, if a material modeled can go through a
complex phase change, the specific heat can be defined in user subroutine UMATHT in sufficient detail to
capture the phase change.
Thermal expansion coefficients are not meaningful in an uncoupled heat transfer analysis problem
since deformation of the structure is not considered.
Elements
The heat transfer element library in Abaqus/Standard includes diffusive heat transfer elements, which
allow for heat storage (specific heat and latent heat effects) and heat conduction.
Forced convection/diffusion heat transfer elements are also available: in addition to heat storage and
heat conduction these elements allow for forced convection caused by fluid flowing through the mesh.
These elements cannot be used with latent heat—see “Solid (continuum) elements,” Section 28.1.1,
for additional details. Forced convection/diffusion elements with dispersion control are available for
problems where the temperature transient in the fluid must be calculated accurately. See “Choosing the
appropriate element for an analysis type,” Section 27.1.3.
6.5.2–9
Abaqus Version 5.8 ID:
Printed on:
UNCOUPLED HEAT TRANSFER ANALYSIS
Multiple temperatures are available through the thickness of shell heat transfer elements. See
“Choosing a shell element,” Section 29.6.2.
The first-order heat transfer elements (such as the 2-node link, 4-node quadrilateral, and 8-node
brick) use a numerical integration rule with the integration stations located at the corners of the
element for the heat capacitance terms and for the calculations of the distributed surface fluxes.
First-order diffusive elements are preferred in cases involving latent heat effects since they use
such a special integration technique to provide accurate solutions with large latent heats. The forced
convection/diffusion elements cannot use this special integration technique and, therefore, are unsuitable
for problems with latent heat effects. The second-order heat transfer elements use conventional Gaussian
integration. Thus, the second-order elements are to be preferred for problems when the solution will
be smooth (without latent heat effects), and usually give more accurate results for the same number of
nodes in the mesh.
Thermal interactions between adjacent surfaces and thermal gap elements are also provided to model
heat transfer across the boundary layer between a solid and a fluid or between two closely adjacent solids.
See “Thermal contact properties,” Section 36.2.1.
Output
The following heat transfer output variables are available:
Element integration point variables:
HFL
HFLn
HFLM
TEMP
MFR
MFRn
Magnitude and components of the heat flux vector.
Component n of the heat flux vector (n=1, 2, 3).
Magnitude of the heat flux vector.
Integration point temperatures.
User-specified mass flow rates.
Component n of the mass flow rate (n=1, 2, 3).
Whole element variables:
FLUXS
NFLUX
FILM
RAD
Current values of uniform distributed heat fluxes.
Fluxes at the nodes caused by heat conduction (internal fluxes).
Current values of film conditions.
Current values of radiation conditions.
Nodal variables:
NT
NTn
RFL
RFLn
CFL
CFLn
Nodal point temperatures.
Temperature degree of freedom n at a node (n=11, 12, …).
Reaction flux values due to prescribed temperature.
Reaction flux value n at a node (n=11, 12, …).
Concentrated flux values.
Concentrated flux value n at a node (n=11, 12, …).
6.5.2–10
Abaqus Version 5.8 ID:
Printed on:
UNCOUPLED HEAT TRANSFER ANALYSIS
RFLE
Total flux at a node, including flux convected through the node in forced
convection/diffusion elements but excluding external fluxes due to user-defined
concentrated fluxes, distributed fluxes, film conditions, radiation conditions, and
cavity radiation. Since RFLE is a scalar nodal output variable, care should be
taken when summing it over on two surfaces with shared nodes. If node sets on
both surfaces include the shared nodes, the output of RFLE on the common nodes
will contribute to the sums of this output quantity on both surfaces.
RFLEn
Total flux value n at a node (n=11, 12, …).
All of the output variables available in Abaqus/Standard are listed in “Abaqus/Standard output variable
identifiers,” Section 4.2.1.
Input file template
*HEADING
…
*PHYSICAL CONSTANTS, ABSOLUTE ZERO=
*INITIAL CONDITIONS, TYPE=TEMPERATURE
Data lines to prescribe initial temperatures at the nodes
*AMPLITUDE, NAME=trefamp
Data lines to define amplitude curve to be used for radiation reference temperature,
*FILM PROPERTY, NAME=film
Data lines to define the convection film coefficient, h, as a function of temperature
**
*STEP
Transient analysis including forced convection through the mesh
*HEAT TRANSFER, END=SS, DELTMX=
Data line to define incrementation and steady state
**
*CFLUX and/or *DFLUX
Data lines to define concentrated and/or distributed fluxes
*FILM
Data lines referring to film property table film
*RADIATE, AMPLITUDE=trefamp
Data lines to define boundary radiation
**
*EL PRINT
TEMP, HFL
NFLUX, FILM, RAD
*NODE PRINT
NT11, RFL
*END STEP
6.5.2–11
Abaqus Version 5.8 ID:
Printed on:
COUPLED THERMAL-STRESS ANALYSIS
6.5.3
FULLY COUPLED THERMAL-STRESS ANALYSIS
Products: Abaqus/Standard
Abaqus/Explicit
Abaqus/CAE
References
•
•
•
•
•
•
•
“Defining an analysis,” Section 6.1.2
“Heat transfer analysis procedures: overview,” Section 6.5.1
*COUPLED TEMPERATURE-DISPLACEMENT
*DYNAMIC TEMPERATURE-DISPLACEMENT
“Specifying an inelastic heat fraction,” Section 12.10.3 of the Abaqus/CAE User’s Manual, in the
online HTML version of this manual
“Configuring a fully coupled, simultaneous heat transfer and stress procedure” in “Configuring
general analysis procedures,” Section 14.11.1 of the Abaqus/CAE User’s Manual, in the online
HTML version of this manual
“Configuring a dynamic fully coupled thermal-stress procedure using explicit integration” in
“Configuring general analysis procedures,” Section 14.11.1 of the Abaqus/CAE User’s Manual, in
the online HTML version of this manual
Overview
A fully coupled thermal-stress analysis:
•
•
•
•
•
is performed when the mechanical and thermal solutions affect each other strongly and, therefore,
must be obtained simultaneously;
requires the existence of elements with both temperature and displacement degrees of freedom in
the model;
can be used to analyze time-dependent material response;
cannot include cavity radiation effects but may include average-temperature radiation conditions
(see “Thermal loads,” Section 33.4.4); and
takes into account temperature dependence of material properties only for the properties that are
assigned to elements with temperature degrees of freedom.
In Abaqus/Standard a fully coupled thermal-stress analysis:
•
•
neglects inertia effects; and
can be transient or steady-state.
In Abaqus/Explicit a fully coupled thermal-stress analysis:
•
•
includes inertia effects; and
models transient thermal response.
6.5.3–1
Abaqus Version 5.8 ID:
Printed on:
COUPLED THERMAL-STRESS ANALYSIS
Fully coupled thermal-stress analysis
Fully coupled thermal-stress analysis is needed when the stress analysis is dependent on the temperature
distribution and the temperature distribution depends on the stress solution. For example, metalworking
problems may include significant heating due to inelastic deformation of the material which, in
turn, changes the material properties. In addition, contact conditions exist in some problems where
the heat conducted between surfaces may depend strongly on the separation of the surfaces or the
pressure transmitted across the surfaces (see “Thermal contact properties,” Section 36.2.1). For such
cases the thermal and mechanical solutions must be obtained simultaneously rather than sequentially.
Coupled temperature-displacement elements are provided for this purpose in both Abaqus/Standard
and Abaqus/Explicit; however, each program uses different algorithms to solve coupled thermal-stress
problems.
Fully coupled thermal-stress analysis in Abaqus/Standard
In Abaqus/Standard the temperatures are integrated using a backward-difference scheme, and the
nonlinear coupled system is solved using Newton’s method. Abaqus/Standard offers an exact as well
as an approximate implementation of Newton’s method for fully coupled temperature-displacement
analysis.
Exact implementation
An exact implementation of Newton’s method involves a nonsymmetric Jacobian matrix as is illustrated
in the following matrix representation of the coupled equations:
where
and
are the respective corrections to the incremental displacement and temperature,
are submatrices of the fully coupled Jacobian matrix, and
and
are the mechanical and thermal
residual vectors, respectively.
Solving this system of equations requires the use of the unsymmetric matrix storage and solution
scheme. Furthermore, the mechanical and thermal equations must be solved simultaneously. The method
provides quadratic convergence when the solution estimate is within the radius of convergence of the
algorithm. The exact implementation is used by default.
Approximate implementation
Some problems require a fully coupled analysis in the sense that the mechanical and thermal solutions
evolve simultaneously, but with a weak coupling between the two solutions. In other words, the
components in the off-diagonal submatrices
,
are small compared to the components in
the diagonal submatrices
,
. An example of such a situation is the disc brake problem
(“Thermal-stress analysis of a disc brake,” Section 5.1.1 of the Abaqus Example Problems Manual).
For these problems a less costly solution may be obtained by setting the off-diagonal submatrices to
zero so that we obtain an approximate set of equations:
6.5.3–2
Abaqus Version 5.8 ID:
Printed on:
COUPLED THERMAL-STRESS ANALYSIS
As a result of this approximation the thermal and mechanical equations can be solved separately,
with fewer equations to consider in each subproblem. The savings due to this approximation, measured
as solver time per iteration, will be of the order of a factor of two, with similar significant savings in
solver storage of the factored stiffness matrix. Further, in many situations the subproblems may be fully
symmetric or approximated as symmetric, so that the less costly symmetric storage and solution scheme
can be used. The solver time savings for a symmetric solution is an additional factor of two. Unless
you explicitly choose the unsymmetric matrix storage and solution scheme, selection of the scheme will
depend on other details of the problem (see “Defining an analysis,” Section 6.1.2).
This modified form of Newton’s method does not affect solution accuracy since the fully coupled
effect is considered through the residual vector
at each increment in time. However, the rate of
convergence is no longer quadratic and depends strongly on the magnitude of the coupling effect, so more
iterations are generally needed to achieve equilibrium than with the exact implementation of Newton’s
method. When the coupling is significant, the convergence rate becomes very slow and may prohibit
obtaining a solution. In such cases the exact implementation of Newton’s method is required. In cases
where it is possible to use this approximation, the convergence in an increment will depend strongly on the
quality of the first guess to the incremental solution, which you can control by selecting the extrapolation
method used for the step (see “Defining an analysis,” Section 6.1.2).
Input File Usage:
Use the following option to specify a separated solution scheme:
Abaqus/CAE Usage:
*SOLUTION TECHNIQUE, TYPE=SEPARATED
Step module: Create Step: General: Coupled temp-displacement:
Other: Solution technique: Separated
Steady-state analysis
A steady-state coupled temperature-displacement analysis can be performed in Abaqus/Standard. In
steady-state cases you should assign an arbitrary “time” scale to the step: you specify a “time” period
and “time” incrementation parameters. This time scale is convenient for changing loads and boundary
conditions through the step and for obtaining solutions to highly nonlinear (but steady-state) cases;
however, for the latter purpose, transient analysis often provides a natural way of coping with the
nonlinearity.
Frictional slip heat generation is normally neglected in for the steady-state case. However, it can still
be accounted for if motions are used to specify translational or rotational nodal velocities in disk braketype problems or if user subroutine FRIC provides the incremental frictional dissipation through the
variable SFD. If frictional heat generation is present, the heat flux into the two contact surfaces depends
on the slip rate of the surfaces. The “time” scale in this case cannot be described as arbitrary, and a
transient analysis should be performed.
Input File Usage:
Abaqus/CAE Usage:
*COUPLED TEMPERATURE-DISPLACEMENT, STEADY STATE
Step module: Create Step: General: Coupled temp-displacement:
Basic: Response: Steady state
6.5.3–3
Abaqus Version 5.8 ID:
Printed on:
COUPLED THERMAL-STRESS ANALYSIS
Transient analysis
Alternatively, you can perform a transient coupled temperature-displacement analysis. You can control
the time incrementation in a transient analysis directly, or Abaqus/Standard can control it automatically.
Automatic time incrementation is generally preferred.
Automatic incrementation controlled by a maximum allowable temperature change
The time increments can be selected automatically based on a user-prescribed maximum allowable nodal
temperature change in an increment,
. Abaqus/Standard will restrict the time increments to ensure
that this value is not exceeded at any node (except nodes with boundary conditions) during any increment
of the analysis (see “Time integration accuracy in transient problems,” Section 7.2.4).
Input File Usage:
Abaqus/CAE Usage:
*COUPLED TEMPERATURE-DISPLACEMENT, DELTMX=
Step module: Create Step: General: Coupled temp-displacement:
Basic: Response: Transient; Incrementation: Type: Automatic, Max.
allowable temperature change per increment:
Fixed incrementation
If you do not specify
, fixed time increments equal to the user-specified initial time increment,
, will be used throughout the analysis.
Input File Usage:
*COUPLED TEMPERATURE-DISPLACEMENT
Abaqus/CAE Usage:
Step module: Create Step: General: Coupled temp-displacement: Basic:
Response: Transient; Incrementation: Type: Fixed: Increment size:
Spurious oscillations due to small time increments
In transient analysis with second-order elements there is a relationship between the minimum usable time
increment and the element size. A simple guideline is
where
is the time increment, is the density, c is the specific heat, k is the thermal conductivity, and
is a typical element dimension (such as the length of a side of an element). If time increments smaller
than this value are used in a mesh of second-order elements, spurious oscillations can appear in the
solution, in particular in the vicinity of boundaries with rapid temperature changes. These oscillations
are nonphysical and may cause problems if temperature-dependent material properties are present.
In transient analyses using first-order elements the heat capacity terms are lumped, which eliminates
such oscillations but can lead to locally inaccurate solutions for small time increments. If smaller time
increments are required, a finer mesh should be used in regions where the temperature changes rapidly.
There is no upper limit on the time increment size (the integration procedure is unconditionally
stable) unless nonlinearities cause convergence problems.
6.5.3–4
Abaqus Version 5.8 ID:
Printed on:
COUPLED THERMAL-STRESS ANALYSIS
Automatic incrementation controlled by the creep response
The accuracy of the integration of time-dependent (creep) material behavior is governed by the
user-specified accuracy tolerance parameter,
. This parameter is used
to prescribe the maximum strain rate change allowed at any point during an increment, as described
in “Rate-dependent plasticity: creep and swelling,” Section 23.2.4. The accuracy tolerance parameter
can be specified together with the maximum allowable nodal temperature change in an increment,
(described above); however, specifying the accuracy tolerance parameter activates automatic
incrementation even if
is not specified.
,
Input File Usage:
*COUPLED TEMPERATURE-DISPLACEMENT, DELTMX=
CETOL=tolerance
Abaqus/CAE Usage:
Step module: Create Step: General: Coupled temp-displacement: Basic:
Response: Transient, Include creep/swelling/viscoelastic behavior;
Incrementation: Type: Automatic, Max. allowable temperature
, Creep/swelling/viscoelastic
change per increment:
strain error tolerance: tolerance
Selecting explicit creep integration
Nonlinear creep problems (“Rate-dependent plasticity: creep and swelling,” Section 23.2.4) that exhibit
no other nonlinearities can be solved efficiently by forward-difference integration of the inelastic
strains if the inelastic strain increments are smaller than the elastic strains. This explicit method is
efficient computationally because, unlike implicit methods, iteration is not required as long as no other
nonlinearities are present. Although this method is only conditionally stable, the numerical stability
limit of the explicit operator is in many cases sufficiently large to allow the solution to be developed in
a reasonable number of time increments.
For most coupled thermal-stress analyses, however, the unconditional stability of the backward
difference operator (implicit method) is desirable. In such cases the implicit integration scheme may be
invoked automatically by Abaqus/Standard.
Explicit integration can be less expensive computationally and simplifies implementation of userdefined creep laws in user subroutine CREEP; you can restrict Abaqus/Standard to using this method
for creep problems (with or without geometric nonlinearity included). See “Rate-dependent plasticity:
creep and swelling,” Section 23.2.4, for further details.
Input File Usage:
*COUPLED TEMPERATURE-DISPLACEMENT, CETOL=tolerance,
CREEP=EXPLICIT
Abaqus/CAE Usage:
Step module: Create Step: General: Coupled temp-displacement: Basic:
Response: Transient, Include creep/swelling/viscoelastic behavior;
Incrementation: Type: Automatic, Creep/swelling/viscoelastic
strain error tolerance: tolerance, Creep/swelling/viscoelastic
integration: Explicit
6.5.3–5
Abaqus Version 5.8 ID:
Printed on:
COUPLED THERMAL-STRESS ANALYSIS
Excluding creep and viscoelastic response
You can specify that no creep or viscoelastic response will occur during a step even if creep or viscoelastic
material properties have been defined.
Input File Usage:
*COUPLED TEMPERATURE-DISPLACEMENT, DELTMX=
CREEP=NONE
Abaqus/CAE Usage:
Step module: Create Step: General: Coupled tempdisplacement: Basic: Response: Transient, toggle off Include
creep/swelling/viscoelastic behavior
,
Unstable problems
Some types of analyses may develop local instabilities, such as surface wrinkling, material instability,
or local buckling. In such cases it may not be possible to obtain a quasi-static solution, even with
the aid of automatic incrementation. Abaqus/Standard offers a method of stabilizing this class of
problems by applying damping throughout the model in such a way that the viscous forces introduced
are sufficiently large to prevent instantaneous buckling or collapse but small enough not to affect the
behavior significantly while the problem is stable. The available automatic stabilization schemes are
described in detail in “Automatic stabilization of unstable problems” in “Solving nonlinear problems,”
Section 7.1.1.
Units
In coupled problems where two different fields are active, take care when choosing the units of the
problem. If the choice of units is such that the terms generated by the equations for each field are
different by many orders of magnitude, the precision on some computers may be insufficient to resolve the
numerical ill-conditioning of the coupled equations. Therefore, choose units that avoid ill-conditioned
matrices. For example, consider using units of Mpascal instead of pascal for the stress equilibrium
equations to reduce the disparity between the magnitudes of the stress equilibrium equations and the
heat flux continuity equations.
Fully coupled thermal-stress analysis in Abaqus/Explicit
In Abaqus/Explicit the heat transfer equations are integrated using the explicit forward-difference time
integration rule
where
is the temperature at node N and the subscript i refers to the increment number in an explicit
dynamic step. The forward-difference integration is explicit in the sense that no equations need to be
solved when a lumped capacitance matrix is used. The current temperatures are obtained using known
are computed at the beginning of the
values of
from the previous increment. The values of
increment by
6.5.3–6
Abaqus Version 5.8 ID:
Printed on:
COUPLED THERMAL-STRESS ANALYSIS
where
is the lumped capacitance matrix,
is the applied nodal source vector, and
is the
internal flux vector.
The mechanical solution response is obtained using the explicit central-difference integration rule
with a lumped mass matrix as described in “Explicit dynamic analysis,” Section 6.3.3. Since both the
forward-difference and central-difference integrations are explicit, the heat transfer and mechanical
solutions are obtained simultaneously by an explicit coupling. Therefore, no iterations or tangent
stiffness matrices are required.
Explicit integration can be less expensive computationally and simplifies the treatment of contact.
For a comparison of explicit and implicit direct-integration procedures, see “Dynamic analysis
procedures: overview,” Section 6.3.1.
Stability
The explicit procedure integrates through time by using many small time increments. The centraldifference and forward-difference operators are conditionally stable. The stability limit for both operators
(with no damping in the mechanical solution response) is obtained by choosing
where
is the highest frequency in the system of equations of the mechanical solution response and
is the largest eigenvalue in the system of equations of the thermal solution response.
Estimating the time increment size
An approximation to the stability limit for the forward-difference operator in the thermal solution
response is given by
where
is the smallest element dimension in the mesh and
is the thermal diffusivity of the
material. The parameters k, , and c represent the material’s thermal conductivity, density, and specific
heat, respectively.
In most applications of explicit analysis the mechanical response will govern the stability limit. The
thermal response may govern the stability limit when material parameter values are non-physical or a
very large amount of mass scaling is used. The calculation of the time increment size for the mechanical
solution response is discussed in “Explicit dynamic analysis,” Section 6.3.3.
Stable time increment report
Abaqus/Explicit writes a report to the status (.sta) file during the data check phase of the analysis
that contains an estimate of the minimum stable time increment and a listing of the elements with the
smallest stable time increments and their values. The initial minimum stable time increment accounts
6.5.3–7
Abaqus Version 5.8 ID:
Printed on:
COUPLED THERMAL-STRESS ANALYSIS
for the stability requirements of both the thermal and mechanical solution responses. The initial stable
time increments listed do not include damping (bulk viscosity), mass scaling, or penalty contact effects
in the mechanical solution response.
This listing is provided because often a few elements have much smaller stability limits than the
rest of the elements in the mesh. The stable time increment can be increased by modifying the mesh to
increase the size of the controlling element or by using appropriate mass scaling.
Time incrementation
The time increment used in an analysis must be smaller than the stability limits of the centraland forward-difference operators. Failure to use such a time increment will result in an unstable
solution. When the solution becomes unstable, the time history response of solution variables, such
as displacements, will usually oscillate with increasing amplitudes. The total energy balance will also
change significantly.
Abaqus/Explicit has two strategies for time incrementation control: fully automatic time
incrementation (where the code accounts for changes in the stability limit) and fixed time incrementation.
Scaling the time increment
To reduce the chance of a solution going unstable, the stable time increment computed by Abaqus/Explicit
can be adjusted by a constant scaling factor. This factor can be used to scale the default global time
estimate, the element-by-element estimate, or the fixed time increment based on the initial element-byelement estimate; it cannot be used to scale a fixed time increment that you specified directly.
Input File Usage:
Use any of the following options:
*DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT,
SCALE FACTOR=f
*DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT,
ELEMENT BY ELEMENT, SCALE FACTOR=f
*DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT,
FIXED TIME INCREMENTATION, SCALE FACTOR=f
Abaqus/CAE Usage:
Step module: Create Step: General: Dynamic, Temp-disp, Explicit:
Incrementation: Time scaling factor: f
Automatic time incrementation
The default time incrementation scheme in Abaqus/Explicit is fully automatic and requires no user
intervention. Two types of estimates are used to determine the stability limit: element-by-element for
both the thermal and mechanical solution responses and global for the mechanical solution response.
An analysis always starts by using the element-by-element estimation method and may switch to the
global estimation method under certain circumstances, as explained in “Explicit dynamic analysis,”
Section 6.3.3.
In an analysis Abaqus/Explicit initially uses a stability limit based on the thermal and mechanical
solution responses in the whole model. This element-by-element estimate is determined using the
smallest time increment size due to the thermal and mechanical solution responses in each element.
6.5.3–8
Abaqus Version 5.8 ID:
Printed on:
COUPLED THERMAL-STRESS ANALYSIS
The element-by-element estimate is conservative; it will give a smaller stable time increment than
the true stability limit, which is based upon the maximum frequency of the entire model. In general,
constraints such as boundary conditions and kinematic contact have the effect of compressing the
eigenvalue spectrum, and the element-by-element estimates do not take this into account (see “Explicit
dynamic analysis,” Section 6.3.3)
The stable time increment size due to the mechanical solution response will be determined by
the global estimator as the step proceeds unless the element-by-element estimator is chosen, fixed
time incrementation is specified, or one of the conditions explained in “Explicit dynamic analysis,”
Section 6.3.3, prevents the use of global estimation. The stable time increment size due to the thermal
solution response will always be determined by using an element-by-element estimation method. The
switch to the global estimation method in mechanical solution response occurs once the algorithm
determines that the accuracy of the global estimation method is acceptable. For details, see “Explicit
dynamic analysis,” Section 6.3.3
For three-dimensional continuum elements and elements with plane stress formulations (shell,
membrane, and two-dimensional plane stress elements) an “improved” estimate of the element
characteristic length is used by default. This “improved” method usually results in a larger element
stable time increment than a more traditional method. For analyses using variable mass scaling, the
total mass added to achieve a given stable time increment will be less with the improved estimate.
Input File Usage:
Use the following option to specify the element-by-element estimation method:
*DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT,
ELEMENT BY ELEMENT
Use the following option to activate the “improved” element time estimation
method:
*DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT,
IMPROVED DT METHOD=YES
Use the following option to deactivate the “improved” element time estimation
method:
*DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT,
IMPROVED DT METHOD=NO
Abaqus/CAE Usage:
Step module: Create Step: General: Dynamic, Temp-disp,
Explicit: Incrementation: Type: Automatic, Stable increment
estimator: Element-by-element
The ability to deactivate the “improved” element time estimation method is not
supported in Abaqus/CAE.
Fixed time incrementation
A fixed time incrementation scheme is also available in Abaqus/Explicit. The fixed time increment size
is determined either by the initial element-by-element stability estimate for the step or by a user-specified
time increment.
6.5.3–9
Abaqus Version 5.8 ID:
Printed on:
COUPLED THERMAL-STRESS ANALYSIS
Fixed time incrementation may be useful when a more accurate representation of the higher mode
response of a problem is required. In this case a time increment size smaller than the element-by-element
estimates may be used. The element-by-element estimate can be obtained simply by running a data check
analysis (see “Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution,” Section 3.2.2).
When fixed time incrementation is used, Abaqus/Explicit will not check that the computed response
is stable during the step. You should ensure that a valid response has been obtained by carefully checking
the energy history and other response variables.
If you choose to use time increments the size of the initial element-by-element stability limit
throughout a step, the dilatational wave speed and the thermal diffusivity in each element at the
beginning of the step are used to compute the fixed time increment size. To reduce the chance of a
solution going unstable, the initial stable time increment that Abaqus/Explicit computes can be adjusted
by a constant scaling factor, as described above in “Scaling the time increment.” Alternatively, you can
specify a time increment size directly.
Input File Usage:
Use the following option to request time increments the size of the element-byelement stability limit:
*DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT,
FIXED TIME INCREMENTATION
Use the following option to specify the time increment size directly:
*DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT,
DIRECT USER CONTROL
Abaqus/CAE Usage:
Step module: Create Step: General: Dynamic, Temp-disp, Explicit:
Incrementation: Type: Fixed, Use element-by-element time increment
estimator or User-defined time increment:
Reducing the computational cost by using selective subcycling
The selective subcycling method can be used in a coupled thermal-stress analysis exactly as in a
pure mechanical analysis, as described in “Explicit dynamic analysis,” Section 6.3.3 and “Selective
subcycling,” Section 11.7.1.
Monitoring output variables for extreme values
The extreme values defined as the element and nodal variables in a coupled thermal-stress analysis can
be monitored exactly as described in “Explicit dynamic analysis,” Section 6.3.3, for a pure mechanical
analysis.
Initial conditions
By default, the initial temperature of all nodes is zero. You can specify nonzero initial temperatures.
Initial stresses, field variables, etc. can also be defined; “Initial conditions in Abaqus/Standard and
Abaqus/Explicit,” Section 33.2.1, describes all of the initial conditions that are available for a fully
coupled thermal-stress analysis.
6.5.3–10
Abaqus Version 5.8 ID:
Printed on:
COUPLED THERMAL-STRESS ANALYSIS
Boundary conditions
Boundary conditions can be used to prescribe both temperatures (degree of freedom 11) and
displacements/rotations (degrees of freedom 1–6) at nodes in fully coupled thermal-stress analysis (see
“Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1). Shell elements in
Abaqus/Standard have additional temperature degrees of freedom 12, 13, etc. through the thickness
(see “Conventions,” Section 1.2.2).
Boundary conditions can be specified as functions of time by referring to amplitude curves
(“Amplitude curves,” Section 33.1.2).
Boundary conditions applied during a dynamic coupled temperature-displacement response
step should use appropriate amplitude references (“Amplitude curves,” Section 33.1.2). If boundary
conditions are specified for the step without amplitude references, they are applied instantaneously at
the beginning of the step. Since Abaqus/Explicit does not admit jumps in displacement, the value of
a nonzero displacement boundary condition that is specified without an amplitude reference will be
ignored, and a zero velocity boundary condition will be enforced.
Loads
The following types of thermal loads can be prescribed in a fully coupled thermal-stress analysis, as
described in “Thermal loads,” Section 33.4.4:
•
•
•
•
•
Concentrated heat fluxes.
Body fluxes and distributed surface fluxes.
Node-based film and radiation conditions.
Average-temperature radiation conditions.
Element and surface-based film and radiation conditions.
The following types of mechanical loads can be prescribed:
•
Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6); see
“Concentrated loads,” Section 33.4.2.
•
Distributed pressure forces or body forces can be applied; see “Distributed loads,” Section 33.4.3.
The distributed load types available with particular elements are described in Part VI, “Elements.”
Predefined fields
Predefined temperature fields are not allowed in a fully coupled thermal-stress analysis. Boundary
conditions should be used instead to prescribe temperature degree of freedom 11 (and 12, 13, etc. in
Abaqus/Standard shell elements), as described earlier.
Other predefined field variables can be specified in a fully coupled thermal-stress analysis. These
values will affect only field-variable-dependent material properties, if any. See “Predefined fields,”
Section 33.6.1.
6.5.3–11
Abaqus Version 5.8 ID:
Printed on:
COUPLED THERMAL-STRESS ANALYSIS
Material options
The materials in a fully coupled thermal-stress analysis must have both thermal properties, such as
conductivity, and mechanical properties, such as elasticity, defined. See Part V, “Materials,” for details
on the material models available in Abaqus.
In Abaqus/Standard internal heat generation can be specified; see “Uncoupled heat transfer
analysis,” Section 6.5.2.
Thermal strain will arise if thermal expansion (“Thermal expansion,” Section 26.1.2) is included in
the material property definition.
In Abaqus/Standard a fully coupled temperature-displacement analysis can be used to analyze static
creep and swelling problems, which generally occur over fairly long time periods (“Rate-dependent
plasticity: creep and swelling,” Section 23.2.4); viscoelastic materials (“Time domain viscoelasticity,”
Section 22.7.1); or viscoplastic materials (“Rate-dependent yield,” Section 23.2.3).
Inelastic energy dissipation as a heat source
You can specify an inelastic heat fraction in a fully coupled thermal-stress analysis to provide for inelastic
energy dissipation as a heat source. Plastic straining gives rise to a heat flux per unit volume of
where
is the heat flux that is added into the thermal energy balance, is a user-defined factor (assumed
constant), is the stress, and
is the rate of plastic straining.
Inelastic heat fractions are typically used in the simulation of high-speed manufacturing processes
involving large amounts of inelastic strain, where the heating of the material caused by its deformation
significantly influences temperature-dependent material properties. The generated heat is treated as a
volumetric heat flux source term in the heat balance equation.
An inelastic heat fraction can be specified for materials with plastic behavior that use the Mises
or Hill yield surface (“Inelastic behavior,” Section 23.1.1). It cannot be used with the combined
isotropic/kinematic hardening model. The inelastic heat fraction can be specified for user-defined
material behavior in Abaqus/Explicit and will be multiplied by the inelastic energy dissipation coded in
the user subroutine to obtain the heat flux. In Abaqus/Standard the inelastic heat fraction cannot be used
with user-defined material behavior; in this case the heat flux that must be added to the thermal energy
balance is computed directly in the user subroutine.
In Abaqus/Standard an inelastic heat fraction can also be specified for hyperelastic material
definitions that include time-domain viscoelasticity (“Time domain viscoelasticity,” Section 22.7.1).
The default value of the inelastic heat fraction is 0.9. If you do not include the inelastic heat fraction
behavior in the material definition, the heat generated by inelastic deformation is not included in the
analysis.
Input File Usage:
*INELASTIC HEAT FRACTION
Abaqus/CAE Usage:
Property module: material editor: Thermal: Inelastic Heat Fraction:
Fraction:
6.5.3–12
Abaqus Version 5.8 ID:
Printed on:
COUPLED THERMAL-STRESS ANALYSIS
Elements
Coupled temperature-displacement elements that have both displacements and temperatures as
nodal variables are available in both Abaqus/Standard and Abaqus/Explicit (see “Choosing the
appropriate element for an analysis type,” Section 27.1.3). In Abaqus/Standard simultaneous
temperature/displacement solution requires the use of such elements; pure displacement elements can be
used in part of the model in the fully coupled thermal-stress procedure, but pure heat transfer elements
cannot be used. In Abaqus/Explicit any of the available elements, except Eulerian elements, can be
used in the fully coupled thermal-stress procedure; however, the thermal solution will be obtained only
at nodes where the temperature degree of freedom has been activated (i.e., at nodes attached to coupled
temperature-displacement elements).
The first-order coupled temperature-displacement elements in Abaqus use a constant temperature
over the element to calculate thermal expansion. The second-order coupled temperature-displacement
elements in Abaqus/Standard use a lower-order interpolation for temperature than for displacement
(parabolic variation of displacements and linear variation of temperature) to obtain a compatible
variation of thermal and mechanical strain.
Output
See “Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable
identifiers,” Section 4.2.2, for a complete list of output variables. The types of output available are
described in “Output,” Section 4.1.1.
