Handling Parts in a Multi-Document Environment

In this task, you are going to copy a part body from one CATPart document to another, then edit the initial part body. This scenario shows you how the application harmonizes this type of ulterior modifications. Thanks to the underlying methodology, you can work in concurrent engineering.

Open the MultiDocument.CATPart document.
This scenario assumes there are two CATPart documents. Part3.CATPart is the target document, MultiDocument.CATPart contains the part body that will be copied, then edited in Part3.

The part body to be copied looks like this:

  1. Select Part Body.

  2. Select Edit > Copy to copy the part body.

  3. Open a new CATPart document 'Part3.CATPart' and position the cursor anywhere in the specification tree.

  4. Select Edit > Paste Special....
    The Paste Special dialog box appears. Three paste options are available:

    • As specified in Part document: the object is copied as well as its design specifications
    • As Result With Link: the object is copied without its design specifications and the link is maintained between the reference and the copy.
    • As Result: the object is copied without its design specifications and there is no link between the reference and the copy.
  5. For our scenario, select the As Result With Link option if not already selected, and click OK.
    Part Body is copied into the Part3.CATPart document. You will notice that the specification tree displays it under the name of Solid.1.
    A cube represents this solid. 

  6. Now, if you wish, you can fillet four edges. You can actually perform any modification you need.

  7. Return into the first document.

  8. Use Remove to remove material from the part body.

  9. In the Part3.CATPart document, the cube graphic symbol used for Solid.1 in the tree now contains a red point. This means that the initial Part Body underwent transformations.

    You can also notice that the update symbol is displayed next to Part3.
  10. What you need to do is synchronize the copied object with its reference. Just right-click Solid.1 in the specification tree and select Synchronize.
    The Synchronize command synchronizes copied geometry with its external references.

  11. Update the geometry.
    The solid now reflects the change: material is removed. The specification tree indicates that the part body has integrated the modifications made to the original part body.

Synchronize All

If your document contains several solids linked to external references to be synchronized, you just need to select the part and right-click Synchronize All.

The command also synchronizes knowledge parameters.

Opening Pointed Documents

The Open Pointed Document contextual command is available for external references. If you apply it onto Solid.1 for example, MultiDocument.CATPart opens (if closed of course) in your session.