Help Cutting 316 Stainless on CNC

[Cartierusm]

I've never had good success with cutting stainless, lately I've tried to stick to 303 which cuts like butter, but now I've got to cut 316.

I'm using a home made Bridgeport CNC, very accurate, and trying to cut 316 Stainless Plate 1/4" Thick. I'm using a new 4 flute Solid Carbide End Mill, 5 IPM at 800 RPMs, .07" DOC. I don't get more than 1/2" - 1" before the thing glows red and that's with HEAVY Mist coolant, brand new bit is toast. Is it possible I'm going way to slow. I just hate to waste another bit. What should I be doing? THANKS I NEED HELP!

[spotter]

you might want to try flooding it with coolant, as well as going faster.

[REIDMANS]

Hi get your self a coated hss ripper cutter with cobalt in for roughing and finish using your carbide. I use rippers for roughing most things they use less power break the chips better and are cheaper than carbide. But flood the cutter with plenty of coolant.

[kling8]

I agree with the others flood the coolant, but I would say for sure your speed is too slow, and your feedrate is probably off too. One way to check your speeds and feeds is talk to the tool rep that you bought the tool from and see what he recommends,
kling8

[Geof]

What is your cutter diameter?

With a coated carbide cutter I would run at about 100 to 150 FPM (this is a bit conservative I think) and if the cutter was large enough to take it, something like 0.003" to 0.005" per tooth. 316 work hardens and unless the feed per tooth is deep enough to get under the hardened surface from the previous cut all you do is polish the stainless to a very hard surface.

Using coolant is debatable; with coated carbide running under the correct conditions it may be better to go with a strong air blast, coolant whether it is mist or flood causes thermal shock to the tool and can cause premature failure.

[Cartierusm]

Thanks for the help. I'm so gun shy these days with it cause I ruin new bits in about 3 seconds.

Geof, it's a 1/2" Solid Carbide End Mill.

What I ended up doing was use a 1/2" Indexable Carbide Endmill to chew through it at 1300 RPM and 8 IPM, it got through it and the carbide index got a little chewed but then I was able to to a clean up pass with the regular 1/2" Solid Carbide End Mill and that seemed to work.

Unfortunately I don't have flood only mist, but it's a real heavy mist.

[BobWarfield]

cartierusm, stainless likes to work harden if you feed too slowly, which is probably what's killing your tools.

G-Wizard would suggest 1280 rpm (167 SFM, pretty close, Geof!) and 10.2 IPM (0.002 chipload) for a 1/2" 4 flute cutting 0.07 deep and a full slot.

You're welcome to sign on for the G-Wizard Beta Test if you need a feeds and speeds calculator. Details below.

Cheers,

BW

[Cartierusm]

Cool, thanks, I'll check it out.

[ctate2000]

Counter to the others recommendation (as usual I like to be different) I would suggest using a good quality HSS end mill. HSS will be dead sharp if you are using quality tools. The keen edge will decrease the size of the primary shear zone thereby decreasing the volume of heat introduced into the work piece. Heat promotes chip welding. Chip welding increases the rake angle of the tool which increases the amount of energy required to move the chip. More energy means more heat and you find yourself in a cycle that spirals out of control until tool failure.

Climb cutting will also help. The thickest portion of the chip is formed first which allows more mass to absorb the heat, it also diminishes heat caused by friction. Tools rub when you are conventional milling.

Of course this applies to carbide tools also. I suspect the issues you were having to be caused by chip welding. If you have to use carbide try decreasing the cutting speed and increasing the chip load to help decrease the heat in the shear zone. Cutting speed has more effect on heat that any other factor.

[Cartierusm]

Thanks I'll keep that in mind next time I cut stainless, hss is way cheaper too.