NX Reference Sets - Again
NX Reference Sets - Again
(OP)
I have been searching the threads all day, and still haven't found a solution to my problem with reference sets.
My assembly problem is more complicated, but I have simplified it here: (NX10)
I have a part "A" with a crimped and uncrimped body in the part. I made 2 reference sets in the part named crimped and uncrimped. Each with the other body not shown.
In my first assembly "B", other parts are assembled with part "A", but no crimping is involved, so I use the uncrimped reference set in this assembly.
In the next higher assembly "C" which contains assembly "B", the parts are crimped. This is where I am thrown off - if I change the reference set in assembly "C",
it messes up the assembly "B". Is there a way to show different bodies of the same parts in different assemblies?
I understand reference sets were not intended to be made in assemblies, so I have avoided that. I have seen suggestions to use arrangements instead,
but as I understand arrangements control position and visibility of instances, not visibility of bodies. Any help would be appreciated.
My assembly problem is more complicated, but I have simplified it here: (NX10)
I have a part "A" with a crimped and uncrimped body in the part. I made 2 reference sets in the part named crimped and uncrimped. Each with the other body not shown.
In my first assembly "B", other parts are assembled with part "A", but no crimping is involved, so I use the uncrimped reference set in this assembly.
In the next higher assembly "C" which contains assembly "B", the parts are crimped. This is where I am thrown off - if I change the reference set in assembly "C",
it messes up the assembly "B". Is there a way to show different bodies of the same parts in different assemblies?
I understand reference sets were not intended to be made in assemblies, so I have avoided that. I have seen suggestions to use arrangements instead,
but as I understand arrangements control position and visibility of instances, not visibility of bodies. Any help would be appreciated.
Product Designer: I-Deas/NX/Catia
Automotive Industry





RE: NX Reference Sets - Again
John R. Baker, P.E. (ret)
EX-Product 'Evangelist'
Irvine, CA
Siemens PLM:
UG/NX Museum:
The secret of life is not finding someone to live with
It's finding someone you can't live without
RE: NX Reference Sets - Again
Product Designer: I-Deas/NX/Catia
Automotive Industry
RE: NX Reference Sets - Again
John R. Baker, P.E. (ret)
EX-Product 'Evangelist'
Irvine, CA
Siemens PLM:
UG/NX Museum:
The secret of life is not finding someone to live with
It's finding someone you can't live without
RE: NX Reference Sets - Again
So to get the result you want, you need to create the same ref sets again in assembly B.
- Ref set Crimped shows component A with ref set Crimped
- Ref set Uncrimped shows component A with ref set Uncrimped
I also always love the Statement "Ref sets are not meant to be used in Assemblies" So what are they meant to be used for then?Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX9 / TC10.1.2
Building new PLM environment from Scratch using NX11 / TC11
RE: NX Reference Sets - Again
So now I have to go back and create separate components for all of my formed parts? If component reference sets only work one level up, that is good news.
This is the result I was looking for, just have to prove it out...
One of the selling points of NX was the multiple body feature - so now I'm confused, what is the purpose of having more than one body in a part?
Product Designer: I-Deas/NX/Catia
Automotive Industry
RE: NX Reference Sets - Again
The example I showed you is with bodies. It is 1 component with multiple bodies. Each body is in a separate reference set.
Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX9 / TC10.1.2
Building new PLM environment from Scratch using NX11 / TC11
RE: NX Reference Sets - Again
I have 2 ref sets in PART1 (FORMED and UNFORMED). I set assembly1 to use UNFORMED. But I can't get assembly2 to show it formed.
This is a pretty common scenario - it shouldn't be this difficult, should it?
Product Designer: I-Deas/NX/Catia
Automotive Industry
RE: NX Reference Sets - Again
Product Designer: I-Deas/NX/Catia
Automotive Industry
RE: NX Reference Sets - Again
Product Designer: I-Deas/NX/Catia
Automotive Industry
RE: NX Reference Sets - Again
Views are out of date? (showing the clock icon)
Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX9 / TC10.1.2
Building new PLM environment from Scratch using NX11 / TC11
RE: NX Reference Sets - Again
Product Designer: I-Deas/NX/Catia
Automotive Industry
RE: NX Reference Sets - Again
Drawing views show out of date while nothing has changed...
Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX9 / TC10.1.2
Building new PLM environment from Scratch using NX11 / TC11
RE: NX Reference Sets - Again
Product Designer: I-Deas/NX/Catia
Automotive Industry
RE: NX Reference Sets - Again
RE: NX Reference Sets - Again
After looking at deformable parts, I don't think that would work for me. My crimped parts have a different sketch profile, not just a variable
that can be changed for different formations. The reference set option seems to be what I need, I just can't get it to work right.
