Modeling Lare Deformations Phenomenon with Altair OptiStruct

2015 European Altair Technology Conference
September 29 to October 1 | Paris
Technical Seminar
Modeling Lare Deformations
Phenomenon with Altair
OptiStruct
Harold Thomas – thomas@altair.com
Join, Contribute, Exchange
See full agenda at www.altairatc.com/europe

Harold Thomas
Vice President, OptiStruct
Altair Engineering
Large Displacement Analysis with OptiStruct
Concepts and Analysis for Structures using Nonlinear Methods

Copyright © 2015 Altair Engineering, Inc. Proprietary and Confidential. All rights reserved.
4
HyperWorks Unlimited
Unlimited Vendors
Limited Benefits
Single Vendor
Unlimited Benefits
Single Vendor
Unlimited Benefits
Traditional
HPC CAE
HWUL
Physical Appliance
HWUL
Virtual Appliance

5
Agenda
• Nonlinear Analysis
• Large Displacements
• Nonlinear Geometry
• Follower Forces and Pressures
• Hyperelastic Materials
• Finite Sliding (14.0)

6
NLPARM Definition
NLPARM entry controls the incremental and iterative solution processes
• NINC: Number of load increments
• MAXITER: Maximum number of iterations before the computation is terminated
• CONV: Flags to select convergence criteria (U,P,W or any combination)
• U: Displacement P: Load W: Work
• EPSU, EPSP, EPSW: Error tolerances
• MAXLS: Maximum number of line search iterations
• LSTOL: Line search tolerance
(1) (2) (3) (4) (5) (6) (7) (8) (9)
NLPARM ID NINC KSTEP MAXITER CONV
EPSU EPSP EPSW MAXLS LSTOL

7
Setting up Path-Dependent Problems
Path-dependent problems require setting up subcases which continue from
the final state of a previously run subcase
• Subcase continuation is activated using the control card CNTNLSUB
• Path dependent problems include plasticity and contact analysis with friction
• Can create complex loading paths, e.g. loading-unloading process in plasticity
CNTNLSUB added above subcase list will be active for all nonlinear subcases
CNTNLSUB can also be added to specific subcases
• CNTNLSUB, YES:
This nonlinear subcase continues the solution from the nonlinear subcase preceding.
“Preceding” refers to the sequence in the input deck and NOT the numbering of the subcases
• CNTNLSUB, NO:
This nonlinear subcase executes a new solution sequence starting from the initial, stress-free
state of the model.
• CNTNLSUB, SID:
This nonlinear subcase continues the nonlinear solution from the subcase with the ID given
through SID. The subcase must precede the current subcase in the deck and must be a
nonlinear subcase of the same type.

8
Geometric Nonlinearity
A typical challenge for geometric nonlinear analysis is a snap-through model
• The full force displacement curve is only for displacement controlled scenario
• The applied load necessary to move the bars down increases until they are horizontal
• Then the load changes sign as it transitions back into a stable position
• Finally the load starts to increase again when the stable position has been reached

9
Large Displacements Setup in OptiStruct
Large displacements consideration can be toggled using PARAM, LGDISP
• For a value of 0, large displacements are not considered
• For a value of 1, large displacements are considered
• Not available for Optimization
Allowable elements in large displacement solutions include:
• CHEXA, CTETRA, RROD, CBAR, CBEAM, RBAR, RBE2, and RBE3 are fully supported
and give large displacement results
• Shell, Gasket, and Bushing elements are allowed in the deck but use small displacement
theory
Elements that are currently not allowed in the deck for large displacement
analysis
• CGAP, CGAPG, CWELD, CSEAM, CFAST, RBE1, CROD, CELAS, CONM
Supported materials include:
• Elastic and elasto-plastic material cards (MAT1,MATS1)
• Hyperelastic materials (MATHE)
• Nonlinear Elasticity is not allowed.
• Anisotropic Solid (MAT9) materials

10
Follower forces and pressure
Follower forces and pressure are used if the force/pressure used for loading
will need to update its orientation with respect to changing geometry location
and orientation throughout the analysis
No Follower Force Follower Force

11
Follower Forces and Pressure Setup
There are two ways to enable follower forces and pressures in an OS deck
• PARAM, FLLWER
• Simple setup
• One entry for all loads
• Bulk card FLLWER and Subcase Information Entry
• Subcase specific setting
• Different setting for specific load case ID
GRIDs used in the above loads are necessary to
determine the direction with changing geometry

12
Follower Forces and Pressure Setup
Currently, the following load types are supported for follower force/pressure:
• FORCE1
• FORCE2
• PLOAD4
• GRIDs used in the above cards (G1, G2, Gn…) are necessary to determine
the direction with changing geometry
(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)
FORCE1 SID G F G1 G2
(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)
FORCE2 SID G F G1 G2 G3 G4
(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)
PLOAD4 SID EID P1 P2 P3 P4 G1 G3 or G4
CID N1 N2 N3

13
Example of Follower Forces
Shown below is an example of a material undergoing large displacement
without and with follower force activated.

