NX10 Flat Solid In Drawing

[jerry1423]

I am using master model for this, so the drawing and model files are separate, and it is in Teamcenter.
What I have is not actually a sheet metal part, but it is a flat rubber piece that gets attached to a curved surface, and using the sheet metal package worked very nicely for this application.
I cannot have the flat solid in the model file because it doubles the part weight in Teamcenter.
In the model space of my drawing file I wave linked the solid body, converted to sheet metal, and created a flat solid, which worked well.

I cannot figure out how to get the flat solid to appear in my drawing. All my layers are visible and selectable.
I know I had this problem several years ago, but I cannot figure out how it was solved.

Jerry J.
UGV5-NX11

 

[cowski]

When you place a base view, make sure the "part" selected is your drawing file. In NX 10, when you use the master model method, it automatically chooses the master part, which is not what you want in this case.

www.nxjournaling.com

 

[jerry1423]

Thank you very much.
I did not realize there is a View Creation Wizard, which is made for something like this.

Jerry J.
UGV5-NX11

 

[thomaskoer]

Hi

I cannot have the flat solid in the model file because it doubles the part weight in Teamcenter.

You should put the FS Body on an other layer and work with reference sets.
When you do so, the Solid of the Bent Part has the right weight, e.g. in refset "Model". The FS is then in Reference Set "Flat_Solid". It's at least in NX 12. We work like that - also in managed mode with TC. The Reference Set "Flat_Solid" is available out of the box.

Edit: Take care that you use the RefSet "Entire Part" for the part in the Drawing. If you don't do it and you have only "Model", then you can Change "Layer Visible in View" and you will not see the Flat Solid...

Thomas