Model is not translating in drawing

[Jashe]

I'm having trouble with a part when I bring it in to a drawing it isn't coming out very well. I've attached a screen shot of a close of of an edge of this part and it's all broken up at the corner as well as other features. Also, I can't seem to grab edges to create intersections. Anybody know whats going on here. This is NX 8.5.

 

[JohnRBaker]

Try selecting the view, pressing MB3 and selecting the 'Style' button. Go to the 'General' tab and if the 'View Configuration' 'Representation' is set to 'Lightweight', change it to 'Exact'.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[Jashe]

It's not highlighted so the dropdown menu isn't active but it is set to 'Exact'. I've attached the drawing I'm working with here. I really want to know what is going on here.

 

[cowski]

Unfortunately, the drawing file by itself isn't much use for troubleshooting this issue.

I'd suggest opening the model file and running the 'examine geometry' command. Turn on all the body and face checks, window select around your entire model when doing the selection step - this will select the solid body along with all faces and edges (if you select by just clicking on the body, only the body will be selected). Errors in the model geometry may lead to strange errors/anomalies in the drawing views.

www.nxjournaling.com

 

[SDETERS]

have you tried doudble clicking the border and change your view toleralnce? we have this issue a couple time it gets set to .010 and we go in and set it to .0003. I do not know if this option is available in NX8.5

 

[Jashe]

SDETERS: That option is available in 8.5 and it worked! thank you.
cowski: I used that 'examine geometry' command and it is a good tool to use. Thanks. I'm going to be using that alot more in my modeling.