1. Solution and Simulation Controls
Chapter 7
Solution and Simulation Controls

2. Chapter Objectives
Upon completion of this chapter, students will be able to specify solution and simulation controls in the ANSYS/LS-DYNA program.
1. Describe the basic solution control options in ANSYS/LS-DYNA
2. Describe how to control the writing of LS-DYNA binary and ASCII output files
3. Define and describe how to use mass scaling
4. Describe how simulation control is used
5. Describe how a user can edit the LS-DYNA input stream
6. Given step-by-step guidance, simulation controls will be demonstrated in a beam buckling example.
March 15, 2001
Inventory #001458
7-2

3. Basic Solution Controls
In many aspects, the solution control parameters specified in an explicit analysis are very similar to those encountered during an implicit run.
The basic parameters to be specified in an explicit solution are:
1. Time: the actual time for which the physical process is being simulated [TIME]
Solution: Time Controls -> Solution Time…
The actual solution time should be of very short duration, often in milliseconds.
March 15, 2001
Inventory #001458
7-3

4. Basic Solution Controls
The basic parameters to be specified in an explicit solution (continued)
2. Number integration points for shell and beam elements [EDINT]
Solution: Output Controls -> Integ Pt Storage…
3. Number of time steps results will be written to the .rst and .his files [EDRST, EDHTIME] . Output frequency times also available.
Solution: Output Controls -> File Output Freq ->Number of Steps...
3-5 integration points are required for shell elements to adequately capture plastic effects
The .rst file records results for the entire model for general postprocessing. It should typically have output steps to reduce disk space (100 default).
The .his file records results for a subset of the model for time history postprocessing. It generally has ,000 output steps (1000 default).
The output frequency for restarts can also be input.
March 15, 2001
Inventory #001458
7-4

5. Controlling Binary Output Files
Since LS-TAURUS, the LS-DYNA postprocessor, is provided with ANSYS/LS-DYNA, the user has the ability to create the LS-DYNA results files d3plot and d3thdt in addition to the ANSYS .his and .rst binary files.
Determining which binary results files are output by the program is controlled by the EDOPT command:
Solution: Output Controls -> Output File Type…
File Options include ADD, DELETE, and LIST a file
Output can be produced for ANSYS only (.rst and .his) LS-TAURUS and LS-POST only (d3thdt, d3plot) or both.
March 15, 2001
Inventory #001458
7-5

6. Controlling ASCII Output Files
In addition to LS-TAURUS binary files, the user can also output a series of ASCII output files that contain specialized information about an analysis.
The following is a list and description of the files available:
GLSTAT Global model data (global statistics)
BNDOUT Boundary condition forces and energy
RWFORC Rigid wall forces
DEFORC Discrete element forces
MATSUM Material energies data (on a part basis)
NCFORC Nodal interface forces
RCFORC Resultant interface forces
DEFGEO Deformed geometry data
SPCFORC Single point constraint forces
SWFORC Nodal constraint reaction forces (spotwelds)
RBDOUT Rigid body data
GCEOUT Geometry contact entities
SLEOUT Sliding interface energies data
JNTFORC Joint force data
NODOUT Node data
ELOUT Element data
March 15, 2001
Inventory #001458
7-6

7. (continued) Controlling ASCII Output Files
The EDOUT command controls which ASCII files are written:
Solution: Output Controls -> ASCII Output...
Simply select which individual ASCII file that output data should be generated for (e.g., MATSUM)
The following OPTIONS can also be selected:
ALL - write all ASCII output files
LIST - list all time history output specifications
DELE - Delete all ASCII output specifications
It is important to note that the information contained in some of the ASCII files is for a small subset of the model. The EDHIST command controls the nodes or elements for which the ASCII files will be written:
Solution: Output Controls -> Select Component…
The information contained in the ASCII output files will be for the nodal or element component specified
The time interval for output of the ASCII files is controlled by the EDHTIME command.
Multiple specifications are permitted on different components
March 15, 2001
Inventory #001458
7-7

8. Advanced Solution Controls
In ANSYS/LS-DYNA, there are three advanced solution controls that are commonly used:
1. CPU Control: Specifies CPU limit for an ANSYS/LS-DYNA analysis.
2. Mass Scaling: Adjusts element mass to increase the time step size.
3. Sub-cycling: Tunes model to decrease CPU time (not recommended).
CPU Control
The overall CPU time limit is specified using the EDCPU command:
Solution: Analysis Options->CPU Limit…
Specify the CPU time limit (in seconds) to terminate an analysis. A value of 0 (default) will set no time limit.
March 15, 2001
Inventory #001458
7-8