Nonlinear Analysis
• Follower loading
• Pressure and forces are supported
• Subcase dependent switch (FLLWER)
Pressure applied normal to the face

15
Hyperelasticity
Hyperelastic materials respond elastically when subject to very large strains
• Examples of hyperelastic materials include rubbers and foams
• Hyperelastic material modeling must account for both nonlinear behavior and large
reversible deformation
• Hyperelastic materials are fully or approximately incompressible

3
OptiStruct – Optimization-driven Design
Design and Optimization
Stiffness
Durability
Stability
Noise
Vibrations
Powertrain
Durability
Heat Transfer
Kinematics
Dynamics

17
Hyperelasticity is a Large Displacement Solution
Large Displacement Nonlinear Analysis does have limitations for resolution
and element compatibility
• The following elements can exist in the model, but they will be resolved using small
displacement theory:
• SHELL
• GASKET
• BUSHING
• The following elements are not allowed and OptiStruct will error out if they are present:
• CGAP
• CGAPG
• CWELD
• CSEAM
• CFAST
• RBE1
• CROD
• CELAS
• CONM

18
Stress-Strain relationship
A general hyperelastic constitutive law can be stated as:
This stress-strain relationship derives from a strain energy potential function (U) where
• S = second Piola_Kirchhoff stress tensor
• E = Lagrangian strain tensor
• U= strain energy function per unit undeformed volume
• C = Right Cauchy-Green deformation tensor
The strain energy potential function defines the strain energy stored in the
material per unit of initial/undeformed volume
This definition depends on two important concepts:
• Principal stretch ratios
• Volume strain
C
CU
E
EU
S
∂
∂
=
∂
∂
=
)(
2
)(

19
Principal Stretch Ratios
The principal stretch ratio is a deformative measure λ, calculated by:
where are principal stretch ratios alone the edges of the block such that
it follows:
321 ,, λλλ
eng
undeformed
deformed
L
L
ελ +== 1

20
Volume Strain
Similarly, the volume strain J is a ratio of deformed to undeformed volume
• If thermal expansion is involved, elastic volume strain becomes
• For incompressible hyperelastic material J=1.
thermal
total
elas
J
J
JJ ==

21
Strain Energy Potential
For isotropic hyperelasticity, strain energy potential U is a function of the
principal invariants of C:
where I1, I2, I3 are the three strain invariants. They can be expressed as a
function of principal stretch, λ1, λ2, λ3, and volume strain, J, through the
following relations:
))(),(),(( 321 CICICIUU =
22
3
2
2
2
13
2
1
2
3
2
3
2
2
2
2
2
12
2
3
2
2
2
11
JI
I
I
==
++=
++=
λλλ
λλλλλλ
λλλ

22
Strain Energy Potential
For incompressible hyperelastic material, the strain energy function can be
expressed in the term of deviatoric and volumetric strain energy functions,
Where the deviatoric invariants for incompressible material are:
)(),( 21 JUIIUU vd +=
3,2,1
3/2
=
= −
i
IJI ii
12
3 == JI

23
Hyperelasticity in FEA
Hyperelastic material behavior is described with a number of models:
• Mooney-Rivlin
• Yeoh
• Arruda-Boyce
• Several other types of mathematical models
These models are developed based on a combination of physical behaviors
and theoretical considerations
Given empirical data, parameters for these models can be closely fitted to
best represent the given test data over the desired strain range by deriving
the constants for the models from the data.
Assumptions for these hyperelastic material models include:
• Isotropic material response: linear thermal expansion, fully reversible deformation
• Fully or nearly incompressible: the volume of the material doesn’t change except for
thermal expansion

24
Volumetric Strain Energy Functions in OptiStruct
OptiStruct uses a first-order volumetric strain energy function for hyperelastic
material modeling

25
MATHE Card Parameters
The MATHE card is used to represent hyperelastic materials in OptiStruct
• Polynomial form is available and various material types can be defined by specifying
the corresponding coefficients
• User can directly define the material constants
• User can define the test data and evaluate the material constants using experimental
curve fit method
(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)
MATHE MID Model NU RHO TEXP TREF
C10 C01 D1 TAB1 TAB2 TAB4
C20 C11 C02 D2 NA ND
C30 C21 C12 C03 D3
…

