Siemens | TW 701 Series | Nonlinear Analysis Using Femap with NX Nastran

Nonlinear Analysis Using Femap with NX Nastran
Nonlinear Analysis Using Femap with NX Nastran
Chip Fricke, Principal Applications Engineer, Siemens PLM Software
Unrestricted © Siemens AG 2013 All rights reserved.
Agenda
Nonlinear Analysis Using Femap with NX Nastran
Who am I?
Overview of Nonlinear Analysis
Comparison of the NX Nastran
Nonlinear and NX Nastran Advanced
Nonlinear Solvers
Nonlinear Material Models
Comparison of Results –
Basic vs. Advanced Nonlinear
NX Nastran Basic Nonlinear Analysis
NX Nastran Advanced Nonlinear
Analysis
Femap Examples and NX Nastran
Technical References
Unrestricted © Siemens AG 2013 All rights reserved.
Page 2
Siemens PLM Software
About Your Presenter
Principal Applications Engineer with the
Femap Product Development Group of
Siemens PLM Software
31 years experience in the PLM Software
industry
• Pre-sales
• Technical Marketing
• Product Management
Aerospace Industry experience at Boeing
• Lead Engineer on the 757 program
BSCEE, University of Wisconsin –
Madison
Email: chip.fricke@siemens.com
Unrestricted © Siemens AG 2013 All rights reserved.
Page 3
Twitter: @ae4mcae
Siemens PLM Software
What Defines Nonlinear Analysis
Material Nonlinearity
Transient (time-dependent) loading
Large displacement
Contact due to
• Closure or opening of large gaps
• Rigid contact bodies
• “Double-sided” contact
• Edge to Edge contact
• Collision or impact
Unrestricted © Siemens AG 2013 All rights reserved.
Page 4
Siemens PLM Software
NX Nastran Basic Nonlinear vs.
NX Nastran Advanced Nonlinear
NX Nastran
Basic Nonlinear
NX Nastran
Advanced Nonlinear
Large Strain (> 10%)
-

Linear Elastic Material


Elasto-plastic Material


Plastic Material


Creep Material


(added in NX Nastran 8)

Transient loading


Gap and Slide Line Contact


Rigid Body Contact
-

Double-sided Contact
-

Edge-to-edge Contact

-
Impact
-

Capability
Hyperelastic Material
Unrestricted © Siemens AG 2013 All rights reserved.
Page 5
Siemens PLM Software
Nonlinear Material Models
For Isotropic materials, select the Nonlinear
tab in the Define Material dialog box
• Specify the Nonlinearity Type and their
parameters
Hyperelastic materials are designated by
setting the Type to Hyperelastic
• Hyperelastic material properties
are complex and should be supplied by the
material supplier or by testing
Additional NX Nastran
Nonlinear Materials are
available as “Other Types”
Unrestricted © Siemens AG 2013 All rights reserved.
Page 6
Siemens PLM Software
Linear Elastic Material
No strain hardening
• Used only for Isotropic materials.
• Define with a vs. Stress OR a
Stress vs. Strain Function
Unrestricted © Siemens AG 2013 All rights reserved.
Page 7
Siemens PLM Software
Elasto-Plastic Material
Basic assumptions:
• Von Mises yield condition
• Isotropic, kinematic or mixed hardening
• Bilinear or multi-linear stress-strain curves
• Thermal strains can be included
This material can be used with:
• Small displacements/small strains
• Large displacements/small strains
• Large displacements/large strains
• Temperature dependence
Unrestricted © Siemens AG 2013 All rights reserved.
Page 8
Siemens PLM Software
Nonlinear Plastic Material
Strain hardening
Specify Initial Yield Stress, Yield Criterion and Function Dependence (vs.
Stress or Stress vs. Strain Function)
Unrestricted © Siemens AG 2013 All rights reserved.
Page 9
Siemens PLM Software
NX Nastran Plasticity Test Model
Simple Test Coupon Meshed with Hex
Elements
• Applied Tension Load = 2 MegaN
Generic Carbon Steel Material
• E = 200,000 Mpa
• Yield Stress = 472 MPa
Unrestricted © Siemens AG 2013 All rights reserved.
Page 10
Siemens PLM Software
Comparison between NX Nastran Linear Statics,
Basic Nonlinear and Advanced Nonlinear Analyses
Maximum
Von Mises
Stress
Axial
Deformation
Linear Statics
1041 MPa
1.52 mm
NL Statics with
Plasticity
1035 MPa
36.2 mm
Adv. NL Statics
with Plasticity
1218 Mpa
26.8 mm
Unrestricted © Siemens AG 2013 All rights reserved.
Page 11
Siemens PLM Software
Comparison of NX Nastran Basic Nonlinear
vs. Advanced Nonlinear Results Von Mises Stress vs. Strain Curves
Unrestricted © Siemens AG 2013 All rights reserved.
Page 12
Siemens PLM Software
NX Nastran Basic Nonlinear Analysis
Settings
All NX Nastran Basic Nonlinear analyses
require the specification of:
• Basic Iteration settings
• Stiffness Updates
• Output Control
• Convergence Tolerances
• Optional Solution Strategy Overrides
Define these options in either:
• As part of a Load Set in the Load Set Options
for Nonlinear Analysis dialog box OR
• Nonlinear Options in an Analysis Set’s Master
Requests and Conditions – Nonlinear Options
dialog box
Unrestricted © Siemens AG 2013 All rights reserved.
Page 13
Siemens PLM Software
NX Nastran Basic Nonlinear Significant Differences in Analysis Options
Analysis Set Manager Options
Nonlinear
Statics
Stiffened Modal – Runs a Stressstiffened Normal Modes Analysis
at the End of each Subcase

