Consistency in "Examine Geometry" NX8.5

[jerry1423]

When I have faces that do not pass the Consistency criteria in Examine Geometry,
What am I being told is wrong with those faces?

 

[JohnRBaker]

To see a description of exactly what constitutes an 'inconsistency', when you have the 'Examine Geometry' dialog open, press the 'F1' button to bring up the context-specific Help for the current function, in this case, 'Examine Geometry'. On the right side of the Help page you'll find some links to some addition Help pages. Select the one titled 'Examine Geometry related topics'. There you will find a more detailed description of each of the various issues that 'Examine Geometry' might indicate as there being a problem.

Now I suspect that even after you've read the rather detailed explanation of what sorts of 'consistency' issues the software is looking for, that this may not help you all that much since even if you knew exactly what was causing 'consistency' warning, on what I assume is one of your models, there is very little that you can do.

That being said, first a couple of questions:

What is it that happened that led to you even running 'Examine Geometry' in the first place? Did you have problems with model when performing some task or operation? Or did something just not look right? Or is this just part of your normal workflow, running 'Examine Geometry' on all of your models, whether there are any apparent problems or not?

Is the model-of-interest something that you modeled yourself or was it imported from some other system via some sort of neutral translation code, like STEP or IGES?

If it's not an imported model, what version of NX was the model created in? NX 8.5 or a much older version?

Is the model feature-based or is it a so-called 'dumb' model with no features or parameters, which would be the case if it were an imported model?

As for what you might try, there are a couple of things that might help.

First, if it's an imported model, you could go to...

File -> Export -> Heal Geometry...

...where NX will create a duplicate Part file after it has attempted to 'clean-up' the model, correcting/removing poor topology. The resulting model will have no feature or parameters, but if the original model was imported, then you've not really lost anything. Now run 'Examine Geometry' on the newly created Part model to see if the inconsistencies have been dealt with.

However if the model is feature-based and you would like to keep as much of this structure as possible, and particularly if the model was created in a much older version of NX, you might try this: With the model open, go to...

Edit -> Feature -> Playback...

...and select the 'Continue' icon (it looks like the a VCR 'Play' button). This will, on occasion, cause the model to sort of fix itself during playback. It's a long-shot but you've nothing to lose. If it makes it all the way through the playback with no error messages, try running 'Examine Geometry' again to see if that fixed the model. If so, save your part and consider yourself lucky.

Now if none of these suggestions worked, you only alternative is to call GTAC and have them look at you model. We have better tools for looking at and repairing model so it's possible that we could resolve these consistency issues for you.

Anyway, I hope this helps.

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

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

 

[cowski]

Now if none of these suggestions worked, you only alternative is to call GTAC and have them look at you model.

If you are working with a native, history-based file, I wouldn't give up on it so soon; I've seen a lot of bad parts, and they usually are not that difficult to fix. Nine times out of ten, the problem will be caused by a blend or a freeform feature. Recent versions of NX have improved in the blending department; it does a much better job these days of telling you when and why a blend can't be applied. If it is a freeform feature, take a good look at the input curves. They may have sharp 'hooks' on the end, self-intersections, or small segments of high curvature; any of these can cause problems. Sometimes NX will build the sheet body even though the geometry is no good and the problem doesn't manifest itself until later operations (such as when performing a boolean and you get the "through face does not intersect" error when the target and tool obviously intersect).

The first order of business is to find where the bad geometry crept in. I posted a journal a while back that helps with this task.
thread561-336862
When you run the journal, it will roll back the modeling history to the last place where the model passed the checks. The next few features are a great place to start looking for the bad geometry.

www.nxjournaling.com