Input file template
*HEADING
…
** Specify the coupled temperature-displacement element type
*ELEMENT, TYPE=CPS4T
…
**
*STEP
*COUPLED TEMPERATURE-DISPLACEMENT or
*DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT
Data line to define incrementation
*BOUNDARY
Data lines to define nonzero boundary conditions on displacement or
temperature degrees of freedom
*CFLUX and/or *CFILM and/or
*CRADIATE and/or *DFLUX and/or
*DSFLUX and/or *FILM and/or
*SFILM and/or *RADIATE and/or
*SRADIATE
6.5.3–13
Abaqus Version 5.8 ID:
Printed on:
COUPLED THERMAL-STRESS ANALYSIS
Data lines to define thermal loads
*CLOAD and/or *DLOAD and/or *DSLOAD
Data lines to define mechanical loads
*FIELD
Data lines to define field variable values
*END STEP
6.5.3–14
Abaqus Version 5.8 ID:
Printed on:
ADIABATIC ANALYSIS
6.5.4
ADIABATIC ANALYSIS
Products: Abaqus/Standard
Abaqus/Explicit
Abaqus/CAE
References
•
•
•
•
•
•
•
•
•
“Defining an analysis,” Section 6.1.2
“Heat transfer analysis procedures: overview,” Section 6.5.1
*DYNAMIC
*STATIC
*DENSITY
*INELASTIC HEAT FRACTION
*SPECIFIC HEAT
“Configuring general analysis procedures,” Section 14.11.1 of the Abaqus/CAE User’s Manual, in
the online HTML version of this manual
“Defining thermal material models,” Section 12.10 of the Abaqus/CAE User’s Manual, in the online
HTML version of this manual
Overview
An adiabatic stress analysis:
•
•
•
•
•
•
is used in cases where mechanical deformation causes heating but the event is so rapid that this heat
has no time to diffuse through the material—for example, a very high-speed forming process;
can be conducted as part of a dynamic analysis (“Implicit dynamic analysis using direct integration,”
Section 6.3.2, or “Explicit dynamic analysis,” Section 6.3.3) or as part of a static analysis (“Static
stress analysis,” Section 6.2.2);
in Abaqus/Standard is available only for the isotropic hardening metal plasticity models with a
Mises yield surface (“Classical metal plasticity,” Section 23.2.1);
in Abaqus/Explicit is relevant only for the metal plasticity models (including both Mises and Hill
yield surfaces);
can be conducted if parts of the model are elastic only—no change in temperature occurs in the
elastic regions; and
requires that a material’s density, specific heat, and inelastic heat fraction (fraction of inelastic
dissipation rate that appears as heat flux) be specified.
Adiabatic analysis
Adiabatic thermal-stress analysis is typically used to simulate high-speed manufacturing processes
involving large amounts of inelastic strain, where the heating of the material caused by its deformation
is an important effect because of temperature-dependent material properties. The temperature increase
6.5.4–1
Abaqus Version 5.8 ID:
Printed on:
ADIABATIC ANALYSIS
is calculated directly at the material integration points according to the adiabatic thermal energy
increases caused by inelastic deformation; temperature is not a degree of freedom in the problem. No
allowance is made for conduction of heat in an adiabatic analysis. For problems where both inelastic
heating and conduction of the heat are important, a fully coupled temperature-displacement analysis
must be performed (“Fully coupled thermal-stress analysis,” Section 6.5.3).
In an adiabatic analysis plastic straining gives rise to a heat flux per unit volume of
where
is the heat flux that is added into the thermal energy balance, is the user-specified inelastic
heat fraction (assumed constant; discussed below), is the stress, and
is the rate of plastic straining.
The heat equation solved at each integration point is
where is the material density and
heat,” Section 26.2.3).
is the specific heat (see “Density,” Section 21.2.1, and “Specific
Input File Usage:
Use any of the following procedures to perform an adiabatic analysis:
Abaqus/CAE Usage:
*DYNAMIC, ADIABATIC
*DYNAMIC, EXPLICIT, ADIABATIC
*STATIC, ADIABATIC
Use any of the following procedures to perform an adiabatic analysis:
Step module:
Create Step: Dynamic, Implicit: Basic: Include adiabatic heating effects
Create Step: Dynamic, Explicit: Basic: Include adiabatic heating effects
Create Step: Static, General: Basic: Include adiabatic heating effects
Subsequent thermal diffusion analysis in Abaqus/Standard
In Abaqus/Standard thermal diffusion analysis can be performed after the adiabatic calculation (for
example, to study the cool-down of a component after sudden deformation). In this case the temperatures
at the end of the adiabatic analysis must be written to the Abaqus/Standard results file as element
variables averaged at the nodes. Since temperature values in an adiabatic analysis can be written to
the results file as element quantities only by using the TEMP output variable identifier, they cannot
be read directly into a subsequent thermal diffusion analysis as initial conditions. However, if you
postprocess the results file to produce a second results file in which the temperature data are provided
as nodal quantities, a subsequent heat transfer analysis can be performed with these temperatures as
initial conditions. See “Predefined fields,” Section 33.6.1, and “Accessing the results file information,”
Section 5.1.3, for details. Alternatively, you could postprocess the results file to produce a data list
containing data pairs consisting of nodes and temperatures.
The temperatures, NT, obtained from the heat transfer analysis can then be used to drive a
continuation of the previous stress analysis. This stress analysis should be restarted from the end of the
adiabatic analysis and will provide the response to the change of the temperature field obtained during
6.5.4–2
Abaqus Version 5.8 ID:
Printed on:
ADIABATIC ANALYSIS
the heat transfer analysis. In this case Abaqus/Standard will automatically read the temperatures from
the results file that was obtained from the heat transfer analysis and apply them in the restarted analysis.
Example
The following input options could be used to perform a heat transfer analysis using the temperatures
from an adiabatic analysis and then continue the stress analysis:
**Static adiabatic analysis
…
*STEP
*STATIC, ADIABATIC
…
**Write the temperatures to the results file as element
**variables averaged at the nodes
*EL FILE, POSITION=AVERAGED AT NODES
TEMP
*END STEP
**Heat transfer analysis using the temperatures from the
**static analysis as initial conditions
…
*INITIAL CONDITIONS, TYPE=TEMPERATURE, FILE=new results file,
STEP=step, INC=increment
*STEP
*HEAT TRANSFER
…
*NODE FILE
NT
*END STEP
**Restart from the adiabatic analysis using temperatures
**obtained from the heat transfer analysis
*RESTART, WRITE, READ, STEP=k, INC=i, END STEP
…
*STEP
*STATIC
…
*TEMPERATURE, FILE=heat_transfer_results_file
…
*END STEP
Fully coupled temperature-displacement analysis
If the continuation of the analysis into thermal diffusion requires a fully coupled temperaturedisplacement analysis (see “Fully coupled thermal-stress analysis,” Section 6.5.3), the simplest (but
6.5.4–3
Abaqus Version 5.8 ID:
Printed on:
ADIABATIC ANALYSIS
more expensive) approach is to use coupled temperature-displacement elements throughout the
adiabatic analysis. At the end of the static or the dynamic adiabatic calculations, the temperatures
must be written to the results file as element variables averaged at the nodes. In addition, you must
constrain all temperature degrees of freedom since they are not used in the adiabatic analysis. The
adiabatic analysis can then be restarted to apply the correct temperature distribution obtained from the
adiabatic analysis to the temperature degree of freedom of each node in the model. To create the input
for the boundary conditions, you must postprocess the results file obtained from the adiabatic analysis
and extract the value of TEMP at each node in the model (see “Accessing the results file information,”
Section 5.1.3). The temperature boundary conditions can be released as needed in subsequent coupled
temperature-displacement analysis steps.
Example
The following input options could be used to perform a coupled temperature-displacement analysis using
the temperatures from an adiabatic analysis:
**Static adiabatic analysis, coupled temperature-displacement
**plane stress elements
…
*ELEMENT, TYPE=CPS4T, ELSET=EALL
…
*BOUNDARY
nodes, 11, 11, 0.0
*STEP
*STATIC, ADIABATIC
…
**Write the temperatures to the results file as element
**variables averaged at the nodes
*EL FILE, POSITION=AVERAGED AT NODES
TEMP
*END STEP
**Restart from the adiabatic analysis
*RESTART, WRITE, READ, STEP=k, INC=i, END STEP
…
*STEP
*STATIC
**Dummy step to associate the temperature variable TEMP with
**the temperature degree of freedom at each node
1.0, 1.0
…
*BOUNDARY, OP=NEW
node, 11, 11, temperature
…
6.5.4–4
Abaqus Version 5.8 ID:
Printed on:
ADIABATIC ANALYSIS
*END STEP
**Coupled temperature displacement run for cool down of
**structure: continuation of the restart analysis
…
*STEP
*COUPLED TEMPERATURE-DISPLACEMENT
0.1, 1.0
…
*BOUNDARY, OP=NEW
**no temperature boundary condition specified
*END STEP
Initial conditions
Initial temperatures can be prescribed at nodes as initial conditions. Initial values of stresses, field
variables, solution-dependent state variables, etc. can also be specified (see “Initial conditions in
Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1).
Boundary conditions
Boundary conditions can be applied to displacement degrees of freedom in an adiabatic analysis in the
same way that they are applied in nonadiabatic dynamic, explicit dynamic, or static analysis steps (see
“Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1). Temperature is not a
degree of freedom in an adiabatic analysis.
Loads
The loading options available for an adiabatic analysis are the same as those available for nonadiabatic
dynamic, explicit dynamic, or static analysis steps (see “Applying loads: overview,” Section 33.4.1).
The following types of mechanical loads can be prescribed:
•
Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6); see
“Concentrated loads,” Section 33.4.2.
•
Distributed pressure forces or body forces can be applied; see “Distributed loads,” Section 33.4.3.
The distributed load types available with particular elements are described in Part VI, “Elements.”
Predefined fields
Predefined temperature fields cannot be used during an adiabatic analysis step.
The values of user-defined field variables can be specified; these values affect only field-variabledependent material properties, if any. See “Predefined fields,” Section 33.6.1.
6.5.4–5
Abaqus Version 5.8 ID:
Printed on:
ADIABATIC ANALYSIS
Material options
In Abaqus/Standard only Mises plasticity with isotropic elasticity and isotropic hardening (“Inelastic
behavior,” Section 23.1.1) is allowed in adiabatic stress analysis. Kinematic or combined hardening
is not available, but rate effects can be included. However, portions of the model can include only
elastic material; no change in temperature occurs in the elastic regions, since there is no source of heat
generation. In Abaqus/Explicit both Mises and Hill plasticity are allowed in adiabatic stress analysis.
You must specify the density, the inelastic heat fraction, and the specific heat as part of the material
definition for the material in which heat will be generated by plastic dissipation. You can also specify
latent heat if necessary (“Latent heat,” Section 26.2.4).
The inelastic heat fraction is the amount of inelastic dissipation used to calculate the increase in
temperature. The default value of the inelastic heat fraction is 0.9. If the inelastic heat fraction is not
included in the material definition, the heat generated by inelastic deformation is not included in the
analysis.
In Abaqus/Standard adiabatic analyses can also be carried out with user subroutine UMAT. In this
case the temperature must be defined as a solution-dependent state variable, and all coupling terms must
be included in the user subroutine. If conductivity (“Conductivity,” Section 26.2.2) is defined for the
material, it will be ignored during adiabatic analysis steps.
Input File Usage:
All of the following options must be included in the material definition:
*DENSITY
*INELASTIC HEAT FRACTION
*SPECIFIC HEAT
The following option can be included if latent heat effects are important:
Abaqus/CAE Usage:
*LATENT HEAT
All of the following must be included in the material definition:
Property module:
Material editor: General→Density
Material editor: Thermal→Inelastic Heat Fraction
Material editor: Thermal→Specific Heat
The following can be included if latent heat effects are important:
Property module: material editor: Thermal→Latent Heat
Temperature-dependent material properties
Material properties can be temperature dependent. Since the only source of temperature change in
adiabatic analysis is inelastic deformation, the temperature can only rise. This temperature rise may
cause thermal expansion (usually a small effect) and localization of the deformation if the flow stress is
reduced by the temperature rise. Since the adiabatic assumption applies only in rapid events and inelastic
deformation usually causes significant temperature rises only if the deformation is substantial, the strain
rates are often large in adiabatic analysis. The softening of the material caused by the temperature rise
6.5.4–6
Abaqus Version 5.8 ID:
Printed on:
ADIABATIC ANALYSIS
may, thus, be offset somewhat by strengthening associated with rate dependence if the material is rate
sensitive.
Elements
Any of the stress/displacement or coupled temperature-displacement elements in Abaqus can be used in
an adiabatic analysis (see “Choosing the appropriate element for an analysis type,” Section 27.1.3). Mass
or spring elements will not contribute to the heating of the material since they cannot generate plastic
strains.
If coupled temperature-displacement elements are used in an adiabatic analysis, the temperature
degrees of freedom will be ignored.
Output
Since temperatures are updated at the material calculation points, output of temperature is available with
output variable TEMP, not with output variable NT.
The element output available for an adiabatic analysis includes stress; strain; energies; the values
of state, field, and user-defined variables; and composite failure measures. The nodal output available
includes displacements, reaction forces, and coordinates. All of the output variable identifiers are
outlined in “Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output
variable identifiers,” Section 4.2.2.
Input file template
*HEADING
…
*MATERIAL, NAME=name
*ELASTIC, TYPE=ISOTROPIC
Data lines to define isotropic linear elasticity
*PLASTIC
Data lines to define metal plasticity
*DENSITY
Data lines to define density
*INELASTIC HEAT FRACTION
Data line to define inelastic heat fraction
*SPECIFIC HEAT
Data lines to define specific heat
…
*BOUNDARY
Data lines to specify zero-valued boundary conditions
*INITIAL CONDITIONS, TYPE=type
Data lines to specify initial conditions
*AMPLITUDE, NAME=name
Data lines to define amplitude variations
**
6.5.4–7
Abaqus Version 5.8 ID:
Printed on:
ADIABATIC ANALYSIS
*STEP, NLGEOM
The NLGEOM parameter is used in Abaqus/Standard to include geometric nonlinearity
*DYNAMIC, ADIABATIC or *DYNAMIC, EXPLICIT, ADIABATIC or
*STATIC, ADIABATIC
Data line to control time incrementation or to specify the time period of the step
*BOUNDARY, AMPLITUDE=name
Data lines to describe nonzero or zero-valued boundary conditions
*CLOAD and/or *DLOAD and/or *DSLOAD
Data lines to specify loads
*FIELD
Data lines to specify field variable values
*END STEP
6.5.4–8
Abaqus Version 5.8 ID:
Printed on:
FLUID DYNAMIC ANALYSIS
6.6
Fluid dynamic analysis
•
•
“Fluid dynamic analysis procedures: overview,” Section 6.6.1
“Incompressible fluid dynamic analysis,” Section 6.6.2
6.6–1
Abaqus Version 5.8 ID:
Printed on:
FLUID DYNAMIC ANALYSIS
6.6.1
FLUID DYNAMIC ANALYSIS PROCEDURES: OVERVIEW
Overview
Abaqus/CFD provides advanced computational fluid dynamics capabilities with extensive support for
preprocessing and postprocessing provided in Abaqus/CAE. These scalable parallel CFD simulation
capabilities address a broad range of nonlinear coupled fluid-thermal and fluid-structural problems.
Abaqus/CFD can solve the following types of incompressible flow problems:
•
Laminar and turbulent: Internal or external flows that are steady-state or transient, span a broad
Reynolds number range, and involve complex geometry may be simulated with Abaqus/CFD. This
includes flow problems induced by spatially varying distributed body forces.
•
Thermal convective: Problems that involve heat transfer and require an energy equation and that
may involve buoyancy-driven flows (i.e., natural convection) can also be solved with Abaqus/CFD.
This type of problem includes turbulent heat transfer for a broad range of Prandtl numbers.
•
Deforming-mesh ALE: Abaqus/CFD includes the ability to perform deforming-mesh analyses
using an arbitrary Lagrangian-Eulerian (ALE) description of the equations of motion, heat transfer,
and turbulent transport. Deforming-mesh problems may include prescribed boundary motion that
induces fluid flow or FSI problems where the boundary motion is relatively independent of the fluid
flow.
For more details, see “Incompressible fluid dynamic analysis,” Section 6.6.2.
Activation of fields in Abaqus/CFD
In Abaqus/CFD the active fields (degrees of freedom) are determined by the analysis procedure and the
options specified, such as turbulence models and auxiliary transport equations. For example, using the
energy equation in conjunction with the incompressible flow procedure activates the velocity, pressure,
and temperature degrees of freedom. For a complete listing of the available degrees of freedom, see
“Active degrees of freedom” in “Boundary conditions in Abaqus/CFD,” Section 33.3.2.
6.6.1–1
Abaqus Version 5.8 ID:
Printed on:
INCOMPRESSIBLE FLUID DYNAMICS
6.6.2
INCOMPRESSIBLE FLUID DYNAMIC ANALYSIS
Products: Abaqus/CFD
Abaqus/CAE
References
•
•
“Defining an analysis,” Section 6.1.2
“Fluid dynamic analysis procedures: overview,” Section 6.6.1
Overview
An incompressible fluid dynamics analysis:
•
•
•
•
•
•
•
is one where the velocity field is divergence-free and the pressure does not contain a thermodynamic
component;
is one where the energy contained in acoustic waves is small relative to the energy transported by
advection (i.e., when the Mach number is in the range
);
can be either laminar or turbulent, steady or time-dependent;
can be used to study either internal or external flows;
can include energy transport and buoyancy forces;
can be used with a deforming mesh for ALE calculations; and
can be performed with conjugate heat transfer or fluid-structure interaction.
Incompressible fluid dynamic analysis
Incompressible flow is one of the most frequently encountered flow regimes encompassing a diverse set
of problems that include: atmospheric dispersal, food processing, aerodynamic design of automobiles,
biomedical flows, electronics cooling, and manufacturing processes such as chemical vapor deposition,
mold filling, and casting.
Input File Usage:
Abaqus/CAE Usage:
*CFD, INCOMPRESSIBLE NAVIER STOKES
Step module: Create Step: General: Flow; Flow type: Incompressible
Governing equations
The momentum equations in integral form for an arbitrary control volume can be written as
where
is an arbitrary control volume with surface area ,
is the outward normal to ,
6.6.2–1
Abaqus Version 5.8 ID:
Printed on:
INCOMPRESSIBLE FLUID DYNAMICS
is the fluid density,
is the pressure,
is the velocity vector,
is the velocity of the moving mesh,
is the body force, and
is the viscous shear stress.
The viscous shear stress, , is also referred to as the deviatoric stress,
information, see “Viscosity,” Section 26.1.4.
Incompressibility requires a solenoidal velocity field expressed by
, where
. For more
Numerical implementation
The solution of the incompressible Navier-Stokes equations poses a number of algorithmic issues
due to the divergence-free velocity condition and the concomitant spatial and temporal resolution
required to achieve solutions in complex geometries for engineering applications. The Abaqus/CFD
incompressible solver uses a hybrid discretization built on the integral conservation statements for
an arbitrary deforming domain. For time-dependent problems, an advanced second-order projection
method is used with a node-centered finite-element discretization for the pressure. This hybrid approach
guarantees accurate solutions and eliminates the possibility of spurious pressure modes while retaining
the local conservation properties associated with traditional finite volume methods. An edge-based
implementation is used for all transport equations permitting a single implementation that spans a broad
variety of element topologies ranging from simple tetrahedral and hexahedral elements to arbitrary
polyhedral. In Abaqus/CFD tetrahedral, wedge, and hexahedral elements are supported.
Projection method
The basic concept for projection methods is the legitimate segregation of pressure and velocity fields for
efficient solution of the incompressible Navier-Stokes equations. Over the past two decades, projection
methods have found broad application for problems involving laminar and turbulent fluid dynamics,
large density variations, chemical reactions, free surfaces, mold filling, and non-Newtonian behavior.
In practice, the projection is used to remove the part of the velocity field that is not divergencefree (“div-free”). The projection is achieved by splitting the velocity field into div-free and curl-free
components using a Helmholtz decomposition. The projection operators are constructed so that they
satisfy prescribed boundary conditions and are norm-reducing, resulting in a robust solution algorithm
for incompressible flows.
Least-squares gradient estimation
The solution methods in Abaqus/CFD use a linearly complete second-order accurate least-squares
gradient estimation. This permits accurate evaluation of dual-edge fluxes for both advective and
6.6.2–2
Abaqus Version 5.8 ID:
Printed on:
INCOMPRESSIBLE FLUID DYNAMICS
diffusive processes. All transport equations in Abaqus/CFD make use of the second-order least-squares
operators.
Advection methods
The advection treatment in Abaqus/CFD is edge-based, monotonicity-preserving, and preserves
smooth variations to second order in space. The advection algorithm relies on a least-squares gradient
estimation with unstructured-grid slope limiters that are topology independent. Sharp gradients are
captured within approximately 2–3 elements; i.e.,
, and the use of slope limiting in conjunction
with a local diffusive limiter precludes over-/under-shoots in advected fields. The advection terms in
the momentum and transport equations can be treated either explicitly or implicitly (see the discussion
in “Time incrementation” below).
Energy equation
The energy transport equation is optionally activated in Abaqus/CFD for non-isothermal flows. For
small density variations, the Boussinesq approximation provides the coupling between momentum and
energy equations. In turbulent flows, the energy transport includes a turbulent heat flux based on the
turbulent eddy viscosity and turbulent Prandtl number. Abaqus/CFD provides a temperature-based
energy equation.
The energy equation, in temperature form, can be obtained from the first law of thermodynamics
and is given by
where
is the constant pressure specific heat, is the temperature, is heat flux due to conduction
defined by Fourier’s law, and is the heat supplied externally into the body per unit volume. The energy
equation is solved in terms of temperature in Abaqus/CFD.
Input File Usage:
Use the following option to specify an isothermal flow problem (default):
*CFD, ENERGY EQUATION=NO ENERGY
Use the following option to specify a thermal (heat) transport problem with
temperature as the primary transport scalar variable:
Abaqus/CAE Usage:
*CFD, ENERGY EQUATION=TEMPERATURE
Use the following option to specify an isothermal flow problem:
Step module: Create Step: General: Flow; Basic tabbed
page: Energy equation: None
Use the following option to specify a thermal (heat) transport problem with
temperature as the primary transport scalar variable:
Step module: Create Step: General: Flow; Basic tabbed page:
Energy equation: Temperature
6.6.2–3
Abaqus Version 5.8 ID:
Printed on:
INCOMPRESSIBLE FLUID DYNAMICS
Turbulence models
Turbulence modeling is a pacing technology for computational fluid dynamics. There is no single
universal turbulence model that can adequately handle all possible flow conditions and geometrical
configurations. This is complicated by the plethora of turbulence models and modeling approaches that
are currently available; e.g., Reynolds Averaged Navier-Stokes (RANS), Unsteady Reynolds Averaged
Navier-Stokes (URANS), Large-Eddy Simulation (LES), Implicit Large-Eddy Simulation (ILES), and
hybrid RANS/LES (HRLES). Ultimately, you must ensure that the approximations made in a given
turbulence model are consistent with the physical problem being modeled.
The following turbulent flow models are available: ILES, Spalart-Allmaras (SA), and RNG k– .
These models span a relatively broad set of flow problems that include time-dependent flows, fluidstructure interaction (FSI), and conjugate heat transfer (CHT).
Implicit Large-Eddy Simulation (ILES)
Large-eddy simulation relies on a segregation of length and time scales in turbulent flows and a
modeling approach that permits the direct simulation of grid-resolved flow structures and the modeling
of unresolved subgrid features. Implicit LES is a methodology for modeling high Reynolds number
flows that combines computational efficiency and ease of implementation with predictive calculations
and flexible application. In Abaqus/CFD ILES relies on the discrete monotonicity-preserving form
of the advective operator to implicitly define the subgrid-scale model. This model is inherently
time-dependent requiring time-accurate solutions to the incompressible Navier-Stokes equations where
the time scale is approximately that of an eddy-turnover time for resolve-scale flow features. In addition,
this model must be run in full three dimensions, which typically imposes larger grid densities and
stringent grid resolution criteria relative to more traditional steady-state RANS simulations. However,
this approach is extremely flexible and can be applied to a broad range of flows and FSI problems.
There are no user settings required for ILES.
Input File Usage:
Use the *CFD option without the *TURBULENCE MODEL option.
Abaqus/CAE Usage:
Step module: Create Step: General: Flow; Turbulence tabbed page: None
Spalart-Allmaras (SA) turbulence model
The Spalart-Allmaras (SA) model is a one-equation turbulence model that uses an eddy-viscosity
variable with a nonlinear transport equation. The model was developed based on empiricism,
dimensional analysis, and a requirement for Galilean invariance. The model has found broad use and
has been calibrated for two-dimensional mixing layers, wakes, and flat-plate boundary layers. The
model produces reasonably accurate predictions of turbulent flows in the presence of adverse pressure
gradients and may be used for flows where separation occurs. This model is spatially local and requires
only moderate resolution in boundary layers. Although initially designed for external and free-shear
flows, the Spalart-Allmaras model can also be used for internal flows.
The basic form of the one-equation Spalart-Allmaras model consists of one transport equation
for the turbulent eddy viscosity, . The model requires the normal distance from the wall used in the
damping functions needed to control the turbulent viscosity in the near-wall region. Abaqus/CFD
6.6.2–4
Abaqus Version 5.8 ID:
Printed on:
INCOMPRESSIBLE FLUID DYNAMICS
automatically computes the normal distance function, permitting simple specification of the model
boundary conditions. The turbulent viscosity transport equation for the Spalart-Allmaras model is given
by
where the damping functions and model coefficients are defined as:
where
is the normal distance from the wall, and the effective turbulent viscosity is defined as
6.6.2–5
Abaqus Version 5.8 ID:
Printed on:
INCOMPRESSIBLE FLUID DYNAMICS
The Spalart-Allmaras model coefficients are shown in Table 6.6.2–1. In addition, a turbulent Prandtl
number (
) can be specified.
Table 6.6.2–1
0.1355
0.622
7.1
Spalart-Allmaras model coefficients.
0.6667
0.3
2
0.41
5
The Spalart-Allmaras model can provide very accurate boundary layer results if the near-wall
region is resolved (near-wall resolution such that the nondimensional wall distance is approximately 3).
However, the implementation of boundary conditions for the Spalart-Allmaras model in Abaqus/CFD
permits the use of coarser meshes as well.
Input File Usage:
Abaqus/CAE Usage:
Use both of the following options:
*CFD
*TURBULENCE MODEL, TYPE=SPALART ALLMARAS
Step module: Create Step: General: Flow; Turbulence
tabbed page: Spalart-Allmaras
RNG k–epsilon turbulence model
The RNG k– model is a two-equation turbulence model that evolves an equation for the turbulent
kinetic energy, k, and the energy dissipation rate, . The model equations are developed from
fundamental physical principles and dimensional analysis. In general, the coefficients of the model
are usually calibrated using canonical flows and experimental data. However, the RNG version of the
model computes the coefficients using Renormalization Group theory (Yakhot et al., 1992). The model
equations are
where
6.6.2–6
Abaqus Version 5.8 ID:
Printed on:
INCOMPRESSIBLE FLUID DYNAMICS
the turbulent viscosity
is
and
The second and third terms on the right-hand-side of the k– transport equations above represent the
production and dissipation of k and , respectively.
The RNG k– model coefficients are shown in Table 6.6.2–2. In addition, a turbulent Prandtl number
(
) can be specified.
Table 6.6.2–2
0.085
Input File Usage:
Abaqus/CAE Usage:
1.42
1.68
RNG k– model coefficients.
0.72
0.72
0.012
4.38
Use both of the following options:
*CFD
*TURBULENCE MODEL, TYPE=RNG KEPSILON
Step module: Create Step: General: Flow; Turbulence tabbed
page: k-epsilon renormalization group (RNG)
Wall functions
It is well known that the k– model has limitations, especially on wall-bounded flows where high values
of eddy viscosity in the near-wall region are usually reproduced. For high Reynolds number flows often
encountered in many industrial applications, a full resolution of the thin viscous sub-layer that occurs
near a wall using a fine mesh may not be economical. Consequently, for meshes that cannot resolve the
viscous sub-layer, wall functions are used to represent the effects of the viscous sub-layer on the transport
6.6.2–7
Abaqus Version 5.8 ID:
Printed on:
INCOMPRESSIBLE FLUID DYNAMICS
processes. In Abaqus/CFD wall functions are used to avoid the need for highly resolved boundary layer
meshes. This approach relies on the law of the wall to obtain the wall shear stress.
The law of the wall is a universal velocity profile that wall-bounded flows develop in the absence
of pressure gradients. The law of the wall is
if
if
,
where
is the wall tangent velocity, is the kinematic viscosity, is the density,
is the shear stress at the
wall, and
and
are constants.
The standard law of the wall profile is limited in its usage. For example, in recirculating flows the
turbulent kinetic energy k becomes zero at separation and reattachment points, where, by definition, is
zero. This singular behavior causes the predicted results to be erroneous. To overcome this, the standard
law of the wall is modified based on a new scale for the friction velocity following the method proposed
by Launder and Spalding (1974). The modified friction velocity is given by
which does not suffer from a singular behavior at flow reattachment, separation, and at points of flow
impingement. Correspondingly, the wall distances are re-scaled as follows:
The modified law of the wall reduces to the standard law of the wall under the conditions of uniform
wall shear stress, and when the generation and dissipation of turbulent kinetic energy are in balance (i.e.,
when the turbulence structure is in equilibrium). Under such conditions,
and thus,
.
The wall shear stress for the modified law of the wall can be evaluated as (Albets-Chico, et al.,
2008)
if
if
6.6.2–8
Abaqus Version 5.8 ID:
Printed on:
,
INCOMPRESSIBLE FLUID DYNAMICS
where the subscript p denotes the wall element center at which all the quantities of interest are evaluated.
The use of the wall function requires the modification of the transport equations for k and for the wall
layer of elements. Specifically, the production and dissipation terms in the governing transport equation
for the turbulent kinetic energy k are modified to account for the presence of the wall.
Following the procedure outlined in (Craft et al., 2002), an average value of the production of k as
given below is used in the transport equation. Such an average is obtained based on a two-layer model
of the wall element (i.e., the wall element is divided into a partly viscous sub-layer region and a partly
turbulent log-layer or inertial layer region).
if
if
,
is the maximum of the wall normal distances of all the vertices of a given wall element, and
where
is the wall normal distance of the edge of the viscous sub-layer, where
Similarly, an average value of the dissipation rate for k is also prescribed for the wall elements based
on a two-layer integration and is given by
if
if
.
The transport equation for is not solved for the wall layer elements. Instead, the value of
directly prescribed at the point p as follows:
is
if
if
.
Therefore, integration of the k and transport equations is performed with a zero-flux (i.e., homogeneous
Neumann boundary conditions) at the walls.
Guidelines on wall functions
The main advantage of wall functions is the relaxed requirement on mesh resolution at walls. However,
the main disadvantage of using wall functions is the dependence on the near-wall mesh resolution. Wall
functions based on the law of the wall approach usually work best for wall elements whose centers lie
in the fully turbulent layer (inertial or log layer) for which such functions are designed. This effectively
imposes a lower limit on the value of the scaled wall coordinate, . For complex geometries, ensuring
that all the near wall cells are outside the viscous sublayer is difficult. The precise location of the
logarithmic region is solution dependent and may vary with time. To accommodate a more flexible
mesh, a resolution-insensitive wall function (Durbin, 2009) has been implemented. Briefly, this wall
6.6.2–9
Abaqus Version 5.8 ID:
Printed on:
INCOMPRESSIBLE FLUID DYNAMICS
function is based on limiting the minimum value of
such that the value of the velocity gradient at
the first wall-attached element is the same as if it was located on the edge of the viscous sub-layer. A
best practice for wall-bounded flows is to have at least 8–10 points in the boundary layer region where
(see Casey and Wintergerste, 2000).
Deforming-mesh ALE
Many industrial CFD/FSI/CHT problems involve moving boundaries or deforming geometries. This
class of problem includes prescribed boundary motion that induces fluid flow or where the boundary
motion is relatively independent of the fluid flow. Abaqus/CFD uses an arbitrary Lagrangian-Eulerian
(ALE) formulation and automated mesh deformation method that preserves element size in boundary
layers. The ALE and deforming-mesh algorithms are activated automatically for problems that involve
a moving boundary prescribed by the user or identified as a moving boundary in an FSI co-simulation.
Abaqus/CFD offers distortion control to prevent elements from inverting or distorting excessively in
fluid mesh movement (see “Controlling the solution accuracy in an Abaqus/CFD to Abaqus/Standard or
to Abaqus/Explicit co-simulation” in “Commonly used control parameters,” Section 7.2.2).
To properly control the mesh motion during a simulation, it is the user’s responsibility to prescribe
appropriate displacement boundary conditions on the computational mesh.
Porous media flows
Flows through fluid-saturated porous media occur in a wide range of industrial and environmental
applications. Such flows can be isothermal (no heat transfer) or non-isothermal in nature. Examples
include packed-bed heat exchangers, heat pipes, thermal insulation, petroleum reservoirs, nuclear waste
repositories, geothermal engineering, thermal management of electronic devices, metal alloy casting,
and flow past porous scaffolds in bioreactors.
Isothermal flows
For isothermal flows in porous media, many studies are usually carried out using the Darcy flow model,
which is an empirical law for creeping flow through an infinitely extended uniform medium. However,
non-Darcian effects such as fluid inertial effects are quite important for certain applications. The model
implemented in Abaqus/CFD is based on the volume-averaged Darcy-Brinkman-Forchheimer equations
that account for both Darcian and inertial non-Darcian effects. The following assumptions are made in
deriving the governing equations:
•
the porosity of the medium does not vary with time or the time scale of variation of the porosity is
considered to be much larger than the dominant time scales of the fluid motion; and
•
the permeability of the porous medium is isotropic and dependent only on the porosity of the
medium.
