Bodies created with sewn sheets, unable to Unite 1

[Twullf]

I have very complex geometries, the only way I have successfully managed to create the solid is to use spline and creating a Sheet using the "Through Curve Mesh" Tool. I then use Sew to create the solid bodies, but the final step of uniting the features together always gives me the error:

"Thru face does not intersect path of too", when cross-sectional analyses shows consistent and very clear intersection.

Has anyone else had any trouble with this, any help would be appreciated, it is a common problem at this point and though I'm sure if I export the bodies as parasolid and import them as mere bodies it will work, but I still want to be able to edit these features later if we do decide to change something.

Thanks for any help available.

 

[Xwheelguy]

Without having the part on hand, the responses could be limitless. Have you tried Sewing the solids together? I'm guessing that to get to the bottom of the issue, if your solids are absolutely intersecting without doubt, and you're sure you've created a decent freeform surface and your Sew tolerances aren't moving all over the place, you'll probably have to contact GTAC and send the part to them to have a look. Try your theory about the Parasolid and see if that works - also try a Heal Geometry export as well - it also might be that the TCM could be improved in order to get face intersections that NX prefers.

NX version is always helpful to some folks when asking for help or reporting a possible bug.

Tim Flater
NX Designer
NX 7.5.4.4 MP2
WinXP Pro x64 SP2
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB

 

[mmauldin]

I run into this from time to time. Typically there is a situation where the surface of the tool body is tangent to the target body creating a "zero" condition that seems to give NX problems. My general work around is to offset the surface of the tool solid by .0001 to .0002. This will generally fix the problem.

 

[cowski]

Start by examining the quality of your geometry (Analysis -> Examine geometry). The bodies you are uniting must pass all the body checks and all the face checks (the object and edge checks are less important). Attached is an article from GTAC explaining the use of the examine geometry tool (it references an older version of NX, but the process is still the same).

I wouldn't get GTAC involved until you are sure you have valid geometry.

www.nxjournaling.com

 

[Twullf]

I'm trying the Examine Geometry, and the Body passes, but the Face Checks get No Results, If I just choose a face then the Face Checks Pass and the Body Checks get No Result.

As for the edges being tangent that is a valid possibility as I use some of the same splines for both bodies. I'll try modifying that and see what happens.

 

[JohnRBaker]

You can also try repairing the model by using the...

File -> Export -> Heal Geometry...

...utility.

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.

 

[cowski]

I'm trying the Examine Geometry, and the Body passes, but the Face Checks get No Results, If I just choose a face then the Face Checks Pass and the Body Checks get No Result.

Use select all or window select around the body you are interested in (using no selection filter); that way you will be selecting the body, all faces, and all edges.

www.nxjournaling.com

 

[Twullf]

After heal geometry I am still experiencing the same problem.

However when I ensured that there were no tangent surfaces, though tangent edges still exist, it did work.

Thanks for everyone's help.

 

[Xwheelguy]

Twullf,

If you're going to be doing Booleans (Unite, Subtract, Intersect, etc.) or a few other commands (Patch, Trim Body - although NX isn't as picky with these as the Booleans), it's generally good practice to avoid touching face to face (basically, tangent) if at all possible. This creates what is often called a Non-Manifold condition and the results you had are common when that occurs.

Go all the way through the outermost faces/surfaces, even if it seems like overkill - this is also good practice when working with surfaces/sheets which you intend to trim to one another at a later point in time. Basically try to avoid situations where you're looking at face to face and edge to edge conditions. This doesn't apply 100% of the time, but when tolerance starts getting introduced, you can paint yourself into a corner quite easily.

Tim Flater
NX Designer
NX 7.5.4.4 MP2
WinXP Pro x64 SP2
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB