Solid subtraction?

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

Martin,

The "indent" feature pretty much does this

Mark

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 pattern> As I understand what you are saying you want to drive the "sphere"

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...

=B7Use "Join" or "Insert-->Part" to bring in the spherical body to the part file you wish to cut. =B7Use "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

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.

1. 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.

1. 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