Method to Remove a Relational Reference From a Part to an Assembly

Description

A Relational Reference from a part to an assembly is usually created when the part or part feature is created in assembly mode. The reference is not required in order to regenerate the part in Pro/ENGINEER. This type of relationship often needlessly binds a part to an assembly in Pro/INTRALINK, affecting Check Out/Check In performance, Copy options, and Purge/Delete performance. Users should avoid creating these references whenever possible in order to keep parts independent of assemblies.

Unfortunately, after the reference is created, it will be preserved each time the part is saved to a Pro/INTRALINK Workspace. Even if the assembly is not present, a virtual or "ghost" version of the assembly (shown in parentheses in the Workspace browser) is created during the save from Pro/ENGINEER. This ghost assembly may be deleted before the part is Checked In, but it will be recreated again the next time the part is used in Pro/ENGINEER.

There is a method to remove the Relational Reference using Pro/ENGINEER 2000i and later.

Resolution

1. Retrieve the part into Pro/ENGINEER without the assembly.

2. Select #Info/#Model Info and find the feature(s) which list(s) the assembly as a reference.

3. Select #Feature/#Redefine, and select the feature with the reference.

4. (This step may vary depending on the reference. Most references are contained within the Section, but some may be in other feature elements.) Select the element "Section", and #Define.

5. Select #Sketch. Pro/ENGINEER will ask "Assembly is not present; unalign all external references?". Select Yes. The enhanced Sketcher in Pro/ENGINEER 2000i and later will automatically recreate the dimensioning needed to define the section without requiring a new sketch.

6. At this point some additional questions regarding alignment may need to be resolved.

7. Select #Done to finish redefining the sketch, and #Ok to complete the feature redefine.

   Repeat steps 3 through 7 for each feature which references the assembly.

After redefining the features, when the part is saved to Pro/INTRALINK, it will not reference the assembly.