Reference only part

[FunRuSSkiMAN]

Dear all,

I have run into a little problem that is driving me nuts. I created an assembly and added some reference only parts to the drawings. i.e. they only show up in the drafting environment not in modeling. The 'reference only parts' icons show up in the assembly navigator as the yellow cube (part) with a drawing boarder in the background. I took this assembly and added it to another assembly and these part became regular parts somewhere in the process. Can I toggle parts to become 'reference only'. I.e. so that the part goes back to only being visible in the drafting environment and the icon changes back to the part with a white drawing boarder behind it?

Many thanks

 

[JohnRBaker]

What version of NX are you using?

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.

 

[FunRuSSkiMAN]

sorry....
NX6

 

[JohnRBaker]

Thinking about what you're doing it appears that this is not in accordance with the way Master Model drawings are created nor intended to be used. In reality, the first drawing you created, despite the ability to 'add' components as reference objects, this Part file itself should NEVER be considered an 'assembly' in the sense that it could be added as a 'sub-assembly' in the next higher level of your product model.

If you need to add this first assembly (not the Drawing Part file, but the file which contains the original assembly BEFORE you created your first drawing) as a sub-assembly in some other assembly, when you create your drawing of THAT higher-level assembly, if it's still important for you to see these same reference-only components from the first drawing, and for them to remain as reference-only components, in the second drawing, then you will need to re-add them as explicit reference-only components TO the top level Drawing. Perhaps is we had called them 'view-dependent' components, it might have been clearer that they only behave as expected when SEEN in their 'view', i.e. the original drawing.

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.

 

[FunRuSSkiMAN]

Thank you for your answer! And I completely agree with you. I should have done that from the start - and will do so in the future. But i really dont have time to be reworking things therefore if you know how I could toggle the part back - i.e. if there is a assembly component property where i could check "for reference only" - i would very much like to know how to get there.

Thanks again! Your help is greatly appreciated!


Materials Engineer
Rolls-Royce Corp.
UGS - NX6

 

[JohnRBaker]

There is NO way to 'toggle' the 'Reference Only' status of a Component since, as I alluded to earlier, it's really a state which was related to the ORIGINAL drawing and it's only possible to establish that status at the time that the components were added to the 'drawing'. However, once they became part of the original drawing, when it was later added to the second drawing, those components are now treated like any other since their special status was only in effect while viewing the original drawing. Sorry.

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.