Based on the above assumptions, the volume-averaged mass conservation and the Darcy-BrinkmanForchheimer momentum equations governing the flow of an incompressible fluid in a fluid-saturated
porous media can be written as follows (Nield and Bejan, 2010):
6.6.2–10
Abaqus Version 5.8 ID:
Printed on:
INCOMPRESSIBLE FLUID DYNAMICS
where
is the extrinsic average or the superficial velocity vector, where the average is taken over a
representative volume incorporating both the solid (matrix) and the fluid phases;
is the intrinsic average of the pressure (average taken only over the fluid-phase);
is the density of the fluid;
is the viscosity of the fluid;
is the porosity (volume fraction of the fluid phase) of the porous medium; and
is the permeability of the porous medium.
The second term on the right-hand side of the momentum equation is the Brinkman term accounting for
the presence of solid boundaries, the third term represents the Darcy drag term (linear in velocity), and the
last term represents the inertial (quadratic in velocity) or the Forchheimer drag. The parameter
is the
inertial drag coefficient (also referred to as the form drag coefficient). Based on Ergun’s equation (Nield
and Bejan, 2010),
, where is a constant that is set to a default value of
.
The porous drag forces (namely, the Darcy and Forchheimer drag forces) are activated for a prescribed
element set by specifying them as distributed loads (see “Specifying porous drag body force load in
Abaqus/CFD” in “Distributed loads,” Section 33.4.3).
Thus, the porous media flow problem requires the specification of the porosity, , and the
permeability, , of the porous medium. The default value of can also be changed in the material
property definition (see “Permeability,” Section 26.6.2). For the case of turbulent flow within a porous
medium, the fluid viscosity includes the contribution of both the molecular and the turbulent eddy
viscosities.
For conjugate flows involving domains consisting of both pure fluid regions and fluid-saturated
porous media, the pure fluid porosity is set to a value of 1 by default.
Permeability-Porosity relationships
The permeability of a porous medium is generally a function of the physical properties of the
interconnected pore system such as porosity and tortuosity. Determination of the appropriate
permeability-porosity relationship requires a detailed knowledge of the size distribution and spatial
arrangement of the pore channels in the porous medium. The permeability-porosity relation can be
specified directly in Abaqus/CFD using the material property definition.
Another permeability-porosity relation supported in Abaqus/CFD is the widely accepted CarmanKozeny model. This relation is given as follows:
6.6.2–11
Abaqus Version 5.8 ID:
Printed on:
INCOMPRESSIBLE FLUID DYNAMICS
where
represents the Carman-Kozeny constant and
particles/fibers.
represents the average radius of the porous
Limitations
•
•
While turbulence can be activated for a porous media flow problem, a rigorous volume-averaging
procedure has not been implemented in Abaqus/CFD to account for turbulence transport within
the porous media. The equations governing the transport of the turbulence variables are solved
by neglecting the effects of the presence of porous medium. In other words, the porous medium
remains transparent (fully open) to the transport of turbulence variables.
When the arbitrary Lagrangian-Eulerian (ALE) and deforming mesh algorithms are activated for a
porous flow problem, changes in the porosity of the medium associated with large mesh/domain
deformations are not taken into account. The model is strictly valid only for the case of
undeformable porous media.
Non-isothermal flows (heat transfer)
The following assumptions are made in the implementation of the volume-averaged energy equation for
porous media in Abaqus/CFD:
•
•
•
•
The medium is isotropic.
Radiative effects, viscous dissipation, and work done by the changes in pressure are negligible.
Local thermal equilibrium is valid (i.e., solid and fluid phase temperatures are the same).
No net heat transfer takes place between the different phases in the porous media.
Based on the above assumptions, the effective energy equation for the porous medium can be given as
follows (Nield and Bejan, 2010):
where
and
Here, is the extrinsic average or the superficial velocity vector, and is the temperature. The subscripts
, , and
denote the fluid phase, solid (matrix) phase, and effective medium, respectively.
is
the specific heat capacity at constant pressure, is the thermal conductivity, and
is the effective
heat production per unit volume or the heat source (
). For the case of turbulent
heat transfer within a porous medium, the fluid conductivity
includes the contribution of both the
molecular and turbulent eddy conductivities.
6.6.2–12
Abaqus Version 5.8 ID:
Printed on:
INCOMPRESSIBLE FLUID DYNAMICS
As seen from the above equation, the porous media heat transfer problem requires the specification
of the following input:
•
The thermal properties of the solid (matrix) phase: the density,
specific heat capacity,
; and
•
The thermal properties of the fluid (matrix) phase: the molecular conductivity, ; and specific heat
capacity,
, apart from the specification of other fluid properties such as the density, , viscosity,
, and permeability, .
; the conductivity,
; and the
Linear equation solvers
The solution methods for the momentum and auxiliary transport equations in Abaqus/CFD rely on
scalable parallel preconditioned Krylov solvers. The pressure, pressure-increment, and distance
function equations are solved with user-selectable Krylov solvers and a robust algebraic multigrid
preconditioner. A set of preselected default convergence criteria and iteration limits are prescribed for
all linear equation solvers. The default solver settings should provide computationally efficient and
robust solutions across a spectrum of CFD problems. However, full access to diagnostic information,
convergence criteria, and optional solvers is provided. In practice, the pressure-increment equation
may be the most sensitive linear system and could require user intervention based on knowledge of the
specific flow problem.
Input File Usage:
Use the following option to specify parameters for solving the momentum
transport equations:
*MOMENTUM EQUATION SOLVER
Use the following option to specify parameters for solving other transport
equations, such as the energy or turbulence transport equations:
*TRANSPORT EQUATION SOLVER
Use the following option to specify parameters for solving the pressure
equation:
*PRESSURE EQUATION SOLVER
Convergence criteria and diagnostics
Iterative solvers compute an approximate solution to a given set of equations; therefore, convergence
criteria are required to determine if the solution is acceptable. While default settings should be adequate
for most problems, you can modify the convergence criteria. In addition to the option of setting
convergence criteria, convergence history output is available that may be useful for some advanced
users to tune the solvers for performance or robustness. For the algebraic multigrid preconditioner,
diagnostic information such as the number of grids, grid sparsity, and largest eigenvalue and condition
number estimates are available upon request. The diagnostic information for the algebraic multigrid
preconditioner is printed every time the preconditioner is computed.
6.6.2–13
Abaqus Version 5.8 ID:
Printed on:
INCOMPRESSIBLE FLUID DYNAMICS
Specifying convergence criteria
The linear convergence limit (also commonly referred to as the convergence tolerance), the frequency
of convergence checking, and the maximum number of iterations can be set. The iterative solver will
stop when the relative residual norm of the system of equations and the relative correction of the solution
norm fall below the convergence limit.
Input File Usage:
Use the following options to specify convergence criteria for the momentum
and auxiliary transport equations:
*MOMENTUM EQUATION SOLVER
max iterations, frequency check, convergence limit
*TRANSPORT EQUATION SOLVER
max iterations, frequency check, convergence limit
*PRESSURE EQUATION SOLVER
max iterations, frequency check, convergence limit
Abaqus/CAE Usage:
Step module: Create Step: General: Flow; Solvers tabbed page:
Momentum Equation, Pressure Equation, or Transport Equation
tabbed page; enter values for Iteration limit, Convergence checking
frequency, and Linear convergence limit
Accessing convergence output
You can monitor the convergence of the iterative solver by accessing convergence output. When you
activate the convergence output, the current relative residual norm and the relative solution correction
norm are output each time the convergence is checked.
Input File Usage:
Use the following options to write convergence output to the log file for the
linear equation solvers:
*MOMENTUM EQUATION SOLVER, CONVERGENCE=ON
*TRANSPORT EQUATION SOLVER, CONVERGENCE=ON
*PRESSURE EQUATION SOLVER, CONVERGENCE=ON
Abaqus/CAE Usage:
Step module: Create Step: General: Flow; Solvers tabbed page:
Momentum Equation, Pressure Equation, or Transport Equation
tabbed page; toggle on Include convergence output
Accessing diagnostic information
Diagnostic output is useful only for the algebraic multigrid preconditioner. For other preconditioners,
only a solver initialization message is printed for diagnostic output. For the algebraic multigrid
preconditioner, the number of grids, grid sparsity, and largest eigenvalue and condition number
estimates are output each time the preconditioner is computed.
Input File Usage:
Use the following option to write diagnostic output to the log file for the
pressure equation solver using the algebraic multigrid preconditioner:
*PRESSURE EQUATION SOLVER, TYPE=AMG, DIAGNOSTICS=ON
6.6.2–14
Abaqus Version 5.8 ID:
Printed on:
INCOMPRESSIBLE FLUID DYNAMICS
Abaqus/CAE Usage:
Step module: Create Step: General: Flow; Solvers tabbed page: Pressure
Equation tabbed page; toggle on Include diagnostic output
Specifying a solver for the pressure equation
Three solver types are available for the solving the pressure equation. The default AMG solver uses
an algebraic multigrid preconditioner and offers the choice of three Krylov solvers: conjugate gradient,
bi-conjugate gradient stabilized, and flexible generalized minimal residual. The SSORCG solver uses a
symmetric successive over-relaxation preconditioner and conjugate gradient Krylov solver. The DSCG
solver uses a diagonally scaled preconditioner and conjugate gradient Krylov solver. The AMG solver
provides many additional options that are intended for advanced usage and in cases where convergence
difficulties are encountered.
Input File Usage:
Use one of the following options to specify the solver type:
Abaqus/CAE Usage:
*PRESSURE EQUATION SOLVER, TYPE=AMG (default)
*PRESSURE EQUATION SOLVER, TYPE=SSORCG
*PRESSURE EQUATION SOLVER, TYPE=DSCG
Use the following option to specify the AMG solver:
Step module: Create Step: General: Flow; Solvers tabbed page: Pressure
Equation tabbed page: Solver options: Use analysis defaults
Use the following option to specify the SSORCG solver:
Step module: Create Step: General: Flow; Solvers tabbed page: Pressure
Equation tabbed page: Solver options: Specify, Preconditioner
Type: Symmetric successive over-relaxation
The DSCG solver is not supported in Abaqus/CAE.
Specifying the complexity level
For the AMG solver, you can choose from three preset levels or you can specify the Krylov solver and
smoother settings directly. The presets are provided for convenience. Preset level 1 is primarily intended
for use with meshes with good element aspect ratios and in some cases may provide a performance
benefit over the default preset level 2. Preset level 3 is intended for problems that encounter convergence
difficulties, which typically have elements with high aspect ratios or highly distorted elements.
Input File Usage:
Preset level 1 corresponds to the following:
*PRESSURE EQUATION SOLVER, TYPE=AMG
250, 2, 10−5
CHEBYCHEV, 2, 2, CG
V
Preset level 2 (default) corresponds to the following:
*PRESSURE EQUATION SOLVER, TYPE=AMG
250, 2, 10−5
ICC, 1, 1, CG
6.6.2–15
Abaqus Version 5.8 ID:
Printed on:
INCOMPRESSIBLE FLUID DYNAMICS
V
Preset level 3 corresponds to the following:
*PRESSURE EQUATION SOLVER, TYPE=AMG
250, 2, 10−5
ICC, 2, 2, BCGS
V
Abaqus/CAE Usage:
Step module: Create Step: General: Flow; Solvers tabbed page:
Pressure Equation tabbed page: Solver options: Specify,
Preconditioner Type: Algebraic multi-grid
Use one of the following options to choose a preset complexity level:
Complexity Level: Preset: 1, 2, or 3
Use the following option to specify the Krylov solver and smoother settings
directly:
Complexity Level: User defined
Specifying the solver type
Three Krylov solver options are provided for the AMG solver. The default conjugate gradient solver is
the fastest; however, in some cases where convergence difficulties are observed, the bi-conjugate gradient
stabilized or flexible generalized minimal residual solvers are recommended. These two solvers are more
robust but computationally more expensive than the conjugate gradient solver.
Input File Usage:
Use the following option to specify the Krylov solver type:
*PRESSURE EQUATION SOLVER, TYPE=AMG
first data line
, , , solver type
where solver type is CG for the conjugate gradient solver (default), BCGS
for the bi-conjugate gradient squared solver, and FGMRES for the flexible
generalized minimum residual solver.
Abaqus/CAE Usage:
Step module: Create Step: General: Flow; Solvers tabbed page:
Pressure Equation tabbed page: Solver options: Specify,
Preconditioner Type: Algebraic multi-grid
Use one of the following options to specify the Krylov solver:
Solver Type: Conjugate gradient, Bi-conjugate gradient, stabilized,
or Flexible generalized minimal residual
Specifying the residual smoother settings
You can choose between incomplete factorization and polynomial residual smoothers that are used
within the AMG preconditioner. While incomplete factorization is computationally more expensive
than polynomial smoothing, in many cases this cost is amortized by fast convergence and robustness.
Polynomial smoothing is recommended for problems with a very good mesh quality (i.e., no skewed or
6.6.2–16
Abaqus Version 5.8 ID:
Printed on:
INCOMPRESSIBLE FLUID DYNAMICS
large aspect ratio elements). The number of pre- and post-smoothing sweeps can also be specified. It is
recommended that you apply the same number of pre- and post-sweeps. For the polynomial smoother,
a minimum of two pre- and post-sweeps are recommended.
Input File Usage:
Use the following option to specify the residual smoother settings:
*PRESSURE EQUATION SOLVER, TYPE=AMG
first data line
smoother, pre-smoothing sweeps, post-smoothing sweeps
Abaqus/CAE Usage:
Step module: Create Step: General: Flow; Solvers tabbed page: Pressure
Equation tabbed page: Solver options: Specify, Preconditioner Type:
Algebraic multi-grid, Residual Smoother: Incomplete factorization or
Polynomial, Pre-sweeps: select number, Post-sweeps: select number
Time incrementation
Abaqus/CFD uses second-order time-accurate integration by default, where all diffusive terms,
advective terms, and body forces are integrated with the trapezoidal rule (Crank-Nicolson method).
The default method is “second-order accurate” in that truncation errors within a time increment are
proportional to the time increment squared, thus they decrease by a factor of four if the time increment
is halved. You can individually select alternative time integrators for each of these terms. A fully
implicit advection treatment is also available, which is particularly useful for quickly advancing toward
steady-state solutions.
Time increment size control
By default, Abaqus/CFD uses an automatic time incrementation algorithm that continually adjusts the
time increment size to satisfy the Courant-Friedrichs-Lewy (CFL) stability condition for advection. The
default value, CFL=0.45, guarantees the solution’s stability. You can further limit the automatically
computed time increment size by specifying a maximum value. You can also specify an initial time
increment size. This value is automatically decreased as necessary to satisfy a maximum initial CFL
value of 0.45 based on the starting conditions of the flow.
Alternatively, you can select fixed time incrementation and specify the time increment size. In this
case the time increment size remains constant throughout the step, but stability is not guaranteed.
Input File Usage:
Use the following option to specify automatic time incrementation (default):
*CFD, INCREMENTATION=FIXED CFL
time increment, time period, scale factor, suggested CFL, check increment,
max allowable time increment
divergence tolerance, , , ,
Use the following option to specify fixed time step incrementation:
*CFD, INCREMENTATION=FIXED STEP SIZE
time increment, time period,
divergence tolerance, , , ,
6.6.2–17
Abaqus Version 5.8 ID:
Printed on:
INCOMPRESSIBLE FLUID DYNAMICS
For both options above, can be set to 0.5 for the Crank-Nicolson method
(default), 0.6667 for the Galerkin method, or 1 for the first-order backwardEuler method.
Abaqus/CAE Usage:
Use the following options to specify automatic time incrementation:
Step module: Create Step: General: Flow; Basic tabbed page:
enter a value for Time period; Incrementation tabbed page: Type:
Automatic (Fixed CFL); enter values for Initial time increment,
Maximum CFL number, Increment adjustment frequency, Time
step growth scale factor, Divergence tolerance
Use the following option to specify fixed time step incrementation:
Step module: Create Step: General: Flow; Basic tabbed page: enter a
value for Time period; Incrementation tabbed page: Type: Fixed, enter
values for Time increment and Divergence tolerance
Use the following options to specify the time integration method for
viscous/diffusive terms, boundary conditions, and advective terms:
Viscous, Load/Boundary condition, or Advective: Trapezoid
(1/2), Galerkin (2/3), or Backward-Euler (1)
Time-accurate analysis
The time integration parameters are all set by default to
, which produces a second order–accurate
semi-implicit method suitable for time-accurate transient analysis. When automatic time incrementation
is used, you should specify CFL
to maintain stability and time accuracy.
Steady-state analysis
In analyses where the goal is to reach a steady-state solution, the fully implicit (backward-Euler) method
can be activated by setting all time integration parameters to
. This method is unconditionally
stable, allowing you to specify large CFL values to significantly increase the time increment size. Strict
guidelines for selecting the maximum allowable CFL number are not available, and this maximum value
may vary for different flows and meshes. CFL values of 10 or more have been used successfully for
some analyses where only the final result is of interest.
Monitoring output variables
Abaqus/CFD provides a number of output variables that are useful for monitoring the health of a
calculation and are good indicators for situations where the flow has reached a steady-state condition.
These variables are written to the status (.sta) file and can be examined as the analysis job is executing.
The RMS divergence output variable is useful for determining if a calculation is proceeding normally.
Values of the RMS divergence output variable that are O(1) can indicate that the problem is incorrectly
specified or that the calculation has become unstable. The global kinetic energy (KE) provides a good
indicator for when the flow has reached a steady state; i.e., when the kinetic energy asymptotically
approaches a constant value, the flow is typically achieving a steady-state condition where the velocities
6.6.2–18
Abaqus Version 5.8 ID:
Printed on:
INCOMPRESSIBLE FLUID DYNAMICS
and pressure do not vary in time. Alternatively, the global kinetic energy can indicate a steady-periodic
or chaotic flow situation as well.
Initial conditions
Initial conditions for the density, velocity, temperature, turbulent eddy viscosity, turbulent kinetic energy,
and dissipation rate can be specified (see “Initial conditions in Abaqus/CFD,” Section 33.2.2). If the
density is omitted, the specified material density is used for incompressible flow simulations.
For a well-posed incompressible flow problem, the initial velocity must satisfy the boundary
conditions and also the imposed divergence-free condition; i.e., the solvability conditions. Abaqus/CFD
automatically uses the user-defined boundary conditions and tests the specified velocity initial conditions
to be sure the solvability conditions are satisfied. If they are not, the initial velocity is projected onto
a divergence-free subspace, yielding initial conditions that define a well-posed incompressible
Navier-Stokes problem. Therefore, in some circumstances, user-specified velocity initial conditions
may be overridden with velocity conditions that satisfy solvability.
Boundary conditions
Boundary conditions for velocity, temperature, pressure, and eddy viscosity can be defined (see
“Boundary conditions in Abaqus/CFD,” Section 33.3.2). During the analysis prescribed boundary
conditions can be varied using an amplitude definition (see “Amplitude curves,” Section 33.1.2). All
amplitude definitions except smooth step and solution-dependent amplitudes are available. By default,
all boundary conditions are applied instantaneously. Velocity and pressure boundary conditions can
be specified via user subroutines (see “SMACfdUserPressureBC,” Section 1.3.1 of the Abaqus User
Subroutines Reference Manual, and “SMACfdUserVelocityBC,” Section 1.3.2 of the Abaqus User
Subroutines Reference Manual).
Displacement and velocity boundary conditions at FSI interfaces are prescribed automatically
by the definition of a co-simulation region; therefore, you should not prescribe these conditions at an
FSI interface. Similarly, you should not define the temperature at a CHT interface; the temperature
is automatically prescribed by the definition of a co-simulation region. For more information, see
“Preparing an Abaqus analysis for co-simulation,” Section 17.2.1.
The specification of no-slip/no-penetration boundary conditions at walls requires the specification
of the turbulent eddy viscosity and normal-distance function, which is handled automatically by
Abaqus/CFD.
Hydrostatic pressure condition
In incompressible flows, the pressure is only known within an arbitrary additive constant value or the
hydrostatic pressure. In many practical situations, the pressure at an outflow boundary may be prescribed,
which, in effect, sets the hydrostatic pressure level. In cases where there is no pressure prescribed, it is
necessary to set the hydrostatic pressure level at a minimum of one node in the mesh.
The fluid reference pressure can be used to specify the hydrostatic pressure level. When there are
no prescribed pressure boundary conditions, the fluid reference pressure establishes the hydrostatic
pressure level and makes the pressure-increment equation non-singular. If pressure boundary conditions
6.6.2–19
Abaqus Version 5.8 ID:
Printed on:
INCOMPRESSIBLE FLUID DYNAMICS
are prescribed in addition to the reference pressure level, the reference pressure simply adjusts the
output pressures according to the specified pressure level. For more information, see “Specifying a fluid
reference pressure” in “Concentrated loads,” Section 33.4.2.
Loads
The loading types for Abaqus/CFD include applied heat flux, volumetric heat-generation sources,
general body forces, and gravity loading. Gravity loading defines the gravity vector used with a
Boussinesq-type body force in buoyancy driven flow (see “Specifying gravity loading” in “Distributed
loads,” Section 33.4.3). Gravity loading can be used only in conjunction with the energy equation and
will be ignored if used without the energy equation. During the analysis prescribed loads can be varied
using an amplitude definition (see “Amplitude curves,” Section 33.1.2). All amplitude definitions
except smooth step and solution-dependent amplitudes are available.
Material options
Material definitions in Abaqus/CFD follow the Abaqus conventions but also present several material
properties specific to fluid dynamics. In Abaqus/CFD the typical material properties include viscosity,
constant-pressure specific heat, density, and coefficient of thermal expansion. The thermal expansion is
used with a Boussinesq-type body force in buoyancy driven flow.
In contrast to Abaqus/Standard and Abaqus/Explicit, which use the constant-volume specific
heat, the constant-pressure specific heat is required when the energy equation is used for thermal-flow
problems. For problems involving an ideal gas, the user may optionally specify constant-volume
specific heat and the ideal gas constant.
Elements
Abaqus/CFD supports three element types: the 8-node hexahedral element, FC3D8; the 6-node triangular
prism element, FC3D6; and the 4-node tetrahedral element, FC3D4 (see “Fluid (continuum) elements,”
Section 28.2.1). These elements cannot be mixed in a single connected fluid domain. However, a single
flow model can contain multiple domains, each with a different element type.
Output
The output available from Abaqus/CFD for an incompressible fluid dynamic analysis includes both nodal
and surface field data and element and surface time-history data. For the nodal and element output, the
preselected field and history data include velocity (V), temperature (TEMP), pressure (PRESSURE),
and turbulent eddy viscosity (TURBNU). In addition, preselected field data include displacement (U).
Preselected data are not available for surface output.
In addition to the preselected output, you can request several derived and auxiliary variables. All of
the output variable identifiers are outlined in “Abaqus/CFD output variable identifiers,” Section 4.2.3.
6.6.2–20
Abaqus Version 5.8 ID:
Printed on:
INCOMPRESSIBLE FLUID DYNAMICS
Input file template
*HEADING
…
*NODE
…
*ELEMENT, TYPE=FC3D4
…
*MATERIAL, NAME=matname
*CONDUCTIVITY
Data lines to define the thermal conductivity
*DENSITY
Data lines to define the fluid density
*SPECIFIC HEAT, TYPE=CONSTANT PRESSURE
Data lines to define the specific heat
*VISCOSITY
Data lines to define the fluid viscosity
*INITIAL CONDITIONS, TYPE=TEMPERATURE, ELEMENT AVERAGE
Data lines to prescribe initial temperatures at the elements
*INITIAL CONDITIONS, TYPE=VELX, ELEMENT AVERAGE
Data lines to prescribe initial x-velocity at the elements
*INITIAL CONDITIONS, TYPE=VELY, ELEMENT AVERAGE
Data lines to prescribe initial y-velocity at the elements
*INITIAL CONDITIONS, TYPE=VELY, ELEMENT AVERAGE
Data lines to prescribe initial y-velocity at the elements
…
*AMPLITUDE, NAME=velxamp, DEFINITION=TABULAR
Data lines to define amplitude curve to be used for inlet x-velocity
**
*STEP
** Incompressible flow example
*CFD, INCOMPRESSIBLE NAVIER STOKES, INCREMENTATION=FIXED CFL
Data lines to define incrementation
**
** Boundary conditions
**
*FLUID BOUNDARY, TYPE=SURFACE
inlet_surface, VELX, value for x-velocity
inlet_surface, VELY, value for y-velocity
inlet_surface, VELZ, value for z-velocity
**
*FLUID BOUNDARY, TYPE=SURFACE
6.6.2–21
Abaqus Version 5.8 ID:
Printed on:
INCOMPRESSIBLE FLUID DYNAMICS
temperature_surface, TEMP, value for temperature
**
*FLUID BOUNDARY, TYPE=SURFACE
outlet_surface, P, value for pressure
**
** Field output
**
*OUTPUT, FIELD, TIME INTERVAL=interval for field output
*ELEMENT OUTPUT
PRESSURE, TEMP, TURBNU, V
*NODE OUTPUT
PRESSURE, TEMP, TURBNU, V
**
** History output
**
*OUTPUT, HISTORY, FREQUENCY=interval for history output
*ELEMENT OUTPUT, ELSET=element set for history output, FREQUENCY=SURFACE
…
*END STEP
Additional references
•
Albets-Chico, X., C. D. Perez-Segarra, A. Olivia, and J. Bredberg, “Analysis of Wall-Function
Approaches using Two-Equation Turbulence Models,” International Journal of Heat and Mass
Transfer, vol. 51, p. 4940–4957, 2008.
•
Casey, M., and T. Wintergerste, ERCOFTAC Special Interest Group on “Quality and Trust
in Industrial CFD”, European Research Community on Flow, Turbulence and Combustion
(ERCOFTAC), 2000.
•
Craft, T. J., A. V. Gerasimov, H. Iacovides, and B. E. Launder, “Progress in the Generalization
of Wall-Function Treatments,” International Journal of Heat and Fluid Flow, vol. 23, p. 148–160,
2002.
•
Durbin, P. A., “Limiters and wall treatments in applied turbulence modeling,” Fluid Dynamics
research, vol. 41, p. 1–17, 2009.
•
Launder, B. E., and D. B. Spalding, “The Numerical Computation of Turbulent Flows,” Computer
Methods in Applied Mechanics and Engineering, vol. 3, p. 269–289, 1974.
•
•
Nield, D.A., and A. Bejan, Convection in Porous Media, Springer, New York, Third edition, 2010.
Yakhot, V., S. A. Orszag, S. Thangam, T. B. Gatski, and C. G. Speziale, “Development of
Turbulence Models for Shear Flows by a Double Expansion Technique,” Physics of Fluids A,
vol. 4, no. 7, p. 1510–1520, 1992.
6.6.2–22
Abaqus Version 5.8 ID:
Printed on:
ELECTROMAGNETIC ANALYSIS
6.7
Electromagnetic analysis
•
•
•
•
•
•
“Electromagnetic analysis procedures,” Section 6.7.1
“Piezoelectric analysis,” Section 6.7.2
“Coupled thermal-electrical analysis,” Section 6.7.3
“Fully coupled thermal-electrical-structural analysis,” Section 6.7.4
“Eddy current analysis,” Section 6.7.5
“Magnetostatic analysis,” Section 6.7.6
6.7–1
Abaqus Version 5.8 ID:
Printed on:
ELECTROMAGNETIC ANALYSIS
6.7.1
ELECTROMAGNETIC ANALYSIS PROCEDURES
Overview
Abaqus/Standard offers several analysis procedures to model piezoelectric, electrical conduction,
and electromagnetic phenomena. The distinct electrical phenomena modeled by these procedures is
described first, followed by a brief overview of each procedure.
Electrostatic, electrical conduction, magnetostatic, and electromagnetic analyses
Piezoelectric effect is the electromechanical interaction exhibited by some materials. This coupled
electrostatic-structural response is modeled using piezoelectric analysis in Abaqus/Standard. In this
procedure the electric potential is a degree of freedom and its conjugate is the electric charge.
Coupled thermal-electrical conduction, with or without structural coupling, is modeled using
electrical procedures. In these procedures the electric potential is a degree of freedom and its conjugate
is the electric current. While transient effects are ignored in electrical conduction, thus making it steady
state, thermal fields can be modeled either as transient or steady state.
Magnetostatic analysis is used to compute the magnetic fields due to direct currents. It solves
the magnetostatic approximation to Maxwell’s equations. The magnetic vector potential is a degree
of freedom in a magnetostatic analysis, and its conjugate is the surface current.
Electromagnetic analysis is used to model the full coupling between time-varying electric and
magnetic fields by solving Maxwell’s equations. In such an analysis the magnetic vector potential is a
degree of freedom and its conjugate is the surface current.
Electrostatic procedure
The following electrostatic analysis procedure is available in Abaqus/Standard:
•
In a piezoelectric material an electric potential gradient causes straining,
while stress causes an electric potential in the material (“Piezoelectric analysis,” Section 6.7.2). This
coupling is provided by defining the piezoelectric and dielectric coefficients of a material and can
be used in natural frequency extraction, transient dynamic analysis, both linear and nonlinear static
stress analysis, and steady-state dynamic analysis procedures. In all procedures, including nonlinear
statics and dynamics, the piezoelectric behavior is always assumed to be linear.
Piezoelectric analysis:
Steady electrical conduction procedures
The following electrical conduction analyses procedures are available in Abaqus/Standard:
•
Coupled thermal-electrical analysis: The electric potential and temperature fields can
be solved simultaneously by performing a coupled thermal-electrical analysis (“Coupled
thermal-electrical analysis,” Section 6.7.3). In these problems the energy dissipated by an
electrical current flowing through a conductor is converted into thermal energy, and the electrical
conductivity can, in turn, be temperature dependent. Thermal loads can be applied, but deformation
of the structure is not considered. Coupled thermal-electrical problems can be linear or nonlinear.
6.7.1–1
Abaqus Version 5.8 ID:
Printed on:
ELECTROMAGNETIC ANALYSIS
•
A coupled thermal-electrical-structural
analysis is used to solve simultaneously for the stress/displacement, the electric potential, and the
temperature fields. A coupled analysis is used when the thermal, electrical, and mechanical solutions
affect each other strongly. An example of such a process is resistance spot welding, where two or
more metal parts are joined by fusion at discrete points at the material interface. The fusion is caused
by heat generated due to the current flow at the contact points, which depends on the pressure applied
at these points.
These problems can be transient or steady state and linear or nonlinear. Cavity radiation effects
cannot be included in a fully coupled thermal-electrical-structural analysis. See “Fully coupled
thermal-electrical-structural analysis,” Section 6.7.4, for more details.
Fully coupled thermal-electrical-structural analysis:
Magnetostatic procedure
The following magnetostatic analysis procedure is available in Abaqus/Standard:
•
A magnetostatic analysis is used to solve for the magnetic vector
potential, from which the magnetic field is computed in the entire domain. For example, the
magnetic field due to the flow of direct current can be modeled. The procedure supports linear as
well as nonlinear magnetic material properties. See “Magnetostatic analysis,” Section 6.7.6, for
more details.
Magnetostatic analysis:
Electromagnetic procedures
Electromagnetic analyses are used to solve for the magnetic vector potential, from which both electric and
magnetic fields are computed in the entire domain. The following electromagnetic analysis procedures
are available in Abaqus/Standard:
•
•
This procedure assumes time-harmonic excitation and
response. It supports linear electrical conductivity and linear magnetic material behavior. For
example, eddy currents induced in a workpiece that is in the vicinity of a source of excitation (such
as a coil carrying alternating current) can be modeled. See “Time-harmonic analysis” in “Eddy
current analysis,” Section 6.7.5, for more details.
Time-harmonic eddy current analysis:
Transient eddy current analysis: This procedure assumes general time variation of the
excitation and response. It supports linear electrical conductivity and both linear and nonlinear
magnetic material behavior. For example, eddy currents induced in a workpiece that is in the
vicinity of a source of excitation (such as a coil carrying time-varying current) can be modeled.
See “Transient analysis” in “Eddy current analysis,” Section 6.7.5, for more details.
6.7.1–2
Abaqus Version 5.8 ID:
Printed on:
PIEZOELECTRIC ANALYSIS
6.7.2
PIEZOELECTRIC ANALYSIS
Products: Abaqus/Standard
Abaqus/CAE
References
•
•
•
•
•
•
“Piezoelectric behavior,” Section 26.5.2
“Defining an analysis,” Section 6.1.2
“Electromagnetic analysis procedures,” Section 6.7.1
“Defining a concentrated charge,” Section 16.9.30 of the Abaqus/CAE User’s Manual, in the online
HTML version of this manual
“Defining a surface charge,” Section 16.9.31 of the Abaqus/CAE User’s Manual, in the online
HTML version of this manual
“Defining a body charge,” Section 16.9.32 of the Abaqus/CAE User’s Manual, in the online HTML
version of this manual
Overview
Coupled piezoelectric problems:
•
•
•
•
•
are those in which an electric potential gradient causes straining, while stress causes an electric
potential gradient in the material;
are solved using an eigenfrequency extraction, modal dynamic, static, dynamic, or steady-state
dynamic procedure;
require the use of piezoelectric elements and piezoelectric material properties;
can be performed for continuum problems in one, two, and three dimensions; and
can be used in both linear and nonlinear analysis (however, in nonlinear analysis the piezoelectric
part of the constitutive behavior is assumed to be linear).
