Appendix A - Input File Modifications
A new input file is created when you export a structural model from Advanced Material Exchange. The new input file contains the following modifications.
- User Material Definition
- Solution Controls
- State Variable Outputs
User Material Definition
User material definition for Ansys
MAT,ID
TB,STATE,ID,,20
TB,USER,ID,,0The MAT,ID command gives the ID of the material. This ID is automatically set to match the ID of the material stored in the .sif file. You should not modify the material ID.
The TB,STATE command identifies the number of solution dependent state variables to be tracked. All Advanced Material Exchange analyses with fiber filled materials use 20 state variables. Analyses with unfilled materials use 14 state variables. These state variables are described in Appendix B.
The TB,USER command denotes the use of a user material definition. The complete material definition is defined in the .sif file. This definition contains the adjustable plasticity and rupture coefficients. In older versions of Advanced Material Exchange, the coefficients could be adjusted in the input file. Now, the HIN file can be used to adjust the user material properties.
User material definition for Nastran
$------1-------2-------3-------4-------5-------6-------7-------8-------9-------0
MATXM* 10000 10000The MATXM entry defines the Advanced Material Exchange material and material ID. Additionally, the PSOLID entry is updated with the new Advanced Material Exchange material ID.
$------1-------2-------3-------4-------5-------6-------7-------8-------9-------0
PSOLID* 1 10000 0Solution Controls
Solution controls for Ansys
NROPT, FULL, , OFF
PRED, OFF, , OFF
NEQIT, 1000
CNVTOL, F, , , 0The NROPT, FULL, , OFF command instructs Ansys to use the 'Full' Newton Raphson algorithm and prevents ANSYS from using the Adaptive Descent algorithm.
The PRED, OFF, , OFF command turns off the substep and load step predictors for nonlinear analyses. When turned ON, the PRED command interfere's with the Helius PFA solver's ability to manage material nonlinearity.
The NEQIT, 1000 command instructs Ansys to use up to 1000 equilibrium iterations before evaluating the need to cut-back the time increment size.
The CNVTOL, F, , , 0 command instructs Ansys to use force convergence with infinite norm which allows the Helius PFA solver to better handle the nonlinear solution process.
When used in conjunction with the Helius PFA solver, these commands collectively improve Ansys' ability to obtain a converged solution at every time increment. Refer to the Ansys help for more information about these commands.
Solution controls for Nastran
NLPARM 1 100 ITER 1 1000 P ALL+
+ 1000 +
+ +
+ The NLPARM entry controls the time incrementation, stiffness, and convergence settings.
The ITER field allows the solver to iteratively update the stiffness matrix of the material.
The subsequent 1 in field 6 instructs the solver to update the stiffness after every iteration.
The first instance of 1000 in field 7 instructs the solver to use a maximum of 1000 iterations in each load increment. A large value like 1000 allows the solver to take full advantage of the improved convergence characteristics provided by Helius PFA.
The P in field 8 instructs the solver to use the load convergence criteria and error tolerances.
The final 1000 in line 2 instructs the solver to use up to 1000 divergence conditions per iteration.
When used in conjunction with the Helius PFA solver, these commands collectively improve Nastran's ability to obtain a converged solution at every time increment. Refer to the Nastran Reference Manual for more information about these commands.
State Variable Outputs
State variable outputs for Ansys
OUTRES,SVAR,ALLThe OUTRES,SVAR,ALL command instructs Ansys to include all state variables in the results .rst file.