[SOLVED] Filling a shell

Depending on the complexity of the part....but one way could be to offset a surface on the inside....then make a suface fill and at the same time "try to form solid"

Krister L

"Jay Guthrie" skrev i meddelandet news:oI3sc.10741$hi6.1097490@attbi_s53...

Even easier would be to open a sketch on the face removed by the shell, convert entities around the inside (select shell thickness face, ctrl select inside edge and hit convert entities), then extrude up to body, and turn off the merge button. This gives you a multi body part which can be split into separate parts using the insert, features, split function.

matt

"Krister L" wrote in news: snipped-for-privacy@uni-berlin.de:

That was my first thought too......then.... maybe the face to insert the sketch on isn't flat....

Krister L

"matt" skrev i meddelandet news:Xns94F2869871986mlombardfrontiernetn@66.133.130.30...

Thanks for the idea's guy's.

The part is rather complex. It's a combination of air foil shapes lofted into the shape of a wheel. The wheel is going to be carbon fiber and I want to CNC the foam core for it. Doing the offset surface method seems the best. I can't get it to merge into a solid though. Also, if I offset it more than a few thousands, it fails.

So I think I got my work cut out for me figuring out a good method for doing this and getting it to work.

Jay

how about combining 2 bodies with subtract option

"Krister L" wrote in news: snipped-for-privacy@uni-berlin.de:

You can extrude a 3D sketch. It's kind of far fetched, but you can do it.

matt

If this is imported geometry then you might want to look it over very carefully. Use diagnostics, TOOLS/CHECK, verification on rebuild and manual inspection.

If the part is a closed shell with a def> I have a rather shapely part that is shelled out .030 thick. Now, I need

Jay, As neil metioned above, the way to do it is with the subtract feature. I'm going to assume that what you have is an enclosed shell (like a box or ball) with no openings. Create a volume completely around your part but uncheck "Merge result" to form two (2) bodies. Now go to Insert>Features>Combine... and use the subtract check box. That should give you what you want.

Muggs

cavity?

Forming two body's and then subtracting method worked out perfect!

Thanks much for all the idea's and time you guy's took to respond!

Jay

Glad it worked out for you!

I've been on the receiveing end of this NG more times then I can count, so it's nice to be able to help.

Muggs

You've heard it before "Giving is better than receiving." Well, ok, sometimes. Anyway it's always fun to find that you actually do know something. :-)

WT

LOL!

Thanks Wayne (I think).

Muggs

message

You already found that Cavity worked for you, but I think Krister meant to offset 0 from the inside surface. Still, I have parts where offset 0 doesn't even work on some faces!

Jerry Steiger Tripod Data Systems "take the garbage out, dear"