1.5" Dia High Speed hanging 6"

[Machine1]

Im machining 6061-T6 cast aluminum and I have to use a 1.5 dia endmill hanging out 6" for clearance. The problem that I am having is I am taking a 3.5 DOC .075 off of the wall and the part is hanging out in the air. The endmill is not buried in part it is an outside cut. I am getting terrible chatter. running 250sfm @ .006 chip load. Any help out there. Do I need to increase my chip load or my SFM or both?

[wms]

Machine1,

If you are getting chatter, I would first reduce the sfm, then if needed increase feed. You need to "load" up the tool. And by reducing speed you will increase the chip load. Same for increasing feed.

The other option would be to reduce the depth of cut, but it sounds like that is not an option.

Or if you could use a shorter end mill first, then jump to the long one.

You could if possible cut multiple passes at say .025 to .050 doc at say 1500 - 2000 sfm and something like 100 ipm. I don't know if this is possible with your setup and part.

[HuFlungDung]

Machine1,

When you say the part is hanging out in the air, that sounds like a big part of the problem. Is there any way to put a finger stop against it from one side, while you go at the other? Anything to help soak up the resonant vibes.

Also, brand new HSS endmills often have a little too much clearance, which "enhances" the chattering tendency. As a rule of thumb, when I set up to sharpen a cutter or a hand reamer, I like to see about .005" drop in 1/8" of circumferential rotation for a low clearance cutter that will not chatter so badly.

If you could "break it in" on something else without buggering it up, it might quiet down a little later. They say this is what a honing stone is good for, but it is pretty tough to hand hone the flutes of an endmill.

[camminc]

Hello Machine1. I am in the Tulsa area, Claremore. There are several possibilities to improve and or eliminate the chatter problem you are having. Possibly giving you up to 30% improved machining time. Anywhere from using a solid carbide shanked cutter, maximize your holder type or just plain going after chatter by frequency analysis with your existing setup. These are just a few idea's. We devise special cutters along with dynamic optimization methods. If your interested just email me. Thanks. Randy

[Rich Monfo]

Hi Machine 1

Using endmills are a thing of the past. We have specially designed carbide cutters to cut aluminum.
they work great with no chatter taking a depth of .500 to .750. in depth and working your way down at a 150 IPM
Depending on how your machining this manually or CNC will determine weather you are able to look into these types of cutters. They range from 5" to 1" in diameter. Here is a website where we buy our tooling if you are interested. http://www.ramstar.net/

[Paul_S]

Originally posted by Machine1 Im machining 6061-T6 cast aluminum and I have to use a 1.5 dia endmill hanging out 6" for clearance. The problem that I am having is I am taking a 3.5 DOC .075 off of the wall and the part is hanging out in the air. The endmill is not buried in part it is an outside cut. I am getting terrible chatter. running 250sfm @ .006 chip load. Any help out there. Do I need to increase my chip load or my SFM or both?

My intial calculation for this type of cut would be 1020 RPM with of a feed of 29.6 IPM. Thats .0145 IPT for a 2 flute cutter.

But because of the chatter problem I would use 128 RPM and same IPT at 3.7 IPM. I would try that.

(3/6)^3 = .125
1/8 the RPM, and 1/8 the feed estimated. 1020 x .125 = 127.5
29.6 x .125 = 3.7

At about 1/3 horsepower required at the spindle.

This is assuming the chatter is do to the EM.

At 128 RPM finish second spring pass at a mininum of 2.5 IPM, a maximum of 5. IPM depending on finish requirment.

Let me know what you had finally got to work.