Piezoelectric response
The electrical response of a piezoelectric material is assumed to be made up of piezoelectric and dielectric
effects:
where
is the electrical potential,
is the component of the electric flux vector (also known as the electric displacement) in the
ith material direction,
is the piezoelectric stress coupling,
6.7.2–1
Abaqus Version 5.8 ID:
Printed on:
PIEZOELECTRIC ANALYSIS
is a small-strain component,
is the material’s dielectric matrix for a fully constrained material, and
is the gradient of the electrical potential along the ith material direction,
.
Defining piezoelectric and dielectric properties is discussed in “Piezoelectric behavior,” Section 26.5.2.
The theoretical basis of the piezoelectric analysis capability in Abaqus is defined in “Piezoelectric
analysis,” Section 2.10.1 of the Abaqus Theory Manual.
Procedures available for piezoelectric analysis
Piezoelectric analysis can be carried out with the following procedures:
•
•
•
•
•
•
•
“Static stress analysis,” Section 6.2.2
“Implicit dynamic analysis using direct integration,” Section 6.3.2
“Direct-solution steady-state dynamic analysis,” Section 6.3.4
“Natural frequency extraction,” Section 6.3.5
“Transient modal dynamic analysis,” Section 6.3.7
“Mode-based steady-state dynamic analysis,” Section 6.3.8
“Subspace-based steady-state dynamic analysis,” Section 6.3.9
Initial conditions
Initial conditions of piezoelectric quantities cannot be specified.
See “Initial conditions in
Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1, for a description of the initial conditions that
can be applied in static or dynamic procedures.
Boundary conditions
The electric potential at a node (degree of freedom 9) can be prescribed using a boundary condition
(see “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1). Displacement
and rotation degrees of freedom can also be prescribed by using boundary conditions as described in the
relevant static and dynamic analysis procedure sections. See “Boundary conditions in Abaqus/Standard
and Abaqus/Explicit,” Section 33.3.1.
Boundary conditions can be prescribed as functions of time by referring to amplitude curves
(“Amplitude curves,” Section 33.1.2).
In an eigenfrequency extraction step (“Natural frequency extraction,” Section 6.3.5 ) involving
piezoelectric elements, the electric potential degree of freedom must be constrained at least at one node
to remove singularities from the dielectric part of the element operator.
Loads
Both mechanical and electrical loads can be applied in a piezoelectric analysis.
6.7.2–2
Abaqus Version 5.8 ID:
Printed on:
PIEZOELECTRIC ANALYSIS
Applying mechanical loads
The following types of mechanical loads can be prescribed in a piezoelectric analysis:
•
Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6); see
“Concentrated loads,” Section 33.4.2.
•
Distributed pressure forces or body forces can be applied; see “Distributed loads,” Section 33.4.3.
Applying electrical loads
The following types of electrical loads can be prescribed, as described in “Electromagnetic loads,”
Section 33.4.5:
•
•
Concentrated electric charge.
Distributed surface electric charge and body electric charge.
Loading in mode-based and subspace-based procedures
Electrical charge loads should be used only in conjunction with residual modes in the eigenvalue
extraction step, due to the “massless” mode effect. Since the electrical potential degrees of freedom do
not have any associated mass, these degrees of freedom are essentially eliminated (similar to Guyan
reduction or mass condensation) during the eigenvalue extraction. The residual modes represent
the static response corresponding to the electrical charge loads, which will adequately represent the
potential degree of freedom in the eigenspace.
Predefined fields
The following predefined fields can be specified in a piezoelectric analysis, as described in “Predefined
fields,” Section 33.6.1:
•
Although temperature is not a degree of freedom in piezoelectric elements, nodal temperatures can
be specified. The specified temperature affects only temperature-dependent material properties, if
any.
•
The values of user-defined field variables can be specified. These values affect only field-variabledependent material properties, if any.
Material options
The piezoelectric coupling matrix and the dielectric matrix are specified as part of the material definition
for piezoelectric materials, as described in “Piezoelectric behavior,” Section 26.5.2. They are relevant
only when the material definition is used with coupled piezoelectric elements.
The mechanical behavior of the material can include linear elasticity only (“Linear elastic behavior,”
Section 22.2.1).
6.7.2–3
Abaqus Version 5.8 ID:
Printed on:
PIEZOELECTRIC ANALYSIS
Elements
Piezoelectric elements must be used in a piezoelectric analysis (see “Choosing the appropriate element
for an analysis type,” Section 27.1.3). The electric potential, , is degree of freedom 9 at each node of
these elements. In addition, regular stress/displacement elements can be used in parts of the model where
piezoelectric effects do not need to be considered.
Output
The following output variables are applicable to the electrical solution in a piezoelectric analysis:
Element integration point variables:
EENER
EPG
EPGM
EPGn
EFLX
EFLXM
EFLXn
Electrostatic energy density.
Magnitude and components of the electrical potential gradient vector,
Magnitude of the electrical potential gradient vector.
Component n of the electrical potential gradient vector (n=1, 2, 3).
Magnitude and components of the electrical flux (displacement) vector, .
Magnitude of the electrical flux (displacement) vector.
Component n of the electrical flux (displacement) vector (n=1, 2, 3).
Whole element variables:
CHRGS
ELCTE
Values of distributed electrical charges.
Total electrostatic energy in the element,
.
Nodal variables:
EPOT
RCHG
CECHG
Electrical potential degree of freedom at a node.
Reactive electrical nodal charge (conjugate to prescribed electrical potential).
Concentrated electrical nodal charge.
Input file template
*HEADING
…
*MATERIAL, NAME=matl
*ELASTIC
Data lines to define linear elasticity
*PIEZOELECTRIC
Data lines to define piezoelectric behavior
*DIELECTRIC
Data lines to define dielectric behavior
…
6.7.2–4
Abaqus Version 5.8 ID:
Printed on:
.
PIEZOELECTRIC ANALYSIS
*AMPLITUDE, NAME=name
Data lines to define amplitude curve for defining concentrated electric charge
**
*STEP, (optionally NLGEOM)
*STATIC
** or *DYNAMIC, *FREQUENCY, *MODAL DYNAMIC,
** *STEADY STATE DYNAMICS (, DIRECT or , SUBSPACE PROJECTION)
*BOUNDARY
Data lines to define boundary conditions on electrical potential and
displacement (rotation) degrees of freedom
*CECHARGE, AMPLITUDE=name
Data lines to define time-dependent concentrated electric charges
*DECHARGE and/or *DSECHARGE
Data lines to define distributed electric charges
*CLOAD and/or *DLOAD and/or *DSLOAD
Data lines to define mechanical loading
*END STEP
6.7.2–5
Abaqus Version 5.8 ID:
Printed on:
COUPLED THERMAL-ELECTRICAL ANALYSIS
6.7.3
COUPLED THERMAL-ELECTRICAL ANALYSIS
Products: Abaqus/Standard
Abaqus/CAE
References
•
•
•
•
•
•
•
“Defining an analysis,” Section 6.1.2
“Electromagnetic analysis procedures,” Section 6.7.1
“Electrical conductivity,” Section 26.5.1
*COUPLED THERMAL-ELECTRICAL
*JOULE HEAT FRACTION
“Specifying a joule heat fraction,” Section 12.10.4 of the Abaqus/CAE User’s Manual, in the online
HTML version of this manual
“Configuring a fully coupled, simultaneous heat transfer and electrical procedure” in “Configuring
general analysis procedures,” Section 14.11.1 of the Abaqus/CAE User’s Manual, in the online
HTML version of this manual
Overview
Coupled thermal-electrical problems:
•
•
•
•
•
•
•
•
are those in which coupling between the electrical potential and temperature fields make it necessary
to solve both fields simultaneously;
require the use of coupled thermal-electrical elements, although pure heat transfer elements can also
be used in the model;
can include a specification of the fraction of electrical energy that will be released as heat;
can include thermal interactions such as gap radiation, gap conductance, and heat generation
between surfaces (see “Thermal contact properties,” Section 36.2.1);
can include cavity radiation effects (see “Cavity radiation,” Section 40.1.1);
can include electrical interactions such as electrical current flowing across surfaces (see “Electrical
contact properties,” Section 36.3.1);
allow for transient or steady-state thermal solutions and for steady-state electrical solutions; and
can be linear or nonlinear.
Coupled thermal-electrical analysis
Joule heating arises when the energy dissipated by an electrical current flowing through a conductor is
converted into thermal energy. Abaqus/Standard provides a fully coupled thermal-electrical procedure
for analyzing this type of problem: the coupled thermal-electrical equations are solved simultaneously
for both temperature and electrical potential at the nodes.
6.7.3–1
Abaqus Version 5.8 ID:
Printed on:
COUPLED THERMAL-ELECTRICAL ANALYSIS
The capability includes the analysis of the electrical problem, the thermal problem, and the
coupling between the two problems. Coupling arises from two sources: temperature-dependent
electrical conductivity and internal heat generation, which is a function of the electrical current density.
The thermal part of the problem can include heat conduction and heat storage (“Thermal properties:
overview,” Section 26.2.1) as well as cavity radiation effects (“Cavity radiation,” Section 40.1.1).
Forced convection caused by fluid flowing through the mesh is not considered.
The thermal-electrical equations are unsymmetric; therefore, the unsymmetric solver is invoked
automatically if you request coupled thermal-electrical analysis. For problems where coupling between
the thermal and electrical solutions is weak or where a pure electrical conduction analysis is required
for the entire model, the unsymmetric terms resulting from the interfield coupling may be small or zero.
In these problems you can invoke the less costly symmetric storage and solution scheme by solving
the thermal and electrical equations separately. The separated technique uses the symmetric solver by
default. The thermal-electrical solution schemes are discussed below.
The theoretical basis of coupled thermal-electrical analysis is described in detail in “Coupled
thermal-electrical analysis,” Section 2.12.1 of the Abaqus Theory Manual.
Governing electric field equation
The electric field in a conducting material is governed by Maxwell’s equation of conservation of charge.
Assuming steady-state direct current, the equation reduces to
where V is any control volume whose surface is S, is the outward normal to S, is the electrical current
density (current per unit area), and is the internal volumetric current source per unit volume.
The flow of electrical current is described by Ohm’s law:
where
)
is the electrical field intensity, defined as the negative of the gradient of the
electrical potential
,
is the electrical potential,
is the electrical conductivity matrix,
is the temperature, and
are predefined field variables.
Using Ohm’s law in the conservation equation, written in variational form, provides the governing
equation of the finite element model:
6.7.3–2
Abaqus Version 5.8 ID:
Printed on:
COUPLED THERMAL-ELECTRICAL ANALYSIS
where
is the current density entering the control volume across S.
Defining the electrical conductivity
The electrical conductivity,
, can be isotropic, orthotropic, or fully anisotropic (see “Electrical
conductivity,” Section 26.5.1). Ohm’s law assumes that the electrical conductivity is independent of the
electrical field, . The coupled thermal-electrical problem is nonlinear when the electrical conductivity
depends on temperature.
Specifying the amount of thermal energy generated due to electrical current
Joule’s law describes the rate of electrical energy,
as
, dissipated by current flowing through a conductor
The amount of this energy released as internal heat within the body is
, where
is an energy
conversion factor. You specify
in the material definition. It is assumed that all the electrical energy
is converted into heat (
) if you do not include the joule heat fraction in the material description.
The fraction given can include a unit conversion factor, if required.
Input File Usage:
Abaqus/CAE Usage:
*JOULE HEAT FRACTION
Property module: material editor: Thermal→Joule Heat Fraction
Steady-state analysis
Steady-state analysis provides the steady-state solution directly. Steady-state thermal analysis means that
the internal energy term (the specific heat term) in the governing heat transfer equation is omitted. Only
direct current is considered in the electrical problem, and it is assumed that the system has negligible
capacitance. (Electrical transient effects are so rapid that they can be neglected.)
Input File Usage:
Abaqus/CAE Usage:
*COUPLED THERMAL-ELECTRICAL, STEADY STATE
Step module: Create Step: General: Coupled thermal-electric:
Basic: Response: Steady state
Assigning a “time” scale to the analysis
A steady-state analysis has no intrinsic physically meaningful time scale. Nevertheless, you can assign
a “time” scale to the analysis step, which is often convenient for output identification and for specifying
prescribed temperatures, electrical potential, and fluxes (heat flux and current density) with varying
magnitudes. Thus, when steady-state analysis is chosen, you specify a “time” period and “time”
incrementation parameters for the step; Abaqus/Standard then increments through the step accordingly.
Any fluxes or boundary condition changes to be applied during a steady-state step should be
given using appropriate amplitude references to specify their “time” variations (“Amplitude curves,”
Section 33.1.2). If fluxes and boundary conditions are specified for the step without amplitude
6.7.3–3
Abaqus Version 5.8 ID:
Printed on:
COUPLED THERMAL-ELECTRICAL ANALYSIS
references, they are assumed to change linearly with “time” during the step—from their magnitudes at
the end of the previous step (or zero, if this is the beginning of the analysis) to their newly specified
magnitudes at the end of this step (see “Defining an analysis,” Section 6.1.2).
Transient analysis
Alternatively, the thermal portion of the coupled thermal-electrical problem can be considered
transient. As in steady-state analysis, electrical transient effects are neglected. See “Uncoupled heat
transfer analysis,” Section 6.5.2, for a more detailed description of the heat transfer capability in
Abaqus/Standard.
Input File Usage:
Abaqus/CAE Usage:
*COUPLED THERMAL-ELECTRICAL
Step module: Create Step: General: Coupled thermal-electric:
Basic: Response: Transient
Time incrementation
Time integration in the transient heat transfer problem is done with the same backward Euler method
used in uncoupled heat transfer analysis. This method is unconditionally stable for linear problems.
You can specify the time increments directly, or Abaqus can select them automatically based on a userprescribed maximum nodal temperature change in an increment. Automatic time incrementation is
generally preferred.
Automatic incrementation
The time increment size can be selected automatically based on a user-prescribed maximum allowable
nodal temperature change in an increment,
. Abaqus/Standard will restrict the time increments to
ensure that these values are not exceeded at any node (except nodes with boundary conditions) during
any increment of the analysis (see “Time integration accuracy in transient problems,” Section 7.2.4).
Input File Usage:
Abaqus/CAE Usage:
*COUPLED THERMAL-ELECTRICAL, DELTMX=
Step module: Create Step: General: Coupled thermal-electric: Basic:
Response: Transient; Incrementation: Type: Automatic: Max.
allowable temperature change per increment:
Fixed incrementation
If you select fixed time incrementation and do not specify
, fixed time increments equal to the
user-specified initial time increment,
, will then be used throughout the analysis.
Input File Usage:
*COUPLED THERMAL-ELECTRICAL
Abaqus/CAE Usage:
Step module: Create Step: General: Coupled thermal-electric: Basic:
Response: Transient; Incrementation: Type: Fixed: Increment size:
6.7.3–4
Abaqus Version 5.8 ID:
Printed on:
COUPLED THERMAL-ELECTRICAL ANALYSIS
Spurious oscillations due to small time increments
In transient heat transfer analysis with second-order elements there is a relationship between the
minimum usable time increment and the element size. A simple guideline is
where
is the time increment, is the density, c is the specific heat, k is the thermal conductivity, and
is a typical element dimension (such as the length of a side of an element). If time increments smaller
than this value are used in a mesh of second-order elements, spurious oscillations can appear in the
solution, in particular in the vicinity of boundaries with rapid temperature changes. These oscillations
are nonphysical and may cause problems if temperature-dependent material properties are present.
In transient analyses using first-order elements the heat capacity terms are lumped, which eliminates
such oscillations but can lead to locally inaccurate solutions for small time increments. If smaller time
increments are required, a finer mesh should be used in regions where the temperature changes rapidly.
There is no upper limit on the time increment size (the integration procedure is unconditionally
stable) unless nonlinearities cause convergence problems.
Ending a transient analysis
By default, a transient analysis will end when the specified time period has been completed. Alternatively,
you can specify that the analysis should continue until steady-state conditions are reached. Steady state
is defined by the temperature change rate; when the temperature changes at a rate that is less than the
user-specified rate (given as part of the step definition), the analysis terminates.
Input File Usage:
Use the following option to end the analysis when the time period is reached:
*COUPLED THERMAL-ELECTRICAL, END=PERIOD (default)
Use the following option to end the analysis based on the temperature change
rate:
Abaqus/CAE Usage:
*COUPLED THERMAL-ELECTRICAL, END=SS
Step module: Create Step: General: Coupled thermal-electric:
Basic: Response: Transient; Incrementation: End step when
temperature change is less than
Fully coupled solution schemes
Abaqus/Standard offers an exact as well as an approximate implementation of Newton’s method for
coupled thermal-electrical analysis.
Exact implementation
An exact implementation of Newton’s method involves a nonsymmetric Jacobian matrix as is illustrated
in the following matrix representation of the coupled equations:
6.7.3–5
Abaqus Version 5.8 ID:
Printed on:
COUPLED THERMAL-ELECTRICAL ANALYSIS
where
and
are the respective corrections to the incremental electrical potential and temperature,
are submatrices of the fully coupled Jacobian matrix, and
and
are the electrical and thermal
residual vectors, respectively.
Solving this system of equations requires the use of the unsymmetric matrix storage and solution
scheme. Furthermore, the electrical and thermal equations must be solved simultaneously. The method
provides quadratic convergence when the solution estimate is within the radius of convergence of the
algorithm. The exact implementation is used by default.
Approximate implementation
Some problems require a fully coupled analysis in the sense that the electrical and thermal solutions
evolve simultaneously, but with a weak coupling between the two solutions. In other words, the
components in the off-diagonal submatrices
,
are small compared to the components in the
diagonal submatrices
,
. For these problems a less costly solution may be obtained by setting
the off-diagonal submatrices to zero, so that we obtain an approximate set of equations:
As a result of this approximation the electrical and thermal equations can be solved separately, with
fewer equations to consider in each subproblem. The savings due to this approximation, measured as
solver time per iteration, will be of the order of a factor of two, with similar significant savings in solver
storage of the factored stiffness matrix. Further, in situations without strong thermal loading due to cavity
radiation, the subproblems may be fully symmetric or approximated as symmetric, so that the less costly
symmetric storage and solution scheme can be used. The solver time savings for a symmetric solution is
an additional factor of two. Unless you explicitly select the unsymmetric solver for the step (“Defining
an analysis,” Section 6.1.2), the symmetric solver will be used with this separated technique.
This modified form of Newton’s method does not affect solution accuracy since the fully coupled
effect is considered through the residual vector
at each increment in time. However, the rate of
convergence is no longer quadratic and depends strongly on the magnitude of the coupling effect, so more
iterations are generally needed to achieve equilibrium than with the exact implementation of Newton’s
method. When the coupling is significant, the convergence rate becomes very slow and may prohibit
the attainment of a solution. In such cases the exact implementation of Newton’s method is required.
In cases where it is possible to use this approximation, the convergence in an increment will depend
strongly on the quality of the first guess to the incremental solution, which you can control by selecting
the extrapolation method used for the step (see “Defining an analysis,” Section 6.1.2).
Input File Usage:
Use the following option to specify a separated solution scheme:
Abaqus/CAE Usage:
*SOLUTION TECHNIQUE, TYPE=SEPARATED
Step module: Create Step: General: Coupled thermal-electric:
Other: Solution technique: Separated
6.7.3–6
Abaqus Version 5.8 ID:
Printed on:
COUPLED THERMAL-ELECTRICAL ANALYSIS
Uncoupled electric conduction and heat transfer analysis
The coupled thermal-electrical procedure can also be used to perform uncoupled electric conduction
analysis for the whole model or just part of the model (using coupled thermal-electrical elements).
Uncoupled electrical analysis is available by omitting the thermal properties from the material
description, in which case only the electric potential degrees of freedom are activated in the element and
all heat transfer effects are ignored. If heat transfer effects are ignored in the entire model, you should
invoke the separated solution technique described above. Use of this technique will then invoke the
symmetric storage and solution scheme, which is an exact representation of a purely electrical problem.
Similarly, coupled thermal-electrical elements can be used in an uncoupled heat transfer analysis
(“Uncoupled heat transfer analysis,” Section 6.5.2), in which case all electric conduction effects are
ignored. This feature is useful if a thermal-electrical analysis is followed by a pure heat conduction
analysis. A typical example is a welding process, where the electric current is applied instantaneously,
followed by a cooldown period during which no electrical effects need to be considered. The symmetric
solver is activated by default in an uncoupled heat transfer analysis.
Cavity radiation
Cavity radiation can be activated in a heat transfer step. This feature involves interacting heat transfer
between all of the facets of the cavity surface, dependent on the facet temperatures, facet emissivities,
and the geometric viewfactors between each facet pair. When the thermal emissivity is a function of
temperature or field variables, you can specify the maximum allowable emissivity change during an
increment in addition to the maximum temperature change to control the time incrementation. See
“Cavity radiation,” Section 40.1.1, for more information.
Input File Usage:
Use the following option in the step definition to activate cavity radiation:
*RADIATION VIEWFACTOR
Use the following option to specify the maximum allowable emissivity change:
Abaqus/CAE Usage:
*HEAT TRANSFER, MXDEM=max_delta_emissivity
You can specify the maximum allowable emissivity change for a heat transfer
step.
Step module: Create Step: General: Heat transfer: Incrementation:
Max. allowable emissivity change per increment
Initial conditions
By default, the initial temperature of all nodes is zero. You can specify nonzero initial temperatures
or field variables (see “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1).
Since only steady-state electrical currents are considered, the initial value of the electrical potential is
not relevant.
6.7.3–7
Abaqus Version 5.8 ID:
Printed on:
COUPLED THERMAL-ELECTRICAL ANALYSIS
Boundary conditions
Boundary conditions can be used to prescribe the electrical potential,
(degree of freedom
9), and the temperature,
(degree of freedom 11), at the nodes. See “Boundary conditions in
Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1.
Boundary conditions can be specified as functions of time by referring to amplitude curves (see
“Amplitude curves,” Section 33.1.2).
A boundary without any prescribed boundary conditions corresponds to an insulated surface.
Loads
Both thermal and electrical loads can be applied in a coupled thermal-electrical analysis.
Applying thermal loads
The following types of thermal loads can be prescribed in a coupled thermal-electrical analysis, as
described in “Thermal loads,” Section 33.4.4:
•
•
•
•
Concentrated heat fluxes.
Body fluxes and distributed surface fluxes.
Average-temperature radiation conditions.
Convective film conditions and radiation conditions.
Applying electrical loads
The following types of electrical loads can be prescribed, as described in “Electromagnetic loads,”
Section 33.4.5:
•
•
Concentrated current.
Distributed surface current densities and body current densities.
Predefined fields
Predefined temperature fields are not allowed in coupled thermal-electrical analyses. Boundary
conditions should be used instead to specify temperatures, as described above.
Other predefined field variables can be specified in a coupled thermal-electrical analysis. These
values affect only field-variable-dependent material properties, if any. See “Predefined fields,”
Section 33.6.1.
Material options
Both thermal and electrical properties are active in coupled thermal-electrical analyses. If thermal
properties are omitted, an uncoupled electrical analysis will be performed.
All mechanical behavior material models (such as elasticity and plasticity) are ignored in a coupled
thermal-electrical analysis.
6.7.3–8
Abaqus Version 5.8 ID:
Printed on:
COUPLED THERMAL-ELECTRICAL ANALYSIS
Thermal material properties
For the heat transfer portion of the analysis, the thermal conductivity must be defined (see “Conductivity,”
Section 26.2.2). The specific heat must also be defined for transient heat transfer problems (see “Specific
heat,” Section 26.2.3). If changes in internal energy due to phase changes are important, latent heat can
be defined (see “Latent heat,” Section 26.2.4). Thermal expansion coefficients (“Thermal expansion,”
Section 26.1.2) are not meaningful in a coupled thermal-electrical analysis since deformation of the
structure is not considered. Internal heat generation can be specified (see “Uncoupled heat transfer
analysis,” Section 6.5.2).
Electrical material properties
For the electrical portion of the analysis, the electrical conductivity must be defined (see “Electrical
conductivity,” Section 26.5.1). The electrical conductivity can be a function of temperature and
user-defined field variables. The fraction of electrical energy dissipated as heat can also be defined, as
explained above.
Elements
The simultaneous solution in a coupled thermal-electrical analysis requires the use of elements that have
both temperature (degree of freedom 11) and electrical potential (degree of freedom 9) as nodal variables.
The finite element model can also include pure heat transfer elements (so that a pure heat transfer analysis
is provided for that part of the model) and coupled thermal-electrical elements for which no thermal
properties are given (so that a pure electrical conduction solution is provided for that part of the model).
Coupled thermal-electrical elements are available in Abaqus/Standard in one dimension, two
dimensions (planar and axisymmetric), and three dimensions. See “Choosing the appropriate element
for an analysis type,” Section 27.1.3.
Output
The following output variables can be used to request output relating to the electric conduction solution:
Element integration point variables:
EPG
EPGM
EPGn
ECD
JENER
Magnitude and components of the electrical potential gradient vector,
Magnitude of the electrical potential gradient vector.
Component n of the electrical potential gradient vector (n=1, 2, 3).
Magnitude and components of the electrical current density vector, J.
Electrical energy dissipated due to flow of current,
.
.
Whole element variables:
ECURS
NCURS
ELJD
Distributed applied electrical current.
Electrical current at nodes due to electric conduction.
Total electrical energy dissipated due to flow of current,
6.7.3–9
Abaqus Version 5.8 ID:
Printed on:
.
COUPLED THERMAL-ELECTRICAL ANALYSIS
Nodal variables:
EPOT
RECUR
CECUR
Electrical potential, .
Reactive electrical current.
Concentrated applied electrical current.
Whole model variables:
ALLJD
Electrical energy summed over the model.
Surface interaction variables (see “Electrical contact properties,” Section 36.3.1):
ECD
ECDA
ECDT
ECDTA
SJD
SJDA
SJDT
SJDTA
WEIGHT
Electrical current density.
ECD multiplied by area.
Time integrated ECD.
Time integrated ECDA.
Heat flux per unit area generated by the electrical current.
SJD multiplied by area.
Time integrated SJD.
Time integrated SJDA.
Heat distribution between interface surfaces, f.
Considerations for steady-state coupled thermal-electrical analysis
In a steady-state coupled thermal-electrical analysis the electrical energy dissipated due to flow of
electrical current at an integration point (output variable JENER) is computed using the following
relationship:
where
denotes the electrical energy dissipated due to flow of electrical current and
is the current
step time. In the above relationship it is assumed that the rate of the electrical energy dissipation,
,
has a constant value in the step that is equal to the value currently computed.
The output variable JENER and the derived output variables ELJD and ALLJD contain the values
of electrical energies dissipated in the current step only. Similarly, the contribution from the electrical
current flow to the output variable ALLWK includes only the external work performed in the current
step.
Input file template
*HEADING
…
*MATERIAL, NAME=mat1
*CONDUCTIVITY
Data lines to define thermal conductivity
6.7.3–10
Abaqus Version 5.8 ID:
Printed on:
COUPLED THERMAL-ELECTRICAL ANALYSIS
*ELECTRICAL CONDUCTIVITY
Data lines to define electrical conductivity
* HEAT FRACTION
Data lines to define the fraction of electric energy released as heat
**
*STEP
*COUPLED THERMAL-ELECTRICAL
Data line to define incrementation and steady state
*BOUNDARY
Data lines to define boundary conditions on electrical potential and
temperature degrees of freedom
*CECURRENT
Data lines to define concentrated currents
*DECURRENT and/or *DSECURRENT
Data lines to define distributed current densities
*CFLUX and/or *DFLUX and/or *DSFLUX
Data lines to define thermal loading
*FILM and/or *SFILM and/or *RADIATE and/or *SRADIATE
Data lines to define convective film and radiation conditions
…
*CONTACT PRINT or *CONTACT FILE
Data lines to request output of surface interaction variables
*END STEP
6.7.3–11
Abaqus Version 5.8 ID:
Printed on:
COUPLED THERMAL-ELECTRICAL-STRUCTURAL ANALYSIS
6.7.4
FULLY COUPLED THERMAL-ELECTRICAL-STRUCTURAL ANALYSIS
Products: Abaqus/Standard
Abaqus/CAE
References
•
•
•
•
•
“Defining an analysis,” Section 6.1.2
“Fully coupled thermal-stress analysis,” Section 6.5.3
“Coupled thermal-electrical analysis,” Section 6.7.3
*COUPLED TEMPERATURE-DISPLACEMENT
“Configuring a fully coupled, simultaneous heat transfer, electrical, and structural procedure” in
“Configuring general analysis procedures,” Section 14.11.1 of the Abaqus/CAE User’s Manual, in
the online HTML version of this manual
Overview
A fully coupled thermal-electrical-structural analysis:
•
•
•
•
•
•
•
•
•
is performed when coupling between the displacement, temperature, and electrical potential fields
makes it necessary to obtain solutions for all three fields simultaneously;
requires the existence of elements with displacement, temperature, and electrical potential degrees
of freedom in the model;
allows for transient or steady-state thermal solutions, static displacement solutions, and steady-state
electrical solutions;
can include thermal interactions such as gap radiation, gap conductance, and gap heat generation
between surfaces (see “Thermal contact properties,” Section 36.2.1);
can include electrical interactions such as gap electrical conductance (see “Electrical contact
properties,” Section 36.3.1);
cannot include cavity radiation effects but may include radiation boundary conditions (see “Thermal
loads,” Section 33.4.4);
takes into account temperature dependence of material properties only for the properties that are
assigned to elements with temperature degrees of freedom;
neglects inertia effects; and
can be transient or steady state.
Fully coupled thermal-electrical-structural analysis
A fully coupled thermal-electrical-structural analysis is the union of a coupled thermal-displacement
analysis (see “Fully coupled thermal-stress analysis,” Section 6.5.3) and a coupled thermal-electrical
analysis (see “Coupled thermal-electrical analysis,” Section 6.7.3).
6.7.4–1
Abaqus Version 5.8 ID:
Printed on:
COUPLED THERMAL-ELECTRICAL-STRUCTURAL ANALYSIS
Coupling between the temperature and electrical degrees of freedom arises from temperaturedependent electrical conductivity and internal heat generation (Joule heating), which is a function of the
electrical current density. The thermal part of the problem can include heat conduction and heat storage
(“Thermal properties: overview,” Section 26.2.1). Forced convection caused by fluid flowing through
the mesh is not considered.
Coupling between the temperature and displacement degrees of freedom arises from
temperature-dependent material properties, thermal expansion, and internal heat generation,
which is a function of inelastic deformation of the material. In addition, contact conditions exist in
some problems where the heat conducted between surfaces may depend strongly on the separation of
the surfaces and/or the pressure transmitted across the surfaces as well as friction (see “Mechanical
contact properties: overview,” Section 36.1.1, and “Thermal contact properties,” Section 36.2.1).
Coupling between the electrical and displacement degrees of freedom arises in problems where
electricity flows between contact surfaces. The electrical conduction may depend strongly on the
separation of the surfaces and/or the pressure transmitted across the surfaces (see “Electrical contact
properties,” Section 36.3.1).
An example of a simulation that requires a fully coupled thermal-electrical-structural analysis is
resistance spot welding. In a typical spot welding process two or more thin metal sheets are pinched
between two electrodes. A large current is passed between the electrodes, which melts the metal between
the electrodes and forms a weld. The integrity of the weld depends on many parameters including the
electrical conductance between the sheets (which can be a function of contact pressure and temperature).
Steady-state analysis
Steady-state analysis provides the steady-state solution directly. Steady-state thermal analysis means
that the internal energy term (the specific heat term) in the governing heat transfer equation is omitted.
A static displacement solution is assumed. Only direct current is considered in the electrical problem,
and it is assumed that the system has negligible capacitance. Electrical transient effects are so rapid that
they can be neglected.
Input File Usage:
*COUPLED TEMPERATURE-DISPLACEMENT, ELECTRICAL,
STEADY STATE
Abaqus/CAE Usage:
Step module: Create Step: General: Coupled thermal-electricalstructural: Basic: Response: Steady state
Assigning a “time” scale to the analysis
In steady-state cases you should assign an arbitrary “time” scale to the step: you specify a “time”
period and “time” incrementation parameters. This time scale is convenient for changing loads and
boundary conditions through the step and for obtaining solutions to highly nonlinear (but steady-state)
cases; however, for the latter purpose, transient analysis often provides a natural way of coping with
the nonlinearity.
6.7.4–2
Abaqus Version 5.8 ID:
Printed on:
COUPLED THERMAL-ELECTRICAL-STRUCTURAL ANALYSIS
Accounting for frictional slip heat generation
Frictional slip heat generation is normally neglected in the steady-state case. However, it can still be
accounted for if motions are used to specify translational or rotational nodal velocities in disk brake-type
problems or if user subroutine FRIC provides the incremental frictional dissipation through the variable
SFD. If frictional heat generation is present, the heat flux into the two contact surfaces depends on the
slip rate of the surfaces. The “time” scale in this case cannot be described as arbitrary, and a transient
analysis should be performed.
Transient analysis
Alternatively, you can perform a transient coupled thermal-electrical-structural analysis. As in steadystate analysis, electrical transient effects are neglected and a static displacement solution is assumed.
