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

 

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

 

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

 

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

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

 

how about combining 2 bodies with subtract option

 

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 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,
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

 

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"