1/8" ENDMILLS

[rc]

Having trouble with milling half hard brass using an 1/8" endmill. I've tried every brand in the MSC catalog. Tried 2 fl, 3 fl, 4fl in every manufacturer in carbide, and every speed and feed combination. The parts are for electronic/microwave application, and must have a 16 or better finish with no chamfer or radii in the corners.

[Trevor Bailey]

Try making your coolant really "soupy". Add a lot of concentrate.

[rc]

I also went up on the concentrate also. Still getting chatter, and a poor finish.

[Keith Graydon]

Hmmm,

Robb Jack or Niagara cutters ought to do it. They do for me. What speeds and feeds are you using? Depth of cut ? any nfo to help us troubleshoot. old machine,new machine?.............

-KLG

[rc]

Using 4500 rpm and 12 i.p.m depth of cut is .074 deep. Roughing first and leaving .005 for a finish pass on wall, and floor. Machine is about 6 yrs old.

[Chips Ahoy]

Maybe you could shorten your tool up a bit or put it in a more rigid holder???

[Trevor Bailey]

Try shortening the tool as much as possible. Try a different holder. If the job warrants it, try a "shrink" type holder. If your cut length in not to deep, get a tool with an extended shank and only the flute length you need. Do this if you are using a collet holder and are not able to get a good "bite" on the tool. I have cut a lot of brass golf clubs with 1/8" tools and smaller. All of the above factors may/will have some affect on the end result.

There are no direct hit answers for situations like this, but there are many different things you can try.

Good Luck,

[Scott Bond]

Hi

Rough with a rougher,even if you are using a finisher as a rougher. Then the finisher is still fresh for its only cut. If the bottom of the finish tool will be cutting or even toughing while the sides are being cut,be sure the bottom has a hallow grind.

Use cutting oil for coolant.

[Mykal]

RC,

I agree with Keith on the RJ or Niagara cutters. You might ponder the fact that you don't want to have a real real sharp tool when cutting Brass. It will pull and tear vs cut as it does if you drill brass and you don't stone the edge of the drill. Kind of falls in the same class as acrylics and plexiglass. You will notice it less in an NC machine vs. a manual machine so you may not even see or hear it happen. You might try stoning the edge or using Carbide, (as they tend to rub more,) and see if that gets you a better outcome.

Also, I agree with the others on the concentration issues but consider Virgin Mineral Oil. This stuff does wonders for materials and there finish. Brass, Copper, and Aluminum especially.

Good Luck!

Mike

[Guest CNC Apps Guy 1]

I use stubbys almost always. If I need longer reach, I'll get a stub LOC and grind back the shank for relief.

[Keith Graydon]

I think Trevor and MAhall are on the right track here.

Trevor is pointing to the fact that run-out my be an issue. accurate tool holders are a must.

MAhall thinks your tool might be "grabbing". Get a diamond hone and stone it up a bit. go lightly. You'll need to be able to repeat this if this is a long production run.

Also, your chip load sounds high. .00133 with a 2 flt mill. If the mill has excessive overhang it's gonna whip all over thee place. 4 flt will 1/2 the load and they're much stiffer than 2 fluters. Shorten it up to a minimum overhang. As per James Mayette.

 

my.02

hth

-KLG

[rc]

Thanks everyone! I went to a 2 fl stub and hit it with the diamond. Finish is almost mirrorlike.