"Solid Body" becoming "Faceted Body" in assemblies? 2

[tdp240]

I don't know if this is a glitch or something I can fix easily with a settings change.

Whenever I create a new assembly for the first time (usually small assemblies, 2-3 components), and I go to create a step file (by "Selected Objects", not "Entire Part") I can export all of the components as solid bodies with no problems. However, after saving the file and closing it, the next time I open it up (loading all components fully), it changes the components from "Solid Bodies" to "Faceted Bodies", and thus I am unable to export a step file as solids. The only way I've been able to do this is to delete the components and bring them into the assembly as new components, and that is very frustrating to have to do every time when the change is minor.

This also affects my assembly drawings. The views in drafting don't update properly.

Any thoughts?

 

[cowski]

What reference set is being used for the components after you reopen the assembly? (right click on the component in the assembly navigator and choose replace reference set - the current will be gray, available options will be black).

My guess is that when you reopen the assembly, the system is defaulting to a lightweight reference set.

 

[looslib]

Set your system preferences to always use the SOLID default reference set when adding a component to an assembly.
Also, set the preference to use the SOLID reference set when opening an assembly.
For mating anthings, switch to entire part or another reference set, then switch back to SOLID before saving the file.


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

Ben Loosli

 

[tdp240]

Thanks, cowski and looslib. I was able to change the reference set from "REP" to "Entire Part" by right clicking on the components in the assembly navigator, and that worked.

I couldn't find how to change the default in the Customer Defaults, but I don't work with assemblies that often, so having to replace the reference set each time isn't too bad. It's much better than the way I was doing it, replacing the components each time!

Thanks again.

tedepe
NX5.0.4.1

 

[CEGraves]

File-Options_Assembly Load Options:

Move Entire Part above Rep or Facet Reference Set, then Save as Default.

C. Graves
Gehl Company
www.gehl.com

 

[tdp240]

Thanks CEGraves. I guess I was looking in the wrong spot altogether.

 

[hudson888]

Since you're obviously new to NX you may now have the correct answers but I'll add something to the above that may help you better to find what you're looking for. You should always let us know what version you're using by the way. The out of the Box installations of NX-5 and NX-6 will save parts with two reference sets called MODEL and FACET. Older versions or customer preferences will call the MODEL reference set SOLID or PART on occasions and the FACET was often called REP. Obviously the FACET reference set contains faceted representations and the MODEL on contains solids and the occasional sheet body.

So if you go into File>Options>Load Options you can control which reference sets are loaded when you open an assembly as CEGraves above showed. Most people stick with "As Saved" for much if the time. Depending on what your reference sets are called and which you prefer then for large assemblies may people load FACET by default to avoid using all of their memory. Similarly they may not automatically open all components and they'll turn ON "Partial Loading". These settings can all be set before you open an assembly on a session by session basis or saved as your defaults. The important thing to know is that the purpose of the faceted representations is to speed graphics display and save memory when working with larger assemblies and users are advised to know a little about strategies for their use in order to be more effective.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[tdp240]

I've actually been using NX for about 8 years now (7+ years of NX3 and a couple of months in NX5). I was in my comfort zone for all those years in NX3 and had all of my settings just the way I liked them, so most of my questions lately have been little quirks or default settings that changed when I migrated to NX5 and I've had to figure out how to get them back to the way I like them.

In NX3, we always had the defaults set to open all components fully because we only work with assemblies about 5-10% of the time, and when we do work with assemblies, they are very small in size (2-3 components usually, rarely more), so memory is not an issue for us.

Sorry about not posting my version of NX in my first post. I meant to, but forgot, so I posted it in my second post (see above).

 

[Xwheelguy]

tedepe,

I'd suggest doing some searching on here or on bbsnotes about running a customized environment. Once you get that all set up and working, upgrades/migrations are much easier (IMO) to handle unless Siemens makes a major change to any of those defaults files.

You can specify a unique location/folder for all of your startup and environment files (different than that of the base install), then when you migrate or upgrade, you just need to either copy everything and do some minor edits or you can set the correct paths to the location of the customizations.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

Some people are like slinkies....they don't really have a purpose, but they still bring a smile to your face when you push them down the stairs.