You can control the time incrementation in a transient analysis directly, or Abaqus/Standard can control
it automatically. Automatic time incrementation is generally preferred.
Automatic incrementation controlled by a maximum allowable temperature change
The time increments can be selected automatically based on a user-prescribed maximum allowable nodal
temperature change in an increment,
. Abaqus/Standard will restrict the time increments to ensure
that this value is not exceeded at any node (except nodes with boundary conditions) during any increment
of the analysis (see “Time integration accuracy in transient problems,” Section 7.2.4).
Input File Usage:
*COUPLED TEMPERATURE-DISPLACEMENT, ELECTRICAL,
DELTMX=
Abaqus/CAE Usage:
Step module: Create Step: General: Coupled thermal-electricalstructural: Basic: Response: Transient; Incrementation: Type:
Automatic: Max. allowable temperature change per increment:
Fixed incrementation
If you do not specify
, fixed time increments equal to the user-specified initial time increment,
, will be used throughout the analysis.
Input File Usage:
*COUPLED TEMPERATURE-DISPLACEMENT, ELECTRICAL
Abaqus/CAE Usage:
Step module: Create Step: General: Coupled thermal-electricalstructural: Basic: Response: Transient; Incrementation:
Type: Fixed: Increment size:
Spurious oscillations due to small time increments
In transient analysis with second-order elements there is a relationship between the minimum usable time
increment and the element size. A simple guideline is
6.7.4–3
Abaqus Version 5.8 ID:
Printed on:
COUPLED THERMAL-ELECTRICAL-STRUCTURAL ANALYSIS
where
is the time increment, is the density, c is the specific heat, k is the thermal conductivity, and
is a typical element dimension (such as the length of a side of an element). If time increments smaller
than this value are used in a mesh of second-order elements, spurious oscillations can appear in the
solution, in particular in the vicinity of boundaries with rapid temperature changes. These oscillations
are nonphysical and may cause problems if temperature-dependent material properties are present.
In transient analyses using first-order elements the heat capacity terms are lumped, which eliminates
such oscillations but can lead to locally inaccurate solutions for small time increments. If smaller time
increments are required, a finer mesh should be used in regions where the temperature changes rapidly.
There is no upper limit on the time increment size (the integration procedure is unconditionally
stable) unless nonlinearities cause convergence problems.
Automatic incrementation controlled by the creep response
The accuracy of the integration of time-dependent (creep) material behavior is governed by the
user-specified accuracy tolerance parameter,
. This parameter is used
to prescribe the maximum strain rate change allowed at any point during an increment, as described
in “Rate-dependent plasticity: creep and swelling,” Section 23.2.4. The accuracy tolerance parameter
can be specified together with the maximum allowable nodal temperature change in an increment,
(described above); however, specifying the accuracy tolerance parameter activates automatic
incrementation even if
is not specified.
Input File Usage:
*COUPLED TEMPERATURE-DISPLACEMENT, ELECTRICAL,
DELTMX=
, CETOL=tolerance
Abaqus/CAE Usage:
Step module: Create Step: General: Coupled thermal-electricalstructural: Basic: Response: Transient, toggle on Include
creep/swelling/viscoelastic behavior; Incrementation: Type:
Automatic: Max. allowable temperature change per increment:
Creep/swelling/viscoelastic strain error tolerance: tolerance
,
Selecting explicit creep integration
Nonlinear creep problems (“Rate-dependent plasticity: creep and swelling,” Section 23.2.4) that exhibit
no other nonlinearities can be solved efficiently by forward-difference integration of the inelastic
strains if the inelastic strain increments are smaller than the elastic strains. This explicit method is
efficient computationally because, unlike implicit methods, iteration is not required as long as no other
nonlinearities are present. Although this method is only conditionally stable, the numerical stability
limit of the explicit operator is in many cases sufficiently large to allow the solution to be developed in
a reasonable number of time increments.
For most coupled thermal-electrical-structural analyses, however, the unconditional stability of the
backward difference operator (implicit method) is desirable. In such cases the implicit integration scheme
may be invoked automatically by Abaqus/Standard.
Explicit integration can be less expensive computationally and simplifies implementation of userdefined creep laws in user subroutine CREEP; you can restrict Abaqus/Standard to using this method
6.7.4–4
Abaqus Version 5.8 ID:
Printed on:
COUPLED THERMAL-ELECTRICAL-STRUCTURAL ANALYSIS
for creep problems (with or without geometric nonlinearity included). See “Rate-dependent plasticity:
creep and swelling,” Section 23.2.4, for further details.
Input File Usage:
*COUPLED TEMPERATURE-DISPLACEMENT, ELECTRICAL,
CETOL=tolerance, CREEP=EXPLICIT
Abaqus/CAE Usage:
Step module: Create Step: General: Coupled thermal-electricalstructural: Basic: Response: Transient, toggle on Include
creep/swelling/viscoelastic behavior; Incrementation:
Creep/swelling/viscoelastic strain error tolerance: tolerance,
Creep/swelling/viscoelastic integration: Explicit
Excluding creep and viscoelastic response
You can specify that no creep or viscoelastic response will occur during a step even if creep or viscoelastic
material properties have been defined.
Input File Usage:
*COUPLED TEMPERATURE-DISPLACEMENT, ELECTRICAL,
DELTMX=
, CREEP=NONE
Abaqus/CAE Usage:
Step module: Create Step: General: Coupled thermal-electricalstructural: Basic: Response: Transient, toggle off Include
creep/swelling/viscoelastic behavior
Unstable problems
Some types of analyses may develop local instabilities, such as surface wrinkling, material instability,
or local buckling. In such cases it may not be possible to obtain a quasi-static solution, even with
the aid of automatic incrementation. Abaqus/Standard offers a method of stabilizing this class of
problems by applying damping throughout the model in such a way that the viscous forces introduced
are sufficiently large to prevent instantaneous buckling or collapse but small enough not to affect the
behavior significantly while the problem is stable. The available automatic stabilization schemes are
described in detail in “Automatic stabilization of unstable problems” in “Solving nonlinear problems,”
Section 7.1.1.
Units
In coupled problems where two or three different fields are active, take care when choosing the units of
the problem. If the choice of units is such that the terms generated by the equations for each field are
different by many orders of magnitude, the precision on some computers may be insufficient to resolve the
numerical ill-conditioning of the coupled equations. Therefore, choose units that avoid ill-conditioned
matrices. For example, consider using units of Mpascal instead of pascal for the stress equilibrium
equations to reduce the disparity between the magnitudes of the stress equilibrium equations, the heat
flux continuity equations, and the conservation of charge equations.
6.7.4–5
Abaqus Version 5.8 ID:
Printed on:
COUPLED THERMAL-ELECTRICAL-STRUCTURAL ANALYSIS
Initial conditions
By default, the initial temperature of all nodes is zero. You can specify nonzero initial temperatures.
Initial stresses, field variables, etc. can also be defined; “Initial conditions in Abaqus/Standard and
Abaqus/Explicit,” Section 33.2.1, describes all of the initial conditions that are available for a fully
coupled thermal-electrical-structural analysis.
Boundary conditions
Boundary conditions can be used to prescribe temperatures (degree of freedom 11),
displacements/rotations (degrees of freedom 1–6), or electrical potentials (degree of freedom 9) at nodes
in a fully coupled thermal-electrical-structural analysis (see “Boundary conditions in Abaqus/Standard
and Abaqus/Explicit,” Section 33.3.1).
Boundary conditions can be specified as functions of time by referring to amplitude curves
(“Amplitude curves,” Section 33.1.2).
Loads
The following types of thermal loads can be prescribed in a fully coupled thermal-electrical-structural
analysis, as described in “Thermal loads,” Section 33.4.4:
•
•
•
•
•
Concentrated heat fluxes.
Body fluxes and distributed surface fluxes.
Node-based film and radiation conditions.
Average-temperature radiation conditions.
Element and surface-based film and radiation conditions.
The following types of mechanical loads can be prescribed:
•
Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6); see
“Concentrated loads,” Section 33.4.2.
•
Distributed pressure forces or body forces can be applied; see “Distributed loads,” Section 33.4.3.
The following types of electrical loads can be prescribed, as described in “Electromagnetic loads,”
Section 33.4.5:
•
•
Concentrated current.
Distributed surface current densities and body current densities.
Predefined fields
Predefined temperature fields are not allowed in a fully coupled thermal-electrical-structural analysis.
Boundary conditions should be used instead to prescribe temperature degree of freedom 11, as described
earlier.
6.7.4–6
Abaqus Version 5.8 ID:
Printed on:
COUPLED THERMAL-ELECTRICAL-STRUCTURAL ANALYSIS
Other predefined field variables can be specified in a fully coupled thermal-electrical-structural
analysis. These values will affect only field-variable-dependent material properties, if any. See
“Predefined fields,” Section 33.6.1.
Material options
The materials in a fully coupled thermal-electrical-structural analysis must have thermal properties (such
as conductivity), mechanical properties (such as elasticity), and electrical properties (such as electrical
conductivity) defined. See Part V, “Materials,” for details on the material models available in Abaqus.
Internal heat generation can be specified; see “Uncoupled heat transfer analysis,” Section 6.5.2.
Thermal strain will arise if thermal expansion (“Thermal expansion,” Section 26.1.2) is included in
the material property definition.
A fully coupled thermal-electrical-structural analysis can be used to analyze static creep
and swelling problems, which generally occur over fairly long time periods (“Rate-dependent
plasticity: creep and swelling,” Section 23.2.4); viscoelastic materials (“Time domain viscoelasticity,”
Section 22.7.1); or viscoplastic materials (“Rate-dependent yield,” Section 23.2.3).
Inelastic energy dissipation as a heat source
You can specify an inelastic heat fraction in a fully coupled thermal-electrical-structural analysis to
provide for inelastic energy dissipation as a heat source. Plastic straining gives rise to a heat flux per unit
volume of
where
is the heat flux that is added into the thermal energy balance, is a user-defined factor (assumed
constant), is the stress, and
is the rate of plastic straining.
Inelastic heat fractions are typically used in the simulation of high-speed manufacturing processes
involving large amounts of inelastic strain, where the heating of the material caused by its deformation
significantly influences temperature-dependent material properties. The generated heat is treated as a
volumetric heat flux source term in the heat balance equation.
An inelastic heat fraction can be specified for materials with plastic behavior that use the Mises
or Hill yield surface (“Inelastic behavior,” Section 23.1.1). It cannot be used with the combined
isotropic/kinematic hardening model. The inelastic heat fraction can be specified for user-defined
material behavior in Abaqus/Explicit and will be multiplied by the inelastic energy dissipation coded in
the user subroutine to obtain the heat flux. In Abaqus/Standard the inelastic heat fraction cannot be used
with user-defined material behavior; in this case the heat flux that must be added to the thermal energy
balance is computed directly in the user subroutine.
In Abaqus/Standard an inelastic heat fraction can also be specified for hyperelastic material
definitions that include time-domain viscoelasticity (“Time domain viscoelasticity,” Section 22.7.1).
The default value of the inelastic heat fraction is 0.9. If you do not include the inelastic heat fraction
behavior in the material definition, the heat generated by inelastic deformation is not included in the
analysis.
6.7.4–7
Abaqus Version 5.8 ID:
Printed on:
COUPLED THERMAL-ELECTRICAL-STRUCTURAL ANALYSIS
Input File Usage:
*INELASTIC HEAT FRACTION
Specifying the amount of thermal energy generated due to electrical current
Joule’s law describes the rate of electrical energy,
as
, dissipated by current flowing through a conductor
The amount of this energy released as internal heat within the body is
, where
is an energy
conversion factor. You specify
in the material definition. It is assumed that all the electrical energy
is converted into heat (
) if you do not include the joule heat fraction in the material description.
The fraction given can include a unit conversion factor, if required.
Input File Usage:
*JOULE HEAT FRACTION
Elements
Coupled thermal-electrical-structural elements that have displacements, temperatures, and electrical
potentials as nodal variables are available. Simultaneous temperature/electrical potential/displacement
solution requires the use of such elements; pure displacement and temperature-displacement elements
can be used in part of the model in a fully coupled thermal-electrical-structural analysis, but pure heat
transfer elements cannot be used.
The first-order coupled thermal-electrical-structural elements in Abaqus use a constant temperature
over the element to calculate thermal expansion. The second-order coupled thermal-electrical-structural
elements in Abaqus use a lower-order interpolation for temperature than for displacement (parabolic
variation of displacements and linear variation of temperature) to obtain a compatible variation of thermal
and mechanical strain.
Output
See “Abaqus/Standard output variable identifiers,” Section 4.2.1, for a complete list of output variables.
The types of output available are described in “Output,” Section 4.1.1.
Considerations for steady-state coupled thermal-electrical-structural analysis
In a steady-state coupled thermal-electrical-structural analysis the electrical energy dissipated due to flow
of electrical current at an integration point (output variable JENER) is computed using the following
relationship:
where
denotes the electrical energy dissipated due to flow of electrical current and
is the current
step time. In the above relationship it is assumed that the rate of the electrical energy dissipation,
,
has a constant value in the step that is equal to the value currently computed.
6.7.4–8
Abaqus Version 5.8 ID:
Printed on:
COUPLED THERMAL-ELECTRICAL-STRUCTURAL ANALYSIS
The output variable JENER and the derived output variables ELJD and ALLJD contain the values
of electrical energies dissipated in the current step only. Similarly, the contribution from the electrical
current flow to the output variable ALLWK includes only the external work performed in the current
step.
Input file template
*HEADING
…
** Specify the coupled thermal-electrical-structural element type
*ELEMENT, TYPE=Q3D8
…
**
*STEP
*COUPLED TEMPERATURE-DISPLACEMENT, ELECTRICAL
Data line to define incrementation
*BOUNDARY
Data lines to define nonzero boundary conditions on displacement,
temperature or electrical potential degrees of freedom
*CFLUX and/or *CFILM and/or
*CRADIATE and/or *DFLUX and/or
*DSFLUX and/or *FILM and/or
*SFILM and/or *RADIATE and/or
*SRADIATE
Data lines to define thermal loads
*CLOAD and/or *DLOAD and/or *DSLOAD
Data lines to define mechanical loads
*CECURRENT
Data lines to define concentrated currents
*DECURRENT and/or *DSECURRENT
Data lines to define distributed current densities
*FIELD
Data lines to define field variable values
*END STEP
6.7.4–9
Abaqus Version 5.8 ID:
Printed on:
EDDY CURRENT ANALYSIS
6.7.5
EDDY CURRENT ANALYSIS
Products: Abaqus/Standard
Abaqus/CAE
References
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
“Mapping thermal and magnetic loads,” Section 3.2.22
“Electromagnetic analysis procedures,” Section 6.7.1
“Electrical conductivity,” Section 26.5.1
“Magnetic permeability,” Section 26.5.3
“Electromagnetic loads,” Section 33.4.5
“Predefined loads for sequential coupling,” Section 16.1.3
*ELECTROMAGNETIC
*D EM POTENTIAL
*DECURRENT
*DSECURRENT
“UDECURRENT,” Section 1.1.23 of the Abaqus User Subroutines Reference Manual
“UDEMPOTENTIAL,” Section 1.1.24 of the Abaqus User Subroutines Reference Manual
“UDSECURRENT,” Section 1.1.26 of the Abaqus User Subroutines Reference Manual
“Configuring a time-harmonic electromagnetic analysis” in “Configuring linear perturbation
analysis procedures,” Section 14.11.2 of the Abaqus/CAE User’s Manual, in the online HTML
version of this manual
“Defining a magnetic vector potential boundary condition,” Section 16.10.17 of the Abaqus/CAE
User’s Manual, in the online HTML version of this manual
Overview
Eddy current problems:
•
•
•
•
•
•
involve coupling between electric and magnetic fields, which are solved for simultaneously;
solve Maxwell’s equations describing electromagnetic phenomena under the low-frequency
assumption that neglects the effects of displacement currents;
require the use of electromagnetic elements in the whole domain;
require that magnetic permeability is specified in the whole domain and electrical conductivity is
specified in the conducting regions;
allows for both time-harmonic and transient electromagnetic solutions;
calculate as output variables, rate of Joule heating and intensity of magnetic body forces
associated with eddy currents, and these output variables can be transferred from a time-harmonic
electromagnetic solution to drive a subsequent heat transfer, coupled temperature-displacement,
6.7.5–1
Abaqus Version 5.8 ID:
Printed on:
EDDY CURRENT ANALYSIS
or stress/displacement analysis, thereby allowing for the coupling of electromagnetic fields with
thermal and/or mechanical fields in a sequentially coupled manner; and
•
can be solved using continuum elements in two- and three-dimensional space.
Eddy current analysis
Eddy currents are generated in a metal workpiece when it is placed within a time-varying magnetic field.
Joule heating arises when the energy dissipated by the eddy currents flowing through the workpiece is
converted into thermal energy. This heating mechanism is usually referred to as induction heating; the
induction cooker is an example of a device that uses this mechanism. The time-varying magnetic field is
usually generated by a coil that is placed close to the workpiece. The coil carries either a known amount
of total current or an unknown amount of current under a known potential (voltage) difference. The
current in the coil is assumed to be alternating at a known frequency for a time-harmonic eddy current
analysis but may have an arbitrary variation in time for a transient eddy current analysis.
The time-harmonic eddy current analysis procedure is based on the assumption that a time-harmonic
excitation with a certain frequency results in a time-harmonic electromagnetic response with the same
frequency everywhere in the domain. In other words, both the electric and the magnetic fields oscillate at
the same frequency as that of the alternating current in the coil. The transient eddy current analysis does
not make any assumption regarding the time-variation of the current in the coil; in fact any arbitrary time
variation can be specified, and the electric and magnetic fields follow from the solution to Maxwell’s
equations in the time domain.
The eddy current analysis provides output, such as Joule heat dissipation or magnetic body
force intensity, that can be transferred, from a time-harmonic eddy current analysis only, to drive a
subsequent heat transfer, coupled temperature-displacement, or stress/displacement analysis. This
allows for modeling the interactions of the electromagnetic fields with thermal and/or mechanical fields
in a sequentially coupled manner. See “Mapping thermal and magnetic loads,” Section 3.2.22, and
“Predefined loads for sequential coupling,” Section 16.1.3, for details.
Electromagnetic elements must be used to model the response of all the regions in an eddy current
analysis including the coil, the workpiece, and the space in between and surrounding them. To obtain
accurate solutions, the outer boundary of the space (surrounding the coil and the workpiece) being
modeled must be at least a few characteristic length scales away from the device on all sides.
The electromagnetic elements use an element edge-based interpolation of the fields instead of the
standard node-based interpolation. The user-defined nodes only define the geometry of the elements;
and the degrees of freedom of the element are not associated with these nodes, which has implications
for applying boundary conditions (see “Boundary conditions” below).
Governing field equations
The electric and magnetic fields are governed by Maxwell’s equations describing electromagnetic
phenomena. The formulation is based on the low-frequency assumption, which neglects the
displacement current correction term in Ampere’s law. This assumption is appropriate when the
wavelength of the electromagnetic waves corresponding to the excitation frequency is large compared
6.7.5–2
Abaqus Version 5.8 ID:
Printed on:
EDDY CURRENT ANALYSIS
to typical length scales over which the response is computed. In the following discussion, the governing
equations are written for a linear medium.
Time-harmonic analysis
It is convenient to introduce a magnetic vector potential, , such that the magnetic flux density vector
. The solution procedure seeks a time-harmonic electromagnetic response,
,
with frequency radians/sec when the system is subjected to a time-harmonic excitation of the same
frequency; for example, through an impressed oscillating volume current density,
. In the
preceding expressions the vectors
and
represent the amplitudes of the magnetic vector potential
and applied volume current density vector, respectively, while the exponential factors (with
)
represent the corresponding phases. Under these assumptions, Maxwell’s equations reduce to
in terms of the amplitudes of the field quantities,
and ; the magnetic permeability tensor, ; and
the electrical conductivity tensor,
. The magnetic permeability relates the magnetic flux density, ,
to the magnetic field, , through a constitutive equation of the form:
, while the electrical
conductivity relates the volume current density, , and the electric field, , by Ohm’s law:
.
The variational form of the above equation is
where
represents the variation of the magnetic vector potential, and
represents the applied
tangential surface current density, if any, at the external surfaces.
Abaqus/Standard solves the variational form of Maxwell’s equations for the in-phase (real) and
out-of-phase (imaginary) components of the magnetic vector potential. The other field quantities are
derived from the magnetic vector potential.
Transient analysis
It is convenient to introduce a magnetic vector potential, , assumed to be a function of spatial position
and time, such that the magnetic flux density vector
. The solution procedure seeks a
time-dependent electromagnetic response,
, when the system is subjected to a time-dependent
excitation; for example, through an impressed distribution of volume current density,
. Under
these assumptions, Maxwell’s equations reduce to
in terms of the field quantities,
and ; the magnetic permeability tensor, ; and the electrical
conductivity tensor,
. The magnetic permeability relates the magnetic flux density, , to the
6.7.5–3
Abaqus Version 5.8 ID:
Printed on:
EDDY CURRENT ANALYSIS
magnetic field, , through a constitutive equation of the form:
conductivity relates the volume current density, , and the electric field,
, while the electrical
, by Ohm’s law:
.
The variational form of the above equation is
where
represents the variation of the magnetic vector potential, and
tangential surface current density, if any, at the external surfaces.
represents the applied
Abaqus/Standard solves the variational form of Maxwell’s equations for the components of the
magnetic vector potential. The other field quantities are derived from the magnetic vector potential.
Defining the magnetic behavior
The magnetic behavior of the electromagnetic medium can be linear or nonlinear. However, only linear
magnetic behavior is available for time-harmonic eddy current analysis. Linear magnetic behavior is
characterized by a magnetic permeability tensor that is assumed to be independent of the magnetic field.
It is defined through direct specification of the absolute magnetic permeability tensor, , which can be
isotropic, orthotropic, or fully anisotropic (see “Magnetic permeability,” Section 26.5.3). The magnetic
permeability can also depend on temperature and/or predefined field variables. For a time-harmonic eddy
current analysis, the magnetic permeability can also depend on frequency.
Nonlinear magnetic behavior, which is available only for transient eddy current analysis,
is characterized by magnetic permeability that depends on the strength of the magnetic field. The
nonlinear magnetic material model in Abaqus is suitable for ideally soft magnetic materials characterized
by a monotonically increasing response in B–H space, where B and H refer to the strengths of the
magnetic flux density vector and the magnetic field vector, respectively. Nonlinear magnetic behavior
is defined through direct specification of one or more B–H curves that provide B as a function of H and,
optionally, temperature and/or predefined field variables, in one or more directions. Nonlinear magnetic
behavior can be isotropic, orthotropic, or transversely isotropic (which is a special case of the more
general orthotropic behavior).
Defining the electrical conductivity
The electrical conductivity,
, can be isotropic, orthotropic, or fully anisotropic (see “Electrical
conductivity,” Section 26.5.1). The electrical conductivity can also depend on temperature and/or
predefined field variables. For a time-harmonic eddy current analysis, the electrical conductivity can
also depend on frequency. Ohm’s law assumes that the electrical conductivity is independent of the
electrical field, .
6.7.5–4
Abaqus Version 5.8 ID:
Printed on:
EDDY CURRENT ANALYSIS
Time-harmonic analysis
The eddy current analysis procedure provides the time-harmonic solution directly at a given excitation
frequency. You can specify one or more excitation frequencies, one or more frequency ranges, or a
combination of excitation frequencies and ranges.
Input File Usage:
*ELECTROMAGNETIC, LOW FREQUENCY, TIME HARMONIC
lower_freq1, upper_freq1, num_pts1
lower_freq2, upper_freq2, num_pts2
...
single_freq1
single_freq2
...
For example, the following input illustrates the simplest case of specifying
excitation at a single frequency:
*ELECTROMAGNETIC, LOW FREQUENCY, TIME HARMONIC
single_freq1
Abaqus/CAE Usage:
Step module: Create Step: Linear perturbation: Electromagnetic,
Time harmonic; enter data in table, and add rows as necessary
Transient analysis
The eddy current analysis procedure provides the transient solution to a given arbitrary time-dependent
excitation.
Input File Usage:
Abaqus/CAE Usage:
*ELECTROMAGNETIC, LOW FREQUENCY, TRANSIENT
A transient eddy current analysis is not supported in Abaqus/CAE.
Tme incrementation
Time integration in the transient eddy current analysis is done with the backward Euler method. This
method is unconditionally stable for linear problems but may lead to inaccuracies if time increments
are too large. The resulting system of equations can be nonlinear in general, and Abaqus/Standard uses
Newton’s method to solve the system. The solution usually is obtained as a series of increments, with
iterations to obtain equilibrium within each increment. Increments must sometimes be kept small to
ensure accuracy of the time integration procedure. The choice of increment size is also a matter of
computational efficiency: if the increments are too large, more iterations are required. Furthermore,
Newton’s method has a finite radius of convergence; too large an increment can prevent any solution from
being obtained because the initial state is too far away from the equilibrium state that is being sought—it
is outside the radius of convergence. Thus, there is an algorithmic restriction on the increment size.
Automatic incrementation
In most cases the default automatic incrementation scheme is preferred because it will select increment
sizes based on computational efficiency. However, you must ensure that the time increments are such that
6.7.5–5
Abaqus Version 5.8 ID:
Printed on:
EDDY CURRENT ANALYSIS
the time integration results in an accurate solution. Abaqus/Standard does not have any built in checks
to ensure integration accuracy.
Input File Usage:
Abaqus/CAE Usage:
*ELECTROMAGNETIC, LOW FREQUENCY, TRANSIENT
A transient eddy current analysis is not supported in Abaqus/CAE.
Direct incrementation
Direct user control of the increment size is also provided; if you have considerable experience with a
particular problem, you may be able to select a more economical approach.
Input File Usage:
Abaqus/CAE Usage:
*ELECTROMAGNETIC, LOW FREQUENCY, TRANSIENT, DIRECT
A transient eddy current analysis is not supported in Abaqus/CAE.
Ill-conditioning in eddy current analyses with electrically nonconductive regions
In an eddy current analysis it is very common that large portions of the model consist of electrically
nonconductive regions, such as air and/or a vacuum. In such cases it is well known that the associated
stiffness matrix can be very ill-conditioned; i.e., it can have many singularities (Bíró, 1999). Abaqus
uses a special iterative solution technique to prevent the ill-conditioned matrix from negatively
impacting the computed electric and magnetic fields. The default implementation works well for many
problems. However, there can be situations in which the default numerical scheme fails to converge or
results in a noisy solution. In such cases adding a “small” amount of artificial electrical conductivity to
the nonconductive domain may help regularize the problem and allow Abaqus to converge to the correct
solution. The artificial electrical conductivity should be chosen such that the electromagnetic waves
propagating through these regions undergo little modification and, in particular, do not experience
the sharp exponential decay that is typical when such fields impinge upon a real conductor. It is
recommended that you set the artificial conductivity to be about five to eight orders of magnitude less
than that of any of the conductors in the model.
As an alternative to specifying electrical conductivity in the nonconductive domain, Abaqus also
provides a stabilization scheme to help mitigate the effects of the ill-conditioning. You can provide input
to this stabilization algorithm by specifying the stabilization factor, which is assumed to be 1.0 by default
if the stabilization scheme is used. Higher values of the stabilization factor lead to more stabilization,
while lower values of the stabilization factor lead to less stabilization.
Input File Usage:
Use the following to use stabilization in a time-harmonic procedure:
*ELECTROMAGNETIC, LOW FREQUENCY, TIME HARMONIC,
STABILIZATION=stabilization factor
Use the following to use stabilization in a transient procedure:
*ELECTROMAGNETIC, LOW FREQUENCY, TRANSIENT,
STABILIZATION=stabilization factor
6.7.5–6
Abaqus Version 5.8 ID:
Printed on:
EDDY CURRENT ANALYSIS
Initial conditions
Initial values of temperature and/or predefined field variables can be specified. These values affect only
temperature and/or field-variable-dependent material properties, if any. Initial conditions on the electric
and/or magnetic fields cannot be specified in an eddy current analysis.
Boundary conditions
Electromagnetic elements use an element edge-based interpolation of the fields. The degrees of freedom
of the element are not associated with the user-defined nodes, which only define the geometry of the
element. Consequently, the standard node-based method of specifying boundary conditions cannot
be used with electromagnetic elements. The method used for specifying boundary conditions for
electromagnetic elements is described in the following paragraphs.
Boundary conditions in Abaqus typically refer to what are traditionally known as Dirichlet-type
boundary conditions in the literature, where the values of the primary variable are known on the whole
boundary or on a portion of the boundary. The alternative, Neumann-type boundary conditions, refer
to situations where the values of the conjugate to the primary variable are known on portions of the
boundary. In Abaqus Neumann-type boundary conditions are represented as surface loads in the finiteelement formulation.
For electromagnetic boundary value problems, Dirichlet boundary conditions on an enclosing
surface must be specified as
, where is the outward normal to the surface, as discussed in
this section. Neumann boundary conditions must be specified as the surface current density vector,
, as discussed in “Loads” below.
In Abaqus Dirichlet boundary conditions are specified as magnetic vector potential, , on
(element-based) surfaces that represent symmetry planes and/or external boundaries in the model;
Abaqus computes
for the representative surfaces. In applications where the electromagnetic
fields are driven by a current-carrying coil that is close to the workpiece, the model may span a domain
that is up to 10 times the characteristic length scale associated with the coil/workpiece assembly. In
such cases, the electromagnetic fields are assumed to have decayed sufficiently in the far-field, and the
value of the magnetic vector potential can be set to zero in the far-field boundary. On the other hand, in
applications such as one where a conductor is embedded in a uniform (but varying time-harmonically
in a time-harmonic eddy current analysis or with a more general time variation in a transient eddy
current analysis) far-field magnetic field, it may be necessary to specify nonzero values of the magnetic
vector potential on some portions of the external boundary. In this case an alternative method to model
the same physical phenomena is to specify the corresponding unique value of surface current density,
, on the far-field boundary (see “Loads” below).
can be computed based on known values of the
far-field magnetic field.
A surface without any prescribed boundary condition corresponds to a surface with zero surface
currents, or no loads.
Nonuniform boundary conditions can be defined with user subroutine UDEMPOTENTIAL.
6.7.5–7
Abaqus Version 5.8 ID:
Printed on:
EDDY CURRENT ANALYSIS
Prescribing boundary conditions in a time-harmonic eddy current analysis
In a time-harmonic eddy current analysis the boundary conditions are assumed to be time harmonic and
are applied simultaneously to both the real and imaginary parts of the magnetic vector potential. It is not
possible to specify Dirichlet boundary conditions on the real parts and Neumann boundary conditions
on the imaginary parts and vice versa. Abaqus automatically restrains both the real and imaginary parts
even if only one part is prescribed explicitly. The unspecified part is assumed to have a magnitude of
zero.
When you prescribe the boundary condition on an element-based surface for a time-harmonic
eddy current analysis (see “Element-based surface definition,” Section 2.3.2), you must specify the
surface name, the region type label (S), the boundary condition type label, an optional orientation name,
the magnitude of the real part of the boundary condition, the direction vector for the real part of the
boundary condition, the magnitude of the imaginary part of the boundary condition, and the direction
vector for the imaginary part of the boundary condition. The optional orientation name defines the local
coordinate system in which the components of the magnetic vector potential are defined. By default, the
components are defined with respect to the global directions. The specified direction vector components
are normalized by Abaqus and, thus, do not contribute to the magnitude of the boundary condition.
During a time-harmonic eddy current analysis, frequency-dependent boundary conditions can be
prescribed as described in “Frequency-dependent boundary conditions in a time-harmonic eddy current
analysis” below.
Input File Usage:
Use the following option in a time-harmonic eddy current analysis to define
both the real (in-phase) and imaginary (out-of-phase) parts of the boundary
condition on element-based surfaces:
*D EM POTENTIAL
surface name, S, bc type label, orientation, magnitude of real
part, direction vector of real part, magnitude of imaginary part,
direction vector of imaginary part
where the boundary condition type label (bc type label) can be MVP for a
uniform boundary condition or MVPNU for a nonuniform boundary condition.
Abaqus/CAE Usage:
Load module: Create Boundary Condition: choose Electrical/Magnetic
for the Category and Magnetic vector potential for the Types
for Selected Step; Distribution: Uniform or User-defined;
real components + imaginary components
Prescribing boundary conditions in a transient eddy current analysis
The method of specification of the boundary condition for a transient eddy current analysis is substantially
similar to that of the time-harmonic eddy current analysis, except that the concepts of real and imaginary
are not relevant any more. In this case you specify the magnitude of the magnetic vector potential,
followed by its direction vector. The specified direction vector components are normalized by Abaqus
and, thus, do not contribute to the magnitude of the boundary condition.
6.7.5–8
Abaqus Version 5.8 ID:
Printed on:
EDDY CURRENT ANALYSIS
During a transient eddy current analysis, prescribed boundary conditions can be varied using an
amplitude definition (see “Amplitude curves,” Section 33.1.2).
Input File Usage:
Use the following option in a transient eddy current analysis to define the
boundary condition on element-based surfaces:
*D EM POTENTIAL
surface name, S, bc type label, orientation, magnitude, direction vector
where the boundary condition type label (bc type label) can be MVP for a
uniform boundary condition or MVPNU for a nonuniform boundary condition.
Abaqus/CAE Usage:
Transient eddy current analysis is not supported in Abaqus/CAE.