9. Mass Scaling
Mass scaling is used to adjust elements to a specified time step by adjusting the density of each element.
As previously discussed, the time step depends on EX, NUXY and DENS, as well as the element size.
With mass scaling, it is possible to adjust the density of any element to a specified time step depending on the size of the element.
Mass scaling is specified with the EDCTS command:
Solution: Time Controls->Time Step Ctrls...
Specify the minimum time step size to be used and the scale factor to be applied.
March 15, 2001
Inventory #001458
7-9

10. (continued) Mass Scaling
There are two mass scaling alternatives:
Have the same time step size for all elements by adjusting the density. This is only useful when inertial effects are insignificant.
EDCTS, DTMS
where DTMS is the POSITIVE value of the necessary time step size (multiplied with 1.111)
Mass scaling applies only to elements with Dt < Dt specified
where DTMS is the NEGATIVE value of the necessary time step size (multiplied with 1.111)
March 15, 2001
Inventory #001458
7-10

11. (continued) Mass Scaling
Mass scaling for minimum time step size:
element l1 l2 l3
Adjust the density to a user defined time step size:
March 15, 2001
Inventory #001458
7-11

12. Mass Scaling - Example An example for the use of mass scaling (EDCTS)
Car crash model
140 parts
42981 nodes
1580 bricks
60 beams
35170 shells
Termination time 150 ms
100 smallest element time-steps (see LS-DYNA output file d3hsp):
element time-step
shell E-06
shell E-06
shell E-06
shell E-06
shell E-06
shell E-06
...
shell E-06
shell E-06
shell E-06
shell E-06
shell E-06
March 15, 2001
Inventory #001458
7-12

13. (continued) Mass Scaling - Example
Without mass scaling:
Initial time step size depends on the smallest element
Dt = E-07 sec
With mass scaling:
Time step wanted is 6.534E-07 sec. Give the negative value of 111% of the time step to the EDCTS command:
EDCTS, -7.26E-07
Main Menu > Preprocessor > Output Ctrls > Mass scaling > ...
Initial time step size
Dt = 6.534E-07 sec
CPU time is reduced to 68%
Error in mass:
Physical mass 1.26 metric tons
Added mass metric tons (27 grams)
Error in mass 0.002%
The coordinates of the mass center have changed, too.
March 15, 2001
Inventory #001458
7-13

14. Simulation Control
Sense Switch Controls allow the user to interrupt the solution process and to check for the actual state.
Do the following to use sense switch controls:
Type CTRL-C into the output window of ANSYS on Unix platforms or the separate LS-DYNA output window on NT platforms. It interrupts the explicit solver and waits for an input in the output window of ANSYS.
Type sw1 to terminate. A restart file will be written.
Type sw2 into the output window to receive a global statistic of the actual state. LS-DYNA continues.
Type sw3 into the output window to receive a restart file for the actual time. LS-DYNA continues.
Type sw4 to write a results data set. LS-DYNA continues.
March 15, 2001
Inventory #001458
7-14

15. Solution Control
The LS-DYNA solver writes all important messages (errors, warnings, failed elements, contact problems) to the ANSYS output window (separate window on NT) and to the file d3hsp.
The first estimation of CPU time is usually too high. Use CTRL-C to interrupt the solver and type sw2 for the actual values of the global statistics.
March 15, 2001
Inventory #001458
7-15

16. Visualization of Time Step Size
The LS-DYNA solver automatically calculates the minimum time step size of each element based on the length and density.
The actual time step size used by LS-DYNA is the smallest of these values.
The EDTP command can be used to visualize the elements with the smallest time steps before the LS-DYNA solver is invoked.
This information allows the user to evaluate a mesh and take appropriate action (ie. Remeshing or using mass scaling)
EDTP, OPTION, VALUE1, VALUE where:
OPTION = 1, 2, or 3 as described below:
1 = element plot of VALUE1 smallest element time steps
2 = #1 above + element listing of these time step values
3 = #2 above + VALUE2 translucency of remaining elements
VALUE1 = plot/list limit for “smallest” designation (red elements decide size)
VALUE2 = translucency ( 0 = no translucency, 1 = max., 0.9 = default level)
March 15, 2001
Inventory #001458
7-16

17. Visualization of Small Elements
EDTP maps element time step sizes before SOLVE
The smallest elements in the model will control the CPU time
Smallest time step elements plotted in red (intermediate time yellow)
Translucency option and time step size listing options available
Meshing/mass scaling decisions based on estimated time step sizes.
Solution: Time Controls>Time Step Predic….
March 15, 2001
Inventory #001458
7-17

