Drawing creation method

[NickDOS]

When creating a new drawing in NX you have the option to choose the "relationship", either "Reference Existing Part" or "Stand-alone Part". Can someone explain what the function difference is (if any) between these two options?

Thanks,
Nick

 

[JohnRBaker]

The 'Reference Existing Part' approach is what's often referred to as the 'master Model' approach, where the Drawing file is a 'single-level' Assembly where the part, which could be an Assembly itself, is a Component in the Drawing file. What this means is that the Drawing file is 'referencing' the 'Master Model' rather than having BOTH the Model and Drawing data included in a single Part file. This helps keeps the model files smaller, allows multiple people to access the Model file while adding value when creating Drawing, and is also the way we do Manufacturing and FEA, again using this 'Master Model' approach. Note that if you're using Teamcenter, this workflow can be made more automatic and enforced.

And of course, the other option, 'Stand-alone Part', it is just what it says, the Part file would then contain all of the data needed to both define the geometric model and the Drawing annotation and layout.

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

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

 

[NickDOS]

Hello John,

That almost seems backwards to me. If I create a drawing using the "Reference Existing Part" option I can go back into the modeling application and see the 3D model. If I create the drawing using the "Stand-alone Part" option and go back to the modeling application, I can not see the model. Also I noticed the icons in the assembly navigator are different when using the different options. (I uploaded a screen grab showing the different icons).

 

[JohnRBaker]

No, it's what you do next after opening a 'Stand-alone Part' that counts. If you just want to do 2D modeling you can do in right on the face of the Drawing. If you want to do actual 3D modeling, just switch the application to Modeling, create your model and then go back into Drafting and see what happens. You'll have your model and your Drawing in the same part file with no structure in the Assembly navigator.

From your image, it appears that in the first example, after you made your 'Stand-alone Part' you added views from some other model, but it created view-only information which is why it's not seen when in Modeling since the actual model is in some other part file.

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

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