Files and Formats

The SIMULIA Tosca Structure preprocessor can read ANSYS® input files of arbitrary format, however, the ANSYS® input files must be able to be processed in batch mode.

The ANSYS® input file can be created by an arbitrary FE-Preprocessor. In ANSYS®, the CDB file is created with the following command:

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

At least one Solve-Command has always to be specified: solve or lssolve.

To check, if the input file is executable in batch mode, one analysis should be performed in batch mode from the command line before starting the complete optimization. The corresponding batch call of ANSYS® version 14.0 on Windows is as following:

Ansys140 -b -i<input file> -o<output file> -p<product­var>

Error messages and warnings can be found in the *.err file. The input file must be corrected if an error occurs.

As input file for the optimization loop TOSCA_PREP generates an ANSYS® CDB file from the ANSYS® input file. Compared to a complete ANSYS® input file this file contains no solution strategy (/SOLU).

During the optimization procedure the analysis results are read from the *.rst file.

Important:

  • The ANSYS® interface will stop reading element and node definitions when the first /SOLU definition in the input file occurs. Elements that are defined after the first /SOLU (usually elements and nodes generated by macros) are not known in SIMULIA Tosca Structure. In return this allows for more possibilities of using macros and /PREP7 sections after a /SOLU definition. Most definitions after /SOLU are not modified by the interface.
  • For a topology optimization with the controller algorithm using static finite element analysis, which contains only solid elements, the iterative PCG Solver of ANSYS® should be used due to performance reasons. The solver may be activated by adding the following command in the solution block of the corresponding CDB file: 
                eqsl, pcg, 1.e-5
  • The iterative solver is not recommended for sensitivity-based optimizations.
  • It is not allowed to define new nodes or elements after the first /SOLU statement. (The solution part is cut off the .cdb file before the ANSYS® Preprocessing-run.)
  • In SIMULIA Tosca Structure configuration file tosca_ctrl.cfg (see also CONFIG) the environment variable ANSWAIT=1 will be set, to let ANSYS® wait for a free license.
  • In earlier versions of the ANSYS® interface, for shape and bead optimization the positions of nodes used to be modified using the special command NMODIF, which is unsupported by Tosca ANSA® environment. This prevented the user from visually inspecting the modified state of the model. The interface now modifies directly the coordinates of the nodes, thus all intermediate steps of the shape or bead optimization can be visualized with Tosca ANSA® environment.

ANSYS® Files Generated During a SIMULIA Tosca Structure Optimization

During the optimization preprocessing the ANSYS® model will be imported to ANSYS® and exported again to generate a standard blocked CDB file. During this import/export step all macros in the ANSYS® input file will be executed in ANSYS® and can no longer be found as macros in the input files used during the SIMULIA Tosca Structure optimization.

  • The input file (model.cdb) is split into multiple files during the optimization preprocessing (TOSCA_PREP):
    • model_ans.cdb Input file without solution /SOLU
    • model_ans.head File containing the ANSYS® Header
    • model_ans.solu File containing the ANSYS® Solution /SOLU. Eventually, existing load case files *.s0X are copied into the optimization working directory. These remain unchanged during the optimization process.
    • model_ans.tosca temporary file which is used for the generation of the model_ans.cdb file
  • Two files are generated during the fem_modif call:
    • model_<iter>.ans
    • model_<iter>.cdb The CDB file is included in the ans file using a CDREAD The model<iter>.ans file is renamed into model.ans before the finite element analysis is executed. The CDB file is not renamed - it is referenced with the iteration extension in the ans file.
  • Two files are moved in the corresponding SAVE directory:
    • model.ans: is copied (copy_solver_info_list) into the corresponding SAVE directory and gets an iteration counter number before the finite element analysis is executed.
    • model_<iter>.cdb: is moved (move_per_iter_xxx_list) into the corresponding SAVE directory at the end of the design cycle.
  • The newly created CDB file in blocked format is detected and analyzed automatically by the optimization preprocessor. Thus, the FE model is imported into SIMULIA Tosca Structure. The data of the ANSYS® model (coordinates of nodes, materials, properties and assignment of elements) in the CDB file can be modified during the optimization. The load files contain the boundary restrictions which provide information about boundary movements for shape optimization.
  • The solve section contains the solution strategy of the original input file, checks and the definition of which kind of results must be written to the *.rst files for shape and topology optimization, respectively. Thus, during the ANSYS® analysis only the results necessary for the optimization are written to the result file.
  • During the optimization the data in the CDB file is modified. Afterwards the three parts are merged and a new ANSYS® analysis is performed. The load files are not changed during the optimization.