Multi-Case

Modal/Buckling + Dynamics –
equivalent to a Direct or Modal
Transient Dynamic Response
analysis with Nonlinear Materials
• Nonlinear damping must be
specified as a material attribute
• Force and GPForce results not
available
Nonlinear Options – Creep
Nonlinear
Transient


Unrestricted © Siemens AG 2013 All rights reserved.
Page 14
Siemens PLM Software
Contact Modeling –
NX Nastran Basic Nonlinear
Contact can be modeled with two (2) element types:
• SLIDE LINE – element node connectivity must be defined correctly
• GAP – use the Mesh > Connect > Closest Link tool to create multiple Gap
element connections
Initial Gap can
be used to define
a gap other than
the physical gap
between the
ends of the GAP
element
Unrestricted © Siemens AG 2013 All rights reserved.
Page 15
Siemens PLM Software
GAP Element Example –
Use of Orientation Vector and Initial Gap Distance
The Orientation vector of a gap
element defines the direction of
positive direction of a GAP
element.
Unrestricted © Siemens AG 2013 All rights reserved.
Page 16
Siemens PLM Software
GAP Element Example –
Use of Orientation Vector and Initial Gap Distance
Applied Displacement of 0 to -5
to 0 applied to the right end of
the GAP element
• GAP element is oriented with
the X-Axis of the Global
Rectangular CSYS
• Initial Gap is set to 2.5
• Note how the top of the beam
starts to displace after the GAP
displacement = 2.5
Unrestricted © Siemens AG 2013 All rights reserved.
Page 17
Siemens PLM Software
GAP Element Example –
Use of Orientation Vector and Initial Gap Distance
Applied Displacement of 0 to -5
to +5 to 0 applied to the right end
of the GAP element
• GAP element is oriented with
the X-Axis of the Global
Rectangular CSYS
• GAP element is reversed and
the Initial Gap is set to -2.5
• Note how the top of the beam
starts to displace after the GAP
displacement = 2.5
Unrestricted © Siemens AG 2013 All rights reserved.
Page 18
Siemens PLM Software
NX Nastran Advanced Nonlinear Statics and
Transient vs. Advanced Nonlinear Explicit
NX Nastran Advanced Nonlinear Static /
Advanced Nonlinear Transient (SOL 601)
NX Nastran Advanced Nonlinear Explicit
(SOL 701)
For statics and low frequencies dominate the
dynamic response of the structure.
For problems of highly dynamic, short duration
events.
Examples: crush analysis, earthquake response
Examples: wave propagation, high speed impact
Unconditionally stable, so larger time steps can
be used
Conditionally stable; need small time steps
Equilibrium satisfied; greater confidence in
solution
More difficult to assess quality of solution
Assembly and solution of matrix with equilibrium
iterations; computational effort per step is high
No matrix assembly and no iterations;
computational effort per step is low
Requires more memory
Less memory for same mesh
All supported elements can be used
Certain elements and materials not supported
Solution may fail to converge in equilibrium
iterations
Analysis may fail due to diverging solution
Unrestricted © Siemens AG 2013 All rights reserved.
Page 19
Siemens PLM Software
NX Nastran Advanced Nonlinear Solver - Range of
Analyses
Linear
Nonlinear Analysis
Displacement
Small
Small
Small
Large
Large
Strain
Small
Small
Small
Small
Large
Default is small displacement, small strain
Large strain (PARAM,LGSTRN,1) automatically implies large displacement
(PARAM,LGDISP,1)
• Set in the Analysis Set’s NASTRAN Bulk Data Options dialog box.
Large strain formulation is used only for 3D solid, plane strain, axisymmetric and
shell elements
Hyperelastic material models (MATHP and MATHE) automatically use large
strain formulation
Unrestricted © Siemens AG 2013 All rights reserved.
Page 20
Siemens PLM Software
Which Advanced Nonlinear Solution Should You
Use?
In general, use Advanced Nonlinear Statics or Advanced Nonlinear Transient
• Use Advanced Nonlinear Transient if inertia effects are important – otherwise
use Advanced Nonlinear Statics
• If SOL 601 fails to converge, use SOL 701 and compare results at the last SOL
601 converged step
• You can also do a restart of a Sol601 solution in Sol701
Note that for certain classes of problems, such as drop tests and metal forming,
both solutions may be comparable in performance
Unrestricted © Siemens AG 2013 All rights reserved.
Page 21
Siemens PLM Software
Advanced Nonlinear Explicit Notes
Several NX Nastran elements supported for Sol601 are not supported in Sol701:
• Plane strain and axisymmetric elements
• Higher-order elements parabolic elements are also not supported such as 10node tetrahedrals, 20-node bricks, and 8-node shells
