How to reattach dimensions for extracted geometry?

[yy912]

I made a drawing for a body. Then I extracted the body, made some changes on the extracted body. Now I want to create a similar drawing for the extracted body.
But once I replace the body(by switching reference set, for example), all existing dimensions, centerlines, notes with leader, etc, are dangled, even though most geometry of extracted body is the same.
I can still fix some of them by editing them manually. But is there any easy way for NX to "recognize" the unchanged portion and reattach the dimensions automatically?

NX 1919 Windows 11

 

[cowski]

In modeling, NX has a fairly good way to map geometry from the old reference to the new one. Unfortunately, there is no equivalent in drafting. It would be a useful tool and I encourage you to open an enhancement request with Siemens.

www.nxjournaling.com

 

[yy912]

@cowski Thank you for the reply. It's sad that this feature is not available yet. I will see if I can open an enhancement request for it.

NX 1919 Windows 11

 

[Toost]

If you would do a Save As of the model (to New file ) instead of Extract, then NX will keep all the ID's on edges and faces, and, no need to remapping the dimensions.
I am assuming you use Master Modeling , one file for the model and a separate drawing file.

I.e
Model A, + drawing A
Save as into :
Model B + drawing B

Regards,
Tomas


The more you know about a subject, the more you know how little you know about that subject.

 

[yy912]

@Toost Yes "save as" can maintain the dimension attachment, but it does not maintain the associativity between part A and part B.
Part B is mainly based on Part A, and if there are changes to Part A in the future, I want the same changes applied to Part B as well.
I just tried "wavelink" across parts, which seems to work in the same way as "extracted geometry" within same part, that the dimensions are dangled as well.

NX 1919 Windows 11

 

[TCS153518]

In NX Drafting the dimensions are associated to UID of the extracted drafting edges from the solids in drafting environment., So if any of that changes in Modeling, the dimensions loose their associativity in drafting as the UID changes for those entities even though they were extracted in Modeling.
I dont think Siemens has yet found a solution to this and also, IMO its better this way as it gives the user to make sure and confirm if the dimensions are correct on the new extracted body .