26
Full Polynomial
The Mooney-Rivlin hyperelastic model uses a full polynomial approach
• These models are normally used to model the large strain nonlinear behavior of
incompressible materials, e.g. rubber.
• Two term Mooney-Rivlin is equivalent to polynomial form with
• Mooney-Rivlin materials don’t have special physical meaning, but merely are curve-fits of
various polynomials to test data. The coefficients such as are determined from
curve-fitting these equations to experimental data.
20110110 ,,, CCCC
1,121 === elasJNN
2
1
201110 )1(
1
)3()3( −+−+−= elasJ
D
ICICU

27
Partial Polynomial
The partial polynomials models are derived from Mooney-Rivlin, with the
three term Mooney-Rivlin equivalent to the polynomial form:
The James-Green-Simpson (3rd order deformation) model:
Signiorini material:
Third order invariant material:
2
1
3
130
2
1202111201110 )1(
1
)3()3()3)(3()3()3( −+−+−+−−+−+−= elasJ
D
ICICIICICICU
2
1
2
120201110 )1(
1
)3()3()3( −+−+−+−= elasJ
D
ICICICU
2
1
2
1202111201110 )1(
1
)3()3)(3()3()3( −+−+−−+−+−= elasJ
D
ICIICICICU
21 =N 00220 == CC
2
1
2111201110 )1(
1
)3)(3()3()3( −+−−+−+−= elasJ
D
IICICICU

29
Characterization Tests for Calibrating Hyperelasticity
Material characterization employs a series of standard tests to measure the
stress-strain response of materials such as rubber
• Uniaxial tension
• Equal-biaxial extension
• Planar tension to simulate pure shear

30
Characterization Tests for Calibrating Hyperelasticity
Using the empirical and FE data from the tests to perform a curve fitting
shows the applicability of the modeling solutions
Uniaxial test
Biaxial test
Planar test

31
The MATHE card is used to represent hyperelastic materials in OptiStruct
• Polynomial form is available and various material types can be defined by specifying
the corresponding coefficients
• User can directly define the material constants
• User can define the test data and evaluate the material constants using experimental
curve fit method
(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)
C30 C21 C12 C03 D3
…

32
General parameters for the MATHE card include:
• MID: Unique material identification number
• Model: Specifies the type of hyperelastic material model (Mooney, Yeoh)
• NU: Poisson’s ratio
• RHO: Material density
• TEXP: Coefficient of thermal expansion
• TREF: Reference temperature
(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)
C30 C21 C12 C03 D3
…

33
(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)
C30 C21 C12 C03 D3
…
Users can directly define material constants by using Cpq and Dp
• Cpq: Material constants related to distortional deformation
• Dp: Material constants related to volumetric deformation
• NA: Order of the distortional strain energy polynomial function (will be determined
automatically, based on number of Cpq)
• ND: Order of the volumetric strain energy polynomial function (will be determined
automatically, based on number of Dp)

34
MATHE – Test Data Input
Users can define test data tables to curve fit with test data
• NA: Order of the distortional strain energy polynomial function
• ND: Order of the volumetric strain energy polynomial function
• TAB1: Table that contains uniaxial tension-compression data
• TAB2: Table that contains equi-biaxial tension data
• TAB4: Table that contains pure shear (planar test) data
Tables needs to be TABLES1, where x-values are stretch ratios and y-values are
engineering stress
(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)
C30 C21 C12 C03 D3
…

35
Test Data Input
When inputting full/partial polynomial input, the test data is shown in the deck
as follows:
Uni-axial data Bi-axial data
Planar data
Explicitly defined zero
constants

36
Test Data Input
When users have limited test data available, reduced polynomial forms, such
as Yeoh, is recommended.
Only one set of test data is
given
Table data is given as stretch (L/L0) vs engineering stress

37
PLSOLID Definition
PLSOLID cards are used to define hyperelastic solid elements in OptiStruct
• PID: Unique solid element property identification number
• MID: identification number of a MATHE
• Supported elements: first and second order CHEXA, CPENTA, CTETRA
(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)
PLSOLID PID MID

38
Example: Small and Large Displacement of a Block
Objectives:
• Create PLSOLID property
• Create plastic material
• Assign material to property
• Assign property to components
• Create boundary conditions and loads
• Set control cards for small displacement
• Create nonlinear load steps
• Run the model in OptiStruct
• Post-process results in HyperView
• Set control cards for large displacement
• Re-run the model in OptiStruct
• Compare results in HyperView with previous

39
Example: Torque of a Hyperelastic Rectangular Block
Large displacement is necessary to provide the correct spatial and state
representation of parts undergoing significant strains