Reduced integration elements with hour-glassing should not be used. Using such
element formulations can have adverse effects on the accuracy of the solution.
Gasket and creep materials are not supported. For hyperlastic materials,
Mooney-Rivlin and Ogden models are supported but not Arruda-Boyce and
hyperfoam models.
Nearly incompressible material will significantly reduce the stable time step size.
The compressibility of the material can be increased (e.g., reducing bulk modulus
of hyperelastic materials) to achieve a reasonable time step size
Glued contact and pre-load bolt features are not available
Unrestricted © Siemens AG 2013 All rights reserved.
Page 22
Siemens PLM Software
NX Nastran Advanced Nonlinear Setting Connection Properties
To set the Connection Property for Advanced Nonlinear problems involving
contact, you will need to select either the NX Adv Nonlin tab or the NX Explicit
tab in the Define Connection Property dialog box.
• Specify the Contact Type as Contact or Glued for Sol601.
• For details on these settings, see Sections 4.4.3.2 and 4.4.3.3 of the Femap
Commands manual.
• Set Double-Sided and
Offset Type options for
planar element contact
Unrestricted © Siemens AG 2013 All rights reserved.
Page 23
Siemens PLM Software
Advanced Nonlinear Connection Regions
Advanced Nonlinear supports both flexible and RIGID Connection Regions:
• Both regions can be modeled with either Surfaces or Element Faces
• Correct specification of positive or negative directions are critical
• A single Connection Region should be tangent continuous within a reasonable
tolerance – i.e, no sharp discontinuities
Unrestricted © Siemens AG 2013 All rights reserved.
Page 24
Siemens PLM Software
Rigid Connection Regions
RIGID regions require a Reference Node and can only have Enforced
Displacement or Enforced Rotation loads applied to the Reference Noden
RIGID regions internally are treated as
surfaces, therefore, mesh size, aspect
ratio and distortion on planar regions
is not critical – e.g. a planar surface
can be meshed as a single element
Offsets and shell thicknesses are
ignored, use for display purpose
• Femap requires the assignment of a
material to the solid or shell element
faces and a positive thickness
attribute for shell elements
Unrestricted © Siemens AG 2013 All rights reserved.
Page 25
Siemens PLM Software
Advanced Nonlinear Static/Transient Analysis
NXSTRAT Solver Parameters
Unrestricted © Siemens AG 2013 All rights reserved.
Page 26
Siemens PLM Software
Advanced Nonlinear Static/Transient Analysis
NXSTRAT Solver Parameters
Specify the Solver as one of:
• Direct Sparse – default solver
• Multigrid – use for very large models
with Solid Tetrahedral elements only
• 3D Iterative – use for models with
mainly higher order solid elements
Convert Dependency to True Stress
can be used when Material attributes are
defined using true Stress/Strain values
Allow Element Rupture – when element
stress exceeds max allowable, element is
removed from subsequent solution time
steps (including Stiffness, Mass, etc.)
Unrestricted © Siemens AG 2013 All rights reserved.
Page 27
Siemens PLM Software
Advanced Nonlinear Analysis Convergence Control
– SOL601
Unrestricted © Siemens AG 2013 All rights reserved.
Page 28
Siemens PLM Software
NX Nastran Advanced Nonlinear Analysis Control –
SOL701
Unrestricted © Siemens AG 2013 All rights reserved.
Page 29
Siemens PLM Software
Examples and References
Femap Examples for NX Nastran Nonlinear:
• Example 25:
Plastic Deformation of Rod - Nonlinear Material
• Example 26:
Gap Contact - Cantilever Beam
• Example 27:
Large Deformation – Cantilever Beam
• Example 28:
Slide Line Contact – Hyperelastic Seals
• Example 29:
3-D Contact - Plastic Clip and Base
Femap Examples for NX Nastran Advanced Nonlinear:
• Example 30:
Large Deformation – Advanced Nonlinear (SOL 601)
• Example 31:
Surface to Surface Contact - Advanced Nonlinear (SOL 601)
• Same as NX Nastran Example 29, except uses Advanced Nonlinear solver
NX Nastran User Guides
• Handbook of Nonlinear Analysis (SOL 106)
• NX Nastran Basic Nonlinear Analysis User’s Guide
• Unrestricted
Advanced
Nonlinear
and Modeling Guide
© Siemens
AG 2013 Theory
All rights reserved.
Page 30
Siemens PLM Software
Q&A
Thank you!
Unrestricted © Siemens AG 2013 All rights reserved.
Was this manual useful for you? yes no
Thank you for your participation!

* Your assessment is very important for improving the work of artificial intelligence, which forms the content of this project

Download PDF

advertising