18. Adaptive Meshing
Automatic regeneration of SHELL163 mesh can be performed during solution to maintain a uniform bound on the distortion error in the analysis
Adaptive meshing is specified on a part basis (EDADAPT command)
The EDCADAPT command controls how often, on what basis, to what extent, and when adaptive meshing occurs
Each adapted mesh has separate POST1 (Jobname.rs01, Jobname.rs02, …) and POST26 (Jobname.hi01, Jobname.hi02, …) results file
Adaptive meshing is particularly useful in stamping and sheet metal forming problems where there is substantial plastic deformation
EDADAPT, PART, Key ! Set Key=On to activate for part PART
EDCADAPT, FREQ, TOL, OPT, MAXLVL, BTIME, DTIME
FREQ = time interval (real time) between adaptive mesh refinements
TOL = adaptive angle (deg) based on OPT=1 (original) or 2 (incremental) mesh
MAXLVL = maximum number of mesh refinement levels
BTIME/DTIME = birth/death times when adaptive meshing is active in model
March 15, 2001
Inventory #001458
7-18

19. Adaptive Meshing
By the automatic sub-division of highly distorted shell elements, ANSYS/LS-DYNA ensures that more accurate results are obtained.
Adaptive meshing is performed in two steps.
1. Select a Part for which adaptive meshing is to be turned on.
Solution: Analysis Options> Adaptive Meshing> Apply to Part
March 15, 2001
Inventory #001458
7-19

20. Adaptive Meshing 2. Specify the appropriate adaptive meshing controls
Solution: Analysis Options> Adaptive Meshing> Global Settings
March 15, 2001
Inventory #001458
7-20

21. Adaptive Meshing
Once adaptive meshing is specified for a given part, the LS-DYNA solver on the EDCADAPT command.
Animations across different results files are not possible directly, but a macro can be written with FILE and /SEG commands to animate.
Refined
Mesh
March 15, 2001
Inventory #001458
7-21

22. Editing the LS-DYNA Input File
Most general LS-DYNA capabilities are supported by the ANSYS/LS-DYNA program and are easily accessed in the GUI.
There are several additional features of LS-DYNA, however, that cannot be directly accessed through the ANSYS GUI. Some examples include:
Material models: Fabric, soil, geological cap
Elements: Air bags, seat belts, explosives
Constraints: Rigid body local coordinate systems
Although these unsupported capabilities cannot be directly accessed, a user familiar with LS-DYNA input can still use any feature indirectly by editing the LS-DYNA keyword input file.
However, post-processing in ANSYS may not be possible, depending on the changes. LS-TAURUS or LS-POST can always be used to validate the analysis.
Editing the LS-DYNA input file is accomplished using a five step procedure.
March 15, 2001
Inventory #001458
7-22

23. (continued) Editing the LS-DYNA Input File
STEP 1: Issue the EDWRITE command
After all of the general modeling has been completed in ANSYS/LS-DYNA, the EDWRITE command should be issued instead of the SOLVE command.
Solution: Write Jobname.k…
The EDWRITE command writes the Jobname.k without starting the ANSYS/LS-DYNA solution process.
Issuing the EDWRITE command also creates the headers to the .rst and .his files.
EDWRITE is an action command and will immediately write the LS- DYNA input file specified.
March 15, 2001
Inventory #001458
7-23

24. (continued) Editing the LS-DYNA Input File
STEP 2: Exit the ANSYS/LS-DYNA Program
Utility Menu: File->Exit
STEP 3: Edit the input file Jobname.k
Using a standard vi or text editor, add the additional features to the Jobname.k using the required LS-DYNA keyword format.
March 15, 2001
Inventory #001458
7-24

25. (continued) Editing the LS-DYNA Input File
STEP 4: Execute the LS-DYNA Solver
In the directory where the Jobname.rst and Jobname.his reside, directly execute the LS-DYNA script (which, in turn, executes the solver).
The solution produced by LS-DYNA will automatically be appended to the ANSYS results files.
The typical command for executing the LS-DYNA script is:
/ansys57/bin/lsdyna57 i=Jobname.k p= ANSYS product variable (see install. guide)
Additionally, m=drelax is needed for an implicit-to-explicit solution.
Also, MEMORY=# (in words) is used for large jobs (see EDSTART).
Further, R=D3dumpnn for small restarts
STEP 5: Re-enter the ANSYS/LS-DYNA Program
Re-enter the ANSYS/LS-DYNA program after the LS-DYNA solution is done.
The results can be viewed in both the general (Jobname.rst) and time history (Jobname.his) postprocessors.
NOTE: The nodes and elements cannot be modified when using this procedure. Further, editing the Jobname.k file is unsupported.
March 15, 2001
Inventory #001458
7-25

26. Beam Buckling Exercise
The exercise for this chapter begins on page E7-1 of Volume II.
Solution and simulation controls are demonstrated in an example of a beam buckling under axial load.
March 15, 2001
Inventory #001458
7-26