[nfrees114]

Hey All- So this seems like such a dumb issue but for some reason I keep breaking 1/8" End Mills. I am cutting a .150" wide O-Ring groove (roughly 6"x 3" rectangle) .175" deep in 6061T6 Aluminum. I have a Machinists calculator and it told me for grooving to turn @6115rpm and travel at 50ipm, and take out .031" per pass. Well I tried this with a two flute normal Ticn Black coated Nachi. I am climbmilling. I keeps breaking. I have tried 4 of the Nachi's and then i tried 2 solid carbide Iscar's. I've slowed this down to 35, 30 and now i'm running it at 25ipm and it seems to be working. i'm just wondering what everyone else would run. I don't understand why this machinist calculator would even reccomend 70ipm. also they say with a 4 flute to travel at 100ipm. I tried a 4 flute and tried 70ipm and it snapped within the first 1/2" of the 1st pass. I'm getting very frustrated and Broke haha. Any help would be greatly appreciated! Thanks!
-Nate

[Geof]

How fast can your machine run?

That diameter in 6061 could be run at 20,000 to 30,000 rpm. Obviously your machinist's calculator told you to go too slow.

Four flute cutters are not really much good in aluminum because they do not have enough flute clearance and the chips pack up and jam the cutter breaking it; as you found.

And the feed you got from the calculator is a bit fierce for a tiny cutter. A fairly good rule of thumb is 1% of the cutter diameter per tooth, maybe less than this for cutters smaller than 1/2". This gives you about 0.002" per rev for a two flute cutter and at 6,000 rpm this would be 12 ipm.

Also coolant is more or less essential when grooving with a small cutter, lots of coolant to blast the chips out. A powerful mister with lots of air and a little bit of coolant may suffice but whatever you use you do need something to blow the chips away and give some lubrication to the cutting edge.

With coolant, running at 6000 rpm or higher, with a feed of 10 or 12 ipm you should be able to take more than .03" per pass. Taking the full .175" depth in one go may be optimistic but 0.05" should be possible and you may be able to push it to 0.0875" with the feed backed off to about 7 or 8 ipm and take a shorter time overall.

[Get lucky]

I have run a OSG list 2021 three flute end mill at 10,000 28ipm with a 1xD worked well. We did snap a few getting the machine dialed in trying to hit the max on productivity but felt it was worth it to make rate. Another end mil that worked well is YG ALU-POWER runs about the same you have to back them off a little but only about half the cost of the OSG.

Hope this helps
Kyle

[John Welden]

I'd go with a three flute for sure.

[cjjonesarmory]

My calculation says the ideal rpm for 1/8" bit at 400SFM is 12,200. Now AlibreCam also says I could run the feed at 120 IPM with that RPM which seems high.

My machine maxes at 3000 RPM with the standard milling head. I run my 3/32 3-flute bit at 20 IPM at 3000 RPM with no problem. This is about a .002 feed per tooth.

I think a 1/8 bit running at 6000 RPM with 25 IPM sounds about right. Maybe a little slow, but in the ballpark. Not sure why the calcs recommend the higher feed rate. Perhaps you have a setting of 4-flute instead of 2-flute or something causing it to think you are making twice as many cuts per rev.

[mc_n_g]

I think the 4-flute and depth of cut is contributing to the breakage. It can't clear the chips. I am assuming this is not a ballmill. I would use a 3 flute with a slight corner radius or slight chamfer to ease up on the corners so you don't get any corner breakdowns on the endmill. Also is this flood coolant or air? If your chips are being recut on a 1/8 and you don't have clearance there are some issues.

[MDLEON]

3D wax mill noy work for mdx 15 or 20.,dont buy.

[MarkieMark834]

THEY ARE SPECIALIZING IN HIGH SPEED MACHING WITH SMALLER ENDMILLS. THEY HAVE SOME PRETTY GOOD CUSTOMER SERVICE AND TECHNICAL SUPPORT. IF INTERESTED I WILL GET YOU HOOKED UP