Re: [CAD_CAM_EDM_DRO] First example case

Couple of tips:
Hardware store steel is usually junk. Go to a decent metal supplier and get
some 1018 Cold Rolled steel, or, better yet, 12L14 steel, which is a
free-machining steel that machines beautifully.

The short answer is that, for your 0.075" hole, you should use a drill press
and a sharp drill bit (center punch and spot drill for best accuracy).
However, you have a CNC machine, and circularly interpolating large holes is
a piece of cake. You need to use G02 and G03 commands and you nearly always
need to do it half at a time (on a clock face, you'd command a cut from
12:00 to 6:00 and from 6:00 back around to 12:00. For highest precision,
you go in quarter-circles).

On a Taig in steel, you'd be wanting to use a 4 flute end mill because the
greater the number of flutes, the lower the chip load per tooth
(translation: less work for a small machine). You can get 4 flute plunging
end mills, and they're a good investment. Only 2 of the flutes go all the
way to the center. You probably don't want to plunge in steel on a Taig
anyways. Also, a 3/8" diameter cutter is pushing it in steel (you could do
it in aluminum). You might want to start with a 3/16" or 1/4" max cutter.
That would produce a 3/32 or 1/8" corner radius (I assume you meant a 3/16"
radius created by a 3/8" cutter in your original message), but you could
interpolate any radius you wanted.

In general, fixturing and clamping are one of the most challenging of
sucessful machining, but a few pointers:
MDF expendable plates and various clamps are one solution, but much better
IMO is a reusable tooling plate, with a sacrificial sheet metal plate on
top. I have two, both made of 1/2" thick 6061 Aluminum, 3.5" x 12" in
size. The first one I have, a commercial one, has #10-32 tapped holes on a
0.75" x 1" grid, allowing 5 holes across the width and 10 down the length.
I wasn't too fond of the unequal hole spacing, so I made a nearly identical
one with a 1" x 1" grid, with 3 holes across the plate. The plate is
reusable, but I have about a dozen pieces of 1/8" aluminum sheet, sheared to
the same 3.5"x12" size, which I put down in between as a sacrificial
backer. Unlike MDF, it is waterproof (I often run mist coolant) and
reusable. I've made about a dozen different runs since I started using the
aluminum sheets as backers, and I am still reusing the same one. I sand out
any burrs between jobs with a scotchbrite pad to ensure a flat surface.

Unsupported milling or "milling over air" or even with only one end clamped
is generally a bad idea. You can get serious vibrations, and the very
nature of helical endmills is that they tend to want to pull the part up and
out of the fixture. You really want clamping all the way round. You can
get over some of this by drilling extra holes in the part (or utilizing ones
that are already there) and screwing the part down to a tooling plate of
some sort.

Hope that was helpful
Michael

On Jan 28, 2008 11:54 PM, <dannym@...> wrote:

> OK, this is one of the first things on my list of actual things I need
> to do:
> I need to cut a 2D part out. It's part of a crossbow trigger, basically a
> "T" shape, got some curves and things but no complicated features that I
> see. About 2.25" long 1.5" wide.
> The inside corners would be fine with a 3/8" radius.
> It has a single hole 0.075" dia. I have a drill press if necessary.
> I have a 36" long piece of 2" wide steel from the hardware store, 3/16"
> thick, described only as "plain".
>
> My assumptions:
> I need to get an end mill 3/8" and 2-flute would be ok
> The milling process cannot help with my circular hole. I should drill that
> first and use it as a reference point for the CNC process.
> Since this is a 2" wide stock with a 1.5" wide part being cut with a 3/8"
> kerf on either side, I must clamp along the long axis to avoid striking the
> clamps.
> I would get some MDF as a spoil board to protect the Taig rails and
> possibly raise the stock so the chuck won't hit the clamp (hitting the chunk
> on the clamp probably won't be a prob).
> I would modify the design to leave tabs say 1/4" wide on the long, clamped
> sides so it isn't cut free. The tabs can be basically in-line with the
> clamping axis so it's not at risk of forming a "Z" that squishes down and
> loses clamping pressure. I could also thin the metal at these points to make
> it easier to cut free with the band saw. Thinning is also necessary so I can
> see the line to cut.
> I do not have a coolant mister setup. I should spray it with WD40 and set
> the XY speed low to keep the heat down.
>
> I could also clamp the whole strip in a clamp along its 2" width, leaving
> 2.75" extending past the clamp, still resting on MDF, so the machining can
> be done on the part extending past the clamp without running into the
> clamps. That means the clamping force is not trying to flex the part and
> squish it so this sounds better, maybe the tab could be thinner and the
> machine could cut it free as the last step. Also I would not have to worry
> that the cut ends of the stock being put in the clamp are cut square as in
> my first case. Downside is the part's only being supported from one side
> during this process though, but the force isn't going to be high enough to
> bend the part around or anything, is it? This seems like the better plan
> actually.
>
> Comments?
>
> Thanks,
> Danny
>
>


[Non-text portions of this message have been removed]