Missing Parts in an Assembly

[wjlaughlin]

I am currently working on an assembly, and we use the master model concept here. Keeping the drawing seperate from the model.
I took my master model and made it the solid refrence set, and created my drawing part and imported the master model in and it is missing a couple of pieces. Actually the odd thing is that they are still listed in the assemlbly navigator but arent visible in modeling, or drafting.
Any clues as to why this might be.

Thanks in advance

 

[ewh]

Is your master model and all of its components open? If not, check your load options.

 

[looslib]

If they are sub-assemblies be sure that the components are turned on in the sub-assembly AND that all components are included in the proper reference set.

Related question, why are you using reference sets for assemblies when using the master-model paradigm? UG has stated that reference sets are no longer needed since they filter out the pieces of the sub-assembly that you don't need at the assembly level.

"Wildfires are dangerous, hard to control, and economically catastrophic."
"Fixed in the next release" should replace "Product First" as the PTC slogan.

Ben Loosli
CAD/CAM System Analyst
Ingersoll-Rand

 

[Shadowspawn]

Looslib,
Ok, apparently I'm missing something... What do you mean by 'reference sets are no longer needed...'? I'm not sure that I'm following you, are you saying that the preferred method (according to UGS) for building assembly structures doesn't include the use of reference sets? If so, endlighten me, please...

 

[looslib]

Reference sets were designed to filter out extraneous information when putting a component into an assembly. UG now does the filtering if you use the master model of drawings in a separate file from the model.

Also, they are hard to maintain at the assembly level as you add and remove components.

Check out the CAD or Assembly forum on the internal bbsnotes system and search for reference sets.

Okay, I just did some checking. The reference set not being needed is in relation to assembly files that only have pointers to files with real geometry. John Baker doesn't use reference sets except in files that have real geometry.


"Wildfires are dangerous, hard to control, and economically catastrophic."
"Fixed in the next release" should replace "Product First" as the PTC slogan.

Ben Loosli
CAD/CAM System Analyst
Ingersoll-Rand

 

[looslib]

This is taken from the Assemblies forum in the UG bbsnotes system. Written at the time of V16 release.

If you're setting up best practices, we (the assemblies development team) would recommend the following:

- Use reference sets only for controlling how the component is represented - solid, faceted representation, entire part, empty. Set up standard names for the solid/facet reference sets and use them consistently. "MODEL" or "SOLID" and "FACET" are the usual ones. Do not use reference sets for containing variants of individual parts etc. (use part families or a WAVE based solution - i.e. have a different part file for each variant).

- Put the name of the solid reference set into your unigraphics defaults file - there is a setting called "Assemblies_ModelReferenceSet", I believe. This is used in v15 (for storing bounding boxes for components which only include the solid geometry) and more in v16 (we will generate a facet reference set equivalent to the solid reference set automatically) and will be used even more in v17.

- Don't create reference sets in subassemblies. When loading the assembly, use the "load options" reference set preferences to control which reference sets load. Subassembly reference sets are very hard to manage in modern, large assemblies.


"Wildfires are dangerous, hard to control, and economically catastrophic."
"Fixed in the next release" should replace "Product First" as the PTC slogan.

Ben Loosli
CAD/CAM System Analyst
Ingersoll-Rand

 

[jiabao]

Internal Error

When i open a part file it is visible in preview but once i click the open button there is a dialog box appear and states that internal error. Before i can open it but now can't. I am using UGNX3, Please help me how to rettrieve my part files.


Many Thanks,

Jiabao