Reference sets
Reference sets
(OP)
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
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





RE: Reference sets
Make sure your selection filter is set to allow selection of components.
www.nxjournaling.com
RE: Reference sets
Didn't think there would be a filter for that.
Thanks cowski.
RE: Reference sets
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.
RE: 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?
RE: Reference sets
Scott Copeland
RE: Reference sets
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
RE: Reference sets
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.
RE: Reference sets
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.
RE: Reference sets
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.
RE: Reference sets
Would arrangements been part of an appropriate solution in thread561-389505: Large Assembly Model Management in NX ?
"Know the rules well, so you can break them effectively."
-Dalai Lama XIV
RE: Reference sets
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.
RE: Reference sets
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
RE: Reference sets
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.
RE: Reference sets
RE: Reference sets
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
RE: Reference sets
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.