40
Example: Compression of a Hyperelastic Part
Objectives:
• Create Element Properties
• Create MATHE material
• Add PLSOLID property values
• Activate large displacement solution
• Set output requests
• Create load steps
• Edit material polynomial order
• Run the model in OptiStruct
• Post-process results in HyperView

41
Exercise Results:
• File: rubber_original.h3d
• Display type: Shaded elements and mesh lines
• Contour: Element Strains (2D & 3D)(vonMises, Max) result type
Example: Compression of a Hyperelastic Part

42
Hyperelastic Modeling Tips and Tricks
Tips and tricks for modeling hyperelastic materials includes:
• Selection of an appropriate material model is critical to a successful analysis.
• With limited test data, use reduced polynomial (Yeoh), Arruda-Boyce and Van Der Waals
behave similarly to Yeoh form. Full polynomial and Ogden forms behave badly, not
recommended to use.
• Order greater than 2 not recommended for fully polynomial form, third order partial
polynomial behaves nicely .
• Use first order element to avoid element distortion.

Arruda-Boyce Hyperelastic Material Model
OptiStruct v14.0

Comparing Different HE Models
• Benefit of Arruda-Boyce: good
curve-fitting even when test data is
limited, e.g. when only uniaxial data
is available
• A-B is good for higher strains
• A-B captures stiffening (upturn of
curve, not captured by N-H or M-R)
• Yeoh is similar to Arruda-Boyce
* - image courtesy Bbanerje, wikimedia

Implementation in OptiStruct
• Generalized polynomial (Mooney-Rivlin, Neo-Hookean, Yeoh)
• Arruda-Boyce

OptiStruct Setup
• MATHE for nonlinear hyperelastic material property (Arruda-Boyce)

Example – Sealing Analysis of a Packer
• A packer is used to form an annular seal between two concentric pipes
• For isolation purposes
• To separate different fluids
• …
• Usage in oil & gas industry

Model Setup (sectional view)
• Arruda-Boyce hyperelastic material model representing seal
• Surface-to-surface contact
• Finite sliding with friction
• Enforced displacement to piston
• Large displacement analysis
Annular
Seal
Concentric pipes
Fixed
Piston

Analysis Results

Innovation Intelligence®
OptiStruct 14.0

Nonlinear Analysis in 14.0
• The results available for each load increment
• New bulk and subcase information entry, NLOUT
• Output interval “delta” is determined by NINT option on NLOUT
• i.e. NLOUT,id,NINT,5 delta = 1/NINT (0.2,0.4,0.6,0.8,1.0)

Nonlinear Analysis
• Finite sliding
• The relationship between master and slave
will be updated during the nonlinear analysis
• Anisotropic material (MAT9) for solids in a
large displacement analysis
• Subcase dependent large displacement
switch
• NLPARM(LGDISP)

Nonlinear Analysis
• Time dependent loading input
• The amplitude of the loading is defined thru TABLED (TID) which will be
referenced by TLOAD
• No need to create multiple subcases to simulate loading/unloading sequence
• Nonlinear Adaptive convergence and time-stepping parameters for a large
displacement Analysis via NLADAPT
TLOAD SID EXCITEID TYPE TID
SUBCASE 1
DLOAD = 5
SPC = 3
NLPARM = 2
TABLED id

Follower Load

55
How to setup in OptiStruct?
Add FLLWER card for subcase dependence
To define another set of follower force parameters, which overrides the set of
parameters above, for specific loads. It can be repeated any number of times
Field Contents
ID Each FLLWER bulk data card must have a unique ID.
No default (Integer > 0)
OPT Options for the calculation for Follower Loads.
Default = 1 <-1, 0, 1, 2, 3>
= -1, 0: Follower force calculation is not activated.
= 1: Follower effect is activated. For pressure load, both element surface
area and load direction are involved to calculate follower force. For
concentrated force, only the force direction is involved.
= 2: Follower effect is activated. For pressure load, only element surface
area is involved. For concentrated force, only the force direction is involved
(same effect as FLLWER = 1).
= 3: Follower effect is activated. For pressure load, only load direction is
involved. For concentrated force, only the force direction is involved (same
effect as FLLWER = 1).
LSIDi Identification number of a PLOAD4 or FORCE1/FORCE2 Bulk Data Entry.
No default (Integer > 0)

56
Add PARAM,FLLWER card for global definition
Parameter Values Description
FLLWER <-1, 0, 1, 2, 3>
Default = 1
Parameter for the calculation of follower forces introduced by pressure loads
(only PLOAD4 bulk data entry) and concentrated forces
(only FORCE1/FORCE2bulk data entries) in large displacement nonlinear
analysis.
= -1 or 0:
Follower force calculation is deactivated.
= 1:
Follower effect is enabled.
For pressure load, both the changes of element surface area and the direction
of the load are involved to calculate the follower force.
For concentrated force, only the force direction is involved.
= 2:
For pressure load, only the change of element surface area is involved to
calculate the follower force.
For concentrated force, only the force direction is involved (same effect as
FLLWER = 1).
= 3:
For pressure load, only the change of load direction is involved to calculate the
follower force.
For concentrated force, only the force direction is involved (same effect as
FLLWER = 1).

