Hiding solids in drawing views

[Raddy13]

I'm working on a machining drawing for a component that has a lot of linked bodies and faces in it in NX-8. When I create a base view, it has all the reference bodies and such in it, and I can't figure out how to remove them. I tried "View Dependent Edit," but it wouldn't allow me to select a solid body to erase, even with the selection filter set to solid bodies only.

I've seen people ask similar questions, and the solution recommended was to change reference sets or hide layers. I don't have the option to change reference sets on my drawing (or if I do, I can't seem to find it) and even though hiding layers in the modeling view produces the solid I want, when hiding layers in the drafting view doesn't seem to hide anything at all.

Any help is appreciated, thanks!

 

[SDETERS]

You need to change the reference set in the machine 3D model not the drawing. Open the 3D model. Go to show/hide and do a show all. Then go to format reference sets. Then Hold down shift and deselect the bodies you do not want to see in the drawing. This assume you are using the Default model reference sets in your drawing.

 

[cowski]

Is the drawing in the same file as the model or are they separate files (master model method)?

If the drawing is in the same file as the model, reference sets will do you no good; you will have to use "layer visible in view" or view dependent edits.

The preferred method is to use separate files for model and drawing. Then in the model file you can specify what is in the reference set, and in the drawing file you can specify which reference set to use.

www.nxjournaling.com

 

[Raddy13]

Got it, thank you!

 

[Raddy13]

Sorry Cowski, I didn't see your post. How do you separate the drawing from the model file? I see in the "new part" dialog, I can create a drawing and reference an existing part file, but I still don't have the option to change the reference sets.

I solved my first problem, but understanding this method might help me solve a new problem. Thanks!

 

[ewh]

You create the model and reference sets in one file, then bring that file into a drawing file as a component. In the drawing file you can specify which reference set you want to see. It is called the "master model" method and is usually the preferred method.

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

 

[cowski]

If you do as ewh suggests, right click on your component (the model) in the drawing assembly navigator and choose "reference set" in the pop up menu.

www.nxjournaling.com

 

[Raddy13]

Got it, thank you again!