Solid subtraction?

In the context of an assembly, what's the best way to have a part cut a
cavity into another part?

Imagine a simple extruded rectangular plate as the part that will be cut and
a sphere (or some other non orthogonal shape) doing the cutting.

The cut would have to follow the sphere wherever it moves.

The contact volume between the sphere and the pat to be cut could range from
being very small (slight interference) to cutting all the way through (a
hole with the shape of a spherical section, in this case).

Yet another useful feature may be to be able to specify that the cut happen
at a given offset from the surface of the cutting part. Let's say that you
want a 0.005in gap between the hypothetical sphere and the plate.

Thanks,

-Martin

 

turn on mold toolbar, try cavity. may not do everything, but it's a start.

 

The "indent" feature pretty much does this

not enough confidence to use '05 yet

 

As I understand what you are saying you want to drive the "sphere"
along some path and remove material wherever the sphere intersects the
part? If that is what you are saying then you should be looking at
something like a CAM program.

Just cutting out one "sphere" is a trivial problem involving and
assembly and two parts along with the cavity feature.

 

In addition you can use a sweep to remove material but it is not quite like
a sphere.

I also tried patterning a sphere along a curve. 500 equal spaced instances
cuts a fairly smooth pattern using the cavity command but is quite
processor intensive. Again, a CAM program does this better. It was kind of
fun to generate the cut of a regular endmill along a 3D spline.

 

That's exactly what I needed. "Cavity" doesn't quite do it.


Part of the problem I've been running into, I now realize, is that a great
many SW functions are hidden. What I mean by this is that the toolbars
don't show all available tools. You have to explicitly customize them to
add the buttons you need. And so, the process of discovering what is
available is a bit cumbersome.

-Martin

 

Martin,

That's what books are supposed to be for. There is a 300+ page 2004
reference manual in PDF format somwhere on the site. Most of the content is
applicable to 2005.

If you had every icon on every toolbar on the screen at the same time, you'd
have very little area left to work.

Regards

Mark

 

In SW 2003...

If "Cavity" don't do it for ya...

·Use "Join" or "Insert-->Part" to bring in the spherical body to the
part file you wish to cut.
·Use "Insert -->Feature-->Combine" to subtract one body from the
other.

 

Sounds like you are trying to make a sweep cut? What is the original
object you are making clearance for? is it a swept object or
rotational? Simple or complex form? is it actually a cam path, or a
complete part form?

If it is a path, then I would recreate the path in the part file, and
make a sketch with the desired orset and sweep cut.

If you actually have another part and do not want to make a cavity /
core, you can edit the part in the context of the assembly, and make an
in-context (careful...) surface offset from the other interferring
part. Use that surface to cut the part.

Just a learning aside: as someone else mentioned here, books are good
The way I learned SW fast for just this type of dive-in-head-first
that you are doing, was to simply read the help file. If you go to the
help menu, and look by contents, and simply start at the top and go
through, you will discover a world of useful information. I personally
find that if I just cruse through this once, later, when I have a
problem, I at least have a clue that I saw a soltution somewhere... You
will also find very good examples. Highly recommend it!

Daniel

 

Or you can work off the menus at first to see what is there.

 

Yup, yup. You are right... :-(

You don't know the screen I'm running! 30", 2560 x 1600.

Talk about carpal tunnel. I swear that the cursor goes across time-zones
when it moves from the right to the left edge of the screen. Lots of
keyboard shortcuts.

Yet again, you are right.

-Martin

 

It's a medium complexity shape, see http://www.snaptron.com/bl_series.cfm

This is the part I modeled with a couple of rotated configurations as well
as a "cavity cutter" configuration.

A 0.050in rubber plate would cover a whole bunch of these domes. Cavities
need to be created on the underside anywhere the domes are placed. Of
course, you want a small gap for tolerancing and other purposes. The Indent
feature worked perfectly for this. I found it to be a little temperamental,
which is probably more correctly attributed to my lack of experience.

Plodding right along though!

I have to thank a bunch of you who've offered valuable help over the last
couple of days. Thanks, very much.

-Martin

 

Hi Martin,

glad to hear the help is helping and you are making progress!

As for the indent feature, I do not have much experience with it, but
my impression has been that it is as you described - tempermental.
Which is why I might look for other more predictable / controlable
solutions.

Are you using the whole array and making on indent, or are you
patterning the indent?

Just some other thoughts / suggestions:
1.
if you have a master layout sketch for the button coordinates in your
master assembly, then the rubber key caps, snaps, and PCB and housing
can all use that as the parametric driver. I try to avoid in-context
relationships between parts as I tend to have more problems later -
easier to solve if you only make relations to assembly sketches, or
layout sketches in parts. with this technique, the design intend is
available for each part, and is used only for the base or key fatures.

2.
you say you have a cavity cutter config in the snap dome model. Rather
than having a solid form, simply leave this as a sketch - cavity cutter
sketch - no special config. Then in the context of the assembly, edit
the rubber membrane part, create a new sketch using the caity cutter
sketch plane from the dome part, and make an in-context line copy of
the sketch in the rubber part. You can now do a cut revolve. Now
pattern this one for all the button locations.

Or simpler, if you think the dome will not change, simply make the
simple cutter sketch in the rubber part.

3.
Also, if you have not seen these features, have a look at point based
patterns, and assembly patterns based on existing patterns. these are
very powerful! You may find it useful to make one sketch with points at
the coordintates of every button. then in each part that works with
that pattern, you simply pattern off that.

Many ways to skin a cat. I have been working with SW for 5 years, and
each project is new and different, and there is always a new technique
to learn.

Enjoy!
Daniel