"Solid Body" becoming "Faceted Body" in assemblies?
"Solid Body" becoming "Faceted Body" in assemblies?
(OP)
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?
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?





RE: "Solid Body" becoming "Faceted Body" in assemblies?
My guess is that when you reopen the assembly, the system is defaulting to a lightweight reference set.
RE: "Solid Body" becoming "Faceted Body" in assemblies?
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
RE: "Solid Body" becoming "Faceted Body" in assemblies?
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
RE: "Solid Body" becoming "Faceted Body" in assemblies?
Move Entire Part above Rep or Facet Reference Set, then Save as Default.
C. Graves
Gehl Company
www.gehl.com
RE: "Solid Body" becoming "Faceted Body" in assemblies?
RE: "Solid Body" becoming "Faceted Body" in assemblies?
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
RE: "Solid Body" becoming "Faceted Body" in assemblies?
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).
RE: "Solid Body" becoming "Faceted Body" in assemblies?
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.
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.