About Preprocessing with ANSYS®/Prep7

The analysis model for the optimization with SIMULIA Tosca Structure and ANSYS® can be generated in /PREP7 in the standard way.

This page discusses:

For the batch processing of ANSYS®, the ANSYS® CDB, inp, and dat format can be used. An ANSYS® CDB file contains the complete finite element information without the solution strategy (/SOLU). You must add the solution strategy manually.

Generation of the Finite Element Input File

The CDB File is generated in ANSYS®/PREP/ with the following command:


CDWRITE, Option, Fname, Ext, Dir, Fnamei, Exti, Fmat

Use the option DB to ensure that the complete finite element information is written to the file. The file name (Fname) and the extension (Ext) must also be specified. In the examples of the SIMULIA Tosca Structure installation, the extension cdb is used.

A complete command for the generation of a CDB file looks as follows:


CDWRITE, DB, holeplate, ans

This file does not contain the solution strategy.

Load Cases

If only one load case should be calculated, the load case information is already included in the CDB file. In this case, only the solution strategy must be added:


/SOLU
SOLVE
FINISH

If multiple load cases are used, the load cases can be stored in load case files (file.s01, file.s02, ...). These files are generated using the following command:


lswrite, lsnum

The solution strategy for multiple load cases must be added to the CDB file:


/SOLU
LSREAD, 1
SOLVE
LSREAD, 2
SOLVE
...
FINISH

Check of the Batch Input File

To check if the CDB file is running correctly in batch mode, an analysis should be started on the command line before starting the optimization with SIMULIA Tosca Structure. Using the ANSYS® 14.5 solver, the command line looks as follows:

  • Windows 
    ansys145 -b -i [input file] -o [output file] -p[productvar]
  • Linux 
    ansys145 -p -p[productvar] < [input file] > [output
file]

Errors are reported to the *.err file. In case of errors, the input file must be modified.

Generation of Groups

The node and element groups (assemblies and components) are generated using the "component manager" or with the following commands:


CM, Cname, Entity
CMGRP, Aname, Cnam1, Cnam2, Cnam3, Cnam4, Cnam5, Cnam6,
Cnam7, Cnam8

These components or assemblies are treated as node and element groups in SIMULIA Tosca Structure. These groups are extracted from the cdb file and are accessible with the group name in the optimization preprocessor. If node and element groups are generated with the same name, the groups get the suffix "_NODE" and "_ELEM" during the import to keep the group names unique.