A milling problem: need advice

On the roughing cuts... don't go through the center of the piece. Offset the cut, towards the front, the amount you are "over" on the back, plus a few thousandths.

Unless your material is hard... I'd go for about 400 RPM and 3.25 IPM feed (assuming a two flute cutter. If not.... you are asking for deflection.... use a two flute end mill.

Using your present setup and a 2 flute mill you are cutting about .01 per tooth.... that's probably too much.

I think your assessment is correct. The problem as I see it, is your machine choice. This is best accomplished with a horizontal mill, not a vertical. Even a small horizontal will easily remove more material faster and more accurately because the tool stiffness is so much better. However, if you must mill to a vertcal shoulder, a horizontal is out of the question. In that case, I would drill to remove as much material as possible and then do final shaping with the mill. Steve

Yup, with a .300" plunge, the tool deflection will be substantial. How about reducing the plunge to .150 each pass. Or, maybe just go to .200" steps. You might be able to keep the time the same by feeding faster with a shallower plunge each pass. Also, offsetting the full-width plowing cut toward the front might help. Digging into the back wall is exactly what you'd expect from tool deflection.

What kind of machine, what kind of tool holding? Keep the length of overhanging cutter to a minimum, use rigid end mill holders, not collets, keep the quill extension minimum (if the machine has a quill).

Jon

Horizontal mill

Gunner

"A vote for Kerry is a de facto vote for bin Laden." Strider

Don't you love it, fellow horizontalists, when you can gloat about a situation in which a horizontal mill is clearly better.

Boris

Depends on whether his slots are open at the ends, or closed. He doesn't really say. And, of course, you can do these types of jobs with a stub milling arbor and the same cutters. Just mount the work sideways in the vise, or on an angle plate. Put a 3" milling cutter on an arbor, and it is AMAZING how big a pile of chips you can make!

Jon

Horizontal is most always better. ;o) Sue

You sure can, but nothing will beat the horizontal and a plain milling cutter on an arbor - with an overarm support for rigidity.

Jim

================================================== please reply to: JRR(zero) at yktvmv (dot) vnet (dot) ibm (dot) com ==================================================

Thanks to all who replied. We got the part cutting well this morning and were able to run about 18 of them throught the mill.

I mistyped in my original post in that I was running it at 350 rpm, not 250. Anyway, the slot was completely through. I set it to 375 rpm and 3 ipm. The cutter was a .750 roughing end mill, and I wanted a finished slot of .790, hence not much room for deflection problems. We ended up making the first cut .015 off center to the front and back at .008 off center to the back. On two or three of the parts, the finish tool did not complete clean up the back face of the slot, but that was very slight and easily dealt with.

Good learning experience for me. Thanks again to all the inputs.

By the way, it's a very small shop and running a horizontal mill was not an option.

-Bruno

Bruno wrote:

When faced with the same situation in the past, I have ground the o/d undersize on the roughers, kinda like a rougher-finisher tool--easily done on the darex or by your local tool grinding outfit.

Makes for good usage of otherwise dull endmills that are to about the end of their service life, and the o/d can be re-sharpened several times in this manner.