Component as reference

[cubalibre000]

Hi,
I don't remember in which version, maybe NX7 and before, but on RMB on a component in the assembly, further the option to set the component 'is no geometry', it was the option to set the component as reference only.
Starting from NX >7, this setting is possible via onerous rout by the user on the attribute tab or for the possessor of Teamcenter.
I don't think that Teamcenter change the dll used by NX for this mask, but there are some type of setting.
This option is very useful to set to hide some components from the part list and the rout used now is complicated for standard users.
Setting ?
Not documented setting ?
Journal ?

Thank you...

Using NX 8 and TC9.1

 

[cowski]

In NX you can set a component attribute to exclude it from the parts list. In NX 7.5 and earlier it was difficult to find and had to be set up manually. In NX 8 and later, the attribute is already there on your component, you just need to give it a value to activate it. The attributes are named PLIST_IGNORE_MEMBER and PLIST_IGNORE_SUBASSEMBLY; set them as appropriate for your situation.

www.nxjournaling.com

 

[JohnRBaker]

Starting with NX 6.0, even if you're running in 'native' (i.e., non-Teamcenter) mode, simply select the Component of interest, press MB3 and select the 'Properties' item. There you will find an option to indicate that the Component is 'non-geometric'.

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

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

 

[Nham]

Hello all,

Again one topic that while reading this a need to comment and ask became too compelling to resist

While reference only is a great feature, it does have it's downsides as well. Especially when used with teamcenter and multisited material. My experience is that while reference only hides the specified bomline from teamcenter BOM it also therefore makes this bomline invisible to teamcenter plmxml export and multisite exports. Locical but frustrating. To an nx user it is easy and logical to use reference only grom cad. Other not so logical option is to use TCbom row exclusion attribute (occurrence) or if the entire item is never meant to be a part of a bom then use item attribute that says in all cases exclude item and not just occurrence from bom. This is not logical for an NX user to jump to TC in the middle of modelwork to specify occurrence information in structure navigator and get back to his model. (editing a bvr as cad model is open creates interesting complications and so on for inexperienced users that do not know better.)

John and other experienced guys, do you see other options? Workarounds? Problem is created in NX so solution has to be available as well. I suspect that I am not alone with NX and multisite in this universe:

Using reference only is handy but when sending data to other teamcenter sites these reference only items are not visible to tc at all. Therefore they do not get exported via other normal bomlines. Only from receiving end NX users will there be feedback when not all models reach their destination. This creates a challenge for administering multisite data. Currently we are in mixed mode situation with both occurrence and reference-only geometry. So taking out either of the options is not an option.

Now we are thinking a nimimal user interaction ugopen program that will take all reference only parts from chosen assembly and all child levels and copy them in teamcenter navigator and a folder. Then replicate the contents to the other site. There are also challenges in doing this teamcenter navigator has only a fraction of functionaliti compared to real TC client and some features are not accessible easily.

Problem is only replicating items forst time. Then sync will take of the rest. How to know you need to have something replicate because it is only viewable within NX part itself and not TC?

If one of you fellow eng tippers have a solution that you utilize I'm all ears.

NH

 

[JohnRBaker]

While the original question mentioned 'reference' it also brought up the fact that there used to be some way to indicate that a component was to be considered as 'non-geometric', that is, it appears in the Assembly Navigator and the Parts List but is not physically seen when looking at the assembly model. THAT is the question that I was responding to.

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

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