Creating a Design Table from the Current Parameters Values    

A design table is a feature that you create from your document parameters or from external data. No matter the existence of external data, you must create the design table in CATIA.  There are two ways to create a design table:
  • From the current parameter values 
  • From a pre-existing file. 

The scenario described below explains how to proceed in the first case. The design table creation process includes the following steps:

  1. Create a table from the document parameters.

  2. Select the parameters to add to the design table.

  3. Specify a file to contain the generated design table.

  4. Edit the generated CATIA design table.

  5. Apply the design table to your document.

For information on how to use the different dialog boxes related to the design table, see The Design Table Dialog.

  1. Open the KwrStartDocument.CATPart document.

  2. Click the Design Table icon  in the standard toolbar. The Creation of a Design Table dialog box is displayed. See The Design Table Dialog  for further information.

  3. If need be replace the default name and comment for the design table.

  4. Check the  Create a design table with current parameter values option. 

  5. Click OK. The Select parameters to insert dialog box is displayed.

  6. From the Parameters to insert  list,  select the PartBody\Pad.1\FirstLimit\Length and the PartBody\Pad.1\SecondLimit\Length items. Then click the right arrow to add both items to the Inserted parameters list.

  7. Click OK. A file selection box is displayed.

  8. Specify the pathname of the design table to be created. Click OK in the file selection dialog box.
    The design table feature is added to the specification tree and a dialog box displays the newly created design table. This design table contains only one configuration. By default it is active.

    If the file specified already exists, the Creation of a Design Table dialog box is re-displayed as well as a message box asking you whether you want to overwrite the existing file.

  9. Click Edit table... to start an Excel application (under Windows) or open the text editor under Unix.
    Replace the PartBody\Pad.1\FirstLimit\Length parameter value with 80mm.

  10. Save your Excel or .txt file and close your application. Some information messages are displayed in a dialog box warning you about events related to the design table. Click Close.

  11. Click Apply into the CATIA design table dialog,  the document is updated as well as the CATIA design table. Click OK to exit the dialog and add the design table to the document.