1. 3.5 ANSYS/LS-DYNA Enhancements
Elements 2D axisymmetric, plane stress, or plane strain
Materials Discrete, Mooney-Rivlin, Steinberg, Trans Aniso FLD
Part Inertia User-defined rigid body properties
Loading Local CS, birth/death, RB omega loads, EDVEL
Contact 2D, box IDs, part asmb, tied shell-edge to surface
Restarts Change settings, rigid/deformable conversion, etc.
Misc. EDREAD (ASCII Files) & Drop Test Module (DTM)
Workshop minute exercise showing several new features
ANSYS/LS-DYNA 5.6 enhancements focused on “usability” issues:
POST1 plots removed failed elements
RSYS was partially supported
Improved PART maintenance, including part selection
GUI made more “user-friendly” (logic, grouping, etc.)
Visualization tools; Document command mapping; etc.
Some new functions (adaptive meshing, RIMPORT for bricks, AG contact, new materials, etc.)
ANSYS/LS-DYNA 5.7 enhancements center on new functionality:
LS-DYNA 2D element support (including contact)
New EDVEL & EDDC replace deficient EDIVELO & EDCDELE
Greatly expand small restart capability (new commands)
New material models - fix COMBI165, Mooney-Rivlin, ...
New loading features, part inertia input, support of additional ASCII files, etc. increase capability
Training Manual
15 Aug 2000
3.5-1

2. ANSYS/LS-DYNA Enhancements 2D Elements
PLANE D, 4-Node Solid
3-node triangle available (not recommended)
Only Lagrangian formulation supported
UX, UY, VX, VY, AX, AY degrees of freedom
Y axis = symmetry axis for axisymmetric model
NO mixing of 2D and 3D element types permitted
PLANE162 KEYOPT Settings:
Keyopt(2) - Area weighted or volume weighted (AXISYM)
Keyopt(3) - Plane stress, axisymmetric, or plane strain
Only one 2D type can be used in any given analysis (i.e., you cannot have both axisymmetric and plane stress elements present in the same model)
PLANE162 modeled in X-Y plane (+X for axisymmetric case)
No real constants associated with PLANE162
18 materials (e.g., plasticity, composite, Mooney-Rivlin) supported
RSYS supported for displacements and stresses (not strains)
KEYOPT(3) maps to ELFORM parameter of *SECTION_SHELL card:
0=Plane Stress, 1=Axisymmetric, 2=Plane Strain
KEYOPT(2) also maps to ELFORM (Weighting: 0=Area, 1=Volume)
Lagrangian formulation (SETY parameter of *SECTION_SHELL command) is based on large strain deformation theory in which bodies of interest are discretized and the geometry is continuously updated over time as the mesh physically deforms. This formulation is used in implicit ANSYS, as well.
Training Manual
15 Aug 2000
3.5-2

3. ANSYS/LS-DYNA Enhancements Materials
New TB,DISCRETE,,,,TBOPT for COMBI165
8 spring/damper materials instead of real constants
COMBI165 part selection/plotting restriction lifted
Dummy material properties no longer needed
Modified TB,MOONEY,,,,TBOPT
TBOPT=0 - Direct input of Mooney-Rivlin coefficients
TBOPT=2 - Input test data (stress/strain or load/deflection)
Minor incompatibility with ANSYS 5.6 (most real constants not used now).
COMBI165 real constants 1-22 replaced with TB,DISCRETE and old real constants now become real constants 1-6.
Material type specified via TBOPT setting on TB,DISCRETE:
TBOPT 0-7 = MPMOD,,43-50 = LSTC Materials DS1-DS8
TBOPT = 0,2,3,5,6,7 = various spring formulations
TBOPT = 1,4 = linear and nonlinear damper formulations
No longer necessary to define dummy material properties for the COMBI165 elements, which were subsequently ignored. It is also clear that the particular discrete element either has a spring definition OR a damper definition - NOT both.
TB,MOONEY enhanced (including GUI).
*MOONEY (TBOPT=1) not supported, but LS-DYNA calculates 2-term coefficients.
Set gauge length = width = thickness = 1.0 to substitute stress vs. strain data for load vs. deflection data
Training Manual
15 Aug 2000
3.5-3

