[SOLVED] Filling a shell

I have a rather shapely part that is shelled out .030 thick. Now, I need to
create a new filler part that fills the inside volume of the shelled part.
What's the best method to do this?
TIA.
Jay
Reply to
Jay Guthrie
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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...
Reply to
Krister L
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:
Reply to
matt
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...
Reply to
Krister L
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
Reply to
Jay Guthrie
how about combining 2 bodies with subtract option
Reply to
neil
"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
Reply to
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 definite internal space you could extrude a block around it and then use the cavity command. This will create an inner and outer solid if the geometry is OK.
Jay Guthrie wrote:
Reply to
kellnerp
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
Reply to
Muggs
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
Reply to
Jay Guthrie
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
Reply to
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
Reply to
Wayne Tiffany
LOL!
Thanks Wayne (I think).
Muggs
message
Reply to
Muggs
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"
Reply to
Jerry Steiger

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