Ned Simmons wrote:
On Sun, 10 Jan 2010 21:28:29 -0800 (PST), rbce2003
wrote:

The only way I can envision the next step is for the shop to hold the
raw material (in this case a 4" wide x .750 thick aluminum bar stock)
either on a basic jig (called jig A) on the mill table, or in a simple
mill vice, then run a first program to drill the fixturing holes that
I have designed into the part for second step fixturing in JIG B.
They would then have to remove the part from JIG A and install in jig
B, and run the rest of the program. Is this plausable?

Ask the shop. If they're really interested in the work, they'll talk
to you. I've seen many parts, like what I imagine yours to be,
machined in multiples from a large piece of material. The material is
clamped to the table on top of a sacrificial plate. A small attachment
to the plate is left as the last thing to be cut, releasing the
individual parts and leaving a skeleton as scrap. But talk to the
shop.

My Next concern would be the something that only the shop I choose
will answer 100%, but could I expect to give them the DFX file and
they then can convert it over to talk to their machines?

Most shops will appreciate a dxf. But I always tell them they use the
supplied dxf at their risk -- the print is the controlling document.

Then, how does one decide what tooling to use? We are talking about
smaller shops without the budget for the latest/greatest software...
so does something like MACH3 or the other CAM software pick the tool
sizes? Or does the machine programmer look at the print and say... OK,
I'll use a .250 end mill for here, and a .750 for there, etc??

Other than obvious things like avoiding sharp inside corners,
especially on deep pockets, let the shop worry about it.

I suppose this leads to another question... is it prudent for the
person drawing the files to try and use radius' thruout the part that
coincides with common sizes of tooling? I mean if I need a radius on
a part, and the shape is not a critical design element, then Pick
something simple like a .250 radius? Is that just good design work..
meaning everyone in the trade already knows to do that?

Give plenty of latitude on non-critical radii. For example:
R .25 APPROX
R .312/.188
R 1/4 (if your title block allows an appropriate tolerance on
fractional dims)
R.25 +/- .03



I do CNC programming & setup (20 yrs+). Ned's idea of a sacrificial
plate we use very often. We also use a plate, with counterbored tapped
holes in it. A couple of tiedowns to clamp the part, drill through the
part where the counterbored tapped holes are, blow out the holes, put in
bolts, remove tiedowns, and machine the outer profils.

Also, tolerances dictate cost. The looser the tolerance, the lower the
price. Common end mills (lower cost) come in 1/4 inch increments. If
possible, specify I.D. radii in 1/4 inch increments, and tolerance them
+.015 to +.030, and -0.

Surface finish callouts are beneficial to the quoting process. If not
specified, you may get (and pay more for) a smoother finish than you
actually need.

--
Steve Walker
(remove wallet to reply)