How to repair bodies

[slayer001]

Hi people!


I'm working in a model in NX6 and I noticed that my model is somewhat 'broken'.

The problem is: I'm having trouble trying to make an edge blend and I noticed that one of the arcs is formed by two curves instead of one. And sometimes when I try to make the blend, the software doesn't pop any warnings, so I apply and a sheet seems to be gone.

So, I ask for your help to know if there is some way to 'repair' these.

I hope the images explain better what my problem is.

 

[slayer001]

Here is another image

 

[JohnRBaker]

If retaining your parametrics (features) is not an issue you could try...

File -> Export -> Heal Geometry...

...which will attempt to repair small discontinuities and flaws in your model, but it will produce a non-parametric copy of your original model (which will be left as it is).

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
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.

 

[slayer001]

Thank you John, but all the parameters are important for my model.

I'll keep trying to blend with variable radius.

Thanks anyway

 

[jerry1423]

maybe open up the tolerance on your variable radius, you may get better results

 

[Xwheelguy]

I have seen in rare cases in the past where a face exists but NX will just not display it in shaded mode. It's there, it's just never shaded. Hover your mouse over the hole and if you have preselection highlighting turned on and see if the face edges highlight. If this happens, then I wouldn't worry too much about it. Just a display anomoly.

Tim Flater
Senior Designer

 

[cowski]

You should also run the 'examine geometry' tool (in the analysis menu) to see if it reports any problems. Specifically check for consistency or data structure errors.

 

[DaSalo]

If consistency errors are detected what does this mean? How does one interpret the results when highlight areas is selected?

Just yesterday I was helping with a model that had a visible jagged tear near the intersection of two faces when viewed in shaded mode. When switched to static wireframe there was no evidence of this issue and the two faces looked like they intersected cleanly. The internal surfaces of this torn region do not register as faces, i.e. they are not selectable individually. We ran examine geometry and everything passed except "Consistency". We then selected the "highlight areas" option and the intersection in question was highlighted, not just the one problem area but the entire length of the intersection between those two faces. It also displayed a rectangular wire frame box off at an angle to the face intersection. Not sure where to go from there. We know there is a problem but now what?

 

[DaSalo]

Sorry, a bit more information needed with my previous post:

The model mentioned previously is in NX6 but we could bring it into NX7.5 if there are any new tools available there for correcting issues like this. We don't care about the parameters so will try Heal Geometry to see if that helps. I am more interested in understanding what a "consistency" error is, what causes them, and how to interpret the information provided by the analysis tools.

Thanks in advance...

 

[JohnRBaker]

Consistency generally means that there is some sort issue with the topology of the model. You could try perfroming a Part Cleanup.

As for the 'torn surface' what you were seeing is actually the tessellation of the surface needed to render the shaded image. Sometimes playing back the model features will help this. Other times it might help to change the display tolerance. Also you may wish to reset the front and back clipping planes, as well as toggeling ON or OFF perspective viewing.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
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.

 

[cowski]

The important thing is to have a method to find and fix the problem feature(s). I use a technique similar to a root finding algorithm known as 'bisection'.

Run geometry check
if part fails geometry check then
  suppress 1/2 of features and run check again
else
  unsupress 1/2 of suppressed features and run check again
end if
Loop until part passes with all features unsuppressed

Let's assume you have a model with 128 features and unknown to you, #82 is causing a problem. You run the check and it fails, suppress back to #64 and it passes, unsuppress to #96 and it fails, suppress to #80 and it passes, at this point you know the error is somewhere between #80 and #96 (a window of 16 features). You can investigate these features one by one or you can try another iteration or 2 to narrow it down further.

It is a bit tedious, but even with a large model you will quickly zero in on the problem. There are numerous ways to introduce problems into parts so there will be some investigation necessary once the problem feature is found. A couple common causes I have seen are non-planar geometry that looks OK when you extrude/revolve/sweep it but leads to problems down the road and sheet bodies with kinks in them that are subsequently used in a sew or trim operation.