Creating simplified & detailed versions of a part

[imagitec]

I've used SolidWorks for ten years but recently started working for a company that uses NX. The company itself has just switched from I-DEAS to NX, with everyone (including myself) going through a week of training. So we are all starting at about the same level of expertise.

I would like to create a model with simplified and detailed versions. For example, a model of a screw, with the option of showing detailed threads or not. In SolidWorks, I would have two Configurations. In z configuration called Detailed, the threads would be modeled explicitly as a helical cut. In a configuration called Default, the helical cut feature would be suppressed, so that the screw appeared as a simple cylinder. The appropriate configuration could be selected for a given purpose in the assembly model.

From what I learned in the class and read in the help files, it seems like Reference Sets would be the way to accomplish this. But I can't figure out how to control the visibility and/or suppression state of a particular feature in a particular Reference Set.

If I'm on the right track, what am I missing?

If I'm not, what approach would you take?

Thanks for your help,
Rob


Rob Campbell, PE

 

[JohnRBaker]

Here's how I've handled this for years. Open the attached part file and edit the Expression 'Threads' from a '0' to a '1' and hit OK.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

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

 

[t300]

Hi Rob,

a good solution is using reference sets. The standard refence set "model" will use symbolic threads, another reference will use a detailed thread, a third one a simpliefed one.
If you open the attached sample you need to switch on the layers 2 and 3 to see all of the part geometrie.
If you insert the part into an assembly you can switch between the different reference sets.


Meinolf

 

[imagitec]

Meinolf,

That is exactly how I thought it would work, but I can't figure out how to create the different reference sets with the different geometry.

As a test case, I created a plate with a hole in it; the plate is one extrude feature and the hole is another. I created a Detailed reference set. I'd like the hole to appear only in the Detailed reference set, but I can't figure out how to do this.

Could you provide more information on the actual procedure?

Also, how do I activate a specific reference set when I'm working on a part (instead of an assembly)?

Thanks,
Rob

Rob Campbell, PE

 

[imagitec]

John,

Could this be integrated with Reference sets, so that changing to a Detailed reference set would set the value to 1 and switching to the Model reference set would set the value to 0? It wouldn't be as elegant as configurations in SolidWorks, but it would work.

(SolidWorks can track the suppressed/unsuppressed states of individual features. You can also specify whether new features added to a part will be automatically suppressed or unsuppressed in a given configuration, which makes them easier to maintain.)

Thanks,
Rob

Rob Campbell, PE

 

[JohnRBaker]

In order to use Reference Sets, you will have to create to totally separate models, one with threads and one without, and assign each model to its one explicit Reference Set.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

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

 

[BOPdesigner]

In the version before the current Machinery Library fastener selection, the thread styles (centerline, symbolic, detailed) were controlled by reference sets. I have not checked but I suspect that example that Meinolf uploaded is one of these. Current version of ML uses the 0 and 1 expression method to suppress the detailed threads. Advantage 1 is that file size is reduced. Disadvantage is that it is not as easy to toggle on and off at the assembly level.

 

[cowski]

You can approximate what you want with the tools NX offers, but there is no direct functionality like Solidworks configurations (at least none that I'm aware of - I've been using UG/NX for 10 years, but I'd be glad to have someone prove me wrong).