Re: I GOT A PROBLEM

"Arne Chr. Jorgensen" wrote:

> Is it possible for a number of you to write about the way you would
> go by this ? ( In simple terms I and other could understand ?
> ( I don't even know what a rose machine looks like )

Well, I do a variety of things, of course. So, there are all sorts of new
things that I haven't thought of until I try to do it. But, some things
show up over and over. Machining panels is a very common thing for me.
Anywhere from .050 to .250 thick, perhaps, but almost all the work is
constant all the way through, as if it were punched out. If a large hole
is to be machined, it is always faster and easier on the tooling to
trepan it, in other words cut around the edge, repeating as needed
until the full depth is reached, and the blank falls out. Then, you make
a finishing pass at slightly larger dimension to bring the hole to the
required size. For the simplest of these, I use my own routines to
trepan out round and rectangular holes, because they are more
controllable than a CAD to G-code package, and are often a lot
quicker to use. When things get complicated, like wanting radiused
corners, or something beyond the ordinary, then I use Bobcad/CAM,
and often have to do some hacking on the code. One of the common
things I do is to draw a tricky part in Bobcad, and make it generate
G-code for the actual part outline, then manually add the commands
to interpolate cutter radius compensation in and out at the strategic
points. There might be a way to make the 'custom' menu in Bobcad
insert these for me, but I haven't tried that, yet.

I have also made a very complex mold mostly with CNC, including
draft angles and such, with tapered end mills. I also have done some
panel label engraving.

A run of parts I did a few months ago, and have another batch coming up
soon, has a bunch of different things. One is a teflon tube socket that has
21 stepped holes in a circular pattern in it. Each hole has a narrowed part
in the middle. Spring fingers on the metal contacts go through the narrow
part, and then click open on the other side, retaining the contact. I made
a stepped drill by putting the drill bit in the lathe and grinding the diameter
of the tip down to the correct dimension. The face of the part is first drilled
with a spotting drill, then drilled all the way through with the stepped
drill. Then the part is flipped over, and an unmodified drill bit centers
on the through hole and drills in to the correct depth from that side.
The first drilling cycle is done with a peck-peck feed, the second one
can be done in one pass because it is shallower and is drilling a hole
where most of the material has already been removed. I made a fixture
to hold the part, and it has a hole where a keying pin can be dropped in,
to locate the part when it is reinstalled for drilling from the second side.

This thing is held in a housing made from a 4.5" OD tube, with 2 round
end plates. I made a fixture that holds all 3 of these parts (at different
times) for machining. The tube is first trimmed up on a lathe, then
mounted on a ring-groove in the fixture, and a 1/8" keying hole is drilled
with a spot drill on one end. When all the parts are done with that,
a locating pin is put in the fixture, and another keying hole is put in
the other end. Now, all the parts are spot drilled on both ends, using
the keying pin. Then, using the keying holes, each side has 6 holes
spotted. Then, the tool is changed, and all parts have 6 holes drilled
to the correct depth for tapping, and then, finally, the holes are tapped
with a tapping head (I used to have to do this by hand).

The end plates are cut square with a bandsaw, and clamped into the fixture,
6 at a time. First, all the holes are spotted, then drilled through. Chips are
blown out of 3 of the holes, and bolts are driven through to hold the
stack of plates to the fixture, and the clamps on the edges of the plates come
off. Then an end mill is mounted, and the OD of the plates is milled with
an arc program.

So, that might give you an idea of some of the tasks that come up pretty
often it the parts that I make.

Right now, I have designed a rotary valve and I need to cut a groove for
an O ring in the cylindrical side of the rotating plug. Now, I think I can
get away with the sidewalls of the groove being parallel, but the bottom
of the groove must conform to the radius of the cylinder. I almost got
Bobcad/CAM to do this, but it croaked on me. The 'winskin' function
handles drawing a closed surface, but the CAM function to write the
toolpath doesn't allow you to use a point on the guide surface twice,
so it has no end point. I suspect I can make it cut the groove in two
halves, but that is sort of ugly.

Jon