Bodies created with sewn sheets, unable to Unite
Bodies created with sewn sheets, unable to Unite
(OP)
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.
"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.





RE: Bodies created with sewn sheets, unable to Unite
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
RE: Bodies created with sewn sheets, unable to Unite
RE: Bodies created with sewn sheets, unable to Unite
I wouldn't get GTAC involved until you are sure you have valid geometry.
www.nxjournaling.com
RE: Bodies created with sewn sheets, unable to Unite
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.
RE: Bodies created with sewn sheets, unable to Unite
File -> Export -> Heal Geometry...
...utility.
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RE: Bodies created with sewn sheets, unable to Unite
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
RE: Bodies created with sewn sheets, unable to Unite
However when I ensured that there were no tangent surfaces, though tangent edges still exist, it did work.
Thanks for everyone's help.
RE: Bodies created with sewn sheets, unable to Unite
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