Frequency-dependent boundary conditions in a time-harmonic eddy current analysis
An amplitude definition can be used to specify the amplitude of a boundary condition as a function of
frequency (“Amplitude curves,” Section 33.1.2).
Input File Usage:
Use both of the following options:
Abaqus/CAE Usage:
*AMPLITUDE, NAME=name
*D EM POTENTIAL, AMPLITUDE=name
Load or Interaction module: Create Amplitude: Name: amplitude_name
Load module: Create Boundary Condition: choose Electrical/Magnetic
for the Category and Magnetic vector potential for the Types for
Selected Step; Amplitude: amplitude_name
Loads
The following types of electromagnetic loads can be applied in an eddy current analysis (see “Prescribing
electromagnetic loads for eddy current and/or magnetostatic analyses” in “Electromagnetic loads,”
Section 33.4.5, for details):
•
Element-based distributed volume current density vector:
analysis, and
in a transient eddy current analysis
in a time-harmonic eddy current
•
Surface-based distributed surface current density vector:
analysis, and
in a transient eddy current analysis
in a time-harmonic eddy current
All loads in a time-harmonic eddy current analysis are assumed to be time-harmonic with the excitation
frequency. During a transient eddy current analysis all loads can be varied using an amplitude definition
(see “Amplitude curves,” Section 33.1.2).
Nonuniform loads can be specified using user subroutines UDECURRENT and UDSECURRENT.
Frequency-dependent loading in a time-harmonic eddy current analysis
In a time-harmonic eddy current analysis, an amplitude definition can be used to specify the amplitude
of a load as a function of frequency (“Amplitude curves,” Section 33.1.2).
6.7.5–9
Abaqus Version 5.8 ID:
Printed on:
EDDY CURRENT ANALYSIS
Predefined fields
Predefined temperature and field variables can be specified in an eddy current analysis. These values
affect only temperature and/or field-variable-dependent material properties, if any. See “Predefined
fields,” Section 33.6.1.
Material options
Magnetic material behavior (see “Magnetic permeability,” Section 26.5.3) must be specified everywhere
in the model. Only linear magnetic behavior is supported in a time-harmonic eddy current analysis, but
nonlinear magnetic behavior is also supported in a transient eddy current analysis. Linear magnetic
behavior can be defined by specifying the magnetic permeability directly, while nonlinear magnetic
behavior is defined in terms of one or more B–H curves. Electrical conductivity (see “Electrical
conductivity,” Section 26.5.1) must be specified in conductor regions. All other material properties are
ignored in an eddy current analysis.
Both magnetic permeability and electrical conductivity can be functions of frequency, predefined
temperature, and field variables in a time-harmonic eddy current analysis. In a transient eddy current
analysis, all material behavior can be functions of predefined temperature and/or field variables.
Elements
Electromagnetic elements must be used to model all regions in an eddy current analysis. Unlike
conventional finite elements, which use node-based interpolation, these elements use edge-based
interpolation with the tangential components of the magnetic vector potential along element edges
serving as the primary degrees of freedom.
Electromagnetic elements are available in Abaqus/Standard in two dimensions (planar only) and
three dimensions (see “Choosing the appropriate element for an analysis type,” Section 27.1.3). The
planar elements are formulated in terms of an in-plane magnetic vector potential, thereby the magnetic
flux density and magnetic field vectors only have an out-of-plane component. The electric field and the
current density vectors are in-plane for the planar elements.
Output
Eddy current analysis provides output only to the output database (.odb) file (see “Output to the output
database,” Section 4.1.3). Output to the data (.dat) file and to the results (.fil) file is not available.
For the first four vector quantities listed below (which are derived from the magnetic vector potential and
the constitutive equations), the magnitude and components of the real and imaginary parts are output in
a time-harmonic eddy current procedure.
Element centroidal variables:
EMB
EMH
Magnitude and components of the magnetic flux density vector,
Magnitude and components of the magnetic field vector, .
EME
EMCD
Magnitude and components of the electric field vector,
Magnitude and components of the eddy current vector,
6.7.5–10
Abaqus Version 5.8 ID:
Printed on:
.
.
, in conducting regions.
EDDY CURRENT ANALYSIS
EMBF
EMBFC
EMJH
Magnetic body force intensity vector (force per unit volume per unit time) due to
flow of current.
Complex magnetic body force intensity vector (real and imaginary parts of the
force per unit volume) due to flow of current. Only available in a time-harmonic
eddy current analysis.
Rate of Joule heating (amount of heat per unit volume per unit time) due to flow
of current.
Whole element variables:
ELJD
Total rate of Joule heating (amount of heat per unit time) due to flow of current in
an element.
Whole model variables:
ALLJD
Rate of Joule heating (amount of heat per unit time) summed over the model or an
element set.
Input file template
The following is an input file template that makes use of linear magnetic material behavior in a timeharmonic eddy current analysis:
*HEADING
…
*MATERIAL, NAME=mat1
*MAGNETIC PERMEABILITY
Data lines to define magnetic permeability
*ELECTRICAL CONDUCTIVITY
Data lines to define electrical conductivity in the conductor region
**
*STEP
*ELECTROMAGNETIC, LOW FREQUENCY, TIME HARMONIC
Data line to specify excitation frequencies
*D EM POTENTIAL
Data lines to define boundary conditions on magnetic vector potential
*DECURRENT
Data lines to define element-based distributed volume current density vector
*DSECURRENT
Data lines to define surface-based distributed surface current density vector
*OUTPUT, FIELD or HISTORY
Data lines to request element-based output
*ENERGY OUTPUT
Data line to request whole model Joule heat dissipation output
*END STEP
6.7.5–11
Abaqus Version 5.8 ID:
Printed on:
EDDY CURRENT ANALYSIS
The following is an input file template that makes use of nonlinear magnetic material behavior in a
transient eddy current analysis:
*HEADING
…
*MATERIAL, NAME=mat1
*MAGNETIC PERMEABILITY, NONLINEAR
*NONLINEAR BH, DIR=direction
Data lines to define nonlinear B-H curve
*ELECTRICAL CONDUCTIVITY
Data lines to define electrical conductivity in the conductor region
**
*STEP
*ELECTROMAGNETIC, LOW FREQUENCY, TRANSIENT
*D EM POTENTIAL
Data lines to define boundary conditions on magnetic vector potential
*DECURRENT
Data lines to define element-based distributed volume current density vector
*DSECURRENT
Data lines to define surface-based distributed surface current density vector
*OUTPUT, FIELD or HISTORY
Data lines to request element-based output
*ENERGY OUTPUT
Data line to request whole model Joule heat dissipation output
*END STEP
Additional reference
•
Bíró, O., “Edge Element Formulation of Eddy Current Problems,” Computer Methods in Applied
Mechanics and Engineering, vol. 169, pp. 391–405, 1999.
6.7.5–12
Abaqus Version 5.8 ID:
Printed on:
MAGNETOSTATIC ANALYSIS
6.7.6
MAGNETOSTATIC ANALYSIS
Product: Abaqus/Standard
References
•
•
•
•
•
•
•
•
•
•
“Electromagnetic analysis procedures,” Section 6.7.1
“Magnetic permeability,” Section 26.5.3
“Electromagnetic loads,” Section 33.4.5
*MAGNETOSTATIC
*D EM POTENTIAL
*DECURRENT
*DSECURRENT
“UDECURRENT,” Section 1.1.23 of the Abaqus User Subroutines Reference Manual
“UDEMPOTENTIAL,” Section 1.1.24 of the Abaqus User Subroutines Reference Manual
“UDSECURRENT,” Section 1.1.26 of the Abaqus User Subroutines Reference Manual
Overview
Magnetostatic problems:
•
•
•
•
•
•
solve the magnetostatic approximation of Maxwell’s equations describing electromagnetic
phenomena and compute the magnetic fields due to direct currents;
involve only magnetic fields, which are assumed to be vary slowly in time such that electromagnetic
coupling can be neglected;
require the use of electromagnetic elements in the whole domain;
require that magnetic permeability is specified in the whole domain;
can be solved with nonlinear magnetic behavior; and
can be solved using continuum elements in two- and three-dimensional space.
Magnetostatic analysis
A direct current creates a static magnetic field in the space surrounding the current carrying region.
For applications where the magnitude of the direct current can be assumed to be a constant or to vary
slowly with time, coupling between magnetic and electric fields can be neglected. The magnetostatic
approximation to Maxwell’s equations involves the magnetic fields only. Magnetostatic analysis
provides a solution for applications where the above assumptions are valid.
Electromagnetic elements must be used to model the response of all the regions in a magnetostatic
analysis, including regions such as current carrying coils and the surrounding space. To obtain accurate
solutions, the outer boundary of the space being modeled must be at least a few characteristic length
scales away from the region of interest on all sides.
6.7.6–1
Abaqus Version 5.8 ID:
Printed on:
MAGNETOSTATIC ANALYSIS
Electromagnetic elements use an element edge-based interpolation of the fields instead of the
standard node-based interpolation. The user-defined nodes only define the geometry of the elements;
and the degrees of freedom of the element are not associated with these nodes, which has implications
for applying boundary conditions (see “Boundary conditions” below).
Governing field equations
The magnetic fields are governed by the magnetostatic approximation to Maxwell’s equations describing
electromagnetic phenomena.
It is convenient to introduce a magnetic vector potential, , such that the magnetic flux density
vector
. The solution procedure seeks a static magnetic response due to, for example, an
impressed direct volume current density distribution, in some regions of the model. The magnetostatic
approximation to Maxwell’s equations is given by
in terms of the field quantities,
and
and the magnetic permeability tensor, . The magnetic
permeability relates the magnetic flux density, , to the magnetic field, , through a constitutive
equation of the form:
.
The variational form of the above equation is
where
represents the variation of the magnetic vector potential, and
represents the applied
tangential surface current density, if any, at the external surfaces.
Abaqus/Standard solves the variational form of Maxwell’s equations for the components of the
magnetic vector potential. The other field quantities are derived from the magnetic vector potential. In
the following discussion, the governing equations are written for a linear medium.
Defining the magnetic behavior
The magnetic behavior of the electromagnetic medium can be linear or nonlinear. Linear magnetic
behavior is characterized by a magnetic permeability tensor that is assumed to be independent of the
magnetic field. It is defined through direct specification of the absolute magnetic permeability tensor, ,
which can be isotropic, orthotropic, or fully anisotropic (see “Magnetic permeability,” Section 26.5.3).
The magnetic permeability can also depend on temperature and/or predefined field variables.
Nonlinear magnetic behavior is characterized by magnetic permeability that depends on the strength
of the magnetic field. The nonlinear magnetic material model in Abaqus is suitable for ideally soft
magnetic materials characterized by a monotonically increasing response in B–H space, where B and
H refer to the strengths of the magnetic flux density vector and the magnetic field vector, respectively.
Nonlinear magnetic behavior is defined through direct specification of one or more B–H curves that
provide B as a function of H and, optionally, temperature and/or predefined field variables, in one or
more directions. Nonlinear magnetic behavior can be isotropic, orthotropic, or transversely isotropic
(which is a special case of the more general orthotropic behavior).
6.7.6–2
Abaqus Version 5.8 ID:
Printed on:
MAGNETOSTATIC ANALYSIS
Magnetostatic analysis
Magnetostatic analysis provides the magnetic flux density and the magnetic field at a given value of the
impressed direct current.
Input File Usage:
*MAGNETOSTATIC
Ill-conditioning in magnetostatic analyses
In magnetostatic analysis the stiffness matrix can be very ill-conditioned; i.e., it can have many
singularities. Abaqus uses a special iterative solution technique to prevent the ill-conditioned matrix
from negatively impacting the computed magnetic fields. The default implementation works well
for many problems. However, there can be situations in which the default numerical scheme fails to
converge. Abaqus provides a stabilization scheme to help mitigate the effects of the ill-conditioning.
You can provide input to this stabilization algorithm by specifying the stabilization factor, which is
assumed to be 1.0 by default if the stabilization scheme is used. Higher values of the stabilization factor
lead to more stabilization, while lower values of the stabilization factor lead to less stabilization.
Input File Usage:
*MAGNETOSTATIC, STABILIZATION=stabilization factor
Initial conditions
Initial values of temperature and/or predefined field variables can be specified. These values affect only
temperature and/or field-variable-dependent material properties, if any. Initial conditions on magnetic
fields cannot be specified in a magnetostatic analysis.
Boundary conditions
Electromagnetic elements use an element edge-based interpolation of the fields. The degrees of freedom
of the element are not associated with the user-defined nodes, which only define the geometry of the
element. Consequently, the standard node-based method of specifying boundary conditions cannot be
used with electromagnetic elements.
Boundary conditions in Abaqus typically refer to what are traditionally known as Dirichlet-type
boundary conditions in the literature, where the values of the primary variable are known on the whole
boundary or on a portion of the boundary. The alternative, Neumann-type boundary conditions, refer
to situations where the values of the conjugate to the primary variable are known on portions of the
boundary. In Abaqus, Neumann-type boundary conditions are represented as surface loads in the finite
element formulation.
For electromagnetic boundary value problems, including magnetostatic problems, Dirichlet
boundary conditions on an enclosing surface must be specified as
, where is the outward
normal to the surface, as discussed in this section. Neumann boundary conditions must be specified as
the surface current density vector,
, as discussed in “Loads” below.
6.7.6–3
Abaqus Version 5.8 ID:
Printed on:
MAGNETOSTATIC ANALYSIS
In Abaqus, Dirichlet boundary conditions are specified as magnetic vector potential, , on
(element-based) surfaces that represent symmetry planes and/or external boundaries in the model;
Abaqus computes
for the representative surfaces. The model may span a domain that is up to 10
times some characteristic length scale for the problem. In such cases the magnetic fields are assumed
to have decayed sufficiently in the far-field, and the value of the magnetic vector potential can be set to
zero in the far-field boundary. On the other hand, in applications such as one where a magnetic material
is embedded in a uniform far-field magnetic field, it may be necessary to specify nonzero values of the
magnetic vector potential on some portions of the external boundary. In this case an alternative method
to model the same physical phenomena is to specify the corresponding unique value of surface current
density, , on the far-field boundary (see “Loads” below).
can be computed based on known values
of the far-field magnetic field.
In a magnetostatic analysis the boundary conditions are assumed to be either constant or varying
slowly with time. The time variation can be specified using an amplitude definition (“Amplitude curves,”
Section 33.1.2)
A surface without any prescribed boundary condition corresponds to a surface with zero surface
currents or no loads.
When you prescribe the boundary condition on an element-based surface (see “Element-based
surface definition,” Section 2.3.2), you must specify the surface name, the region type label (S), the
boundary condition type label, an optional orientation name, the magnitude of the magnetic vector
potential, and the direction vector for the magnetic vector potential. The optional orientation name
defines the local coordinate system in which the components of the magnetic vector potential are
defined. By default, the components are defined with respect to the global directions.
The specified vector components are normalized by Abaqus and, thus, do not contribute to the
magnitude of the boundary condition.
Nonuniform boundary conditions can be defined with user subroutine UDEMPOTENTIAL.
Input File Usage:
Use the following option to define both the real (in-phase) and imaginary (outof-phase) parts of the boundary condition on element-based surfaces:
*D EM POTENTIAL
surface name, S, bc type label, orientation, magnitude, direction vector
where the boundary condition type label (bc type label) can be MVP for a
uniform boundary condition or MVPNU for a nonuniform boundary condition.
Loads
The following types of electromagnetic loads can be applied in a magnetostatic analysis (see
“Prescribing electromagnetic loads for eddy current and/or magnetostatic analyses” in “Electromagnetic
loads,” Section 33.4.5, for details):
•
•
Element-based distributed volume current density vector,
Surface-based distributed surface current density vector,
During the analysis the prescribed load can be varied using an amplitude definition (“Amplitude curves,”
Section 33.1.2).
6.7.6–4
Abaqus Version 5.8 ID:
Printed on:
MAGNETOSTATIC ANALYSIS
Predefined fields
Predefined temperature and field variables can be specified in a magnetostatic analysis. These values
affect only temperature and/or field-variable-dependent material properties, if any. See “Predefined
fields,” Section 33.6.1.
Material options
The magnetic behavior (see “Magnetic permeability,” Section 26.5.3) must be defined everywhere in the
model, either by specifying the absolute magnetic permeability tensor for linear magnetic behavior or by
specifying the B–H curve-based response for nonlinear magnetic behavior. All other material properties,
including electrical conductivity, are ignored in a magnetostatic analysis. The magnetic behavior can be
functions of predefined temperature and/or field variables.
Elements
Electromagnetic elements must be used to model all regions in a magnetostatic analysis. Unlike
conventional finite elements, which use node-based interpolation, these elements use edge-based
interpolation with the tangential components of the magnetic vector potential along element edges
serving as the primary degrees of freedom.
Electromagnetic elements are available in Abaqus/Standard in two dimensions (planar only) and
three dimensions (see “Choosing the appropriate element for an analysis type,” Section 27.1.3). The
planar elements are formulated in terms of an in-plane magnetic vector potential, thereby the magnetic
flux density and magnetic field vectors have only an out-of-plane component.
Output
Magnetostatic analysis provides output only to the output database (.odb) file (see “Output to the output
database,” Section 4.1.3). Output to the data (.dat) file and to the results (.fil) file is not available.
Element centroidal variables:
EMB
EMH
Magnitude and components of the magnetic flux density vector,
Magnitude and components of the magnetic field vector, .
.
Input file template
*HEADING
…
*MATERIAL, NAME=mat1
*MAGNETIC PERMEABILITY, NONLINEAR
Data lines to define magnetic permeability for linear magnetic behavior; no data required here for
nonlinear magnetic behavior
*NONLINEAR BH, DIR=direction
Data lines to define nonlinear B-H curve
6.7.6–5
Abaqus Version 5.8 ID:
Printed on:
MAGNETOSTATIC ANALYSIS
**
*STEP
*MAGNETOSTATIC
Data line to define time incrementation
*D EM POTENTIAL
Data lines to define boundary conditions on magnetic vector potential
*DECURRENT
Data lines to define element-based distributed volume current density vector
*DSECURRENT
Data lines to define surface-based distributed surface current density vector
*OUTPUT, FIELD or HISTORY
Data lines to request element-based output
*END STEP
6.7.6–6
Abaqus Version 5.8 ID:
Printed on:
COUPLED PORE FLUID FLOW AND STRESS ANALYSIS
6.8
Coupled pore fluid flow and stress analysis
•
•
“Coupled pore fluid diffusion and stress analysis,” Section 6.8.1
“Geostatic stress state,” Section 6.8.2
6.8–1
Abaqus Version 5.8 ID:
Printed on:
COUPLED DIFFUSION/STRESS ANALYSIS
6.8.1
COUPLED PORE FLUID DIFFUSION AND STRESS ANALYSIS
Products: Abaqus/Standard
Abaqus/CAE
References
•
•
•
•
•
“Defining an analysis,” Section 6.1.2
“Pore fluid flow properties,” Section 26.6.1
*SOILS
“Defining pore fluid expansion” in “Defining a fluid-filled porous material,” Section 12.12.3 of the
Abaqus/CAE User’s Manual, in the online HTML version of this manual
“Configuring an effective stress analysis for fluid-filled porous media” in “Configuring general
analysis procedures,” Section 14.11.1 of the Abaqus/CAE User’s Manual, in the online HTML
version of this manual
Overview
A coupled pore fluid diffusion/stress analysis:
•
•
•
•
•
•
•
is used to model single phase, partially or fully saturated fluid flow through porous media;
can be performed in terms of either total pore pressure or excess pore pressure by including or
excluding the pore fluid weight;
requires the use of pore pressure elements with associated pore fluid flow properties defined;
can, optionally, also model heat transfer due to conduction in the soil skeleton and the pore fluid, and
convection due to the flow of the pore fluid, through the use of coupled temperature–pore pressure
displacement elements;
can be transient or steady-state;
can be linear or nonlinear; and
can include pore pressure contact between bodies (see “Pore fluid contact properties,”
Section 36.4.1).
Typical applications
Some of the more common coupled pore fluid diffusion/stress (and, optionally, thermal) analysis
problems that can be analyzed with Abaqus/Standard are:
•
•
Soil mechanics problems generally involve fully saturated flow, since the solid
is fully saturated with ground water. Typical examples of saturated flow include consolidation of
soils under foundations and excavation of tunnels in saturated soil.
Partially saturated flow: Partially saturated flow occurs when the wetting liquid is absorbed
into or exsorbed from the medium by capillary action. Irrigation and hydrology problems generally
include partially saturated flow.
Saturated flow:
6.8.1–1
Abaqus Version 5.8 ID:
Printed on:
COUPLED DIFFUSION/STRESS ANALYSIS
•
•
•
Combined flow: Combined fully saturated and partially saturated flow occurs in problems such
as seepage of water through an earth dam, where the position of the phreatic surface (the boundary
between fully saturated and partially saturated soil) is of interest.
Moisture migration: Although not normally associated with soil mechanics, moisture migration
problems can also be solved using the coupled pore fluid diffusion/stress procedure. These problems
may involve partially saturated flow in polymeric materials such as paper towels and sponge-like
materials; in the biomedical industry they may also involve saturated flow in hydrated soft tissues.
Combined heat transfer and pore fluid flow: In some applications, such as a source of heat
buried in soil, it is important to model the coupling between the mechanical deformation, pore
fluid flow, and heat transfer. In such problems the difference in the thermal expansion coefficients
between the soil and the pore fluid often plays an important role in determining the rate of diffusion
of the pore fluid and heat from the source.
Flow through porous media
A porous medium is modeled in Abaqus/Standard by a conventional approach that considers the medium
as a multiphase material and adopts an effective stress principle to describe its behavior. The porous
medium modeling provided considers the presence of two fluids in the medium. One is the “wetting
liquid,” which is assumed to be relatively (but not entirely) incompressible. Often the other is a gas,
which is relatively compressible. An example of such a system is soil containing ground water. When
the medium is partially saturated, both fluids exist at a point; when it is fully saturated, the voids are
completely filled with the wetting liquid. The elementary volume,
, is made up of a volume of grains
of solid material,
; a volume of voids,
; and a volume of wetting liquid,
, that is free
to move through the medium if driven. In some systems (for example, systems containing particles that
absorb the wetting liquid and swell in the process) there may also be a significant volume of trapped
wetting liquid,
.
The porous medium is modeled by attaching the finite element mesh to the solid phase; fluid can
flow through this mesh. The mechanical part of the model is based on the effective stress principle
defined in “Effective stress principle for porous media,” Section 2.8.1 of the Abaqus Theory Manual.
The model also uses a continuity equation for the mass of wetting fluid in a unit volume of the
medium. This equation is described in “Continuity statement for the wetting liquid phase in a porous
medium,” Section 2.8.4 of the Abaqus Theory Manual. It is written with pore pressure (the average
pressure in the wetting fluid at a point in the porous medium) as the basic variable (degree of freedom 8
at the nodes). The conjugate flux variable is the volumetric flow rate at the node, . The porous medium
is partially saturated when the pore liquid pressure,
, is negative.
Coupled flow and heat transfer through porous media
Optionally, heat transfer due to conduction in the soil skeleton and pore fluid, as well as convection in
the pore fluid, can also be modeled. This capability represents an enhancement to the basic pore fluid
flow capabilities discussed in the earlier paragraphs and requires the use of coupled temperature–pore
pressure elements that have temperature as an additional degree of freedom (degree of freedom 11
at the nodes) in addition to the pore pressure and the displacement components. When you use the
6.8.1–2
Abaqus Version 5.8 ID:
Printed on:
COUPLED DIFFUSION/STRESS ANALYSIS
coupled temperature–pore pressure elements, Abaqus solves the heat transfer equation in addition to
and in a fully coupled manner with the continuity equation and the mechanical equilibrium equations.
Only linear brick, first-order axisymmetric, and second-order modified tetrahedrons are available
for modeling coupled heat transfer with pore fluid flow and mechanical deformation. Coupled
temperature–pore pressure elements are not supported in Abaqus/CAE.
Total and excess pore fluid pressure
The coupled pore fluid diffusion/stress analysis capability can provide solutions either in terms of total
or “excess” pore fluid pressure. The excess pore fluid pressure at a point is the pore fluid pressure in
excess of the hydrostatic pressure required to support the weight of pore fluid above the elevation of the
material point. The difference between total and excess pore pressure is relevant only for cases in which
gravitational loading is important; for example, when the loading provided by the hydrostatic pressure
in the pore fluid is large or when effects like “wicking” (transient capillary suction of liquid into a dry
column) are being studied. Total pore pressure solutions are provided when the gravity distributed load
is used to define the gravity load on the model. Excess pore pressure solutions are provided in all other
cases; for example, when gravity loading is defined with body force distributed loads.
Steady-state analysis
Steady-state coupled pore pressure/effective stress analysis assumes that there are no transient effects in
the wetting liquid continuity equation; that is, the steady-state solution corresponds to constant wetting
liquid velocities and constant volume of wetting liquid per unit volume in the continuum. Thus, for
example, thermal expansion of the liquid phase has no effect on the steady-state solution: it is a transient
effect. Therefore, the time scale chosen during steady-state analysis is relevant only to rate effects in the
constitutive model used for the porous medium (excluding creep and viscoelasticity, which are disabled
in steady-state analysis).
Mechanical loads and boundary conditions can be changed gradually over the step by referring to
an amplitude curve to accommodate possible geometric nonlinearities in the response.
The steady-state coupled equations are strongly unsymmetric; therefore, the unsymmetric matrix
solution and storage scheme is used automatically for steady-state analysis steps (see “Defining an
analysis,” Section 6.1.2).
If heat transfer is modeled using the coupled temperature–pore pressure elements, the steady-state
solution neglects all transient effects in the heat transfer equation and provides only the steady-state
temperature distribution.
Input File Usage:
Abaqus/CAE Usage:
*SOILS
Step module: Create Step: General: Soils: Basic: Pore
fluid response: Steady state
Incrementation
You can specify a fixed time increment size in a coupled pore fluid diffusion/stress analysis, or
Abaqus/Standard can select the time increment size automatically. Automatic incrementation is
6.8.1–3
Abaqus Version 5.8 ID:
Printed on:
COUPLED DIFFUSION/STRESS ANALYSIS
recommended because the time increments in a typical diffusion analysis can increase by several
orders of magnitude during the simulation. If you do not activate automatic incrementation, fixed time
increments will be used.
Input File Usage:
Use the following option to activate automatic incrementation in steady-state
analysis:
*SOILS, UTOL=any arbitrary nonzero value
The solution does not depend on the value specified for UTOL; this value is
simply a flag for automatic incrementation.
Abaqus/CAE Usage:
Step module: Create Step: General: Soils: Basic: Pore fluid response:
Steady state; Incrementation: Type: Automatic
Transient analysis
In a transient coupled pore pressure/effective stress analysis the backward difference operator is used to
integrate the continuity equation and the heat transfer equation (if heat transfer is modeled): this operator
provides unconditional stability so that the only concern with respect to time integration is accuracy. You
can provide the time increments, or they can be selected automatically.
The coupled partially saturated flow equations are strongly unsymmetric, so the unsymmetric solver
is used automatically if you request partially saturated analysis (by including absorption/exsorption
behavior in the material definition). The unsymmetric solver is also activated automatically when
gravity distributed loading is used during a soils consolidation analysis.
For fully saturated flow analyses in which finite-sliding coupled pore pressure-displacement contact
is modeled using contact pairs, certain contributions to the model’s stiffness matrix are unsymmetric.
Using the unsymmetric solver can sometimes improve convergence in such cases since Abaqus does not
automatically do so.
For fully saturated flow analyses in which heat transfer is also modeled, the contributions to the
model’s stiffness matrix arising from convective heat transfer due to pore fluid flow are unsymmetric.
Using the unsymmetric solver can sometimes improve convergence in such cases since Abaqus does not
automatically do so.
Spurious oscillations due to small time increments
The integration procedure used in Abaqus/Standard for consolidation analysis introduces a relationship
between the minimum usable time increment and the element size, as shown below for fully saturated and
partially saturated flows. If time increments smaller than these values are used, spurious oscillations may
appear in the solution (except for partially saturated cases when linear elements or modified triangular
elements are used; in these cases Abaqus/Standard uses a special integration scheme for the wetting liquid
storage term to avoid the problem). These nonphysical oscillations may cause problems if pressuresensitive plasticity is used to model the porous medium and may lead to convergence difficulties in
partially saturated analyses. If the problem requires analysis with smaller time increments than the
relationships given below allow, a finer mesh is required. Generally there is no upper limit on the time
6.8.1–4
Abaqus Version 5.8 ID:
Printed on:
COUPLED DIFFUSION/STRESS ANALYSIS
step except accuracy, since the integration procedure is unconditionally stable unless nonlinearities cause
convergence problems.
Fully saturated flow
A simple guideline that can be used for the minimum usable time increment in the case of fully saturated
flow is
where
E
is the time increment,
is the specific weight of the wetting liquid,
is the Young’s modulus of the soil,
is the permeability of the soil (see “Permeability,” Section 26.6.2),
is the magnitude of the velocity of the pore fluid,
is the velocity coefficient in Forchheimer’s flow law (
in the case of Darcy flow),
is the bulk modulus of the solid grains (see “Porous bulk moduli,” Section 26.6.3), and
is a typical element dimension.
Partially saturated flow
In partially saturated flow cases the corresponding guideline for the minimum time increment is
where
s
is the saturation;
is the permeability-saturation relationship;
is the rate of change of saturation with respect to pore pressure (see “Sorption,”
Section 26.6.4);
is the initial porosity of the material; and the other parameters are as defined for the case of
fully saturated flow.
Fixed incrementation
If you choose fixed time incrementation, fixed time increments equal to the size of the user-specified
initial time increment,
, will be used. Fixed incrementation is not generally recommended because
the time increments in a typical diffusion analysis can increase over several orders of magnitude during
the simulation; automatic incrementation is usually a better choice.
6.8.1–5
Abaqus Version 5.8 ID:
Printed on:
COUPLED DIFFUSION/STRESS ANALYSIS
Input File Usage:
*SOILS, CONSOLIDATION
Abaqus/CAE Usage:
Step module: Create Step: General: Soils: Basic: Pore fluid
response: Transient consolidation; Incrementation: Type:
Fixed, Increment size:
Automatic incrementation
If you choose automatic time incrementation, you must specify two (three if heat transfer is also modeled)
tolerance parameters.
The accuracy of the time integration of the flow continuity equations is governed by the maximum
wetting liquid pore pressure change,
, allowed in an increment. Abaqus/Standard restricts the time
increments to ensure that this value is not exceeded at any node (except nodes with boundary conditions)
during any increment in the analysis.
If heat transfer is modeled, the accuracy of time integration is also governed by the maximum
temperature change,
, allowed in an increment. Abaqus/Standard restricts the time increments to
ensure that this value is not exceeded at any node (except nodes with boundary conditions) during any
increment of the analysis.
The accuracy of the integration of the time-dependent (creep) material behavior is governed by the
maximum strain rate change allowed at any point during an increment,
, as
described in “Rate-dependent plasticity: creep and swelling,” Section 23.2.4.
Input File Usage:
If heat transfer is not modeled:
*SOILS, CONSOLIDATION, UTOL=
, , CETOL=errtol
If heat transfer is modeled:
*SOILS, CONSOLIDATION, UTOL=
CETOL=errtol
Abaqus/CAE Usage:
, DELTMX=
Step module: Create Step: General: Soils: Basic: Pore fluid
response: Transient consolidation; Incrementation: Type:
Automatic, Max. pore pressure change per increment:
Creep/swelling/viscoelastic strain error tolerance: errtol
,
,
Specifying the maximum temperature change per increment is not supported in
Abaqus/CAE.
Ending a transient analysis
Transient soils analysis can be terminated by completing a specified time period, or it can be continued
until steady-state conditions are reached. By default, the analysis will end when the given time period has
been completed. Alternatively, you can specify that the analysis will end when steady state is reached or
the time period ends, whichever comes first. When heat transfer is not modeled, steady state is defined by
a maximum permitted rate of change of pore pressure with time: when all pore pressures are changing at
less than the user-defined rate, the analysis terminates. However, with heat transfer included, the analysis
6.8.1–6
Abaqus Version 5.8 ID:
Printed on:
COUPLED DIFFUSION/STRESS ANALYSIS
terminates only when both the pore pressure and temperature are changing at less than the user-defined
rates.
Input File Usage:
Use the following option to end the analysis when the time period is reached:
*SOILS, CONSOLIDATION, END=PERIOD (default)
Use the following option to end the analysis based on the pore pressure and, if
heat transfer is modeled, temperature change rate:
Abaqus/CAE Usage:
*SOILS, CONSOLIDATION, END=SS
Step module: Create Step: General: Soils: Basic: Pore fluid
response: Transient consolidation; Incrementation: End step
when pore pressure change rate is less than
If heat transfer is modeled, directly specifying the temperature change rate to
define steady state is not supported in Abaqus/CAE.
Neglecting creep during a transient analysis
You can specify that creep or viscoelastic response should be neglected during a consolidation analysis,
even if creep or viscoelastic material properties have been defined.
Input File Usage:
Abaqus/CAE Usage:
*SOILS, CONSOLIDATION, CREEP=NONE
Step module: Create Step: General: Soils: Basic: Pore
fluid response: Transient consolidation, toggle off Include
creep/swelling/viscoelastic behavior
Unstable problems
Some types of analyses may develop local instabilities, such as surface wrinkling, material instability,
or local buckling. In such cases it may not be possible to obtain a quasi-static solution, even with the aid
of automatic incrementation. Abaqus/Standard offers the option to stabilize this class of problems by
applying damping throughout the model in such a way that the viscous forces introduced are sufficiently
large to prevent instantaneous buckling or collapse but small enough not to affect the behavior
significantly while the problem is stable. The available automatic stabilization schemes are described in
detail in “Automatic stabilization of unstable problems” in “Solving nonlinear problems,” Section 7.1.1.
Optional modeling of coupled heat transfer
When coupled temperature–pore pressure elements are used, heat transfer is modeled in these elements
by default. However, you may optionally choose to switch off heat transfer within these elements during
some steps in the analysis. This feature may be helpful in reducing computation time during certain
phases in the analysis when heat transfer is not an important part of the overall physics of the problem.
Input File Usage:
Use the following option either during a transient or a steady-state procedure
to suppress heat transfer modeling:
*SOILS, CONSOLIDATION, HEAT=NO
6.8.1–7
Abaqus Version 5.8 ID:
Printed on:
COUPLED DIFFUSION/STRESS ANALYSIS
Abaqus/CAE Usage:
Switching off the heat transfer part of the physics is not supported in
Abaqus/CAE.
Units
In coupled problems where two or more different fields are being solved, you must be careful when
choosing the units of the problem. If the choice of units is such that the numbers generated by the
equations for the different fields differ by many orders of magnitude, the precision on some computers
may be insufficient to resolve the numerical ill-conditioning of the coupled equations. Therefore, choose
units that avoid badly conditioned matrices. For example, consider using units of Mpascal instead of
pascal for the stress equilibrium equations to reduce the disparity between the magnitudes of the stress
equilibrium equations and the pore flow continuity equations.
Initial conditions
Initial conditions can be applied as defined in “Initial conditions in Abaqus/Standard and
Abaqus/Explicit,” Section 33.2.1.
Defining initial pore fluid pressures
Initial values of pore fluid pressures,
, can be defined at the nodes.
Input File Usage:
*INITIAL CONDITIONS, TYPE=PORE PRESSURE
Abaqus/CAE Usage:
Load module: Create Predefined Field: Step: Initial: choose Other for the
Category and Pore pressure for the Types for Selected Step
Defining initial void ratios
Initial values of the void ratio, e, can be given at the nodes. The void ratio is defined as the ratio
of the volume of voids to the volume of solid material (see “Effective stress principle for porous
media,” Section 2.8.1 of the Abaqus Theory Manual). The evolution of void ratio is governed by the
deformation of the different phases of the material, as discussed in detail in “Constitutive behavior in a
porous medium,” Section 2.8.3 of the Abaqus Theory Manual.
Input File Usage:
Abaqus/CAE Usage:
*INITIAL CONDITIONS, TYPE=RATIO
Load module: Create Predefined Field: Step: Initial: choose Other for
the Category and Void ratio for the Types for Selected Step
Defining initial saturation
Initial saturation values, s, can be given at the nodes. Saturation is defined as the ratio of wetting fluid
volume to void volume (see “Effective stress principle for porous media,” Section 2.8.1 of the Abaqus
Theory Manual).
Input File Usage:
Abaqus/CAE Usage:
*INITIAL CONDITIONS, TYPE=SATURATION
Load module: Create Predefined Field: Step: Initial: choose Other for
the Category and Saturation for the Types for Selected Step
6.8.1–8
Abaqus Version 5.8 ID:
Printed on:
COUPLED DIFFUSION/STRESS ANALYSIS
Defining initial stresses
An initial (effective) stress field can be specified (see “Initial conditions in Abaqus/Standard and
Abaqus/Explicit,” Section 33.2.1).
Most geotechnical problems begin from a geostatic state, which is a steady-state equilibrium
configuration of the undisturbed soil or rock body under geostatic loading and usually includes both
horizontal and vertical components. It is important to establish these initial conditions correctly so
that the problem begins from an equilibrium state. The geostatic procedure can be used to verify that
the user-defined initial stresses are indeed in equilibrium with the given geostatic loads and boundary
conditions (see “Geostatic stress state,” Section 6.8.2).
Input File Usage:
Use one of the following options:
Abaqus/CAE Usage:
*INITIAL CONDITIONS, TYPE=STRESS
*INITIAL CONDITIONS, TYPE=STRESS, GEOSTATIC
Load module: Create Predefined Field: Step: Initial: choose
Mechanical for the Category and Stress or Geostatic stress
for the Types for Selected Step
Defining initial temperature
Initial temperature values can be defined at the nodes.
Input File Usage:
Abaqus/CAE Usage:
*INITIAL CONDITIONS, TYPE=TEMPERATURE
Load module: Create Predefined Field: Step: Initial: choose Other for
the Category and Temperature for the Types for Selected Step
Boundary conditions
Boundary conditions can be applied to displacement degrees of freedom 1–6 and to pore pressure degree
of freedom 8 (“Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1). In
addition, boundary conditions can also be applied to temperature degree of freedom 11 if heat transfer
is modeled using coupled temperature–pore pressure elements. During the analysis prescribed boundary
conditions can be varied by referring to an amplitude curve (“Amplitude curves,” Section 33.1.2). If
no amplitude reference is given, the default variation of a boundary condition in a coupled pore fluid
diffusion/stress analysis step is as defined in “Defining an analysis,” Section 6.1.2.
If the pore pressure is prescribed with a boundary condition, fluid is assumed to enter and leave
through the node as needed to maintain the prescribed pressure. Likewise, if the temperature is prescribed
with a boundary condition, heat is assumed to enter and leave through the node as needed to maintain
the prescribed temperature.
Loads
The following loading types can be prescribed in a coupled pore fluid diffusion/stress analysis:
6.8.1–9
Abaqus Version 5.8 ID:
Printed on:
COUPLED DIFFUSION/STRESS ANALYSIS
•
•
•
Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6); see
“Concentrated loads,” Section 33.4.2.
Distributed pressure forces or body forces can be applied; see “Distributed loads,” Section 33.4.3.
The distributed load types available with particular elements are described in Part VI, “Elements.”
The magnitude and direction of gravitational loading are usually defined by using the gravity
distributed load type.
Pore fluid flow is controlled as described in “Pore fluid flow,” Section 33.4.7.
If heat transfer is modeled, the following types of thermal loading can also be prescribed (“Thermal
loads,” Section 33.4.4). These loads are not supported in Abaqus/CAE during a coupled thermal pore
pressure/stress analysis.
•
•
•
Concentrated heat fluxes.
Body fluxes and distributed surface fluxes.
Convective film conditions and radiation conditions; film properties can be made a function of
temperature.
Predefined fields
The following predefined fields can be prescribed, as described in “Predefined fields,” Section 33.6.1:
•
•
•
For a coupled pore fluid diffusion/stress analysis that does not model heat transfer and uses regular
pore pressure elements, temperature is not a degree of freedom and nodal temperatures can be
specified. Any difference between the applied and initial temperatures will cause thermal strain
if a thermal expansion coefficient is given for the material (“Thermal expansion,” Section 26.1.2).
The specified temperature also affects temperature-dependent material properties, if any.
Predefined temperature fields are not allowed in coupled pore fluid diffusion/stress analysis that
also models heat transfer. Boundary conditions should be used instead to specify temperatures, as
described earlier.
The values of user-defined field variables can be specified; these values affect only field-variabledependent material properties, if any.
Material options
Any of the mechanical constitutive models available in Abaqus/Standard can be used to model the porous
material.
In problems formulated in terms of total pore pressure, you must include the density of the dry
material in the material definition (see “Density,” Section 21.2.1).
You can use a permeability material property to define the specific weight of the wetting liquid, ;
the permeability, , and its dependence on the void ratio, e, and saturation, ; and the flow velocity,
(see “Permeability,” Section 26.6.2).
You can define the compressibility of the solid grains and of the permeating fluid in both fully and
partially saturated flow problems (see “Elastic behavior of porous materials,” Section 22.3.1). If you do
not specify the porous bulk moduli, the materials are assumed to be fully incompressible.
6.8.1–10
Abaqus Version 5.8 ID:
Printed on:
COUPLED DIFFUSION/STRESS ANALYSIS
For partially saturated flow you must define the porous medium’s absorption/exsorption behavior
(see “Sorption,” Section 26.6.4).
Gel swelling (“Swelling gel,” Section 26.6.5) and volumetric moisture swelling of the solid
skeleton (“Moisture swelling,” Section 26.6.6) can be included in partially saturated cases. These
effects are usually associated with modeling of moisture migration in polymeric systems rather than
with geotechnical systems.
Thermal properties if heat transfer is modeled
In problems that model heat transfer, the thermal conductivity for either the solid material or the
permeating fluid, or more commonly for both phases, must be defined. Only isotropic conductivity
can be specified for the pore fluid. The specific heat and density of the phases must also be defined
for transient heat transfer problems. Latent heat for the phases can be defined if changes in internal
energy due to phase changes are important. See “Thermal properties: overview,” Section 26.2.1, for
details on defining thermal properties in Abaqus. Examples of problems that model fully coupled heat
transfer along with pore fluid diffusion and mechanical deformation can be found in “Consolidation
around a cylindrical heat source,” Section 1.15.7 of the Abaqus Benchmarks Manual, and “Permafrost
thawing–pipeline interaction,” Section 10.1.6 of the Abaqus Example Problems Manual.
The thermal properties can be defined separately for the solid material and the permeating fluid.
Input File Usage:
To define the conductivity, specific heat, density, and latent heat of the
permeating fluid, use the following options:
*CONDUCTIVITY, TYPE=ISO, PORE FLUID
*SPECIFIC HEAT, PORE FLUID
*LATENT HEAT, PORE FLUID
*DENSITY, PORE FLUID
To define the conductivity, specific heat, density, and latent heat of the solid
material, use the following options:
Abaqus/CAE Usage:
*EXPANSION, TYPE=ISO or ORTHO or ANISO
*SPECIFIC HEAT
*DENSITY
*LATENT HEAT
Defining the thermal properties and the density of the permeating fluid is not
supported in Abaqus/CAE.
To define the conductivity, specific heat, density, and latent heat of the solid
material, use the following options:
Property module: material editor:
Thermal→Conductivity: Type: Isotropic
Thermal→Specific Heat
General→Density
Thermal→Latent Heat
6.8.1–11
Abaqus Version 5.8 ID:
Printed on:
COUPLED DIFFUSION/STRESS ANALYSIS
Thermal expansion
Thermal expansion can be defined separately for the solid material and for the permeating fluid. In such
a case you should repeat the expansion material property, with the necessary parameters, to define the
different thermal expansion effects (see “Thermal expansion,” Section 26.1.2). Thermal expansion will
be active only in a consolidation (transient) analysis.
To define the thermal expansion of the permeating fluid:
Input File Usage:
*EXPANSION, TYPE=ISO, PORE FLUID
To define the thermal expansion of the solid material:
Abaqus/CAE Usage:
*EXPANSION, TYPE=ISO or ORTHO or ANISO
To define the thermal expansion of the permeating fluid:
Property module: material editor: Other→Pore Fluid→Pore
Fluid Expansion
To define the thermal expansion of the solid material:
Property module: material editor: Mechanical→Expansion
Elements
The analysis of flow through porous media in Abaqus/Standard is available for plane strain,
axisymmetric, and three-dimensional problems. The modeling of coupled heat transfer effects is
available only for axisymmetric and three-dimensional problems. Continuum pore pressure elements
are provided for modeling fluid flow through a deforming porous medium in a coupled pore fluid
diffusion/stress analysis. These elements have pore pressure degree of freedom 8 in addition to
displacement degrees of freedom 1–3. Heat transfer through the porous medium can also be modeled
using continuum coupled temperature–pore pressure elements. These elements have temperature degree
of freedom 11 in addition to pore pressure degree of freedom 8 and displacement degrees of freedom
1–3. Stress/displacement elements can be used in parts of the model without pore fluid flow. See
“Choosing the appropriate element for an analysis type,” Section 27.1.3, for more information.
Output
The element output available for a coupled pore fluid diffusion/stress analysis includes the usual
mechanical quantities such as (effective) stress; strain; energies; and the values of state, field, and
user-defined variables. In addition, the following quantities associated with pore fluid flow are available:
VOIDR
POR
SAT
GELVR
FLUVR
FLVEL
Void ratio, e.
Pore pressure,
.
Saturation, s.
Gel volume ratio, .
Total fluid volume ratio, .
Magnitude and components of the pore fluid effective velocity vector, .
6.8.1–12
Abaqus Version 5.8 ID:
Printed on:
COUPLED DIFFUSION/STRESS ANALYSIS
FLVELM
FLVELn
Magnitude, , of the pore fluid effective velocity vector.
Component n of the pore fluid effective velocity vector (n=1, 2, 3).
If heat transfer is modeled, the following element output variables associated with heat transfer are
also available:
HFL
HFLn
HFLM
TEMP
Magnitude and components of the heat flux vector.
Component n of the heat flux vector (n=1, 2, 3).
Magnitude of the heat flux vector.
Integration point temperatures.
The nodal output available includes the usual mechanical quantities such as displacements, reaction
forces, and coordinates. In addition, the following quantities associated with pore fluid flow are available:
CFF
POR
RVF
RVT
Concentrated fluid flow at a node.
Pore pressure at a node.
Reaction fluid volume flux due to prescribed pressure. This flux is the rate at which
fluid volume is entering or leaving the model through the node to maintain the
prescribed pressure boundary condition. A positive value of RVF indicates that
fluid is entering the model.
Reaction total fluid volume (computed only in a transient analysis). This value is
the time integrated value of RVF.
If heat transfer is modeled, the following nodal output variables associated with heat transfer are
also available:
NT
RFL
RFLn
CFL
CFLn
Nodal point temperatures.
Reaction flux values due to prescribed temperature.
Reaction flux value n at a node (n=11, 12, …).
Concentrated flux values.
Concentrated flux value n at a node (n=11, 12, …).
All of the output variable identifiers are outlined in “Abaqus/Standard output variable identifiers,”
Section 4.2.1.
Input file template
*HEADING
…
***********************************
**
** Material definition
**
***********************************
6.8.1–13
Abaqus Version 5.8 ID:
Printed on:
COUPLED DIFFUSION/STRESS ANALYSIS
*MATERIAL, NAME=soil
Data lines to define mechanical properties of the solid material
…
*EXPANSION
Data lines to define the thermal expansion coefficient of the solid grains
*EXPANSION, TYPE=ISO, PORE FLUID
Data lines to define the thermal expansion coefficient of the permeating fluid
*PERMEABILITY, SPECIFIC=
Data lines to define permeability, , as a function of the void ratio, e
*PERMEABILITY, TYPE=SATURATION
Data lines to define the dependence of permeability on saturation,
*PERMEABILITY, TYPE=VELOCITY
Data lines to define the velocity coefficient,
*POROUS BULK MODULI
Data line to define the bulk moduli of the solid grains and the permeating fluid
*SORPTION, TYPE=ABSORPTION
Data lines to define absorption behavior
*SORPTION, TYPE=EXSORPTION
Data lines to define exsorption behavior
*SORPTION, TYPE=SCANNING
Data lines to define scanning behavior (between absorption and exsorption)
*GEL
Data line to define gel behavior in partially saturated flow
*MOISTURE SWELLING
Data lines to define moisture swelling strain as a function of saturation
in partially saturated flow
*CONDUCTIVITY
Data lines to define thermal conductivity of the solid grains if heat transfer is modeled
*CONDUCTIVITY,TYPE=ISO, PORE FLUID
Data lines to define thermal conductivity of the permeating fluid if heat transfer is modeled
*SPECIFIC HEAT
Data lines to define specific heat of the solid grains if transient heat transfer is modeled
*SPECIFIC HEAT,PORE FLUID
Data lines to define specific heat of the permeating fluid if transient heat transfer is modeled
*DENSITY
Data lines to define density of the solid grains if transient heat transfer is modeled
*DENSITY,PORE FLUID
Data lines to define density of the permeating fluid if transient heat transfer is modeled
*LATENT HEAT
Data lines to define latent heat of the solid grains if phase change due to temperature change
is modeled
*LATENT HEAT,PORE FLUID
6.8.1–14
Abaqus Version 5.8 ID:
Printed on:
COUPLED DIFFUSION/STRESS ANALYSIS
Data lines to define latent heat of the permeating fluid if phase change due to temperature change
is modeled
…
***********************************
**
** Boundary conditions and initial conditions
**
***********************************
*BOUNDARY
Data lines to specify zero-valued boundary conditions
*INITIAL CONDITIONS, TYPE=STRESS, GEOSTATIC
Data lines to specify initial stresses
*INITIAL CONDITIONS, TYPE=PORE PRESSURE
Data lines to define initial values of pore fluid pressures
*INITIAL CONDITIONS, TYPE=RATIO
Data lines to define initial values of the void ratio
*INITIAL CONDITIONS, TYPE=SATURATION
Data lines to define initial saturation
*INITIAL CONDITIONS, TYPE=TEMPERATURE
Data lines to define initial saturation
*AMPLITUDE, NAME=name
Data lines to define amplitude variations
***********************************
**
** Step 1: Optional step to ensure an equilibrium
** geostatic stress field
**
***********************************
*STEP
*GEOSTATIC
*CLOAD and/or *DLOAD and/or *TEMPERATURE and/or *FIELD
Data lines to specify mechanical loading
*FLOW and/or *SFLOW and/or *DFLOW and/or *DSFLOW
Data lines to specify pore fluid flow
*CFLUX and/or *DFLUX
Data lines to define concentrated and/or distributed heat fluxes if heat transfer is modeled
*BOUNDARY
Data lines to specify displacements or pore pressures
*END STEP
***********************************
**
** Step 2: Coupled pore diffusion/stress analysis step
6.8.1–15
Abaqus Version 5.8 ID:
Printed on:
COUPLED DIFFUSION/STRESS ANALYSIS
**
***********************************
*STEP (,NLGEOM)
** Use NLGEOM to include geometric nonlinearities
*SOILS
Data line to define incrementation
*CLOAD and/or *DLOAD and/or *DSLOAD
Data lines to specify mechanical loading
*FLOW and/or *SFLOW and/or *DFLOW and/or *DSFLOW
Data lines to specify pore fluid flow
*CFLUX and/or *DFLUX
Data lines to define concentrated and/or distributed heat fluxes if heat transfer is modeled
*FILM
Data lines referring to film property table if heat transfer is modeled
*BOUNDARY
Data lines to specify displacements, pore pressures, or temperatures
*END STEP
6.8.1–16
Abaqus Version 5.8 ID:
Printed on:
GEOSTATIC STRESS STATE
6.8.2
GEOSTATIC STRESS STATE
Products: Abaqus/Standard
Abaqus/CAE
References
•
•
•
•
“Defining an analysis,” Section 6.1.2
“Coupled pore fluid diffusion and stress analysis,” Section 6.8.1
*GEOSTATIC
“Configuring a geostatic stress field procedure” in “Configuring general analysis procedures,”
Section 14.11.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual
Overview
A geostatic stress field procedure:
•
•
•
•
is used to verify that the initial geostatic stress field is in equilibrium with applied loads and boundary
conditions and to iterate, if necessary, to obtain equilibrium;
accounts for pore pressure degrees of freedom when pore pressure elements are used, and accounts
for temperature degrees of freedom when coupled temperature–pore pressure elements are used;
is usually the first step of a geotechnical analysis, followed by a coupled pore fluid diffusion/stress
(with or without heat transfer) or static analysis procedure; and
can be linear or nonlinear.
Establishing geostatic equilibrium
The geostatic procedure is normally used as the first step of a geotechnical analysis; in such cases gravity
loads are applied during this step. Ideally, the loads and initial stresses should exactly equilibrate and
produce zero deformations. However, in complex problems it may be difficult to specify initial stresses
and loads that equilibrate exactly.
Abaqus/Standard provides two procedures for establishing the initial equilibrium. The first
procedure is applicable to problems for which the initial stress state is known at least approximately.
The second, enhanced, procedure is also applicable for cases in which the initial stresses are not known;
it is supported for only a limited number of elements and materials.
Establishing equilibrium when the initial stress state is approximately known
The geostatic procedure requires that the initial stresses are close to the equilibrium state; otherwise,
the displacements corresponding to the equilibrium state might be large. Abaqus/Standard checks for
equilibrium during the geostatic procedure and iterates, if needed, to obtain a stress state that equilibrates
the prescribed boundary conditions and loads. This stress state, which is a modification of the stress
field defined by the initial conditions (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,”
6.8.2–1
Abaqus Version 5.8 ID:
Printed on:
GEOSTATIC STRESS STATE
Section 33.2.1), is then used as the initial stress field in a subsequent static or coupled pore fluid
diffusion/stress (with or without heat transfer) analysis.
If the stresses given as initial conditions are far from equilibrium under the geostatic loading and
there is some nonlinearity in the problem definition, this iteration process may fail. Therefore, you should
ensure that the initial stresses are reasonably close to equilibrium.
If the deformations produced during the geostatic step are significant compared to the deformations
caused by subsequent loading, the definition of the initial state should be reexamined.
If heat transfer is modeled during the geostatic step through the use of coupled temperature–pore
pressure elements, the initial temperature field and thermal loads, if specified, must be such that the
system is relatively close to a state of thermal equilibrium. Steady-state heat transfer is assumed during
a geostatic step.
Input File Usage:
Abaqus/CAE Usage:
*GEOSTATIC
Step module: Create Step: General: Geostatic
Establishing equilibrium when the initial stress state is unknown
To obtain equilibrium in cases when the initial stress state is unknown or is known only approximately,
you can invoke an enhanced procedure. Abaqus automatically computes the equilibrium corresponding
to the initial loads and the initial configuration, allowing only small displacements within user-specified
tolerances. (The default tolerance is
.) The procedure is available with a limited number of elements
and materials and is intended to be used in analyses in which the material response is primarily elastic;
that is, inelastic deformations are small.
The procedure is supported for both geometrically linear and geometrically nonlinear analyses.
However, in general, the performance in the geometrically linear case will be better. Therefore, it
might be advantageous to obtain the initial equilibrium in a geometrically linear step, even though a
geometrically nonlinear analysis is performed in subsequent steps.
Input File Usage:
Use the following option to invoke the enhanced procedure:
Abaqus/CAE Usage:
*GEOSTATIC, UTOL=displacement tolerance
Step module: Create Step: General: Geostatic: Incrementation
tabbed page: Automatic: Max. displacement change
Limitations
The following limitations apply to the enhanced procedure:
•
It is supported only for a limited number of elements (see “Elements” below) and materials (see
“Material options” below). When the procedure is used with nonsupported elements or material
models, Abaqus issues a warning message. In this case it is the user’s responsibility to ensure that the
displacement tolerances are larger than the displacements in the analysis; otherwise, convergence
problems may occur.
•
It can be used in a restart analysis only if it had been used in the previous analysis.
6.8.2–2
Abaqus Version 5.8 ID:
Printed on:
GEOSTATIC STRESS STATE
Optional modeling of coupled heat transfer
When coupled temperature–pore pressure elements are used, heat transfer is modeled in these elements
by default. However, you may optionally choose to switch off heat transfer within these elements during
a geostatic step. This feature may be helpful in reducing computation time if temperature and associated
heat flow effects are not important.
Input File Usage:
Use the following option to suppress heat transfer modeling:
Abaqus/CAE Usage:
*GEOSTATIC, HEAT=NO
Switching off the heat transfer part of the physics is not supported in
Abaqus/CAE.
Vertical equilibrium in a porous medium
Most geotechnical problems begin from a geostatic state, which is a steady-state equilibrium
configuration of the undisturbed soil or rock body under geostatic loading. The equilibrium state
usually includes both horizontal and vertical stress components. It is important to establish these initial
conditions correctly so that the problem begins from an equilibrium state. Since such problems often
involve fully or partially saturated flow, the initial void ratio of the porous medium, , the initial pore
pressure,
, and the initial effective stress must all be defined.
If the magnitude and direction of the gravitational loading are defined by using the gravity
distributed load type, a total, rather than excess, pore pressure solution is used (see “Coupled pore
fluid diffusion and stress analysis,” Section 6.8.1). This discussion is based on the total pore pressure
formulation.
The z-axis points vertically in this discussion, and atmospheric pressure is neglected. We assume
that the pore fluid is in hydrostatic equilibrium during the geostatic procedure so that
where
is the user-defined specific weight of the pore fluid (see “Permeability,” Section 26.6.2). (The
pore fluid is not in hydrostatic equilibrium if there is significant steady-state flow of pore fluid through the
porous medium: in that case a steady-state coupled pore fluid diffusion/stress analysis must be performed
to establish the initial conditions for any subsequent transient calculations—see “Coupled pore fluid
diffusion and stress analysis,” Section 6.8.1.) If we also take
to be independent of z (which is usually
the case, since the fluid is almost incompressible), this equation can be integrated to define
where
is the height of the phreatic surface, at which
and above which
and the pore
fluid is only partially saturated.
We usually assume that there are no significant shear stresses
,
. Then, equilibrium in the
vertical direction is
6.8.2–3
Abaqus Version 5.8 ID:
Printed on:
GEOSTATIC STRESS STATE
where is the dry density of the porous solid material (the dry mass per unit volume), g is the
gravitational acceleration,
is the initial porosity of the material, and s is the saturation,
(see “Permeability,” Section 26.6.2). Since porosity is the ratio of pore volume to total volume and the
void ratio is the ratio of pore volume to solids volume,
is defined from the initial void ratio by
Abaqus/Standard requires that the initial value of the effective stress, , be given as an initial
condition (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1). Effective stress
is defined from the total stress, , by
where is a unit matrix. Combining this definition with the equilibrium statement in the z-direction and
hydrostatic equilibrium in the pore fluid gives
again using the assumption that
is independent of z.
is the position of the surface that separates
the dry soil from the partially saturated soil. The soil is assumed to be dry (
) for
, and it is
assumed to be partially saturated for
and fully saturated for
.
In many cases s is constant. For example, in fully saturated flow
everywhere below the
phreatic surface. If we further assume that the initial porosity, , and the dry density of the porous
medium, , are also constant, the above equation is readily integrated to give
where
is the position of the surface of the porous medium,
.
In more complicated cases where s, , and/or vary with height, the equation must be integrated
in the vertical direction to define the initial values of
.
6.8.2–4
Abaqus Version 5.8 ID:
Printed on:
GEOSTATIC STRESS STATE
Horizontal equilibrium in a porous medium
In many geotechnical applications there is also horizontal stress, typically caused by tectonic action.
If the pore fluid is under hydrostatic equilibrium and
, equilibrium in the horizontal
directions requires that the horizontal components of effective stress do not vary with horizontal position:
only, where
is any horizontal component of effective stress.
Initial conditions
The initial effective geostatic stress field, , is given by defining initial stress conditions. Unless
the enhanced procedure is used, the initial state of stress must be close to being in equilibrium
with the applied loads and boundary conditions. See “Initial conditions in Abaqus/Standard and
Abaqus/Explicit,” Section 33.2.1.
You can specify that the initial stresses vary only with elevation, as described in “Initial conditions
in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1. In this case the horizontal stress is typically
assumed to be a fraction of the vertical stress: those fractions are defined in the x- and y-directions.
In problems involving partially or fully saturated porous media, initial pore fluid pressures, , void
ratios, , and saturation values, s, must be given (see “Coupled pore fluid diffusion and stress analysis,”
Section 6.8.1).
In partially saturated cases the initial pore pressure and saturation values must lie on or between
the absorption and exsorption curves (see “Sorption,” Section 26.6.4). A partially saturated problem is
illustrated in “Wicking in a partially saturated porous medium,” Section 1.9.3 of the Abaqus Benchmarks
Manual.
You may also specify initial temperatures in the model if heat transfer is modeled during the geostatic
procedure.
Boundary conditions
Boundary conditions can be applied to displacement degrees of freedom 1–6 and to pore pressure
degree of freedom 8 (“Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1).
If coupled temperature–pore pressure elements are used, boundary conditions on temperature degree
of freedom 11 can also be applied to nodes belonging to these elements. If the enhanced procedure
is used and nonzero boundary conditions are applied, it is the user’s responsibility to ensure that the
displacements corresponding to the tolerances specified are larger than the displacements in the analysis;
otherwise, the displacements at the nonzero boundary nodes will be reset to zero with the tolerances
specified.
The boundary conditions should be in equilibrium with the initial stresses and applied loads. If the
horizontal stress is nonzero, horizontal equilibrium must be maintained by fixing the boundary conditions
on any nonhorizontal edges of the finite element model in the horizontal direction or by using infinite
elements (“Infinite elements,” Section 28.3.1). If heat transfer is modeled, the temperature boundary
conditions should be in equilibrium with the initial temperature field and applied thermal loads.
6.8.2–5
Abaqus Version 5.8 ID:
Printed on:
GEOSTATIC STRESS STATE
Loads
The following loading types can be prescribed in a geostatic stress field procedure:
•
•
•
Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6); see
“Concentrated loads,” Section 33.4.2.
Distributed pressure forces or body forces can also be applied; see “Distributed loads,”
Section 33.4.3. The distributed load types available with particular elements are described in
Part VI, “Elements.” The magnitude and direction of gravitational loading are defined by using
the gravity or body force distributed load types.
Pore fluid flow is controlled as described in “Pore fluid flow,” Section 33.4.7.
If heat transfer is modeled, the following types of thermal loading can also be prescribed (“Thermal
loads,” Section 33.4.4). These loads are not supported in Abaqus/CAE during a geostatic analysis.
•
•
•
Concentrated heat fluxes.
Body fluxes and distributed surface fluxes.
Convective film conditions and radiation conditions; film properties can be made a function of
temperature.
Predefined fields
The following predefined fields can be specified in a geostatic stress field procedure, as described in
“Predefined fields,” Section 33.6.1:
•
•
•
For a geostatic analysis that does not model heat transfer and uses regular pore pressure elements,
temperature is not a degree of freedom and nodal temperatures can be specified.
Predefined temperature fields are not allowed in a geostatic analysis that also models heat transfer.
Boundary conditions should be used instead to specify temperatures, as described earlier.
The values of user-defined field variables can be specified; these values affect only field-variabledependent material properties, if any.
Material options
Any of the mechanical constitutive models available in Abaqus/Standard can be used to model the porous
solid material. However, the enhanced procedure can be used only with the elastic, porous elastic,
extended Cam-clay plasticity, and Mohr-Coulomb plasticity models. Use of a nonsupported material
model with this procedure may lead to poor convergence or no convergence if displacements are larger
than the displacements corresponding to the tolerances specified. Abaqus will issue a warning message
if the procedure is used with a nonsupported material model.
If a porous medium will be analyzed subsequent to the geostatic procedure, pore fluid flow quantities
such as permeability and sorption should be defined (see “Pore fluid flow properties,” Section 26.6.1).
If heat transfer is modeled, thermal properties such as conductivity, specific heat, and density should
be defined for both the solid and the pore fluid phases (see “Thermal properties if heat transfer is modeled”
6.8.2–6
Abaqus Version 5.8 ID:
Printed on:
GEOSTATIC STRESS STATE
in “Coupled pore fluid diffusion and stress analysis,” Section 6.8.1, for details on how to specify separate
thermal properties for the two phases).
Elements
Any of the stress/displacement elements in Abaqus/Standard can be used in a geostatic procedure.
Continuum pore pressure elements can also be used for modeling fluid in a deforming porous medium.
These elements have pore pressure degree of freedom 8 in addition to displacement degrees of freedom
1–3. However, the enhanced procedure can be used only with continuum and cohesive elements
with pore pressure degrees of freedom and the corresponding stress/displacements elements. Use
of nonsupported elements with this procedure may lead to poor convergence or no convergence if
displacements are larger than the displacements corresponding to the tolerances specified. Abaqus will
issue a warning message if the procedure is used with a nonsupported element.
Continuum elements that couple temperature, pore pressure, and displacement can be used if heat
transfer needs to be modeled. These elements have temperature degree of freedom 11 in addition to pore
pressure degree of freedom 8 and displacement degrees of freedom 1–3. See “Choosing the appropriate
element for an analysis type,” Section 27.1.3, for more information.
Output
The element output available for a coupled pore fluid diffusion/stress analysis includes the usual
mechanical quantities such as (effective) stress; strain; energies; and the values of state, field, and
user-defined variables. In addition, the following quantities associated with pore fluid flow are available:
VOIDR
POR
SAT
GELVR
FLUVR
FLVEL
FLVELM
FLVELn
Void ratio, e.
Pore pressure,
.
Saturation, s.
Gel volume ratio, .
Total fluid volume ratio, .
Magnitude and components of the pore fluid effective velocity vector, .
Magnitude, , of the pore fluid effective velocity vector.
Component n of the pore fluid effective velocity vector (n=1, 2, 3).
If heat transfer is modeled, the following element output variables associated with heat transfer are
also available:
HFL
HFLn
HFLM
TEMP
Magnitude and components of the heat flux vector.
Component n of the heat flux vector (n=1, 2, 3).
Magnitude of the heat flux vector.
Integration point temperatures.
The nodal output available includes the usual mechanical quantities such as displacements, reaction
forces, and coordinates. In addition, the following quantities associated with pore fluid flow are available:
6.8.2–7
Abaqus Version 5.8 ID:
Printed on:
GEOSTATIC STRESS STATE
POR
RVF
Pore pressure at a node.
