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NX Modeling and Drafting - Separate Files?

Pioneer
Pioneer

When creating a part or an assembly in NX should the detail drawing be a separate file?

1. I know you can change between modeling and drafting under the model file, but doing this doesn't allow use of attributes connected to the title block. (NX-Design-Forum/Numeric-expressions-driven-by-attributes/m-p/519669#M26228)

2. If you create a new file for the drawing associated to the model, you must "add" the model to the drawing file in modeling in order for the template border to update (parts list, attribute name, etc.). However this option doesn't allow you to show the exploded view associated with an assembly.

8 REPLIES 8

Re: NX Modeling and Drafting - Separate Files?

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

If you are creating a true "exploded" view, this must be done in the drawing file, NOT the model file.

 

If you are using an arrangment as the explosion, that should work in either the model or drawing file.

Re: NX Modeling and Drafting - Separate Files?

Pioneer
Pioneer

Thank you for your feedback. Why does NX allow a model and drawing to be on the same file then? Is there any incentive to this?

Re: NX Modeling and Drafting - Separate Files?

Solution Partner Genius Solution Partner Genius
Solution Partner Genius

Master Model approach vs. the embedded drawing approach where master model has separate files for the 3D CAD and the 2D drawing and the embedded drawing is, well, embedded and in a single file. 

 

While I prefer the master model approach as it supports concurrent design/drafting, in a native (non-managed) system, it is easier to have a single file that is both the 3D model and the 2D drawing. Fewer files to maintain. A save-as to a new part number is easy. 

 

If you follow the master model approach in a native (non-managed) system, you have to remember that there is a drawing associated with your part and save-as the drawing and the 3D model. 

 

If you're in Teamcenter, the management of the separate files is automatic making it much easier. 

Re: NX Modeling and Drafting - Separate Files?

Pioneer
Pioneer

I agree, I prefer using the master model approach. I am using Teamcenter, so the management of files is not an issue. It is strange that there is an option though. Shouldn't this be a standard operation? Either a model file contains everything including the drawing, or all files are separate.

Re: NX Modeling and Drafting - Separate Files?

Honored Contributor
Honored Contributor

I think it's just a matter of Unigraphics providing the option to do it either way, depending on the customer needs.  I've worked with master model in Teamcenter (my preference), but also master model in native, and single file in native.  All work, just different.

-Dave
NX 11 testing NX1847+ | Teamcenter 11 | Windows 10

Re: NX Modeling and Drafting - Separate Files?

Pioneer
Pioneer

Okay, fair enough. Thank you for all the input. I appreciate it.

Re: NX Modeling and Drafting - Separate Files?

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

While I prefer master model ("MM") approach, one place that having "everything in one file" seems to work better is for part families, if you want specific drawings for each part family member.  I don't know if NX has made any enhancments to support using MM for part families recently, however.

Ken Akerboom Sr CAx Systems Engr, Moog, Inc.
Production: NX10.0.3.5 MP16/TC11.2
I'd rather be e-steamed than e-diseaseled


Re: NX Modeling and Drafting - Separate Files?

Builder
Builder
We primarily use master model concept. Our assembly files contain about 400-1000 components plus fasteners.

Recently we designed a project for a customer who uses the embedded process. I can tell you our machines were crawling slow. Whereas on other projects using master model had no speed issues. Mind you we had 5 designers working via ethernet from server.

I would recomend not using the embedded system also if you have a corrupt file you dont lose the model worst case you make a new detail dwg.
NX12.0.2.9 Win10 64bit, Tecnomatix PS V14.1.