4. ANSYS/LS-DYNA Enhancements …Materials
Steinberg plasticity via TB,EOS,,,,5,EOSOPT
Deformations of solids at high strain rates with failure
Yield strength a function of temperature and pressure
Equation of State (EOS) used to determine pressure
Transversely anisotropic FLD via TB,PLAW,,,,10
Simulation of sheet forming processes
Flow Limit Diagram to compute maximum strain ratio
Available only for shell elements
*MAT_STEINBERG (LSTC material model #11) requires EOS
EOSOPT = 1 = Steinberg Linear Polynomial EOS = MPMOD,,51
EOSOPT = 2 = Steinberg Gruneisen EOS = MPMOD,,52
EOSOPT = 3 = Steinberg Tabulated EOS = MPMOD,,53
*MAT_FLD_TRANSVERSELY_ANISOTROPIC (LSTC material model #39)
TB,PLAW,,,,10 corresponds to MPMOD,,54
Training Manual
15 Aug 2000
3.5-4

5. ANSYS/LS-DYNA Enhancements Part Inertia
EDIPART Defines inertia for rigid bodies
Default is to have LS-DYNA calculate rigid body inertia properties from the finite element mesh
Specifying properties is more accurate than the default when the object is complicated and the mesh is coarse
Allows meshing only a portion of the total structure
Parts must already be defined (EDPART,CREATE)
Specify inertia properties and initial conditions
Location of center of mass (X, Y, Z)
Translational mass
Inertia tensor (IXX, IXY, IXZ, IYY, IYZ, IZZ)
Initial velocity (RBVX, RBVY, RBVZ, RBOX, RBOY, RBOZ)
Instead of having LS-DYNA calculate the inertia properties of a given rigid body, you can use EDIPART to directly enter inertia data (see below). EDIPART corresponds to the LS-DYNA *PART_INERTIA command.
EDIPART,PART,Option,Cvect,TM,IRCS,Ivect,Vvect,CID
PART = part number of existing rigid body (EDMP,RIGID)
Option = ADD/DELE/LIST (standard EDXX options)
Cvect = global Cartesian CG coordinates. Default = (0,0,0)
TM = translational mass (no default - must be defined)
IRCS = inertia tensor reference CS flag (0=global, 1=local)
Ivect = inertia tensor (cross terms ignored if IRCS=1)
Vvect = velocity vector (translational and rotational terms parallel to global Cartesian coordinate system)
CID = local CS ID previously defined with EDLCS - no default if IRCS=1
Training Manual
15 Aug 2000
3.5-5

6. ANSYS/LS-DYNA Enhancements Loading
EDLOAD,,LAB (LAB = RBOX, RBOY, RBOZ)
Rigid body rotational velocities now supported
EDLOAD,,LAB,KEY (KEY = CID = Local CS no.)
Apply loads in local CS (CID vector defined with EDLCS)
CID not valid for LAB = PRESS, ACLX/Y/Z, OMGX/Y/Z
Local CS for input only (output in global Cartesian CS)
EDLOAD,,, ,,, ,,,,BTIME,DTIME (Load birth and death)
BTIME valid for UX, ROTX, VX, AX, PRESS, RBUX, RBRX, RBVX, RBOX labels (and corresponding Y & Z labels)
DTIME valid for the above, with the exception of PRESS
CID, BTIME, & DTIME restrictions are in LS-DYNA
The LS-DYNA *BOUNDARY_PRESCRIBED_MOTION_RIGID card with VAD=0 provides rigid body rotational velocities.
Local coordinate systems simplify load definition. Labels PRESS (*LOAD_SEGMENT and *LOAD_SHELL_SET) and ACLX, ACLY, ACLZ, OMGX, OMGY, and OMGZ (*LOAD_BODY_GENERALIZED) do NOT support local coordinate systems.
Load curve birth and death times were BETA at 5.6, but are fully supported at Using a death time is more stable than defining the load curve up to the load termination time. EDLOAD labels UX/Y/Z, ROTX/Y/Z, VX/Y/Z, and AX/Y/Z (*BOUNDARY_PRESCRIBED_MOTION_SET) and RBUX/Y/Z, RBRX/Y/Z, RBVX/Y/Z, and RBOX/Y/Z (*BOUNDARY_PRESCRIBED_MOTION_RIGID), support both birth and death times, but EDLOAD label PRESS (*LOAD_SHELL_SET and *LOAD_SEGMENT) supports only an arrival time (BTIME).
The restrictions listed here for CID, BTIME, and DTIME are in the LS-DYNA solver and not due to the ANSYS/LS-DYNA interface.
Training Manual
15 Aug 2000
3.5-6

