shell on swept solid does not work as intended 2

[meCAD2]

I am using NX 2206. I have a very simple model that demonstrates a problem I see when applying a shell to a swept solid. If the scale curve is vertical, I get a tall extruded square that is properly shelled out. However if the scale curve is not vertical, I get a tapered shape that has two clean interior corners, but two interior corners have extra random material that is not wanted. Is there a workaround I can do to get four clean interior corners? Thanks.

 

[cowski]

For the alignment option, use "parameter" - this allows you to turn on the "preserve shape" option. This will handle your input shape better.

Without this option turned on, the swept command will approximate your input sections with splines. Usually this works OK, except when you have sharp corners (as in your rectangular shapes). In your case, it looks like it is using 2 splines to approximate your shape. You will end up with 2 real corners and 2 "sharp turns" in the splines for the other corners. The "sharp turns" are magnified by the offset distance of the shell, resulting in somewhat rounded corners.

www.nxjournaling.com

 

[meCAD2]

Thanks! With "preserve shape" on, this simple model works correctly and so does a more complex shelled-out swept solid. I appreciate your help.