[kdoney]

I bought 2 new high helix, center cutting, 2 flute, HSS mills from Niagara (D201's) and both of them are grabbing the workpiece. This is a simple circle pocket with conventional milling. I'm down to shaving .002 per pass at 4 ipm! When I put in a 45 degree carbide from Niagara (A245) it doesn't grab until I get all the way up to .003 at 6 ipm. The head is rock solid until the plunge then it hops and ruins the z location (inexpensive servos). Anyone doing any better with different tooling?

[lakeside]

try droping rpm which will increase tool load or change path to climb mill

[DareBee]

High Helix cutters ar made for cutting aluminum.
You are cutting aluminum - right?

[kdoney]

Sorry, yes I am cutting aluminum. I'm pretty sure it's not the head moving. This is a moving gantry type mill. The x axis is a double nut thomson ballscrew and the y axis is a brand new daedal slide. I tested for backlash to .001 and there is none. The workpiece is a flat piece of 6061 and the grabbing takes place at different portions of the circle at different depths. I have not taken the 45 degree carbide to the grabbing stage yet.

[ger21]

Sounds like the machine may not be rigid enough for what you're trying to do?

[lakeside]

1/4 end mill in alum. 1500 rpm maxs

[Dawson]

try droping rpm which will increase tool load or change path to climb mill

Conventional cutting is more than likely why it's grabbing. Switch the path to climb, and you should have no problems.

[ViperTX]

Good one Dawson....twas what I was going to recommend.

[dertsap]

how much stick out do you have on the tool , 1/4"' highspeed is like a wet noodle ,
try stumping it up the best you can ,and i agree with the climb milling ,especially with a high helix , the tool is most likely pulling the chips right back into the part

[DareBee]

I never use HSS cutters in diameters smaller than 3/8.
They simply have too much flex, carbide only baby.
1/4 carbide cutters are (cheap ones) are about the same money as HSS anyway and work better.
Although a high grade carbide with TiCn or TiAln coating will outlast the cheap carbide 100X and is well justified in cost (and my personal recomendation).

This does not take into consideration any deficencies that your machine may or may not have.

[kdoney]

These are good american made end mills. I found the error though. Thanks to all for the help. I took your advice of slowing the rpms and climb milling and it did help, but I found the flexing was in the gantry itself. After a base plate replacement, both mills are performing well. The mini mill head still makes me take .005 at a pass at 10 ipm. Does roughing end mills speed up the process much? What other tooling have you mini mill guys used to speed up "hogging" large amounts of aluminum?

[warpedmephisto]

What type of minimill is it? You should be able to remove a lot more material than that, even on a minimill. I'm running a stock Taig + flood coolant and am taking 1/4" HSS high helix 2 flute at 4300 RPM 0.100" deep 50% chip load at 20 IPM. For 100% chip load I slow it to 10 IPM.

The thing you have to worry about with the minimills is that the motor doesn't supply enough torque to power through a heavy cut. And the rigidity of a minimill is a lot less so your cuts will start to get sloppy if you go too fast or heavy. What RPM are you running?

Edit: fixed RPM speed mistake.

[kdoney]

Originally I was running at about 2000 RPM but I slowed it down on advice. The mill head is mounted on an extremely heavey and rigid gantry mill so I can take the head as far as anyone. This is a chinese mini mill with the R8 taper. Max speed is 2500 and the 4/5 horsepower claim is a lie. I can't believe I can get to, yet alone, go beyond a .010 cut! I can hear each tooth of the 1/4" 2 flute high helix carbide ticn coated mill slamming into the metal now at .004. If it helps I can change to another head. I have a 10k rpm sherline I could mount if the jobs would get done faster but the torque kept stopping the stock motor on that one.

[JPMach]

All be it I am running a haas vf-4 but in aluminum I run a 1/2 60 deg helix two flute carbide endmill at 5500 rpm and 20ipm at uo to 7/8" depth of cut and full cutter width stepover. Spinle load is only slightly above 50% and the chips just fly out there. You do have to be carful on finish passes though to ensure no recutting of chips, lots of coolant or air helps.

JP

[kdoney]

Thanks. That certainly helps

[carlnpa]

What type of cutting fluid are you using?

[little bubba]

Does roughing end mills speed up the process much? What other tooling have you mini mill guys used to speed up "hogging" large amounts of aluminum?

Not a mini mill guy, but a lot can still be learned. My general rule concerning roughers and finishers is that a rougher can take out at least 3 times more material than a finisher in a given time. Tool pressure drops immensly, your spindle load will go way down. Take a rougher and a finisher on a manual mill and you can really feel the difference when cranking the handle.

My experience with high helix endmills is that they leave a great finish, but really suck at removing large amounts of material. Since your on a mini mill and your rigidity is limited, I would go with a rougher. On a more rigid machine a finisher can really get at it on aluminum, but a rougher will still outdo it.

My rougher aluminum story, one saturday we were screwing around and just seeing what our Mazak could do in aluminum, since we don't get to play with it much. 4 flute carbide rougher at 12000 rpms, at max feed of 708ipm. .375 DOC .25 step over. about .0145 chipload per tooth. I wanted to see what kind of chipload it could take and since at max feed already started backing down the RPMs. I got to a .029 chip load per tooth, thats when I got scared and gave up. The chips were getting bigger than some of the parts we make. We did roast one endmill when we tried cutting on the backside of the "test piece" where the coolant couldn't get in.