Parts are not appearing in assembly 1

[markvdh]

Hello,

I am working in NX 10.0 and am having issues with loading parts into an assembly. I created some parts and wish to load them into an assembly. However, when I load them they do not appear, but show up in the assembly navigator. The only way I can make it appear is making it the work part, but then I am unable to create any constraints with other parts.

I have experience with SolidWorks, but just recently started using NX so I am probably making some simple mistake.

Thanks for your help!

 

[JohnRBaker]

Check your layer status.

John R. Baker, P.E.
EX-Product 'Evangelist'
Irvine, CA
Siemens PLM:
UG/NX Museum:

The secret of life is not finding someone to live with
It's finding someone you can't live without

 

[markvdh]

Layers do not appear to be the problem. I'm just confused because I have parts created by someone else previously that I can load into assemblies fine, but the parts that I have created are not visible when loaded in an assembly...

 

[Arkance/PhoeNX]

I'm guessing reference sets are the issue.
I did a tip for our site a while back about this issue, it might be of help:

http://phoenxplm.com.au/files/tips_tricks/TipsTricks_201510_WhereAreMyObjects.pdf

Anthony Galante
Senior Support Engineer


NX3 to NX10 with almost every MR (29versions)

 

[markvdh]

Thank you, reference sets were the issue. I had tried messing with the reference sets, but I guess I hadn't tried selecting the "Entire Part" reference set because that worked perfectly!

 

[JohnRBaker]

Yes, but 'Entire Part' is just a item of last resort. You really should set-up your Modeling Reference Set with a common name and use it instead as it will help to reduce the amount of data that needs to be opened and loaded into memory when opening an Assembly. Under normal, that is 'buy default' or out-of-the-box, there should be a 'Model' Reference Set created which will automatically only contain you Solid Model and no extra curves or sketch objects. The only regular usage of the 'Entire Part' Reference Set is when creating a Part file that will be used as a Sub-Assembly in a higher-level Assembly. In that case your Part File will generally consists of only Components and therefore you should avoid adding Components to a specific Reference Set (if left to itself, NX will NOT automatically add Components to a defined Reference Set) therefore when you add the Sub-Assembly Part file to your higher Assembly, now is the time to use the 'Entire Part' Reference Set as that will assure you that all of the Sub-Assemblies Components will be included in the full Assembly.

John R. Baker, P.E.
EX-Product 'Evangelist'
Irvine, CA
Siemens PLM:
UG/NX Museum:

The secret of life is not finding someone to live with
It's finding someone you can't live without