hollow a swept solid
hollow a swept solid
(OP)
I am running into a problem when trying to hollow a swept feature. I have basically created a swept feature using a guide string and two end profiles. I want to hollow out the feature, creating a sort of fancy "pipe" (ie pierce 2 end faces and offset the sides). UG NX3 thinks for a while and then says "Cannot Apply Hollow".
Any suggestions? I appreciate it!
Any suggestions? I appreciate it!





RE: hollow a swept solid
RE: hollow a swept solid
RE: hollow a swept solid
RE: hollow a swept solid
RE: hollow a swept solid
If the geometry is ok, but won't offset then that means that the offset (or hollow) operation would cause something to become invalid. In that case you probably need to tweak the original swept geometry.
Hope this helps.
RE: hollow a swept solid
One more thing. My section profiles are rectangular. I've noticed in playing around with a couple simple examples (trying to understand why I'm running into problems) that offsetting of rectangular sweeps seem to magnify surface irregularities. This doesn't seem to be an issue with smooth circular swept features...
RE: hollow a swept solid
If you do Information -> Object (face subtype) and mouse over your solid, you probably won't see what you expect to. It is my experience that a rectangle will end up with 2 faces around the perimeter rather than the expected 4. Two 'corners' get converted to a very small radii which makes it nearly impossible to offset.
If your section stays constant along the guide you might try the 'sweep along guide' feature (not the freeform 'swept' feature), it doesn't take as many liberties with your input geometry. If you need the power of the freeform 'swept' feature (it can cause headaches but it really is a powerful command), you might try blending the corners of your section geometry by at least the value that you plan to offset the surface.
RE: hollow a swept solid
Couple more details: My part is very large (ie XS area = 7m^2). W/the default hollow tol. value of .0254, I had weird "bubbly" surfaces on part of the model. Tightening the tol. to .00254 seemed to correct this.
I'm going to try blending the corners like cowski suggests. (I need to use the "Swept" feature, because the cross sectional area changes over the length)
Thanks for all the replies
RE: hollow a swept solid
RE: hollow a swept solid
I did find that another alternative is to create 2 sets of profiles; representing the inside and outside of the tube. Then "Swept" both of these, and do a Boolean "Subtract" operation to effect the hollow. All these procedures are compute-intensive though, and take a long time to refresh...
RE: hollow a swept solid
RE: hollow a swept solid
that last tip - setting the "SWEPT" dialog tolerance value to "0" works!
Also, it works quickly, without too much CPU time to compute.
THANK YOU very much. A star for you!
RE: hollow a swept solid
The most important thing to try to do though is keep your section strings consistent from end to end. Think about what the software is trying to do when it's making that sweep. It's trying to transition from one section to the next and needs good definition to do so. Try to maintain the same number of points, lines, etc. whenever possible to make it easier for the software to determine the path of least resistance. The best example of this is sweeping a rectangular section to a circular section. If you try to do it just by drawing a box at one end and then a circle at the other it won't work. But if you break the circle up into 4 segments corresponding to the sides of the box and select start points that relate to one another it will do the sweep just fine. All it needed was some help determining what points to use.
Take care....