I'm making a box from 6082T6, I have to machine 41mm deep on the inside and 43mm deep on the outside with a 6mm cutter due to the rad size(4mm).
I've tried cutters from Garr Tool, WNT and others using cutters specific to aluminium (UK) but whatever speed and feed I try I still get a bad finish with lots of chatter. Any help would be apreciated.
Thanks.

Forgot to mention all the cutters I've tried are solid carbide.

A 6mm cutter and 40+mm deep is asking a lot. Have you thought of doing a roughing cut with a larger cutter and then a finish cut to get the final size? Using a Rough End Mill will go a long ways to get things done quickly and should help with the chatter. Having a long bit will always present some issues when it is a small diameter. Other than max spindle speed and a slow feed rate, there is not much else to do, or at least I've not found any. Having a sharp cutter always helps and keeping it cool does too.

For me, I find that doing a climbing cut gives a much better finish than the reverse. You may just want to try that and make the cuts in the opposite direction. May solve your problem without any major fuss.

I am putting a larger cutter in first, its the last bit with the 6mm thats still a problem I am climb milling should I try going the other way? All the cutters I have tried have been new.

What machine are you running it on ?

Phil_H

What machine are you running it on ?

Phil_H

An XYZ 560

i've done quite a bit of deep pocketing with small cutters. 3-4 cutters in decreasing diameters work well.
drilling the corners out with .005 clearance to the finished size helps
half inch to rough
3/8 to finish the inside walls
9/32 to finish as much as allowable between the 3/8 and the finish radius
6mm to finish the radius
relieve the endmill so there is about .450 of flute. this minimizes excess contact on the side walls.the next z depths acts as a dead pass to finish and take care of deflection.
make the z depths about .200 each, and over extend the radius to match the last smallest cutter
2 or 3 flute carbide endmills work best
if the finish is important,or too much chatter, slow the endmill down to 1000-2500 rpm and figure the feedrate for about .01 ipr.
there are also several variable helix endmills available that help to eliminate chatter.
this process is not the most proficient, but it should work well with a little experimentation.