[Eric Olson]

I have a customer who needs some text and graphics (line art) milled into an aluminum plate. The depth of cut is .015", I'm using a down spiral .030" bit and my max. spindle speed for my machine is 18000. I've done some tests with a over the counter bit about the same diameter, ran it at 10ipm and got decent results. With a Kyocera Micro Tools bit, what do you think would be a good place to start with my machine parameters and the material. Aluminum is 1100 H24 .040" thick. (Is there a better section to post this in?)

Thank you

[High_Speed_RJ]

I have cut a lot of text in die steel. I use a 1/32 - 3/32 ball nose usually. Size difference pertains to the width of the lettering I desire. Id run it max spindle speed that you are comfortable with and do a .005-.01 stepdown. What cutter are you using exactly? Carbide? how many flutes? Ballnose? Is this a 1 piece job or production? My depth of cut would depend on the diameter of the cutter.

If carbide use 800 Surface feet per minute.... so formula 3.82 divided by cutter diameter x 800
3.82/.03x1500sfm = 101866 RPM !!!! Yeah thats right. And thats going on the low end for sfm. Well you cant do this so we go to feed per flute. Say you have a 2-flute cutter. I would cut .0004-.0005 per flute for such a small cutter.
So lets take 15000 rpm. .0005 x 2 flutes x 15000 rpm = 15 inches per minute with Lots of coolant or mist.
Or stay at your 10 ipm which is fine also.

When dealing with tiny cutters and aluminum it is important to note that tiny tool can make heat quick. Better off taking light cuts in some situations. You can use WD-40 or kerosene also as a lubricant. Kerosene is from the old school days for glass finish. WD-40 works great too.

[Eric Olson]

HS_RJ,
Thanks for the reply, its a carbide, two flute stub length ball nose end mill. Kyocera's 1635 series. Its kind of production, I'll probably cut 40 total just to have some extras. If you need any more info, please ask.

Eric

[High_Speed_RJ]

Yeah I looked it up and figured that is what you were using.

So lets take 15000 rpm. .0005 x 2 flutes x 15000 rpm = 15 inches per minute with Lots of coolant or mist.
Or stay at your 10 ipm which is fine also. Start With a .005 step down and run a few. If you don't like your timing on per part drop in on the depth. .01 should be O.K. I just don't want ya to snap it for some reason as I cant see what is going on with the coolant situation. You can adjust your step down right? Or are you locked into your program? Just make sure you have lots of coolant on it. Tell me how it works out.

Also I would hand edit that program to go 50 inches per minute for the first 3 0r 4 passes at .005 depth of cut. Than slow it down for the final passes.

[Eric Olson]

HS_RJ,
Thanks for the input, I can adjust the first "roughing" passes and slow it down for a final pass, can also adjust the step down as well.

Eric