Improved Associativity Support on Multi-CAD Data

This section describes the concepts of improved associative support on Multi-CAD data in Batch mode, and discusses the conditions under which this associativity can be guaranteed.
Associativity applies to the document level, not to the geometry level. If you perform a Multi-CAD update, all applicative links will be broken.
 

How associative mode works
When launching the Conversion Batch on Multi-CAD data, Multi-CAD files are converted and stored but this information (source or origin of the part files) cannot be visible by the user and CGR files are not stored into Cache Memory. Only the 3D view can be seen by the user.

By doing a batch conversion over an Acis/DXF 3D/Inventor/VDA-FS part, this part is transferred into a V5 format file: a CATPart. During this transcription, all the part structure, geometrical information as well as original links are transferred.
After this conversion, the CATPart reproduces the 3D View of the original part and also stores a link onto the original file. The last information will enable the Multi-CAD Update Batch to check if V5 data are up-to-date compared with their original data.

The following schema draws a parallel between the CAD System and CATIA V5. Step 3 corresponds to the modification or review of Imported CAD Data in CATIA V5.

From the Import of CAD data to the Synchronization of V5 Session:

Launching the Update Batch means using the associative mode; the Batch operates on V5 data in order to update their structure or geometry according to the changes made by the Acis designer onto the original data.

Here is a schema showing the conversion and update processes of an assembly structure when importing CAD data into CATIA V5.

Multi-CAD Conversion and Update Processes:

The associative mode is the default mode. But if you do not launch the Batch, you will use what was called the non-associative mode in the previous V5 versions.

Associative mode is useful when a user wants to maintain synchronization with structure and/or geometry changes. But if you prefer to keep your assembly as it was at the moment of the conversion, you do not need to launch the Batch. Therefore, in this case, you will not do any synchronization between V5 data and original Acis data.

How to use the Update Batch for Multi-CAD Data

This task shows you how to convert Acis/DXF 3D/Inventor/VDA-FS parts into V5 CATParts and how to keep associativity between the modified CAD data and the converted part files, in V5.

  1. On Windows,  in a Command Prompt window, you can launch the conversion Batch by entering the following command:

    "C:\<install_dir>\intel_a\code\bin\CATDMUUtility.exe" -env CATIA.V5R10.B10 -direnv "C:\Winnt\Profiles\All Users\Application Data\Dassault Systemes\CATEnv" -f E:\tmp\acis_part.sat  -part  E:\tmp\Part1.CATPart
    Where
    -env ... is the default environment and
    -direnv ... is the directory path containing this environment.
    CATIA.V5R10.B10 is an example of environment name, it will vary with the level of CATIA installed.
Please note that this conversion will take into account the settings from the Tools -> Options -> General -> Compatibility -> External Formats.
 

  1. Insert the CATPart into a CATProduct interactively in CATIA V5 using Insert -> Existing Component.

  2. Save the CATProduct as E:\tmp\prod1.CATProduct

  3. Modify the Acis/DXF 3D/Inventor/VDA-FS data in the original CAD system.

  4. Launch the update Batch by entering the command:

    "C:\<install_dir>\intel_a\code\bin\CATMCIReplace.exe" -env CATIA.V5R10.B10 -direnv "C:\Winnt\Profiles\All Users\Application Data\Dassault Systemes\CATEnv" -i E:\tmp\prod1.CATProduct  -update

  5. If you open prod1.CATProduct interactively in CATIA V5, you will be able to see the geometry modification.
For more information about the CATDMUUtility launching, please refer to Running CATDMUUtility Batch Process, in DMU Navigator User Guide.