304 stainless

[ihavenofish]

so i was milling some 304 stainless today.

1st i used a fly cutter on the surface. 500rpm, 1.75" diametre, 0.01" depth at 7 ipm. cut perfectly with no coolant. good finish.

then i took a 1/2" 4 flute variable flute end mill, tialn coated. ran 2500rpm, full width, 0.05" deep at 20ipm. no coolant again, cut great. did a side cut with the sam emill at the same speed, about .08" radial depth, .25" axial. again cut perfectly. also tried some slower cuts with coolant and they were fine as well.

so, i wanted to cut a circle pocket. used a 1/4" bit at 3000rpm . was set to cut 0.25" depth, 0.0625" width, 5ipm. i used coolant. the tool plunged to depth at 1ipm fine, then promptly glowed red hot and broke as it began the circle. it didnt even move more than .02" before breaking.

what have i screwd up? did i hit a sweet spot with the 1/2" tool that i just cant do with the 1/4"? the cut i made was within the manufacturers recomendations and well within the capabilities of the machine. this machine is limited to 3000rpm unfortunately. what speed should the 1/4" bit run at?

[ihavenofish]

well, ill answer my own question maybe. i found some "generic carbide recomendations" for 304 stainless.

1/4" bit
4 flute
tialn coating
1/4" depth
1/16" width
90sfm - 1400 (my first possible mistake)
feed rate - 11ipm (second mistake)
flood coolant

so it seems i did indeed his some sort of HSM sweet spot on the 1/2". i need to be going slower rpm with more aggressive feed for the 1/4" to work well with only 3000rpm.

make sense? seems to explain the overheating and glowing tool - its just rubbing on the work, not cutting.

[Geof]

You discovered that stainless steels work harden.

Small diameter cutters can be problematic on stainless because it may be difficult to take a chipload heavy enough to get beneath the work hardened surface produced from the preceding cutting edge. Under your first conditions all you did was polish the stainless to a very hard condition which simply burnt the edge off your tool. Very easy to do even with larger size cutters if you don't make sure they are making a healthy chip.

I have a question about the conditions you list in your second post; tialn cutter and flood coolant? This is a bit contradictory; this type of coating is intened to be run dry to allow it to perform correctly as it needs the high heat generated in the cutting zone. With flood coolant you do not get the heat not to forget you also get thermal shock which can cause chipping of the cutter.

Of course with smaller cutters and small chips that do not have the mass to dissipate the heat it is possible to overheat the cutter if it is run dry. One approach to alleviating this problem is to reduce the radial depth of cut and increase the feed even more but this can be a bit dicey with a not-very-strong cutter. It is also more or less impossible when interpolating a hole. Sometimes for holes in stainless it is better to drill first then spiral out at full depth with the milling cutter so you are cutting on the flank of the cutter not the tip.

[BobWarfield]

Geof's right, and no doubt it work hardened.

Just for fun, I ran all three of you cutter scenarios through my machinist's calculator. You were very closer on the first two, but your feedrate is too slow on the 1/4", which would result in too low a chipload and the work hardening problem Geof mentions.

FWIW, here are my results:

For the flycutter, you ran 500 rpm at 7 IPM. Assuming the cutter was carbide, the G-Wizard recommends 900 rpm at 12 IPM. I'm going to guess maybe you didn't use a carbide cutter? If it was, it should be sped up.

For the 1/2" 4 flute, you used 2500 rpm at 20 IPM. G-Wizard recommends 2300 rpm at 22 IPM. You're very close on that one.

The 1/4" 4 flute is the problem. You used 3000 rpm at 5 IPM. The recommendation is 3000 at 14.4 IPM, almost 3x the feedrate. The plunge would typically be about half that, maybe 1/3 for a delicate endmill. So your 1 IPM plunge may be too slow as well.

So many different combinations to keep up with, that's why I wrote this little piece of software.

Cheers,

BW

[ihavenofish]

thanks guys.

goef, the second post are recomendations from niagara cutter as "starting points" for generic carbide. they do inded say to use flood coolant on the tialn ones, but also are recomending a seriously slow surface speed.

it does seem though, and bobs numbers point out as well that its less the surface speed giving issues, but the weak feed per tooth. also makes sense with a test i did a while back with a 1/16" 4 flute where i kept the feed constant, and just dropped the rpm until it stopped "smoking" the coolant.

well, that was a $12 lesson learned anyhow