Undeform an assembly component in the assembly drawing

[BOPdesigner]

In NX 7.5, I have an assembly which has a deformable part in a deformed state in it. Now for the assembly drawing file (using master model concept), I have created an exploded view and I want to show that part in the undeformed (shelf) state. How can I do this within the context of the assembly drawing file?

 

[JohnRBaker]

You will need to add an additional undeformed copy of the Component and that one you will need to make visible in the exploded view while making the deformed one invisible. To keep your parts list from indicating that there are now TWO Components in the Assembly, you will need to add the following named Object Attribute to one of the two Components in the Assembly, 'PLIST_IGNORE_MEMBER'. Just set the value to 'YES' and then update your Parts List.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
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To an Engineer, the glass is twice as big as it needs to be.

 

[BOPdesigner]

Hmm. In that case, what would be the downside of adding the undeformed component to the drawing file instead of a 2nd instance in the assembly?

 

[JohnRBaker]

Since the exploded view must be in the same file as the Drawing, you actually would be adding the second undeformed component to the Drawing file.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.