Reaction fluid volume flux due to prescribed pressure. This flux is the rate at which
fluid volume is entering or leaving the model through the node to maintain the
prescribed pressure boundary condition. A positive value of RVF indicates fluid is
entering the model.
If heat transfer is modeled, the following nodal output variables associated with heat transfer are
also available:
NT
RFL
RFLn
CFL
CFLn
Nodal point temperatures.
Reaction flux values due to prescribed temperature.
Reaction flux value n at a node (n=11, 12, …).
Concentrated flux values.
Concentrated flux value n at a node (n=11, 12, …).
All of the output variable identifiers are outlined in “Abaqus/Standard output variable identifiers,”
Section 4.2.1.
Input file template
*HEADING
…
*MATERIAL, NAME=mat1
Data lines to define mechanical properties of the solid material
…
*DENSITY
Data lines to define the density of the dry material
*PERMEABILITY, SPECIFIC=
Data lines to define permeability, , as a function of the void ratio, e
*CONDUCTIVITY
Data lines to define thermal conductivity of the solid grains if heat transfer is modeled
*CONDUCTIVITY,TYPE=ISO, PORE FLUID
Data lines to define thermal conductivity of the permeating fluid if heat transfer is modeled
*SPECIFIC HEAT
Data lines to define specific heat of the solid grains if transient heat transfer is modeled in a
subsequent step
*SPECIFIC HEAT,PORE FLUID
Data lines to define specific heat of the permeating fluid if transient heat transfer is modeled in a subsequent step
*DENSITY
Data lines to define density of the solid grains if transient heat transfer is modeled in a subsequent
step
*DENSITY,PORE FLUID
Data lines to define density of the permeating fluid if transient heat transfer is modeled in a
subsequent step
6.8.2–8
Abaqus Version 5.8 ID:
Printed on:
GEOSTATIC STRESS STATE
*LATENT HEAT
Data lines to define latent heat of the solid grains if phase change due to temperature change is modeled
*LATENT HEAT,PORE FLUID
Data lines to define latent heat of the permeating fluid if phase change due to temperature change
is modeled
…
*INITIAL CONDITIONS, TYPE=STRESS, GEOSTATIC
Data lines to define the initial stress state
*INITIAL CONDITIONS, TYPE=PORE PRESSURE
Data lines to define initial values of pore fluid pressures
*INITIAL CONDITIONS, TYPE=RATIO
Data lines to define initial values of the void ratio
*INITIAL CONDITIONS, TYPE=SATURATION
Data lines to define initial saturation
*INITIAL CONDITIONS, TYPE=TEMPERATURE
Data lines to define initial temperature
*BOUNDARY
Data lines to define zero-valued boundary conditions
**
*STEP
*GEOSTATIC
*CLOAD and/or *DLOAD and/or *DSLOAD
Data lines to specify mechanical loading
*FLOW and/or *SFLOW and/or *DFLOW and/or *DSFLOW
Data lines to specify pore fluid flow
*CFLUX and/or *DFLUX
Data lines to define concentrated and/or distributed heat fluxes if heat transfer is modeled
*BOUNDARY
Data lines to specify displacements or pore pressures
*END STEP
6.8.2–9
Abaqus Version 5.8 ID:
Printed on:
MASS DIFFUSION ANALYSIS
6.9
Mass diffusion analysis
•
“Mass diffusion analysis,” Section 6.9.1
6.9–1
Abaqus Version 5.8 ID:
Printed on:
MASS DIFFUSION
6.9.1
MASS DIFFUSION ANALYSIS
Products: Abaqus/Standard
Abaqus/CAE
References
•
•
•
•
•
“Defining an analysis,” Section 6.1.2
*MASS DIFFUSION
“Configuring a mass diffusion procedure” in “Configuring general analysis procedures,”
Section 14.11.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual
“Creating and modifying prescribed conditions,” Section 16.4 of the Abaqus/CAE User’s Manual
“Defining a concentrated concentration flux,” Section 16.9.33 of the Abaqus/CAE User’s Manual,
in the online HTML version of this manual
•
“Defining a body concentration flux,” Section 16.9.35 of the Abaqus/CAE User’s Manual, in the
online HTML version of this manual
•
“Defining a surface concentration flux,” Section 16.9.34 of the Abaqus/CAE User’s Manual, in the
online HTML version of this manual
Overview
A mass diffusion analysis:
•
models the transient or steady-state diffusion of one material through another, such as the diffusion
of hydrogen through a metal;
•
•
requires the use of mass diffusion elements; and
can be used to model temperature and/or pressure-driven mass diffusion.
Governing equations
The governing equations for mass diffusion are an extension of Fick’s equations: they allow for
nonuniform solubility of the diffusing substance in the base material and for mass diffusion driven by
gradients of temperature and pressure. The basic solution variable (used as the degree of freedom at
the nodes of the mesh) is the “normalized concentration” (often also referred to as the “activity” of the
diffusing material),
, where c is the mass concentration of the diffusing material and s is its
solubility in the base material. Therefore, when the mesh includes dissimilar materials that share nodes,
the normalized concentration is continuous across the interface between the different materials.
For example, a diatomic gas that dissociates during diffusion can be described using Sievert’s law:
, where p is the partial pressure of the diffusing gas. Combining Sievert’s law with the definition
of normalized concentration given earlier,
. Equilibrium requires the partial pressure to be
continuous across an interface, so normalized concentration will be continuous as well. If an expression
6.9.1–1
Abaqus Version 5.8 ID:
Printed on:
MASS DIFFUSION
other than Sievert’s law defines the relationship between concentration and partial pressure for a diffusing
material, solubility should be defined accordingly.
The diffusion problem is defined from the requirement of mass conservation for the diffusing phase:
where V is any volume whose surface is S, is the outward normal to S, is the flux of concentration
of the diffusing phase, and
is the concentration flux leaving S.
Diffusion is assumed to be driven by the gradient of a general chemical potential, which gives the
behavior
where
is the diffusivity;
is the solubility;
is the “Soret effect” factor,
providing diffusion because of temperature gradient; is the temperature;
is the value of absolute
zero on the temperature scale being used;
is the pressure stress factor, providing diffusion
driven by the gradient of the equivalent pressure stress,
; is stress; and are any
predefined field variables.
Whenever D, , or
depends on concentration, the problem becomes nonlinear and the system
of equations becomes nonsymmetric. In practical cases the dependence on concentration is quite strong,
so the nonsymmetric matrix storage and solution scheme is invoked automatically when a mass diffusion
analysis is performed (see “Defining an analysis,” Section 6.1.2).
Fick’s law
Mass diffusion behavior is often described by Fick’s law (Crank, 1956):
Fick’s law is offered in Abaqus/Standard as a special case of the general chemical potential relation. To
establish the relationship between Fick’s law and the general chemical potential, we write Fick’s law as
In most practical cases
, and we can write
The two terms in this equation describe the normalized concentration and temperature-driven
diffusion, respectively. The normalized concentration-driven diffusion term is identical to that given in
6.9.1–2
Abaqus Version 5.8 ID:
Printed on:
MASS DIFFUSION
the general relation. The temperature-driven diffusion term in Fick’s law is recovered in the general
relation if
This conversion is done automatically in Abaqus/Standard when you request Fick’s law (see
“Diffusivity,” Section 26.4.1).
An extended form of Fick’s law can also be chosen by specifying a nonzero value for :
In this case Abaqus/Standard will still define
automatically as discussed earlier.
Units
The units of concentration are commonly given as parts per million (P). On the basis of the applicability
of Sievert’s law to the mass diffusion, the units of solubility are
, where F is force and L is
length. The units of the Soret effect factor are
. The units of the pressure stress factor are
, and the units of equivalent pressure stress are
. The diffusivity, , has units of
,
where T is time. The concentration flux, , then has units of
; and the concentration volumetric
flux,
, has units of
.
Steady-state analysis
Steady-state mass diffusion analysis provides the steady-state solution directly: the rate of change of
concentration with respect to time is omitted from the governing diffusion equation in steady-state
analysis. In nonlinear cases iteration may be necessary to achieve a converged solution.
Since the rate term is removed from the governing equations, the steady-state problem has no
intrinsic physically meaningful time scale; nevertheless, you may assign a “time” scale to the analysis
step. This time scale is often convenient for output identification and for specifying prescribed
normalized concentrations and fluxes with varying magnitudes. Thus, when steady-state analysis
is chosen, you specify a “time” increment and a “time” period for the step; Abaqus/Standard then
increments through the step accordingly. If a steady-state analysis step is to be followed by a transient
analysis step and total time is used in amplitude definitions (“Amplitude curves,” Section 33.1.2), the
time period should be defined to be negligibly small in the steady-state step. For more details on time
scales and time stepping, see “Defining an analysis,” Section 6.1.2.
Input File Usage:
Abaqus/CAE Usage:
*MASS DIFFUSION, STEADY STATE
Step module: Create Step: General: Mass diffusion: Basic:
Response: Steady state
6.9.1–3
Abaqus Version 5.8 ID:
Printed on:
MASS DIFFUSION
Transient analysis
Time integration in transient diffusion analysis is done with the backward Euler method (also referred to
as the modified Crank-Nicholson operator). This method is unconditionally stable for linear problems.
Automatic or fixed time incrementation can be used for transient analysis. The automatic time
incrementation scheme is generally preferred because the response is usually simple diffusion: the rate of
change of normalized concentration varies widely during the step and requires different time increments
to maintain accuracy in the time integration.
Spurious oscillations due to small time increments
In transient mass diffusion analysis with second-order elements there is a relationship between the
minimum usable time step and the element size. A simple guideline is
where
is the time increment, D is the diffusivity, and
is a typical element dimension (such as the
length of a side of an element). If time increments smaller than this value are used, spurious oscillations
can appear in the solution. Abaqus/Standard provides no check on the initial time increment defined for
a mass diffusion analysis; you must ensure that the given value does not violate the above criterion.
In transient analysis using first-order elements the solubility terms are lumped, which eliminates
such oscillations but can lead to locally inaccurate solutions for small time increments. If smaller time
increments are required, a finer mesh should be used in regions where the normalized concentration
changes occur.
Generally there is no upper limit on the time increment because the integration procedure is
unconditionally stable unless nonlinearities cause numerical problems.
Automatic incrementation
The automatic time incrementation scheme for mass diffusion problems is based on the user-specified
maximum normalized concentration change allowed at any node during an increment,
.
Input File Usage:
Abaqus/CAE Usage:
*MASS DIFFUSION, DCMAX=
Step module: Create Step: General: Mass diffusion: Basic: Response:
Transient; Incrementation: Type: Automatic: Max. allowable
normalized concentration change:
Fixed time incrementation
If you choose fixed time incrementation, fixed time increments equal to the size of the user-specified
initial time increment,
, will be used.
Input File Usage:
*MASS DIFFUSION
6.9.1–4
Abaqus Version 5.8 ID:
Printed on:
MASS DIFFUSION
Abaqus/CAE Usage:
Step module: Create Step: General: Mass diffusion: Basic: Response:
Transient; Incrementation: Type: Fixed, Increment size:
Ending a transient analysis
Transient mass diffusion analysis can be terminated by completing a specified time period, or it can be
continued until steady-state conditions are reached. By default, the analysis will end when the given time
period has been completed. Alternatively, you can specify that the analysis will end when steady state is
reached or the time period ends, whichever comes first. Steady state is defined as the point in time when
all normalized concentrations change at less than a user-defined rate.
Input File Usage:
Use the following option to end the analysis when the time period is reached:
*MASS DIFFUSION, END=PERIOD (default)
Use the following option to end the analysis based on the concentration change
rate:
Abaqus/CAE Usage:
*MASS DIFFUSION, END=SS
Step module: Create Step: General: Mass diffusion: Basic: Response:
Transient; Incrementation: Type: Automatic: End step when
normalized concentration change rate is less than
Initial conditions
An initial normalized concentration of the diffusing material at specific nodes that belong to mass
diffusion elements can be defined (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,”
Section 33.2.1). For an analysis in which mass diffusion is driven by gradients of temperature and/or
pressure (“Diffusivity,” Section 26.4.1), the initial temperature and pressure stress fields in a model can
also be defined.
Input File Usage:
Use the following options:
*INITIAL CONDITIONS, TYPE=CONCENTRATION for initial
concentrations
*INITIAL CONDITIONS, TYPE=TEMPERATURE for initial temperatures
*INITIAL CONDITIONS, TYPE=PRESSURE STRESS for initial equivalent
pressure stress
Abaqus/CAE Usage:
Load module: Create Predefined Field: Step: Initial: choose Other for
the Category and Temperature for the Types for Selected Step
Initial concentration and equivalent pressure stress are not supported in
Abaqus/CAE.
Boundary conditions
Boundary conditions can be applied to nodal degree of freedom 11 in any mass diffusion element
to prescribe values of normalized concentration (“Boundary conditions in Abaqus/Standard and
Abaqus/Explicit,” Section 33.3.1). Such values can be specified as functions of time.
6.9.1–5
Abaqus Version 5.8 ID:
Printed on:
MASS DIFFUSION
Any boundary condition changes to be applied during a mass diffusion step should be given in the
respective step using appropriate amplitude definitions to specify their “time” variations (“Amplitude
curves,” Section 33.1.2). If boundary conditions are specified for the step without amplitude references,
they are assumed to change either linearly with “time” during the step or instantly at the start of the
step, according to the user-specified or default time variation associated with the step (see “Defining an
analysis,” Section 6.1.2).
Loads
Concentration fluxes are the only loads that can be applied in a mass diffusion analysis step.
Input File Usage:
Use the following option to specify a concentrated concentration flux at a node:
*CFLUX
node number or node set name, degree of freedom, concentrated flux magnitude
Use the following option to specify a distributed concentration flux acting on
entire elements (body flux) or just on element faces (surface flux):
*DFLUX
element number or element set name, BF or Sn, distributed flux magnitude
Abaqus/CAE Usage:
Use the following input to define a concentrated concentration flux at a node:
Load module: Create Load: choose Mass diffusion for the Category
and Concentrated concentration flux for the Types for Selected
Step: select region: Magnitude: concentrated flux magnitude
Use the following input to define a distributed concentration flux acting on
entire elements (body flux) or just on element faces (surface flux):
Load module: Create Load: choose Mass diffusion for the Category
and Body concentration flux or Surface concentration flux for
the Types for Selected Step: Distribution: Uniform or select an
analytical field, Magnitude: distributed flux magnitude
Modifying or removing concentration fluxes
Concentrated or distributed concentration fluxes can be added, modified, or removed as described in
“Applying loads: overview,” Section 33.4.1.
Specifying time-dependent concentration fluxes
The magnitude of a concentrated or a distributed concentration flux can be controlled by referring to an
amplitude curve (see “Amplitude curves,” Section 33.1.2). If different magnitude variations are needed
for different fluxes, the flux definitions can be repeated, with each referring to its own amplitude curve.
6.9.1–6
Abaqus Version 5.8 ID:
Printed on:
MASS DIFFUSION
Defining nonuniform distributed concentration fluxes in a user subroutine
To define nonuniform distributed concentration fluxes, the variation of the flux magnitude throughout a
step can be defined in user subroutine DFLUX. If a reference flux magnitude is specified directly, it will
be ignored. As a result, any amplitude reference in the flux definition is also ignored.
Input File Usage:
Use the following option to define a nonuniform distributed concentration body
flux:
*DFLUX
element number or element set, BFNU
Use the following option to define a nonuniform distributed concentration
surface flux:
*DFLUX
element number or element set, SnNU
Abaqus/CAE Usage:
Use the following input to define a nonuniform distributed concentration body
flux:
Load module: Create Load: choose Mass diffusion for the Category
and Body concentration flux for the Types for Selected Step:
select region: Distribution: User-defined
Use the following input to define a nonuniform distributed concentration
surface flux:
Load module: Create Load: choose Mass diffusion for the Category
and Surface concentration flux for the Types for Selected Step:
select region: Distribution: User-defined
Predefined fields
Predefined temperatures, equivalent pressure stresses, and field variables can be specified in a mass
diffusion analysis.
Prescribing temperatures
Temperatures are applied to nodes in temperature-driven mass diffusion analyses by defining a
temperature field; absolute zero on the temperature scale used is defined as described in “Specifying the
value of absolute zero” in “Thermal loads,” Section 33.4.4. Alternatively, the temperature field can be
obtained from a previous heat transfer analysis. Time-dependent temperature variations are possible
with either approach.
A simple interface is provided that uses the Abaqus/Standard results file from the heat transfer
analysis to define the temperature field at different times in the mass diffusion analysis. Abaqus/Standard
assumes that the nodes in the mass diffusion analysis have the same numbers as the nodes in the previous
heat transfer analysis. Values in the results file are ignored at nodes that exist in the heat transfer analysis
but not in the mass diffusion analysis, and the temperatures at nodes that did not exist in the heat transfer
analysis will not be set by reading the results file.
6.9.1–7
Abaqus Version 5.8 ID:
Printed on:
MASS DIFFUSION
For specific details on prescribing temperatures, see “Predefined temperature” in “Predefined
fields,” Section 33.6.1.
Prescribing equivalent pressure stresses
Equivalent pressure stress values can be given at nodes by specifying them directly as a predefined field
in the mass diffusion analysis or indirectly by reading the equivalent pressure stresses from the results
file of a previous stress/displacement, fully coupled temperature-displacement, or fully coupled thermalelectrical-structural analysis. Regardless of the manner in which they are specified, pressures should be
entered according to the Abaqus convention that equivalent pressure stresses are positive when they are
compressive.
A simple interface is provided that uses the Abaqus/Standard results file from a mechanical
analysis to define the equivalent pressure stresses at different times in the mass diffusion analysis.
Abaqus/Standard assumes that the nodes in the mass diffusion analysis have the same numbers as the
nodes in the previous mechanical analysis. Values in the results file are ignored at nodes that exist in the
mechanical analysis but not in the mass diffusion analysis, and the pressures at nodes that did not exist
in the mechanical analysis will not be set by reading the results file.
For specific details on prescribing equivalent pressure stresses, see “Predefined pressure stress” in
“Predefined fields,” Section 33.6.1.
Specifying predefined field variables
You can specify values of predefined field variables during a mass diffusion analysis. These values affect
only field-variable-dependent material properties, if any. See “Predefined field variables” in “Predefined
fields,” Section 33.6.1.
Material options
Both diffusivity (“Diffusivity,” Section 26.4.1) and solubility (“Solubility,” Section 26.4.2) must be
defined in a mass diffusion analysis. Optionally, a Soret effect factor and a pressure stress factor can be
defined to introduce mass diffusion caused by temperature and pressure gradients, respectively. The use
of Fick’s law also introduces temperature-driven mass diffusion since a Soret effect factor is calculated
automatically.
Elements
Mass diffusion analysis can be performed using only the two-dimensional, three-dimensional, and
axisymmetric solid elements that are included in the Abaqus/Standard heat transfer/mass diffusion
element library.
Output
In addition to the standard output identifiers available in Abaqus/Standard (“Abaqus/Standard output
variable identifiers,” Section 4.2.1), the following variables have special meaning in mass diffusion
analyses:
6.9.1–8
Abaqus Version 5.8 ID:
Printed on:
MASS DIFFUSION
Element integration point variables:
CONC
ISOL
MFL
MFLM
MFLn
TEMP
Mass concentration.
Amount of solute at the integration point, calculated as the product of the mass
concentration and the integration point volume.
Magnitude and components of the concentration flux vector (excluding the terms
due to pressure and temperature gradients).
Magnitude of the concentration flux vector.
Component n of the concentration flux vector (n = 1, 2, 3).
Magnitude of the applied temperature field.
Whole element variables:
ESOL
NFLUX
FLUXS
Amount of solute in the element, calculated as the sum of ISOL over all the element
integration points.
Fluxes at the nodes of the element caused by mass diffusion in the element.
Distributed mass flux applied to an element.
Whole or partial model variables:
SOL
Amount of solute in the model or specified element set, calculated as the sum of
ESOL over all the elements in the model or set.
Nodal variables:
CFL
CFLn
NNC
NNCn
RFL
RFLn
Input file template
All concentrated flux values.
Concentrated flux value n at a node (n = 11).
All normalized concentration values at a node.
Normalized concentration degree of freedom n at a node (n = 11).
All reaction flux values (conjugate to normalized concentration).
Reaction flux value n at a node (n = 11) (conjugate to normalized concentration).
The following template is representative of a three-step mass diffusion analysis. The first step
establishes an initial steady-state concentration distribution of a diffusing material. In the second step
equivalent pressure stresses are read from a fully coupled temperature-displacement analysis and the
transient mass diffusion response is obtained for the case of mechanical loading of the body. In the final
step a temperature field is read from a fully coupled temperature-displacement analysis and the transient
mass diffusion response is calculated for the case of heating and cooling the body in which diffusion
occurs. An example problem that follows this template is “Thermo-mechanical diffusion of hydrogen
in a bending beam,” Section 1.10.1 of the Abaqus Benchmarks Manual.
*HEADING
…
*MATERIAL,NAME=mat1
6.9.1–9
Abaqus Version 5.8 ID:
Printed on:
MASS DIFFUSION
*SOLUBILITY
Data lines to define solubility
*DIFFUSIVITY
Data lines to define diffusivity
*KAPPA,TYPE=TEMP
Data lines to define diffusion driven by temperature gradients
*KAPPA,TYPE=PRESS
Data lines to define diffusion driven by gradients of equivalent pressure stress
*INITIAL CONDITIONS,TYPE=TEMPERATURE
Data lines to define an initial temperature field
*INITIAL CONDITIONS,TYPE=CONCENTRATION
Data lines to define initial nodal values of normalized concentration
*INITIAL CONDITIONS,TYPE=PRESSURE STRESS
Data lines to define initial nodal values of equivalent pressure stress
*AMPLITUDE,NAME=name
Data lines to define amplitude variations
**
*STEP
Step 1 - steady-state solution
*MASS DIFFUSION,STEADY STATE
Data line to define incrementation
*BOUNDARY
Data lines to prescribe nodal values of normalized concentration
*EL FILE
Data lines to define element integration output to the results file
*NODE FILE
Data lines to define nodal output to the results file
*END STEP
**
*STEP
Step 2 - transient analysis driven by pressure stress gradients
*MASS DIFFUSION,DCMAX=dcmax,END=SS
Data line to define incrementation
*BOUNDARY
Data lines to prescribe nodal values of normalized concentration
*PRESSURE STRESS,FILE=name
*EL FILE
Data lines to define element integration output to the results file
*NODE FILE
Data lines to define nodal output to the results file
*END STEP
**
6.9.1–10
Abaqus Version 5.8 ID:
Printed on:
MASS DIFFUSION
*STEP
Step 3 - transient analysis driven by temperature gradients
*MASS DIFFUSION,DCMAX=dcmax,END=SS
Data line to define incrementation
*BOUNDARY
Data lines to prescribe nodal values of normalized concentration
*TEMPERATURE,FILE=name
*EL FILE
Data lines to define element integration output to the results file
*NODE FILE
Data lines to define nodal output to the results file
*END STEP
Additional reference
•
Crank, J., The Mathematics of Diffusion, Clarendon Press, Oxford, 1956.
6.9.1–11
Abaqus Version 5.8 ID:
Printed on:
ACOUSTIC AND SHOCK ANALYSIS
6.10
Acoustic and shock analysis
•
“Acoustic, shock, and coupled acoustic-structural analysis,” Section 6.10.1
6.10–1
Abaqus Version 5.8 ID:
Printed on:
ACOUSTIC ANALYSIS
6.10.1
ACOUSTIC, SHOCK, AND COUPLED ACOUSTIC-STRUCTURAL ANALYSIS
Products: Abaqus/Standard
Abaqus/Explicit
Abaqus/CAE
References
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
“Acoustic medium,” Section 26.3.1
“Acoustic and shock loads,” Section 33.4.6
“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1
“ALE adaptive meshing: overview,” Section 12.2.1
“Steady-state transport analysis,” Section 6.4.1
*ACOUSTIC FLOW VELOCITY
*ACOUSTIC WAVE FORMULATION
*ADAPTIVE MESH
*BEAM FLUID INERTIA
*CONWEP CHARGE PROPERTY
*IMPEDANCE
*IMPEDANCE PROPERTY
*INCIDENT WAVE
*INCIDENT WAVE INTERACTION
*INITIAL CONDITIONS
*SIMPEDANCE
*TIE
“Defining an acoustic pressure boundary condition,” Section 16.10.19 of the Abaqus/CAE User’s
Manual, in the online HTML version of this manual
“Creating the submodel boundary condition,” Section 38.4 of the Abaqus/CAE User’s Manual
Overview
Analyses performed using acoustic elements, an acoustic medium, and a dynamic procedure can simulate
a variety of engineering phenomena including low-amplitude wave phenomena involving fluids such as
air and water and “shock” analysis involving higher amplitude waves in fluids interacting with structures.
An acoustic analysis:
•
•
is used to model sound propagation, emission, and radiation problems;
can include incident wave loading to model effects such as underwater explosion (UNDEX) on
structures interacting with fluids, airborne blast loading on structures, or sound waves impinging on
a structure;
6.10.1–1
Abaqus Version 5.8 ID:
Printed on:
ACOUSTIC ANALYSIS
•
•
•
•
•
•
•
•
•
•
•
•
•
•
in Abaqus/Explicit can include fluid undergoing cavitation when the absolute pressure drops to a
limit value;
is performed using one of the dynamic analysis procedures (“Dynamic analysis procedures:
overview,” Section 6.3.1);
can be used to model an acoustic medium alone, as in the study of the natural frequencies of vibration
of a cavity containing an acoustic fluid;
can be used to model a coupled acoustic-structural system, as in the study of the noise level in a
vehicle;
can be used to model the sound transmitted through a coupled acoustic-structural system;
requires the use of acoustic elements and, for coupled acoustic-structural analysis, a surface-based
interaction using a tie constraint or, in Abaqus/Standard, acoustic interface elements;
can be used to obtain the scattered wave solution directly under incident wave loading when the
mechanical behavior of the fluid is linear;
can be used to obtain a total wave solution (sum of the incident and the scattered waves) by selecting
the total wave formulation, particularly when nonlinear fluid behavior such as cavitation is present
in the acoustic medium;
can be used to model problems where the acoustic medium interacts with a structure subjected to
large static deformation;
in Abaqus/Standard can be used with symmetric model generation (“Symmetric model generation,”
Section 10.4.1) and symmetric results transfer (“Transferring results from a symmetric mesh or a
partial three-dimensional mesh to a full three-dimensional mesh,” Section 10.4.2);
in Abaqus/Standard can be used with steady-state transport (“Steady-state transport analysis,”
Section 6.4.1) and an acoustic flow velocity (“*ACOUSTIC FLOW VELOCITY,” Section 1.1 of
the Abaqus Keywords Reference Manual) to model acoustic perturbations of a moving fluid;
in Abaqus/Standard can include a coupled structural-acoustic substructure that was previously
defined (“Defining substructures,” Section 10.1.2);
can be used to model both interior problems, where a structure surrounds one or more acoustic
cavities, and exterior problems, where a structure is located in a fluid medium extending to infinity;
and
is applicable to any vibration or dynamic problem in a medium where the effects of shear stress are
negligible.
A shock analysis:
•
•
•
•
•
is used to model blast effects on structures;
often requires double precision to avoid roundoff error when Abaqus/Explicit is used;
may include acoustic elements to model the effects of fluid inertia and compressibility;
may include virtual mass effects to model the effect of an incompressible fluid interacting with a
pipe structure;
is performed using one of the dynamic analysis procedures (“Dynamic analysis procedures:
overview,” Section 6.3.1);
6.10.1–2
Abaqus Version 5.8 ID:
Printed on:
ACOUSTIC ANALYSIS
•
can be used to model both interior problems, where a structure surrounds one or more fluid cavities,
and exterior problems, where a structure is located in a fluid medium extending to infinity; and
•
in Abaqus/Explicit can include air blast loading on structures using the CONWEP model.
Procedures available for acoustic analysis
Acoustic elements model the propagation of acoustic waves and are active only in dynamic analysis
procedures. They are most commonly used in the following procedures:
•
Direct solution, steady-state, harmonic analysis.
analysis,” Section 6.3.4.
•
•
Frequency analysis. See “Natural frequency extraction,” Section 6.3.5.
•
Explicit dynamic analysis. See “Explicit dynamic analysis,” Section 6.3.3.
Subspace-based steady-state dynamic analysis.
analysis,” Section 6.3.9.
See “Direct-solution steady-state dynamic
See “Subspace-based steady-state dynamic
Acoustic analysis can also be performed using:
•
Direct time integration analysis.
Section 6.3.2.
•
•
•
Complex frequency analysis. See “Natural frequency extraction,” Section 6.3.5.
•
Dynamic fully coupled temperature-displacement analysis. See “Fully coupled thermal-stress
analysis,” Section 6.5.3.
See “Implicit dynamic analysis using direct integration,”
Mode-based transient dynamic analysis. See “Transient modal dynamic analysis,” Section 6.3.7.
Mode-based steady-state dynamic analysis. See “Mode-based steady-state dynamic analysis,”
Section 6.3.8.
In general, analysis with acoustic elements should be thought of as small-displacement linear
perturbation analysis, in which the strain in the acoustic elements is strictly (or overwhelmingly)
volumetric and small. In many applications the base state for the linear perturbation is simply ignored:
for solid structures interacting with air or water, the initial stress (if any) in the air or water has negligible
physical effect on the acoustic waves. Most engineering acoustic analyses, transient or steady state, are
of this type.
An important exception is when the acoustic perturbation occurs in a gas or liquid with high-speed
underlying flow. If the magnitude of the flow velocity is significant compared to the speed of sound in
the fluid (i.e., the Mach number is much greater than zero), the propagation of waves is facilitated in
the direction of flow and impeded in the direction against the flow. This phenomenon is the source of
the well-known “Doppler effect.” In Abaqus/Standard underlying flow effects are prescribed for nodes
making up acoustic elements by specifying an acoustic flow velocity.
Acoustic elements can be used in a static analysis, but all acoustic effects will be ignored. A
typical example is the air cavity in a tire/wheel assembly. In such a simulation the tire is subjected
to inflation, rim mounting, and footprint loads prior to the coupled acoustic-structural analysis in which
the acoustic response of the air cavity is determined. See “Defining ALE adaptive mesh domains in
6.10.1–3
Abaqus Version 5.8 ID:
Printed on:
ACOUSTIC ANALYSIS
Abaqus/Standard,” Section 12.2.6, and “ALE adaptive meshing and remapping in Abaqus/Standard,”
Section 12.2.7, for more information.
Acoustic elements also can be used in a substructure generation procedure to generate coupled
structural-acoustic substructures. Only structural degrees of freedom can be retained. The retained
eigenmodes must be selected when an acoustic-structural substructure is generated. In a static analysis
involving a substructure containing acoustic elements, the results will differ from the results obtained in
an equivalent static analysis without substructures. The reason is that the acoustic-structural coupling is
taken into account in the substructure (leading to hydrostatic contributions of the acoustic fluid), while the
coupling is ignored in a static analysis without substructures. More details on coupled structural-acoustic
substructures can be found in “Defining substructures,” Section 10.1.2.
A volumetric drag coefficient, , can be defined to simulate fluid velocity-dependent pressure
amplitude losses. These occur, for example, when the acoustic medium flows through a porous matrix
that causes some resistance (see “Acoustic medium,” Section 26.3.1), such as a sound-deadening
material like fiberglass insulation. For direct time integration dynamic analysis we assume there are
no significant spatial discontinuities in the quantity
, where
is the density of the fluid (acoustic
medium), and that the volumetric drag is small at acoustic-structural boundaries. These assumptions,
which can limit the applicability of the analysis, are discussed further in “Coupled acoustic-structural
medium analysis,” Section 2.9.1 of the Abaqus Theory Manual.
The direct-solution steady-state dynamic harmonic response procedure is advantageous for
acoustic-structural sound propagation problems, because the gradient of
need not be small and
because acoustic-structural coupling and damping are not restricted in this formulation. If there is no
damping or if damping can be neglected, factoring a real-only matrix can reduce computational time
significantly; see “Direct-solution steady-state dynamic analysis,” Section 6.3.4, for details.
Some fluid-solid interaction analyses involve long-duration dynamic effects that more closely
resemble structural dynamic analysis than wave propagation; that is, the important dynamics of the
structure occur at a time scale that is long compared to the compressional wave speed of the solid
medium and the acoustic wave speed of the fluid. Equivalently, in such cases, disturbances of interest in
the structure propagate very slowly in comparison to waves in the fluid and compressional waves in the
structure. In such instances, modeling of the structure using beams is common. When these structural
elements interact with a surrounding fluid, the important fluid effect is due to motions associated with
incompressible flow (see “Loading due to an incident dilatational wave field,” Section 6.3.1 of the
Abaqus Theory Manual). These motions result in a perceived inertia added to the structural beam;
therefore, this case is usually referred to as the “virtual mass approximation.” For this case Abaqus
allows you to modify the inertia properties of beam and pipe elements, as described below. Loads on
the structure associated with incident waves in the fluid can be accommodated under this approximation
as well.
Natural frequency extraction
Abaqus can compute both real and complex eigensolutions for purely acoustic or structural-acoustic
systems, with or without damping. Exterior acoustic problems may also be solved.
6.10.1–4
Abaqus Version 5.8 ID:
Printed on:
ACOUSTIC ANA