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NX Reference Sets - Again

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.

Product Designer: I-Deas/NX/Catia
Automotive Industry

RE: NX Reference Sets - Again

Arrangements can control content as well as position, but it applies to only Assemblies (actually sub-assemblies in this case). But if this really an Assembly then you should be able to define a pair of Arrangements, one where the un-crimped part is used and one where the crimped part is used.

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

(OP)
How is this done? If I make an arrangement, it won't let me hide/show bodies in the arrangement, only instances. If I hide an instance, it hides both bodies.

Product Designer: I-Deas/NX/Catia
Automotive Industry

RE: NX Reference Sets - Again

You may have to make them separate components.

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

Keep in mind that a reference set only works one level up...Which means it will only have effect in the assembly which holds the component.

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

(OP)
I was trying to use reference sets with bodies, not components. This makes the reference set carry up through all assemblies, not just one level.
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

@ Suskam...

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

(OP)
I must be missing something. I created a dummy scenario (see pic). If I create reference sets in assembly2, it won't let me pick the bodies to include/exclude.
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

(OP)
Holy cow, I just figured it out. You don't have to re-define the reference sets in each assembly (pick the bodies), you just have to have them named the same in each assembly (I assume they have to be named EXACTLY the same). I guess that is obvious to a long-time user. After I created the same named reference sets in each assembly, I could replace them in each assembly. Thanks for all of your help, these forums are so helpful, especially for us newbies. Now I have to apply this theory to my real parts and assemblies...

Product Designer: I-Deas/NX/Catia
Automotive Industry

RE: NX Reference Sets - Again

(OP)
One more question - after I fixed all the reference sets, each time I pull up the drawings for these assemblies, it always shows they need updated. Is that common, and if so - why? It's like it has to re-read the ref sets each time you call up the drawing.

Product Designer: I-Deas/NX/Catia
Automotive Industry

RE: NX Reference Sets - Again

What do you mean with update?
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

(OP)
Yes, views need updated.

Product Designer: I-Deas/NX/Catia
Automotive Industry

RE: NX Reference Sets - Again

A common problem with NX.
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

(OP)
I still haven't solved this issue with reference sets. My reference sets in upper assemblies are carrying down to lower assemblies, which they shouldn't. I did notice some of the drawings views are related to drawing items (icon with the titleblock behind it), and some are related to the assembly item. Could this confuse the reference sets somehow? Is there any other thing I should check - very frustrating.

Product Designer: I-Deas/NX/Catia
Automotive Industry

RE: NX Reference Sets - Again

Suskam have you thought about using Deformable Part for this instead trying to do it with Reference Sets? I think it would be worth considering it as well.

RE: NX Reference Sets - Again

(OP)
I saw that option, but have never used it - will look into it. I would like to solve the reference set mystery also, though.

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

Also keep in mind that you can use only 1 reference set on a drawing...

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

(OP)
I'm starting to think my problems are with the drawings. As I change the reference sets in assemblies, the drawing views update incorrectly. I put all the drawings away, and only have the assemblies out, and the reference sets are correct as I look thru the structure.

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

(OP)
I must be doing something wrong. If I have the drawing open then switch to modeling, the assembly looks different than having the assembly open. ????? (I heard that in NX11 you don't have to switch back and forth between modeling & drafting)

Product Designer: I-Deas/NX/Catia
Automotive Industry

RE: NX Reference Sets - Again

(OP)
I'm going to have to abandon reference sets - seems crazy since that was an NX selling point for being able to make multiple bodies in a part.
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

How certain are you that you were doing everything correctly? You seem pretty confident that it's the software. I only ask because in your first post you make a completely inaccurate statement concerning Arrangements - they CAN be used to control visibility, as can layers when used in the correct context/situation. If you don't fully understand one command, then chances are you're not fully understanding another.

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

Yeah...What you are trying to do is indeed not how it is intended by Siemens...
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

(OP)
@Xwheelguy: Not sure what you mean, my first post does say that you can control visibility with arrangements. At this point that is one of the only things I am sure of.
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

(OP)
I must have scared everyone away...
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

Keep in mind that also Arrangements work only 1 level up...
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

Another approach would be to use promote body. You design de uncrimpped body at part level (part A), then you assemble with the wires and you have an assembly with all the parts but not crimped yet (assembly B), then you create another assembly (assembly C) and add the assembly B inside assembly C. Once in assembly C you promote part A body and modify it to crimped. As you are not working with reference set, the drawing of each part/assembly will show you the part/assembly as it is in real life.

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

I am bit confused by what is happening. If I get this right, you are adding a part to an assembly with one reference sent. Then you are adding that assembly to a higher assembly and want the part to be in another ref set?

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. clown

RE: NX Reference Sets - Again

NutAce: This goes a bit off the topic but you can use Arrangements to drive parts two levels below if you use Position Override option in the parts you are driving with Arrangements.

RE: NX Reference Sets - Again

Quote (SS88)

NutAce: This goes a bit off the topic but you can use Arrangements to drive parts two levels below if you use Position Override option in the parts you are driving with Arrangements.

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

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