Updating Geometry Parameters in an Imported Model

You can modify the dimensions of certain geometric features in an imported model in Abaqus/CAE, then propagate the modifications to the original CATIA model.

  1. Load the part or assembly to be exported in the Assembly Design app or the Part Design app.
  2. To create a parameter that can be exported to Abaqus/CAE and to associate the new parameter with an existing CATIA parameter, do the following:
    1. From the Tools section of the action bar, click f(x) Formula.
    1. From the Formulas dialog box that appears, select the CATIA parameter to export.
    2. Enter the name of the new parameter. The parameter name must begin with ABQ_ if you want it to be exported to Abaqus/CAE.

      The parameter name may not contain a period (.).

    3. If desired, modify the value of the new parameter.
    4. Click OK to create the new parameter and to close the Formulas dialog box.
  3. To create a parameter that can be exported to Abaqus/CAE and to create a relationship between the new parameter and an existing CATIA parameter, do the following:
    1. From the Tools section of the action bar, click f(x) Formula.
    1. From the Formulas dialog box that appears, select the type of the new parameter (Real, Integer, Length, or Angle).
    2. Select with Single Value to indicate how the parameter will be defined.
    3. Enter the name of the new parameter. The parameter name must begin with ABQ_ if you want it to be available to Abaqus/CAE.
    4. Enter the value of the new parameter.
    5. From the list of existing CATIA parameters, select the parameter that will be related to your new parameter.
    6. Click Add Formula.
    7. From the Formula Editor dialog box that appears, enter the formula that relates the CATIA parameter to your new parameter.
    8. Click OK to close the Formula Editor dialog box.
    9. Create additional parameters, as desired.
    10. Click OK to create the relationships between the CATIA parameters and your new parameters and to close the Formulas dialog box.
      The parameters and the relationships appear in the specification tree.

    Refer to the Assembly Design or Part Design app documentation for more information about defining parameters and formulae.

    Only those parameters whose names start with the string ABQ_ are passed to Abaqus/CAE and can subsequently be modified using bidirectional update. Each parameter should be referenced only once within a feature definition.

  4. Import the model to Abaqus/CAE using one of the associative import methods described in Using Automatic Associative Export and Import.

    When the SIMULIA Associative Interface for Abaqus/CAE plug-in creates the assembly (.eaf) file, it also creates an XML-format parameters (.par_abq) file. If you are copying files from one computer or directory to another as part of a manual associative import, you must perform the following additional steps:

    1. Copy the parameters file and the original CATIA part (.CATPart) files along with the assembly file.
    2. Edit the parameters file to update the File attribute for each Part element; for example:

      <Part Name="part name" File="new path to .CATPart file">

    When performing a parameter update, Abaqus/CAE identifies the CATIA .CATPart files that must be updated by first looking in the current working directory and then looking in the path specified in the parameters file.
  5. After the model has been imported, display the list of modifiable parameters in Abaqus/CAE:
    • In the Part module, select Tools > CAD Parameters from the main menu.
    • In the Assembly module, select Tools > CAD Interfaces > CAD Parameters from the main menu.
    The CAD Parameters dialog box appears. Clicking on a parameter name highlights the portions of the model affected by that parameter in the viewport.
  6. To modify a parameter value, click the appropriate cell in the Value column and enter a new value.
  7. When you have changed all of the necessary parameter values, you can update the model geometries, generate a new parameters file, or reset the parameters to their initial value:
    • To update the geometries, click Update. The model features are regenerated based on the new parameter values, and the geometry of the model is updated in CATIA and Abaqus/CAE. The original parameters (.par_abq) file is also updated.
    • To generate an updated parameters file, click mouse button 3 on the CAD Parameters table, and select Write to File from the menu that appears. If you are currently in the Part module, only the parameters associated with the current part are included in the file; if you are currently in the Assembly module, all parameters associated with the model are included in the file.

      The model geometries are not updated when you write a new parameters file. You can use the new parameters file to verify the parameters that are being passed to CATIA, or you can use it to manually perform subsequent parameter updates using the Abaqus Scripting Interface.

    • To reset all parameters to their initial values, click Defaults. The default values reflect the values in the current Abaqus/CAE model geometry.