Dimensions become disassociated after assigning geometry to new component

[NXsupport]

NX8.5.3

I have a part file with 3 solids.. In Drafting , I have made views and added the dimensions..

I come back to Modeling , Click on Assemblies >> Create new component >> Type in the name for the component >> Pick one of the solid to add to the new component >> Ok.

The Dimension becomes unassociated..

Is there a way to keep them still associated on the Main assembly level..

 

[JohnRBaker]

Sounds like you're trying to turn a part file, with an embedded Drawing, into a Master Model Drawing, correct? If so, when you convert one of the bodies into it's own Component, inside what is now an Assembly, that part has becomes an 'Instance'. Now the edge ID's of the 'instance' will be different than what the edge ID's were on the original body and those were the ones that the Dimension was looking for. There is no way to avoid this and if stop for a minute and think about it, you'll understand why.

For example, if I had a model with it's own edge ID's and I were to add TWO copies of that part into an Assembly as Components, while there would be a single 'occurrence' of the Componet, there would be TWO different 'instances', and when you make a Drawing and add a dimensions and pick an edge of ONE of the 'instances' that edge ID MUST be unique to THAT 'instance'. It cannot be the same as the original part's edge ID since there are now TWO copies of that part model body in the Assembly so NX would be confused if the edge ID's on both 'instances' were still the same as they were on the original part model bodies. Each 'instance' will be given it's own unique edge ID's for ostensibly the same edge as on another 'instance'. That's just the way we have to do it to make NX behave the way people expect it to.

John R. Baker, P.E.
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