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Missing body lines in the drawings

Valued Contributor
Valued Contributor

Hello community,

 

 

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

 

6 REPLIES

Re: Missing body lines in the drawings

Experimenter
Experimenter

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.

Re: Missing body lines in the drawings

Siemens Phenom Siemens Phenom
Siemens Phenom

Check if 'Show Silhouettes' option is toggled on in that particular view settings.

 

sil.PNG

 

It can also be set under the drafting preferences.

 

sil1.PNG

 

Regards,
Ganesh

Re: Missing body lines in the drawings

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

Is the graphics card/PC on the certified list?

Is the graphics card driver the certified version (or later)?

Ken Akerboom Sr CAx Systems Engr, Moog, Inc.
Production: NX10.0.3.5 MP16/TC11.2
I'd rather be e-steamed than e-diseaseled


Re: Missing body lines in the drawings

Gears Honored Contributor Gears Honored Contributor
Gears Honored Contributor

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:

Body checks:

  • data structures
  • consistency
  • face intersections

Face checks:

  • self-intersection

 

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.

Re: Missing body lines in the drawings

Valued Contributor
Valued Contributor

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.

Re: Missing body lines in the drawings

Siemens Legend Siemens Legend
Siemens Legend
Try this when you see missing lines.
The view tolerance was mentioned above,
use this trick instead of entering any values, Zoom the view to a suitable scale on the screen. keep in mind that zooming absurd scales is not what will be seen if printed, a 0.1 mm missing segment will be very visible when zooming in NX but not if printed. delete the value in the tolerance field. Press Apply or OK.
Most probably the missing lines will be corrected. Note that the value in the tolerance field is depending on the zoom factor.

Regards,
Tomas