Assembly constraints failing when using updated parts

[meche44]

In NX 9 I made a large assembly and unfortunately needed to change the drawing template for the parts. I proceeded to create new parts with the same file names as before but with the new templates. I then imported the old parts into the new part files. I then moved the assembly part over to the folder with these updated parts with the same names as before. When I open the assembly I have the replace option checked and everything comes in just fine except for the mates. The mates are greyed out initially and when I try to open them I get errors on all of them. Is there a way to make this work? Thanks.

 

[JohnRBaker]

That's because the Assembly Constraints are NOT linked to the part file name but rather the object ID's/user-defined names assigned to the edges and faces referenced by the constraints. And note that every part will have its own unique edge and face ID's irrespective of the file name. Unless you go back to the original part file(s) and assign user-defined names to the edges and faces used when creating the original constraints and then assigning those same exact user-defined names to the respective edges and faces on the new part file(s), there will be no way for the software to reattach the constraints automatically. If that's not possible or practical, then you'll need to reassign/reattach the constraints manually after you replace the Component(s).

John R. Baker, P.E.
EX-Product 'Evangelist'
Irvine, CA
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[meche44]

Thank you for that explanation. Is there a better way to go about changing the drawing template? I assume NX 9 still lacks the ability to just change the drawing template once something has been created.

 

[wacio]

Just use master model approach. If you had drawing in separate part file - you'd not have this problem.

NX8.5 + TC8.3