Reference sets

[bbylls]

In UG NX8.5 trying to create a reference set in an assembly.
In the dialog box I click 'Add New Reference Set' but it won't let me select any components.
If I check the box 'Add Components Automatically' I get a message:
'This reference set excludes all components.
Do you want to add them back to the reference set?'
If I say Yes, all the components are added.
If I say No, no components are added.
I cannot just add the ones I want.
HELP

 

[cowski]

In the dialog box I click 'Add New Reference Set' but it won't let me select any components.

Make sure your selection filter is set to allow selection of components.

www.nxjournaling.com

 

[bbylls]

Boy do I feel stupid now.
Didn't think there would be a filter for that.
Thanks cowski.

 

[JohnRBaker]

The question still remains; Why are you wishing to add Components to a Reference Set? Why is it that you feel that you need to do so? What behavior are you attempting to gain access to? Generally speaking, we do NOT recommend that you include Components in a Reference Set except in very special and hopefully, rare cases.

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

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

 

[bbylls]

Then what is the point of Reference Sets?
I have 4 parts in an assembly that are identical except that 2 have a hole and 2 do not.
I made the one, then Insert>Associative Copy>Instance Geometry and then added the hole to the copy.
In the assembly I pick the ref. set for each.
How should this be done?

 

[scope63]

the reason why one would add components to a reference set would be to reduce what is visible when using the assembly for something else. if for example i am designing a fixture that uses the assembly of as example a water pump. i may be needing the components that define the outside of the pump and i don't care about the inner workings of the pump,i will create a reference set that contains the outer components only. i still call up the original assembly file but change the reference set to the one i create.

Scott Copeland

 

[looslib]

A little history on where reference sets came from may help.

Back in the old days of UG2, preV10, reference sets were used in component parts to filter out the miscellaneous objects of the data base so when you created a cube, you would only bring to your assembly the 12 lines used to represent the cube. At that time, the drawing was ususally done in the same file as the geometry so the reference set would exclude all drafting stuff. You would still need reference sets of assemblies to capture only the geometry for the next higher level.

Move up to V10+ with solids and you would have your skecth entities that would be excluded from the reference set. You only wanted the solid model in the ref set to move up to the assembly. Using a ref set at the assembly was considered not necessary with the drafting now in a separate file, if using the master model technique.

After about V16, the programmers got smart enough to leave the sketch geometry behind automatically when you used the 'entire part' ref set in your assembly. They also added an automatic MODEL (or was it SOLID, settable in customer defaults?) reference set to your files that contained the solid body when you created a part. It would update automatically as you worked on the solid.

That should help you understand where reference sets came froma nd their intended use. John will hopefully correct anything I have misstated and correct it. Since NX4, I am not sure what may have changed with the behavior of reference sets.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[JohnRBaker]

For what you're describing, you really should be using Arrangements. And in addition to content, you can also define Arrangement-specific positioning of Components, something that cannot be done using Reference Sets or at least not without starting to add multiple copies of the same Component to the overall Assembly. Where problems can occur is when the Component that you add to the Reference Set is an Assembly itself, particularly if there are sub-assemblies in it. Only the Components that you explicitly select will be included in the Reference Set but if later on some additional Components are added to one of those sub-Assemblies, they will not show-up at the level that that Reference Set is used when the Component was added to the top-level Assembly.

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

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

 

[bbylls]

OK.
The help files talk about arrangements to show parts in different positions in an assembly.
I have not seen where it talks about different configurations of the same part.
Guess I'll have to dig deeper.
Maybe I can find a video that John has made to show how this is done.

 

[JohnRBaker]

What you do is define your Arrangement(s) and then for the Components where you wish to control their presence, you simply Suppress them and you'll be given the opportunity, for each Arrangement in your Assembly, to define whether the selected Components are 'Always Suppressed' or 'Never Suppressed'.

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

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

 

[ewh]

John,
Would arrangements been part of an appropriate solution in thread561-389505 ?

"Know the rules well, so you can break them effectively."
-Dalai Lama XIV

 

[bbylls]

I can't figure it out.
I have an assembly.
In the assembly I have 2 end bars and 4 cross bars. The Assembly navigator looks like this:
+Assembly
End Bar
End Bar
Cross Bar
Cross Bar
Cross Bar
Cross Bar


The cross bar has 2 bodies in it.
One with a hole and one without the hole.
In the assembly I have 2 arrangements (with hole & without hole)
If 'with hole' is my working arrangement, how do I pick the bodies without the hole to be suppressed?
This where I get lost.

 

[cowski]

I made the one, then Insert>Associative Copy>Instance Geometry and then added the hole to the copy.

One solution: instead of creating a copy within your file, you could wave link the copy to a new file. This would leave you with two files (with hole and without). Since the files are separate, you would be able to suppress one or the other in a given arrangement.

www.nxjournaling.com

 

[JohnRBaker]

And if you're going to manufacture the cross bars, one with the extra holes and one without, you're probably going to want to give them different part numbers anyways just to track them and so that you the BOM is correct. And if you don't want to create two different part files from scratch or wish to avoid linking part files, you could simply create a single master Part Family template where one family member includes the holes and one does not. Even though you've only created a single part file, you can add either the 'with' or 'without' holes Components and then you'll have complete control over them when you define your Arrangements.

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

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

 

[bbylls]

Thanks all. Appreciate the help.

 

[Dave K]

@JohnRBaker I know you, and Siemens have always said that an assembly shouldn't have a reference set, only components, but regardless of where I have worked, and tried, we always end up making a model reference set in the assembly. Let me explain why, and maybe you can tell me what we have been doing wrong.

In our world, we have a "car coordinate system". When we build a car assembly, or a chassis assembly, we want to be able to refer to the car's absolute zero, so we put in a datum csys in the assembly file. The hub/spindle/wheel assembly has it's own coordinate system, so there is a datum csys in those assemblies. Now when we get to the top level assembly, if we didn't have the reference sets to filter out the datum csys from these sub assemblies, we would have them sprinkled around the car.

Second example, we have a few weldments where everything is modeled at the assembly level, then waved down into the individual component, so it gets it's own part number and drawing. At the assembly level, we remove all the construction geometry from the model reference set, and only have the components in it. I'm not a big fan of this, but in some cases it seems to be the best way. The alternative, when you skip creating the "seed" in assembly, and use wave links, it is easy to get circular references.

Then there always seems to be a reason to create some sort of geometry in an assembly...which I discourage, but it always seems to happen. Should we be looking at arrangements for more than alternate assembly setups?

-Dave

NX 9, Teamcenter 10

 

[JohnRBaker]

We only 'recommend' that you don't create Reference Sets in an Assembly. If we felt it was something that you should NEVER do, we would have had a very simple solution; we would simply remove the Reference Set function when you were working in a file that we detected was an Assembly (by looking to see if there were any Components in your file for example). NO, we're NOT saying that you should NEVER do this, just that if you do there are some behaviors, that in the past, has caused some users concern, such as not always being able to see the correct sub-assembly structure due to the fact that Components were added to the Sub-assembly's original part file but not subsequently added to the Reference Set(s) created there. Granted, before we had Arrangements, this was really the only practical scheme to create alternate configurations of a sub-assembly that could be added to a higher level assembly. However, now that we have Arrangements, 'most' of those previous situations where Reference Sets were the only option should be revisited.

Now as to your specific situation, there are options available including to simply Hide all the CSYS objects once your assembly has been created.

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

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