I could use some suggestions regarding speeds and feeds.
I'm trying to mill rather deep pockets in 6061 aluminum. I have the pocket rough milled to within .050" per side of finished dimensions. The depth of the pocket is 2.813" finished depth. The maximum corner radius allowed is .187".
I'm not happy with the chatter that is occuring and I am afraid that I will break the solid carbide end mill, especially when it mills the corners. The end mill is a 3/8" 3 flute uncoated with a 3" length of cut.
I will actually be in a more difficult situation with another pocket mill that requires a .140" corner radius but not quite as deep.
I realized that I could have left less stock to finish and that might at least would reduced finish machining time.
Any suggestion?
Thanks

Lots of coolant that will flush chips out of the cutter and not into it. ideally, coolant designed for aluminum. chatter can be caused by to high of rpm and/or too low of a chip load. tight machine? tight spindle bearings? tight fixture? (or clamped very well) as much part to table contact as possible.
Tool designed for aluminum? (higher spiral to the flute)
just some thoughts to look into.

It is difficult to machine at that depth of cut with a .375 e-mill. you may have to take multiple depth passes, but this will leave blend marks. A high helix cutter helps because it changes some of the cutting force(deflection) from horizontal to verticle. Another trick is to use a G02,G03 move in the corner if the machining tolerance will allow it ( maybe a .193" radius) this will put less tool in contact with material and reduce tool vibration(chatter) Lastly slow down the rpm(and feed) until chatter is reduced. It is amazing, some of the things that engineers can draw are not easily made! Good luck. CW

Thanks for the hints.
The machine is real tight, brand new as a matter of fact.
I will look into the helix more closely for future jobs. I still haven't come to any opinion about cutter coating yet. I have been flushing from both sides of the cutter full blast which keeps chip bulid up down.
I'm using a 5/8" endmill to rough the pocket with the G150 cycle, splitting the total depths into 3 separate cycles just in case I have a major problem half way down. And I always have at least one spare cutter on hand. I will try the G02 G03 on the next group of pieces or use the 3/8" end mill and "drill" the corners as I did on this group. I have played with the speed and feed a bit but I have been mainly trying to reduce machining time. I managed to cut about 2 hrs of cutting time. I tend to be too conservative.
Need to show the bosses progress you know. Fortunatly the surface finish is not to critical and I will have to slow things down at some point. I need the hands on experience to see what it will do. It's a bit different when your arm is the power feed if you know what I mean.
Thanks again

I have some suggestions but I don't know how many more of these you have to do or what your machine's capabilities are. If you have to have a finish without steps or chatter I suggest lowering spindle speed and feed significantly. You might use HSS if you can live with the deflection. You would continue to "drill" the corners & minimize radial cut. The next alternative is the opposite; leave 5/16" left on the sides of the walls with a bit less in the corners. Then make a zillion small steps in Z (probably about .040 to .063 deep/pass) @ max. rpm & .004 to .007 ipt with a 2 or 3 fl. long reach, short fl. end mill. I have a 5-axis machining center; I use HSS tapered end mills for rigidity to get around your exact problem.