I can't facemill 316 stainless, what am I doing wrong

Machine is a Haas TM1-P
Facemill is Maritool 2.48" dia 45 degree 5 flute with their ACK300 inserts
316 A240 plate 10" x24" .375" thick
3" of it length wise gets milled on both sides to a total thickness of 8mm, the rest is 5.5mm thick, again both sides
Holding the plate with 3 Kurt 3600 vises the entire 24" length
Using flood coolant
I ran the facemill at 600rpm at 10ipm, 2.2" stepover, .030" DOC, totally trashed the inserts after 2 passes.
I tried several combinations of going as high as 1000rpm 20 ipm to 400rpm 6 ipm, same result each time basically, 75% of my side work is stainless and I've never had a problem. Spindle load was over 100% as the inserts quickly died, 2 shattered on 1 try, I just got this facemill and inserts in the mail today so they are brand new. I have the same facemill in 90 degrees and they didn't last either but they weren't made for stainless specifically.
I ended up changing to a .75" 5 fl .125" CR EM at .60 DOC with .5" stepover, conv direction 1468 rpms started at 20ipm and had to back off part way thru to 10, pretty much trashed that mill too but it finished one side of part
Frustrated........I know I'm doing something wrong I just can't figure out what

Try turning off the coolant. Or maybe you got a junk piece of stainless.

have you tried calling maritool for operating parameters? also may be good to contact the insert manufacture that maritool has sourced the inserts, Sumitomo

i can not locate any operating parameters or what kind of edge prep in on the inserts.

best of luck

316 can have some pretty angry bark on it. I would start with thicker material and/or get your bar stress relieved.

vr6 said:

have you tried calling maritool for operating parameters? also may be good to contact the insert manufacture that maritool has sourced the inserts, Sumitomo

i can not locate any operating parameters or what kind of edge prep in on the inserts.

best of luck

Click to expand...

The parameters were included with the delivery (attached)
To some degree I don't mind running into these issues as they can be learning experiences but given I don't know where I've gone off the rails I'm not learning anything

I put a slight bevel on the raw stock prior to starting, not much but it wasn't a hard square edge

IWUP said:

The parameters were included with the delivery (attached)
To some degree I don't mind running into these issues as they can be learning experiences but given I don't know where I've gone off the rails I'm not learning anything

I put a slight bevel on the raw stock prior to starting, not much but it wasn't a hard square edge

Click to expand...

i would call sumo for help. edge prep can make all the difference, especially with stainless. maritool only offers 1 grade where sumo might have another option or better.

vr6 said:

i would call sumo for help. edge prep can make all the difference, especially with stainless. maritool only offers 1 grade where sumo might have another option or better.

Click to expand...

Thanks, I will look into that

I'm guessing you have a lack of rigidity in your setup. 10" x 24" x .375", even in 3 vises, might be pretty springy. I'd try mounting it to a fixture plate with might bites rather than vises

Teryk

Sent from my moto g(7) optimo (XT1952DL) using Tapatalk

mTeryk said:

I'm guessing you have a lack of rigidity in your setup. 10" x 24" x .375", even in 3 vises, might be pretty springy. I'd try mounting it to a fixture plate with might bites rather than vises

Teryk

Sent from my moto g(7) optimo (XT1952DL) using Tapatalk

Click to expand...

I did have 3 parallels under the plate in each vise but was wondering if it was deforming up in the middle as cut were being taken? I did try a .010" DOC also with no success

Based on Maritool's sheet you should be running 380 rpm with a feed from 7.6-15.2 ipm at the low end to 760 and a feed of 15.2 to 30.4 at the high end, if I can do math today. I would start at 400 rpm and 12 ipm. It is counter intuitive but I find inserts last longer in stainless if I take a larger chip load since I am getting past the work hardening from the previous insert and I am taking fewer "cuts" per inch of travel. At least that is my theory.

I would also look at supporting your work piece better. If you have more sets of parallels add another set of parallels an inch to the inside of your other parallels to help support the center of your work piece. If you don't have any other parallels and no scrap to make any from then some times you can block your parallels so they are spaced away from the jaws towards the center of the part to help the support middle. Or as others have said make a fixture or clamp it flat to the table. If your work piece is well supported and you are still having trouble then you might try brushing some cutting oil or anchor lube on your part.

Slow the Spindle down until it starts doing what you expect. Then adjust for MRR.

R

for some reason I would want chip load of at least .01 per insert, and less rpms,but thats me.
Gw

If the insert edge blows up, SFPM is simply too fast. Slow the spindle down, look at the recommended
number for that material, carbide tooling. I suspect it will one or two hundred RPM. Feed agressively,
do not let the cutter dwell as this material work hardens badly.