Product Designer: I-Deas/NX/Catia
Automotive Industry
RE: NX Reference Sets - Again
If possible (without divulging any secret information) please provide us with an example of your structure with the issue...
Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX9 / TC10.1.2
Building new PLM environment from Scratch using NX11 / TC11
RE: NX Reference Sets - Again
The structure might be hard to explain: (I don't want to show a screenshot)
I have the top assembly with 3 crimped parts, the next asm down, those 3 parts are not crimped, but one of them is shorter (a reference set of an expandable sleeve that is pulled back for assembly). The next asm down, parts are uncrimped, and sleeve is full length. So I have a reference set of 3 parts crimped, 3 parts uncrimped, and a reference set of the sleeve pulled back (shorter ref set). Like I said, the assemblies appear correct, but the drawings update incorrectly. I hope I don't have to re-create the drawings. (Maybe I accidentally applied ref sets to dwg items?)
Product Designer: I-Deas/NX/Catia
Automotive Industry
RE: NX Reference Sets - Again
Product Designer: I-Deas/NX/Catia
Automotive Industry
RE: NX Reference Sets - Again
This seems like a huge fault that should be fixed in NX. Instead of filtering bodies with reference sets in my assemblies, I'm going to try and
make each body a separate part, and then filter their visibility in assemblies with arrangements. I still don't understand the advantage of being
able to make multiple bodies in parts, if you can't use them (reliably) in assemblies.
Hours of re-work ahead...
Product Designer: I-Deas/NX/Catia
Automotive Industry
RE: NX Reference Sets - Again
I'm not intending to come off as insulting, but with what I stated above and your refusing to post example parts/assemblies or even pictures I'm not sure what one can expect to get in terms of direction or help. Help us help you.
Tim Flater
NX Designer
NX 9.0.2.5 Win7 Enterprise x64 SP1
Intel Core i7 2.5GHz 16GB RAM
4GB NVIDIA Quadro K3100M
RE: NX Reference Sets - Again
Although a Drawing is in fact an "Assembly" like structure, as I earlier said, it is not capable of showing more than one reference set. Which means that you cannot just switch reference sets to show different situations on one drawing. (with arrangements you can and in fact show different arrangements in different views)
With reference sets, for each different situation you need to create a separate drawing.
Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX9 / TC10.1.2
Building new PLM environment from Scratch using NX11 / TC11
RE: NX Reference Sets - Again
I am in the process of pulling all of my formed bodies out of my parts and making them separate parts. But I will try and post some pics to explain:
The first pic shows parts before entering 2nd asm.
The 2nd pic shows sleeve (green) pulled back, and uncrimped parts ready to be crimped.
The 3rd pic shows the end result, with 4 parts formed, sleeve is sandwiched in the crimp.
I had all different shapes as bodies in the parts, intending to use reference sets to show different in each assembly. I could not get it to work reliably.
Product Designer: I-Deas/NX/Catia
Automotive Industry
RE: NX Reference Sets - Again
Update: I removed all of the reference sets in the 4 parts, copied the formed bodies into new parts, added both the formed and unformed
parts to the assemblies, and suppressed/unsuppressed as needed in each using arrangements. It seems like reference sets were a good
idea at some point in time, but the programming never followed through to make this feature robust in the assembly structure.
I now agree with JohnRBaker: reference sets in assemblies are not recommended.
Product Designer: I-Deas/NX/Catia
Automotive Industry
RE: NX Reference Sets - Again
You cannot drive arrangements in subassemblies
Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX9 / TC10.1.2
Building new PLM environment from Scratch using NX11 / TC11
RE: NX Reference Sets - Again
The point of promote body in NX is that you can modify the body at assembly level with all the powerful tools you have at part level, so you can cut, extrude, bend...
RE: NX Reference Sets - Again
It seems to me it would be better to show these scenarios in the same level of assembly. Create one assembly with all of the parts you need. If you need to show a component in three different reference sets, you would add the component to the assembly three times on different layer. All three instances of the same component can be set to a different ref set. Then in the drafting views, only show the layers of the component with the correct ref set you want visible. In your pictures above, make the first picture on sheet one with each of those components on layers visible in that view. Turn other layers off. On sheet two you can add a view for picture #2 and show the layers with the components with those ref sets. and so on...
**If I am way off on understanding the problem, please ignore this message.
RE: NX Reference Sets - Again
RE: NX Reference Sets - Again
Yes that's true but! The arrangements are stored in the toplevel of the assembly-A where they are created. When you create assembly-Band use A as a sub assembly you cannot drive those arrangements in Assembly A and store it in Assembly B.
Next time you open the Assembly B it will use the Default arrangement from Assembly A.
Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX9 / TC10.1.2
Building new PLM environment from Scratch using NX11 / TC11