How to mate two planes together in NX4

[CADWHORE]

Does anyone know how to mate a plane in a part with a plane in the assembly level. The problem is that the plane on the part is not visible when I go to select it in the assembly, unless I make that part the work part, then I cannot make an assembly mate. Any ideas from anyone????
Thanks

 

[JohnRBaker]

Change the Reference Set of the component to 'Entire Part', do your mating and then set it back to 'Model'.


John R. Baker, P.E.
Product 'Evangelist'
UGS NX Product Line
SIEMENS
UGS PLM Software
Cypress, CA

http://www.siemens.com/ugs

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

 

[CADWHORE]

WOW!!! Very interesting, thank you so much. I like that little trick, could you explain more on what the reference sets do?

Thank you much

 

[JohnRBaker]

Reference Sets are a means of allowing you the define what it is that you wish to see when that part is used as a Component in an assembly. By default, the only items in the 'Model' Reference Set is the solid body of your model. Any non-bodies, such as sketches, curves, points, datums, etc. are not included in the 'Model' Reference Set unless you explictly add them, however, since you always have the option of using the 'Entire Part' Reference Set there generally is no need to do that, since you can do as I suggested, just swap between them.

Note that if you set your system up properly, in addition to the two default Reference Sets, 'Entire Part' and 'Empty', both of which should be self-explanatory, the system will also create 2 additional ones automatically. Those are called 'Model' and 'Facet'. The 'Model' Reference Set, as I mentioned above, will automatically contain the solid bodies of your model while the 'Facet' will contain a lightwieght faceted representation of whatever bodies are in the 'Model' Reference Set. Also, anytime you make changes in the future to your model, these 2 auto-Reference Sets will be updated.

Now one precaution, since you've just learned about Reference Sets, please let the system work the way it's set up to work. That means DON'T create Reference Sets in part file which are Assemblies, that is they contain only Components and no bodies. While it can be done, we don't recommend it since Reference Sets also act af 'filters' (and in a way that's the way they are intended to work, which you look at how they do what they do for you), but in the case of an Assembly, if you filter-out a component, that can be problematic, particularly if that component was an assembly (sub-assembly) itself.

Anyway, use them as I've described and you should be very happy with them.



John R. Baker, P.E.
Product 'Evangelist'
UGS NX Product Line
SIEMENS
UGS PLM Software
Cypress, CA

http://www.siemens.com/ugs

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

 

[CADWHORE]

John,

Thanks again for this explanation, I am a new user and this helps out alot.

 

[toniechang]

As always, very interesting, John.
I didn't get that 'precaution' in mind
but I'll surely investigate on it.
Thanks. ;-)