Standard Practice for Drafting in NX

[Nahid Mubin]

In NX, I can make drawing of a part file in two ways. One is to switch to the drafting environment in the same file and start making drawing. Another is to make a new drawing file and start making drawing. Why there is two way? Which one is used in standard practice? Is there any use cases for both of the options?

 

[Toost]

NX has an extremely long history for a piece software. ( If John Baker is listening he can add some details on this.)

Siemens NX - Wikipedia

en.wikipedia.org

Back in time the concept was to create everything in a single file, this was before the concept of "assemblies" where other parts where referenced in-to the assembly file.
You created the model , the drawing, the documentation, the CAM, the Finite Elements etc etc all in a single file.

Somewhere early 90-ies, UGS introduced Unigraphics V10 , new user interface and new architecture and, it included Assemblies and along with that the concept of having the different disciplines in different files.

The recommendation is , since then... , to create the drawing in a separate file.
Siemens NX development has a principle of not abandoning the history so you can still do all these operations in single file, which some still do.

 

[JohnRBaker]

NX has an extremely long history for a piece software. ( If John Baker is listening he can add some details on this.)

Siemens NX - Wikipedia

en.wikipedia.org

Back in time the concept was to create everything in a single file, this was before the concept of "assemblies" where other parts where referenced in-to the assembly file.
You created the model , the drawing, the documentation, the CAM, the Finite Elements etc etc all in a single file.

Somewhere early 90-ies, UGS introduced Unigraphics V10 , new user interface and new architecture and, it included Assemblies and along with that the concept of having the different disciplines in different files.

The recommendation is , since then... , to create the drawing in a separate file.
Siemens NX development has a principle of not abandoning the history so you can still do all these operations in single file, which some still do.

Yes, I still watch this forum, even when I'm on vacation like I am at the moment

And you've got it about right. What Toost described is what we called the 'Master Model' concept where you only had to create the geometric model of your item once. After that you referenced that original 'master' model for all of the downstream applications like drafting, analysis, manufacturing, product configuration (assemblies), documentation, etc. This had several benefits. First off you only had create and maintain a single geometric model of your part. Also multiple disciplines, which could be different individuals, could access a read-only copy of that 'master' model, which would appear as a single level 'assembly' but where you would create your drawing(s), create a finite element model, create manufacturing tool-paths, group together with other referenced copies of other parts to create a product model (assembly), etc. In the end, while it might look like you will end up with more files, managing changes and variations will be much easier. Now this is where PDM type produces like Teamcenter comes into play, and while you can manage a master model environment with out a formal PDM system, after all, the 'Master Model' concept had been in use long before we had any real PDM type products, but products like Teamcenter are almost mandatory with today's complex product designs and multi-disciplined environments.

Anyway, I hope this helped explain how NX works when it comes to using a referenced or 'Master Model'.