Analyze Complex Sew Surface for Open Edges/Holes

[ChaseWichert]

NX7.5

Is there some sort of analysis that I can do to a body to find out what edges are causing my sew to not create a solid body? I have looked the model over several times, and have found two openings, but it still isn't creating a solid body, so I believe there are more, just maybe too small for me to see.

Thanks,
Chase

 

[JohnRBaker]

Yes, go to...

Analysis -> Examine Geometry...

...and set at least the 'Sheet Boundaries' check, select all the bodies and push the 'Examine Geometry' button at the bottom of the dialog. You will see the open edges highlighted after you toggle ON the 'Highlight Results' item.

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

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

 

[ChaseWichert]

Hah, thanks! I just found it like 30 seconds ago!

 

[ChaseWichert]

However, I fixed the highlighted problems, nothing comes up to highlight, but it still isn't a solid body...

 

[JohnRBaker]

Do the sheets completely enclose a volume? If so check to make sure that in the Settings section of the Sew dialog that the 'Output Multiple Sheets' is NOT toggled ON. If it is, toggle it OFF and try again.

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

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

 

[ChaseWichert]

I am attempting to make the sheets completely enclose a volume. And the toggle is off

 

[jerry1423]

Maybe try what Cowski suggests in this post.

http://www.eng-tips.com/viewthread.cfm?qid=323933

 

[ChaseWichert]

Yeah I figured it out for real this time.. it came down to missing a few extract surfaces at first, then the second problem was that i was trying to make a bounded plane surface using surfaces that had been mirror to create a cap, but the trim plane that made the cap edges wasn't perfectly perpendicular to the mirror plane. If that makes any sense. Whew, 3 hours later.

Anybody know why when I scale down some solids, surfaces go missing? This is the cause of the problem I am having.

 

[jerry1423]

Sometimes when scaling, the radius of the arc'd surface gets to zero or a negative number.

 

[ChaseWichert]

Normally in other software packages that creates an error. On several occasions when I scaled something down I have sent out models with missing surfaces, because there is no error provided. Is there a reason for this?

 

[jerry1423]

It wasn't that long ago that NX would not process the scaling if the radius got to less than zero, so it is a relativly new thing here.
I have never gotten any missing surfaces, like you have, so I am not sure why that happens.
I guess it would be nice to get some sort of warning when a zero (or less) radius surface falls off.

 

[ChaseWichert]

Yeah it is really weird, I don't see how it could go to zero if it is a scale, however I don't know how the programming actually scales. But it does have something to do with radii. I have to go to the full scale part, delete one radius at a time, until I figure out which the culprit was. This part is different in the fact that it really didn't have any small radii near it, it was basically a cylinder that disappeared and a flat surface. But yes, an error when surface fail to be created would be great. The weird thing is that it still sees it as a solid body. I have tried exporting the body into several different formats to see if it is just a graphical error, but when I import them back in the surfaces are still gone.

 

[JohnRBaker]

If you scale the model down to the point where the width of a face is less than the modeling tolerance the opposing edges will be merged together as if the face was never there. But before you get to that point you may end up with a model which could prove to be problematic due to these small faces, therefore at some point you may wish to 'fix-up' your model using the...

File -> Export -> Heal Geometry...

...utility which will remove small faces, clean-up segmented edges, etc.

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

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

 

[ChaseWichert]

Thats what I used before! I couldn't remember what steps I took to fix the problem.. Although I don't think it fixed every model, just some of them. I will keep that in mind for next time.

Thanks.