57
Capabilities & Limitations
• Supports
• Only elements supported for large displacement
analysis are supported for follower load
• Recommendations
• It is recommended to use hash assembly for
subcases with follower loads
• Follower load stiffness is generally un-symmetric
• OptiStruct supports both symmetric solvers and
un-symmetric solvers for follower loadcase
• BCS solver should not be used with hash
assembly and un-symmetric solver for follower
load subcases
• MUMPS solver should not be used with
PARAM,HASHASSM,NO
• Limitation
• If a load set is applied in both continuation
subcases(CNTNLSUB), the FLLWER option of
the load set must be exactly the same in the two
subcases
• Only PLOAD4, FORCE1 and FORCE2 loads
are currently supported

58
Solver deck
Cards to run follower load
Param card to turn on follower force calculation
Param card to turn on large displacement analysis
Bulk data cards
Param cards

Example
Problem Description
A chair frame has been loaded with 5000N force(extreme loading)
Constrained in all dof

Example
Results
With follower load, the stiffness and strength of the frame are accurately predicted
With Follower Load No Follower Load
Max Disp: 97mm Max Disp: 106mm

Time Dependent Loading

62
• The amplitude of loading can be
time dependent
• It helps combine multiple sequential
subcases into one
• One such example is to simulate
loading/unloading sequence
• This is supported under non-linear
static analysis and not transient
analysis

63
• The amplitude of the loading is defined thru TABLED (TID) card
• TABLED card will be referenced by TLOAD1/TLOAD2
• It is supported in NLSTAT subcase
• TLOAD can be referenced by DLOAD in NLSTAT
• Note that the default termination time is 1 and can be changed on TTERM
field in NLPARM
• Supports DAREA, SPCD, FORCEx, MOMENTx, PLOADx, RFORCE, QVOL,
QBDY1, ACCEL, ACCEL1, ACCEL2, or GRAV entries in EXCITEID
Setup
TLOAD SID EXCITEID TYPE TID
TABLED id: loading curve
SUBCASE 1
ANALYSIS NLSTAT
DLOAD = SID of TLOAD
SPC = 3
NLPARM = 2

64
Solver deck
Cards to run time dependent loading
NLSTAT Analysis
TABLED1 ID
Load Excite ID
Termination time
Default = 1

Example
Problem Description
A chair frame has been loaded with 5000N force(extreme loading) and then unloaded
Constrained in all dof

Example
Displacement Results
Loading-Unloading in One SubcaseLoading-Unloading in Two Subcases

Finite Sliding

68
What is Finite Sliding?
• Master and slave surfaces can
undergo large motion both
absolutely and relatively
• A slave node can transfer load to
any node on the master surface
• Since slave nodes can interact with
any node on master surface, they
have to be constantly monitored
• It is computationally expensive

69
When and why?
• Relative motion between master and
slave surfaces is more than a
fraction of their element sizes
• Contact between master and slave
needs to be updated
• If above points are not true, small
sliding is recommended as it is
computationally inexpensive

70
TRACK = SMALL (default) / FINITE

71
Limitations
• Finite sliding is effective only in
large displacement nonlinear
analysis
• Finite sliding works only with hash
assembly and MUMPS solver
• Finite sliding is not supported for
self contact

72
Solver deck
Cards to run finite sliding
NLSTAT Analysis
Hash Assembly
Track = FINITE
Solver Type = MUMPS

Example
Problem Description
A rack and pinion gear mechanism
A moment is applied to the gear;
Other d.o.f are constrained(12345)
The rack is free to slide on X direction;
Other d.o.f are constrained(23456)

75
Thank you

Modeling Lare Deformations Phenomenon with Altair OptiStruct

Recommended

More Related Content

What's hot (20)

Viewers also liked (11)

Similar to Modeling Lare Deformations Phenomenon with Altair OptiStruct (20)

More from Altair (20)

Recently uploaded (20)

Modeling Lare Deformations Phenomenon with Altair OptiStruct