what controls the exitance of edge in drafting view?

[uwam2ie]

I have a question what is be the reason that an edge is not shown in a drafting view in standard creation without any edits. I 've attached an example pic. An inversely geometrie on one side wrong on the other side its ok.
what can be done / any ideas?(Nx5.06)

 

[JohnRBaker]

There are many factors which could effect this including the display tolerance used on the drawing.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

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

 

[jerry1423]

Double click on the view on the drawing and under the "general" tab open up the tolerance.
You will probably not notice a difference after opening up the tolerance.

 

[uwam2ie]

... display tolerance
are there any defaults related to view or displayed body size.
tipps and tricks workarounds?
thx in ad

 

[cowski]

If it is an assembly of parts, make sure they are not interfering. Interference can lead to strange results on a drawing.

If it is a single part, analyze the geometry. If your model has self intersecting faces, spikes, cuts, etc. it can also lead to strange results on the drawing.

 

[hudson888]

As others have posted you'll possibly be able to remedy the problem by changing the setting under view style. I'd be looking at the tolerances to some extent and also the hidden line display settings. Perhaps by turning off hidden line then turning it on by adding one setting at a time you may hit on a combination that solves your problem.

This kind of behaviour is quite rare so you shouldn't have to deal with it often. It quite often relates to the geometry that you're placing on the view and on a few very rare occasions I have discovered something about the geometry that once remedied corrects the view display problem. In that vein you might try running examine geometry on the model if all else fails and look for tolerance errors of larger and expected magnitude.

Cheers

Hudson

 

[cowski]

I mentioned the 'examine geometry' option because the area in question appears to be a blend (hard to tell from only the picture given). If it is indeed a blend, the blend edges on the right side form an 'X' pattern (a bad sign). I would guess the blends on both sides of the centerline are bad geometry but for some reason one rendered acceptably and the other one did not.

 

[jerry1423]

If a blend is the problem then go into that feature and increase the tolerance on it.

 

[hudson888]

jerry1423,

I would have guessed a tighter tolerance may be required, have you experience to the contrary. I know only of cases where removing and reapplying small blends seemed to do the trick.

Cheers

Hudson

 

[jerry1423]

Not tighter, but looser tolerance (yes, I see that I did not word that properly)

I discovered that when I was working on a very complex casting more than a year ago. There was one place on it where the blend did not show up properly, after I made the tolerance bigger it showed up fine.

Usually I would fix something like that with view dependent editing but for some reason it did not work well that time.

 

[uwam2ie]

... what help in this case was:
go to view style (of this view)to the section tab turn off background apply, turn on background ok - everything is ok.
no tolerances was changed- strange -Why did a manualy forced view update not the same job ( recreating the view)
thx to all