NX4 - Representations
NX4 - Representations
(OP)
Hi all,
I've been having a bit of a play with representations in NX4 and they appear to work really well? The initial reason for looking into representations was to allow me to be able to load a large assembly quickly.
Is there anything I should know or be warned about begore using these?
Many thanks in advance
I've been having a bit of a play with representations in NX4 and they appear to work really well? The initial reason for looking into representations was to allow me to be able to load a large assembly quickly.
Is there anything I should know or be warned about begore using these?
Many thanks in advance
Mark Noyce
Senior Design Engineer/CAD co-ordinator





RE: NX4 - Representations
John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/
RE: NX4 - Representations
I think I may be missing something :(
What I liked about creating a representation in assemblies was that I can load the assembly without components and it would display the assembly without having to change reference set. I can then choose to load the parts I require working on.
I see that I can load an assembly without components, change reference set to FACET and get the same thing, but that seems like more work as when I decide to load a component I have to change reference set back to SOLID.
Please forgive me if I've completely got this wrong and confused myself?
Thank you
Mark Noyce
Senior Design Engineer/CAD co-ordinator
RE: NX4 - Representations
The place where that falls down for mine is that you can't change control and properly manage all the components in all the assemblies all of the time, especially when you have a team of designers work on the parts. Secondly if you are working in a team and different individuals do things slightly differently then what you'll find is that some will have representations in the components and others in the assemblies , and if not that then you'll want to open the components using the solid, model or part reference set (whatever has the real geometry), and then you end up with two versions of the same thing one on top of t'other.
It has all been tried and ended in tears before now, we maintain a rep reference set which collects the rep reference sets of all the components. The system is reasonably capable to maintaining this although users can occasionally intervene to mess things up, so we have a few programs that we use to keep things in check.
You'll find that NX has pretty much been designed around a similar way of working and as such it also avoids the necessity to load twice the representations provided that one version always resides per piece part. To make best use of this partial loading should be turned on.
Best regards
Hudson
RE: NX4 - Representations
Every time I create a part it automatically creates a reference set "FACET" which includes the lightweight model.
Now if I load an assembly "without" loading components, how do I see the lightweight model? It doesn't let me choose the faceted reference set unless I actually load the part. I presume I'm doing something wrong?
regards
Mark Noyce
Senior Design Engineer/CAD co-ordinator
RE: NX4 - Representations
You can set in your load options for the preferred reference set to be the one with the lightweight reference set containing only facets or representations if you like. You address it by name. You set partial loading on, and you do need to load some of the components. At that point you'll have loaded pretty much exactly the same amount of data that you might have used by any other equivalent method.
Firstly some people insist that assemblies contain no reference sets. It may be worth considering and may have been the intent of John's posting. He will likely confirm his intent and you could assume that NX is designed to be used according to his advice.
Many including ourselves set up two reference sets only per part one called "REP" containing facets, and the other containing geometry which we call "MODEL". This is the NX-5 out of the box flavor, as applied to components only (i.e. assemblies don't have reference sets). When I say out of the box they're defined in the customer defaults and maintained automatically when you save the parts. Again you need not have reference sets in assemblies.
But if you did want to create the same reference sets in assemblies manually you would change all the component's reference sets to MODEL and create the MODEL reference set by adding the components to it. You would do the same with REP to create REP reference sets. Logically this would be in line with expectations but in practical terms it can be hard to keep straight.
The benefit of this is that you can switch between the two en masse a little more quickly and easily. However it may occasionally need to be maintained, and if you don't have some means to do so then it will likely be more trouble than it is worth. Where I have seen it done thus then we had programs to be run regularly that maintained the reference sets correctly.
The problem with it is that you can only see the contents of a reference set from the vantage point of an assembly one level higher than it. So that if at lower levels' assemblies contain reference sets then when the top assembly is saved supposing that the contents of some of the components are changed at any level they may need to be saved (where possible), to reflect those changes. Those changes may only be changes affecting which reference sets of the components are shown by the reference sets of the sub-assemblies due to changes made by users working in the top assembly. From time to time in the course of working on the data if things are changed so that non-standard settings are employed then depending on which files you may or may not have write access to when you save then you'll be saving some non-standard reference sets. It is hard enough to explain this let alone keep track of it and remedy the problem on every occasion.
I'd like you to experiment with this because what you've hit upon needs a hands on approach. Also I may have to write several pages of an explanation that always becomes confusing in the language of child parent and grandparent to represent three levels of an assembly. It is a well known three level assembly reference set problem, and most users eventually figure out what's up and decide how to proceed on that basis.
Best Regards
Hudson
RE: NX4 - Representations
I think it's starting to make sense, as you say, it isn't the easiest thing in the world to try and explain and I was most certainly confusing myself.
I'm going to do a bit of experimenting and get my head round it, I'll keep you all posted with my progress and once again, many thanks!
Kind regards
Mark Noyce
Mark Noyce
Senior Design Engineer/CAD co-ordinator
RE: NX4 - Representations
Another useful feature within NX is assembly outline, we use it to help our new starters get a feel of the product and anable them easily navigate to certain areas of the machine visually rather than using some of the more complex tool like open by proximity with true shape filtering. Assembly outline create very light weight bodies that are stored on layer 190 I think and you can open the full machine in a second or two, you can then use the cursor to highlight a part and open it fully. Be careful though as you can easily get out of date and we tell users never to design in context using the assembly outline bodies. Have a go with it and see what you think. No reference sets requires simply layer on or off.
Assemblies > context control > define product outline
Best regards
Simon
RE: NX4 - Representations
Mark Noyce
Senior Design Engineer/CAD co-ordinator