7. ANSYS/LS-DYNA Enhancements …Loading
EDVEL,Option, … New initial velocity command
VGEN - Option corresponding to old EDIVELO command
VELO - Option that can also be used in small restart analyses (i.e., not limited to only new analyses)
VGEN and VELO cannot both be used in same analysis
PHASE field of *INITIAL_VELOCITY_GENERATION automatically set based on EDDRELAX value:
PHASE=0 for EDDRELAX,OFF (or not issued)
PHASE=1 for EDDRELAX,DYNA or EDDRELAX,ANSYS
PHASE applicable to EDVEL,VGEN (not EDVEL,VELO) and determines what geometry (0=undeformed or 1=deformed) that velocities are applied to. No user input required!
EDVEL command needed to support new restart capabilities.
EDDRELAX,OFF = Normal transient dynamic analysis
EDDRELAX,DYNA = Preload by true dynamic relaxation
EDDRELAX,ANSYS = Preload by stress initialization to a prescribed geometry (implicit-to-explicit sequential solution)
Initial velocities are always applied to the structure in the transient dynamic phase of the analysis at TIME=0. The PHASE field on *INITIAL_VELOCITY_GENERATION determines which geometry the velocities will be applied to. LSTC Technical Support does not know of any case in which PHASE=0 would be desired following a preload analysis, so we set the PHASE field automatically, based on the EDDRELAX value (IDRFLG parameter on the *CONTROL_DYNAMIC_RELAXATION command), thereby ensuring the best results possible (i.e., no oscillations resulting from body forces that are not consistent with the applied velocity field).
Training Manual
15 Aug 2000
3.5-7

8. ANSYS/LS-DYNA Enhancements Contact
EDASMP,,ASMID,PART1, PART2, …,PART16
Up to 16 Parts can be grouped into an assembly
ASMID = part assembly no. (greater than highest part no.)
Cont and Targ fields of EDCGEN permit ASMID value
EDCGEN,ASS2D,Cont,Targ,FS
For 2D, only Automatic Single Surface Contact supported
Cont default is to use entire model (Targ not used)
Cont can also be limited to a part assembly (EDASMP)
FS (static coefficient of friction) also supported
Subcycling (EDCSC) not supported with 2D contact
EDASMP,Option,ASMID where Option=Add/Delete/List
EDASMP creates part assemblies via LS-DYNA *SET_PART_LIST
In 5.7, part assemblies only used with contact (Cont,Targ).
You first need to create (or update) the part list (EDPART) before using EDASMP. Further, the user-assigned number for the assembly, ASMID, must be greater than the highest part number in the list. Use LARGE ASMID numbers to be safe, as you may later wish to add more elements (and corresponding parts) to your model.
EDCGEN,ASS2D maps to *CONTACT_2D_AUTOMATIC_SINGLE_SURFACE Currently, this is the only 2D contact algorithm supported.
If Cont is used, the contact will be limited to that part assembly. Note that part IDs and nodal components are not applicable to this contact definition. Further, the Targ field is not used for 2D automatic single surface contact (i.e., the only supported algorithm at this time). The only other EDCGEN field that is supported is FS.
LS-DYNA does not permit using subcycling with 2D contact. Our experience with EDCSC indicates that it is common for this feature to hang an LS-DYNA analysis. Since it is only practical in simple 3D models, we do not recommend its use at all.
Training Manual
15 Aug 2000
3.5-8

9. ANSYS/LS-DYNA Enhancements ...Contact
EDCGEN,TSES - Tied shell-edge to surface contact
Glues the edge of a shell to another surface
Not applicable with rigid bodies
EDBX,,BOXID,XMIN,XMAX,YMIN,YMAX,ZMIN,ZMAX
Box-shaped volumes used to further restrict contact
EDCGEN,,Cont,Targ,,,,,,,,,,,,,BOXID1,BOXID2
Cont and Targ must be part IDs or part assemblies
EDDC - Delete, Deactivate, or Reactivate Contact
EDDC replaces old EDCDELE command
EDCLIST,NUM - Limit Contact Entity Listing
EDCGEN,TSES maps to *CONTACT_TIED_SHELL_EDGE_TO_SURFACE
EDBX,Option,BOXID where Option=Add/Delete/List
BOXIDs reduce the contact and target surfaces specified by the Part IDs or Part Assemblies to those nodes and segments contained within the box volume.
EDDC,Action,Option,Cont,Targ
Action = DELE, DACT, or RACT contact (EDDC very useful in restarts)
Option = Contact type (e.g., NTS, STS, etc.)
Cont = Component name or part number of slave surface
Targ = Component name or part number of master surface
EDDC,Action,ALL operates on the entire model
EDDC controls contact definitions to allow for multi-pass contact scenarios
NUM field added to EDCLIST command (default NUM = ALL)
Training Manual
15 Aug 2000
3.5-9

