Editing Drawing Links

This task will show you how to edit the links which exist from a CATDrawing document to an existing CATPart document. Use the same methodology for links to a CATProduct, a sheet metal part or a V4/V5 .model document.

There are two possibilities:

Read also in this page the More About Links part.
 

Editing drawing links with the reference document loaded
Go to Tools > Options > General, click on the General tab, and make sure the Load referenced documents option is checked (this option is set by default). Then, click OK to validate.
When opening a drawing, if the referenced CATPart does not exist, a message will appear, mentioning that the links could not be found or contain wrong information. 

  1. Open the GenDrafting_part_links.CATDrawing document.

  2. Select Edit > Links.

    The Links dialog box appears with the existing links between the CATDrawing and  its related CATPart. In our example, this corresponds to links applied to the front, top and right views which are found and loaded (currently displayed in our session).

  3. Click OK to validate and exit the dialog box.
 

Editing drawing links with the reference document not loaded
Go to Tools > Options > General, click on the General tab, and uncheck the Load referenced documents option (this option is set by default). Then, click OK to validate.

  1. Open the GenDrafting_part.CATDrawing document.

  2. Select Edit > Links.

    The Links dialog box appears, showing the existing links between the CATDrawing and  its related CATPart. In this example, this corresponds to links applied to the front, rear, top, bottom, left, right and isometric views, which are found but not loaded (although currently displayed in our session).

    Note that when the reference document is not loaded, a number of commands can no longer be used, such as projection, dress-up  and dimension commands. You can still modify the graphic properties of the elements in the views.


     
    Note that the Synchronize, Activate/Deactivate and Isolate commands are unavailable when editing a .CATDrawing document's links.

  3. You can perform the following operations:

    • use the Load button to load parts (and parts only) that are not loaded. The status will change from "Document not loaded" to "OK".

    • use the Replace button to replace the selected link with another one. This button opens the Browse dialog box, which has two options File and Loaded Document. On clicking File, the File Selection dialog box opens to let you navigate to the desired file. Once the link has been replaced, the new element name is displayed along with its status in the Links dialog box.
      On clicking Loaded Document, the Session document dialog box is opened which shows the currently loaded CATPart.

      The views whose link has been replaced are considered as being not-up-to date in all cases, no matter what document you chose for replacement.

    • use the Refresh button to update the links related to the document without having to close then re-open the Links dialog box.

      This is especially useful when trying to re-access pointed documents that are not found (for instance, after a network disconnection): in that case, clicking the Refresh button avoids you to re-select Edit > Links to display an updated view of the links.

More About Drawing Links

  • From R17, links between a CATDrawing and its CATProduct are kept, even if the product is moved to another file. For example, if you move a CATPart into a CATProduct, to complete an assembly, the drawing of this pad will still be linked to the pad, which has become a subproduct of the assembly. 
  • For information on the other capabilities available with the Links dialog box (such as selecting a feature and opening or changing the corresponding source (CATPart)), refer to Editing Document Links in the Infrastructure User's Guide.
  • The Search Order capability allows you to solve links. For more details, see Infrastructure User's Guide.