Looking for some help on the Cavity tool in Solidworks

Would anyone here happen to have, or know of a tutorial, either video
or PPT on the Cavity tool in Solidworks.
For some reason I simply do not understand the help file at all. There
is no kind way to say it, the way it is written it's understanding is
over my head, period.
We have a Solidworks model of an oval shaped Globe cut in half, and
the world map is raised over the radius of the globe and our customer
wants to see it in the exact opposite view. It resembles a watermelon
cut in half, lengthwise, with the stretched out world map superimposed
over the curved side of the cut watermelon, one sixth size. We
ultimately need to end up with a female impression of our male plastic
sample. We will ultimately injection mold it in a plastic-mold
injection machine, after first having the concept approved.

Thanking you for your response in advance

David and Michael

 

The cavity tool has been around almost from the beginning in SW. It is
not that hard to use. Here is some practical information:

1. The cavity tool is applied to a part being edited inside an
assembly.

2. Open an assembly.

3. Drop in the part you wish to use as the cavity cutter. Mate it to
known planes in an orientation that makes sense for you.

4. From the insert menu, create a new part and using the planes that
you mated the cutter to, extrude a box around the cutter.

5. Save the newly created box part and then RMB on it and select edit
part. You are now editing the box into which the cavity will be cut,
in-context of the assembly.

6. Insert a feature (from the Insert/Feature menu) called cavity into
the box part. Select the cutter and click OK.

7. If all is OK you should have the cutter's impression in the box you
just made.

8. Using a section view, open up the box and look at the impression
you just cut.

There are more nuances to doing this. Once you have done it this way,
you can branch out from there using scaling factors for shrink, using
inserted components instead of creating a new box, etc. After cutting
the cavity, use List External references to lock the cavity
calculation down so that SW won'nt recalculate it every time. The part
into which the cavity is being cut need not fully envelope the
cutter.

You cannot import dimensions from a cavity. The scale factor used when
cutting a cavity will not scale reference geometry from the cutter.
Using the scale feature on the cutter will likewise not scale
reference geometry or dimensions.

On a complex cutter, the cavity feature can be very computationally
expensive and may have problems. Before starting and with the cutter
open as a part, use Tools/Check with Tools/Performance/Verification on
Rebuild to make sure your starting geometry is OK. If you have a
general fault shown, stop and fix it before proceeding.

An alternative to creating a cavity in an assembly is to insert a part
into another part and use a Combine feature to subtract the cutter.

TOP

 

The original paper manual of about 250 spirol bound pages titled
"SolidWorks 2000 Getting Started" that SolidWorks used to give out
with SWks 2000 was a superb, short concise step by step introduction
to common early steps in SolidWorks, and if you went through that
manual's section on cavity work, you would be through the basics in
maybe a careful 30 minute run at most. I do not know whether
SolidWorks supplies that little manual any more. I think they should
do so, as that is all the training I had to start my first part with 4
hinges and two break off parts as my first SolidWorks project (worked
fine).

I would ask my VAR to see an old copy if they don't have new "Getting
Started" booklets.

I've not seen or tried very very complex cavities (not my cup of tea),
but given TOP's note, I would have to guess if the cavity work failed
in SolidWorks and you couldn't get it done, that you can still export
to IGES or another format so another CAD system could develop the
tool, as an ultimate backup to SolidWorks.

Bo