10. ANSYS/LS-DYNA Enhancements Restarts
EDSTART,RESTART Small restarts expanded
Most LS-DYNA options now supported for RESTART=2
New commands supporting small restarts
EDSP - Small penetration checking for contact entities
EDRC - Specifies rigid/deformable switch controls
EDRD - Switches parts from deformable to rigid & back
EDRI - Define inertia props. for new rigid body from EDRD
EDTERM - Specifies various termination criteria
EDDUMP - Specifies output frequency for D3DUMP file
EDDC and EDVEL commands previously discussed
Many other commands enhanced (EDWRITE, etc.)
MAJOR expansion of small restart capability at 5.7.
Various new commands allow model conditions to be changed prior to restarting the analyses. The ability to switch a part from deformable to rigid and back to deformable enables longer duration analyses to be performed. For example, an analysis of a vehicle that flips in the air (after an initial impact) before landing on the ground would take an excessive amount of CPU time to run if the parts remained deformable. By switching the parts to rigid while in the air, the CPU time can be greatly reduced. Proximity to the ground (i.e., a coordinate location), initiation of contact, etc. can be used to trigger termination of the run. A restart can then be performed in which the rigid body is converted back into a deformable body for the rest of the transient. The model size can also be reduced by deleting elements or unselecting parts.
Other commands that support the new small restarts include:
EDWRITE creates .R file when EDSTART,RESTART = 2
EDRST and EDHTIME - with new DT field = TIME / NSTEP
EDELE and PARTSEL allow changing the model
EDCURVE, EDDRELAX, EDCTS, EDDAMP, and EDOUT
Please refer to the ANSYS/LS-DYNA 5.7 User’s Guide for more details.
Training Manual
15 Aug 2000
3.5-10

11. ANSYS/LS-DYNA Enhancements Miscellaneous
EDREAD,NSTART,Label,NUM,STEP1,STEP2
Labels NODOUT and RBDOUT now supported
NUM = Node # (NODOUT) or Part # (RBDOUT)
STEP1,STEP2 - read data for specified load step range
EDREAD routine rewritten to parse ASCII strings into the appropriate fields (more robust at interpreting data)
Drop Test Module DTM converted to Tcl/Tk
UIDL character restrictions removed (no longer cryptic)
ANSYS/LS-DYNA User’s Guide is now on-line
Windows launcher for LS-DYNA executable (beta)
Submit edited .K input files from Start > Program Files …
Recurring problems in reading ASCII output files have been greatly reduced by switching over to a “string-friendly” algorithm (using C code instead of FORTRAN).
The DTM became a released product at ANSYS/LS-DYNA At 5.7, it has been converted to tickle (Tcl/Tk) and is now controlled by FLEXlm licensing. At 5.6.1, the licensing was on paper only (i.e., honor system).
The ANSYS/LS-DYNA User’s Guide is now on-line at 5.7 !!! This includes hypertext links to the other ANSYS documentation, like the Elements Reference, Commands Reference, etc. This is especially useful when checking out the TBDATA options for the TB command for the various material models. Navigation is fast and easy…
A launcher (BETA) was created for the PC (Windows operating system) to execute the LS-DYNA solver directly. This launcher determines the appropriate command line options for the LS-DYNA executable, based on user-supplied data, and submits the LS-DYNA job automatically. This eliminates the need to know the LS-DYNA command line format (e.g., ls950.exe i=file.k p=ANE3FLDS m=drelax …)
ANSYS/LS-DYNA should support LINUX on the PC platform.
Training Manual
15 Aug 2000
3.5-11

12. ANSYS/LS-DYNA Enhancements Workshop
20-30 minute exercise showing new features:
Mooney-Rivlin input
Initial velocity format
Part inertia definitions
Discrete material input
Issuing a small restart
Termination criteria
Switch from deformable to rigid and back again
See commented input file for more details …
This workshop demonstrates several new features in ANSYS/LS-DYNA An initial velocity (EDVEL) is applied to a rubber ball (TB,MOONEY) which impacts a rigid body plate - the inertia properties, of which, are user-defined (EDIPART). The ball bounces off of the plate, which pivots about its center of gravity (located above the meshed portion). The motion of the plate is restricted by springs and dampers (TB,DISCRETE), which cause the plate to swing back after the kinetic energy from the ball is converted into internal energy in the springs. The cube becomes a projectile on impact with the plate. The analysis is then stopped.
On restarting the analysis (EDSTART,2), the rubber ball is converted into a rigid body (EDRD,D2R) to reduce the CPU time. A termination criterion (EDTERM) is set to stop the analysis for the second time when the ball reaches a specified location.
In the next restart, the rigid ball is converted back into a deformable body (EDRD,R2D) so that stress data can be saved for the ball when it impacts the fixed wall.
Training Manual
15 Aug 2000
3.5-12