Breaking links in an assembly 1

[jtrist]

Is there a simple way to break all the links in an Assembly? For years I have used UG and created what I call a proper tree. I am at a new company and have been told that I cannot have geometry linked between parts. Don't ask, I have been told and will do as I am told ( trust me I fought as much as I could )Now I have exported out a step and brought it back in, but then I lose all parameters. I would like to keep the links active till the end when I submit the design. Is there a way to break the links in a full assembly without having to do it in each part for every link?

Thanks for the help.

NX 8.0.3.4

 

[gani009]

Simply export assembly once instead of individual then call back assembly in flatten part. you will get dumb bodies only.

GANESH KOTHAKOTA
CAD/CAM LEAD
NX8.5, Vericut7.3.1
TECHMAHINDRA Inc

 

[jtrist]

Thanks gani009, but I am trying to keep the history if possible. Doing that also loses all the taps. I have to go back and redo all my tapped holes with a symbolic thread.

 

[gani009]

If you want your history in part file then remove constraints use fix constraint so your part will be fixed without any reference

GANESH KOTHAKOTA
CAD/CAM LEAD
NX8.5, Vericut7.3.1
TECHMAHINDRA Inc

 

[JohnRBaker]

I think you're talking about inter-part or WAVE links, correct.

If so, is it sufficient to simply 'Break' the links, or do they have to be removed altogether? If simply breaking the links will be adequate, you can use the 'Relationship Browser' to create a diagram of your Assembly and then show all of the links in the list of 'Relations', select them all, press MB3 and select the 'Break Links' option. This will break all links but Interpart Expressions.

Note that you can do the same thing using the 'Interpart Link Browser'.

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.

 

[jtrist]

You are the man John! I figured it had to be there somewhere. Yes I just wanted to break the links, not remove them or the rest of the history.

I found the interpart link browser. Worked great. It was currently hidden. I can not find the Relationship browser. Where is that?

Thanks again.

 

[JohnRBaker]

You can find the 'Relations Browser' at...

Assemblies -> WAVE -> Relations Browser...

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.

 

[jtrist]

Hi John,
Used interpart link browser last week, worked great. This week, it says "available in gateway", I open gateway and it says not available. So confused. I found the relationship browser, but it says can not find Wave license. I am assuming we do not have that bundle.

Help. what am I doing wrong?

Thanks.

 

[cowski]

I'd guess that your company has a limited number of "floating" licenses that grant you the ability to use the wave relationship browser. Last week there was a free license that you were able to access; apparently they are all in use today and you do not have access to it. Your CAD admin should be able to track down who currently has the license(s) so you can get the license from them when they are done with it.

www.nxjournaling.com