Managing CATDrawing Documents in ENOVIA VPM

This task shows you how to manage the integration between CATIA V5 Drafting and ENOVIA VPM. You will learn how to:
   
For more information about interoperability between CATIA and ENOVIA VPM, refer to the ENOVIA-CATIA Interoperability User's Guide. For more information on using ENOVIA VPM, refer to ENOVIA VPM documentation.
   

Have a CATIA V5 and an ENOVIA 3d com Navigator sessions running.

Creating a CATDrawing document and saving it in ENOVIA VPM

  1. From the ENOVIA 3d com Navigator, right-click a CATPart or a CATProduct document and select CATIA_V5 > Load to load this document into CATIA V5.
    For more information, refer to the CATIA V5 / ENOVIA VPM Interoperability via ENOVIA 3d com on Windows chapter in the ENOVIA-CATIA Interoperability User's Guide.
Note that to create a subassembly drawing, the ENOVIA VPM subassembly has to be loaded into CATIA V5 from its own bookmark in the ENOVIA 3d com Navigator web tree.
 

  1. In CATIA V5, select Start > Mechanical Design > Drafting. The New Drawing Creation dialog box is displayed.

  2. Select the views to be automatically created on your drawing, for example the Front, Top and Left icon.

 

 

  1. Click OK. A progress bar appears while the views are being generated from the opened CATPart or CATProduct document.

The views are then displayed in the CATDrawing document.
 

   
 

  1. Create an ENOVIA VPM document with the CATDrawing document, as explained in Creating an ENOVIA VPM Document in CATIA V5 in the ENOVIA-CATIA Interoperability User's Guide.
 

 

Viewing the documents which impact the CATDrawing in ENOVIA VPM

  1. From the ENOVIA 3d com Navigator, right-click the CATDrawing document  (it can be either a part drawing or an assembly drawing) and select Impact As Reference. An impact graph for the drawing is launched in the ENOVIA 3d com Navigator webspace.

  2. Double-click the drawing box to visualize reference-to-reference links for the CATDrawing document.

The drawing dependencies are displayed, letting you view the links between the CATDrawing document and the CATPart and/or CATProduct documents it references.

The impact graph also lets you know whether the drawing is up-to-date or not:

  • a green thumb up means that the drawing is synchronized with the documents it references, and therefore up-to-date.

    For example, in the case of an up-to-date part drawing, you may get something like the following impact graph:
 

 

  • a red thumb down means that the drawing is not synchronized with the documents it references, and therefore not up-to-date.

    For example, in the case of a not-up-to-date part drawing, you may get something like the following impact graph:
 

  1. If the drawing is not up-to-date, you can update it using the following method:

    1. Open the CATDrawing document in CATIA V5 (as described in Opening the CATDrawing document in CATIA V5 below).

    2. Refresh it using the update icon.

    3. Save it in ENOVIA VPM using File > Save.

    If you now go back to the Impacted By Tree View in ENOVIA LCA, the drawing is indicated as being up-to-date.
For more information, refer to Using CATIA V5 Multimodel Link Dependencies in the ENOVIA-CATIA Interoperability User's Guide.
 

Opening the CATDrawing document in CATIA V5
To illustrate this task, you should use an assembly drawing (rather than a part drawing).

  1. From the ENOVIA 3d com Navigator, right-click the CATDrawing document and select CATIA_V5 > Load to load this document into CATIA V5. The drawing is displayed in CATIA V5. In the case of an assembly drawing, the drawing links are broken.

  2. To solve the links, perform as follows, depending on the save mode you chose when saving the assembly in ENOVIA VPM:

  • For an exploded assembly: right-click the drawing in the specification tree and select Load PDM Context (you can also go back to ENOVIA 3d com Navigator, right-click the associated CATProduct and CATPart documents in Content Management, and select CATIA_V5 > Load). This loads the assembly drawing context (i.e. the CATProduct and CATPart documents used for the assembly drawing creation or for the last assembly drawing update) in the Product Structure editor in CATIA V5. Note that the drawing has to be placed in the assembly and that the part instances which were not referenced by the drawing when you last saved it are not loaded.

  • For a "black box" or "work package" assembly: select Edit > Links... and choose the Pointed documents tab to visualize the links between the CATProduct and CATDrawing documents. From the list of pointed documents, select the CATProduct and/or CATPart documents you want to open, and click the Open button. This loads the selected documents in the Product Structure editor in CATIA V5.

Note that you need to load all the parts which make up a given product if you want them to be included in the drawing views at the next update.
 

The drawing links are now solved. The Drafting specification tree indicates whether the drawing is up-to-date or not, whether the drawing is a part drawing or an assembly drawing.

 

If a 3D element (product or part) has been modified before launching the drawing, the update mask appears in front of the drawing elements which need an update (all, in our example):
   
 

If no modification has been performed in 3D before launching the drawing, the various drawing elements in the specification tree are shown as being up-to-date:
If you perform a cut and paste on the assembly in the Enovia 3d com Navigator for which a CATDrawing already exists, you cannot load the document again selecting Load PDM Context.