how to fix chatter in aluminum with extra deep cut HSS - [solved - lower rpm]

[rk9268vc]

Ive got a 2in deep pocket that im trying to finish and it just screams
im clearly doing something wrong and want to know what yall would do differently?
I rough it in multiple steps, but i would like to finish it at full depth

my feeds n speeds
1/2" 4 flute 2" flute length HSS - pocket is 2in deep in 6061

4300 rpm 15in/min .01" stepover 2in deep

i run a spring pass and it doesnt sing near as loud, but still chattery

i tried ramping up and down the feed rat and it still screamed

thoughts?
thanks

 

[crossthread82]

Ditch the HSS for carbide. If it were me I'd run a 1/2" 5flt endmill 8500-10000rpm 75ish IPM. Should cut beautifully.

Of course if you're stuck with HSS I'd slow the rpm down by a lot. Probably close to 1600RPM and like 5IPM

 

[hvnlymachining]

Crossthread82 has the right idea, HSS has quite a bit of flex at 4xD. You're going to have to slow it down or go carbide, unless you can use a larger diameter.

 

[rk9268vc]

Ditch the HSS for carbide. If it were me I'd run a 1/2" 5flt endmill 8500-10000rpm 75ish IPM. Should cut beautifully.

Of course if you're stuck with HSS I'd slow the rpm down by a lot. Probably close to 1600RPM and like 5IPM

wow really only 1600 rpm? i have never tried that slow, i was under the impression i wanted to use all the rpm ive got in aluminum
This mill only does 4300 rpm

i will have to give it a try and update, thanks

 

[MaxPrairie]

Typically, more flutes > thicker core > more rigid tool. If the cuts are already light the next thing I do is drop the rpms. Then I increase the feed to get more pressure on the tool. Often you can go above or below where the harmonic is happening. Pulsing the spindle also helps break up harmonic rhythm.

 

[crossthread82]

wow really only 1600 rpm? i have never tried that slow, i was under the impression i wanted to use all the rpm ive got in aluminum
This mill only does 4300 rpm

i will have to give it a try and update,

Are you doing this on a bridgeport? Yes max rpm for aluminum but that's only if the rigidity of your tool and workpiece can handle it also when most people say that they are referring to carbide tooling. If you're doing this on a cnc bridgeport you can crank the rpm up and down while it's cutting to damp out some of the vibration.

 

[rk9268vc]

Ditch the HSS for carbide. If it were me I'd run a 1/2" 5flt endmill 8500-10000rpm 75ish IPM. Should cut beautifully.

Of course if you're stuck with HSS I'd slow the rpm down by a lot. Probably close to 1600RPM and like 5IPM

man i love this forum, i learn so much stuff

1600 rpm was still screamy for me

winning feeds n speeds
300 rpm (three hundred) and 5 in/min

it is whisper quiet and the finish is awesome.
basically runs like a bridgeport in low gear, and takes a million years, but it is hugely better than what i was doing

thanks guys!

 

[rk9268vc]

cycle is kinda funny too, i rough with a 3/4" shear hog at 5in^3/min MRR and then come in with this guy and go turtle mode.
parts are beautiful though, and right in spec going so slow

also forgot to mention, i tried going conventional instead of climb milling, but at the 5in/min it didnt make much difference that i could tell