does anybody know why NX often makes mistakes in the display of views of body edges?
we have played with many settings but there seems to be no way to make NX to draw complete body edge lines in some views. Please see the pictures I've added.
Many thanks for your help
Right click on the view border, go to Settings, under Configurations there is a tolerance setting.
Increase the tolerance and the lines in the view may show up. The tolerance is usually small, increase it to
0.1 to 0.15 and see it the lines appear.
Check if 'Show Silhouettes' option is toggled on in that particular view settings.
It can also be set under the drafting preferences.
Is the graphics card/PC on the certified list?
Is the graphics card driver the certified version (or later)?
Production: NX10.0.3.5 MP16/TC11.2
I'd rather be e-steamed than e-diseaseled
In addition to the above possibilities, I'd suggest switching to the model and running a geometry check (analysis -> examine geometry -> window select around the entire model to pick up the solid, all faces, and all edges). I have seen cases where corrupt geometry leads to display issues in the model and/or drawing. The following checks are most important to pass:
Also, is this a drawing of an assembly (it is difficult to tell from the screenshots)? If so, is there interference between any of the components? Weird things can happen to drawing views if there is interference. Note that there are options in the NX drafting preferences to help account for and correct these anomolies.
many thanks for your reply.
I just want to give the info that there was a collision between two bodies. We modelled a thin layer on the body that was meant for showing some decoration (paint). When I removed the collision the views in the drawing looked ok.
But on an other part there is no collision and there still are some lines missing in some views.