high material removal rates 6061

[urbanimports02]

just curious what others are doing for high material removal rates on the nm-200 mills? i have a series 1 with 4000rpm ac spindle and tall column. i bought one of the new glacern 3/4 indexable end mills with 3" loc, and it jumps all over the place even at shallow doc and slow feed rates. i bought the aluminum specific inserts with it and expected it to out perform the 3 flute carbide aluminum cutter i currently use. maybe the 3" loc is too long? i am sure the tall column is not helping with rigidness. right now my best option is running 1/2" 3flt carbide aluminum cutters running at 4000rpm 50%doc and woc at 30ipm or up to 20ipm when using the 1.5" loc that i need for some parts. i have run faster, but broke tools. many parts i do require 100ci of 6061 to be removed/pocketed from each, so i am looking for gains here. what do ya think?

[kvom]

I plugged in your numbers into G-Wizard. For the .75" 3-insert face mill the aggressive setting with 100% axial engagement:

4000 RPM DOC-.19" feed-75 MRR-10.67 ci/min

However, that yields a HP rating of 2.24, and I think it's unlikely that you'd really get that from the 3HP motor. Reducing the feed rate to 40 reduces the HP requirement to 1.2 and the MRR to 5.69.

For the 1/2" 3-flute endmill the aggressive numbers are:

3522 RPM, DOC-1.36 feed 14.5 MRR 9.83 HP-2

If you reduce the DOC to .25 then:

4000 RPM feed-38 MRR 4.8 HP-1

Conservative setting has feed-16 MRR-2 HP .42

One of the things G-Wizard brings out is that a larger DOC with slower feeds give a faster MRR. Face mills are often limited to shallow DOC depending on the insert geometry.

Assuming that that 1/2" carbide endmill is expensive, you might start out with the conservative feed and increase gradually until it complains. The G-Wizard settings limit the deflection is less than .001" at the tip, which is the danger point for breakage.

All the calcs I did above assumed full width cuts. For pocketing and 60% axial engagement the feeds would increase.

With the .5" 3-flute at 1.5 DOC and 62% engagement:

2888 RPM feed-16 MRR-7.8 HP-1.6 (aggressive setting)
2475 RPM feed-6 MRR-2.8 HP-.58 (conservative)

So full depth pocketing should work at somewhere in that range.

[urbanimports02]

i have run a lot of those settings in the past, but i think i am limited by machine rigidity. my insert EM is 2 flute btw, and when i ran it at .190 doc 20ipm, it chattered all over the place, so could not ever dream of 40 or even 75! i guess the 3 flute would reduce chatter, and so would a shorter EM (mine is the long length) but glacern does not have a 3 flute. i ran my 1/2 3 flute at 4000rpm 30ipm .310 doc last night and she bogged then snapped the em. same experience in the past, so i run it at 16-20ipm max to make sure i finish the job with tools still intact. that em was getting dull however and i was getting chatter from 15ipm through 30ipm. tried everything in between to make it go away during full slot, but she just kept making racket. my machine has the tall column, so the vise is on top of a large 10x15 angle table, which is rigid, but not helping likely. i have not had the guts to try full depth cutting, although i hear it works great. 1.5" doc full slot or even 50-60% scares the tar out of me even at the slowest feeds, at least with this machine. also, i think my motor is rated at 2hp, not 3. thanks for the help

[DMF_TomB]

i have a series 1 with 4000rpm ac spindle and tall column. i bought one of the new glacern 3/4 indexable end mills with 3" loc, and it jumps all over the place even at shallow doc and slow feed rates. i bought the aluminum specific inserts with it and expected it to out perform the 3 flute carbide aluminum cutter i currently use. maybe the 3" loc is too long?

.... right now my best option is running 1/2" 3flt carbide aluminum cutters running at 4000rpm 50%doc and woc at 30ipm or up to 20ipm when using the 1.5" loc that i need for some parts. i have run faster, but broke tools.

Parameters
End mill 3/4" dia. 3 insert
3" LOC
at that length with a Stickout of 3.13" from collet
4000 rpm
max DOC 0.083"
Feed 62 ipm
Hp 0.96
Force at end is 42 lbs
.
.........with
1/2" dia 3FL end mill
1.5" LOC, Stickout 1.63"
4000 rpm
max DOC 0.195"
WOC 0.500"
Feed 55 ipm
Hp 1.35
End force 59 lbs
..... all max recommendations are often reduced 50%
......... off course there is a limit on your machine's hp and what your machine can take (if it is very tall / less rigid.). A Series 1 Bridgeport type milling machine usually starts vibrating at over 1 hp used by an end mill.
........ A HSS End mill only 2 dia long or shorter is best for high removal rates. So a 1/2"dia 2 FL end mill 1" LOC can take 0.56" max DOC (more than your machine can handle). With aluminum get end mills made for milling aluminum

[urbanimports02]

so what you are saying is, i will never get my 3/4 2 flute insert EM to out perform my 3 flute solid carbide aluminum specific 1/2" EM? based on my experience, and both of your posts, looks like the 1/2" EM wins out, unless i have more rpm, more hp, and more rigid machine? btw, this machine is probably less rigid then a series 1 bp. time to rub my pennies together for a new Sharp!!! so far i get best results using 1/2" 3flt at .250 doc, .250 woc with ocassional .500 woc at 4000rpm 20ipm without braking tools. i was hoping i could improve it somewhere. so would running my pockets at higher step over help? based on what you spec out, should i just run it at .500 or 100% woc? that would reduce number of paths, thus shortening cycle time... i have backed off the travels to accommodate for the occasional full slot, as that is where it would break, so maybe just run it all full slot right? at full slot she sounds like shes working pretty hard, not sure i trust that for 75-100ci removal... thanks

[DMF_TomB]

so far i get best results using 1/2" 3flt at .250 doc, .250 woc with ocassional .500 woc at 4000rpm 20ipm without braking tools.

parameters
DOC 0.250
WOC 0.250
Feed 20 ipm
= 1.25 cubic inches per minute
in general Aluminum has a machinability rating of 4 which is 4 cubic inches per minute per hp so
1.25/4 = 0.313hp
at 524 SFPM with 0.500 dia end mill at 4007 rpm
the end force on cutter 13.8 lbs (torque 3.4 in lbs)
.
you machine may not take more hp and a higher cutter end force. basically at
1) high speeds an end mill has less end force and torque.
2) at a slower rpm to remove the same cubic inches per minute you need a higher DOC and a thicker chip so then the cutter End Force and torque is higher
.
ultimately a machine can only take so much force and torque before it deflects and vibrates and chatters. so carbide at higher speeds is better than HSS at slower SFPM and thus higher end force and torque to remove the same cubic inches per minute. but you might end up with a smaller diameter carbide end mill at high speeds to match what a large dia HSS end mill does at slower speeds
..... some end mills made for aluminum are more efficent
Shear Hog
......some claim 6 cubic inches per minute per hp instead of 4 or 150% higher metal removal rate per the same hp due to a sharper better designed inserts
..... or use end mills made for aluminum which have a higher helix , sharper rake and often polished flutes and some are coated with coatings that reduce friction and lessen metal sticking to the flutes

[kvom]

I also have the tall column with an angle table, so similar configuration. Part of the problem is that the head is retained from moving sideways by two screws, and I have in the past knocked it out of tram by a too aggressive feed. I think doing heavier cuts in the Y direction would be better.

Tool flex increases by the cube of its length, so a 3" long stickout endmill flexes 27 times more than a 1" stickout of the same diameter.

G-Wizard says that axial engagement should not be 50%. I use 60+ or 40- .