Stainless is kicking my #$%%#$

[ghyman]

I am having some severe tool life issues on a stainless job, and would appreciate any assistance anyone might be able to offer.

Setup shown here: https://picasaweb.google.com/snurfle/January102012
Details:
Material: AMS 5645 (321 SS)
Depth of cut (Z-depth): .100
Width of cut (stepover): 80% (max) , ~1.12"
Cutter: EM 1500-3F (Kyocera Ø1.5" 3-insert cutter)
Insert: XPMT 15T316 (Kyocera)
Grade: CA-2325
Speed: 240 SFM - 375 SFM
Feed: .001-.004 inch per tooth per rev

I have gone through 2 sets of 3 inserts in 2 parts.

The cutting conditions came from the Kyocera catalogue; the first piece was run at 300 SFPM and .004" per tooth feedrate.
The second was run at 240 SFM and .002" per tooth, but was dropped to appx 50% for the last 2 passes when it began to sound as bad as the first pc.

Are these the best inserts for this material given this setup?
Or, for that matter, is this the best cutter?

Any advice you could offer would be greatly appreciated.

[Geof]

I cannot comment on the inserts because I am not familiar with them but I think the speed is a bit high and the feed a bit low. Machining stainless at 0.002" per tooth means each insert is cutting in the work hardened surface created by the preceding insert.

My approach would be to take the speed down to 200fpm and bump the feed to 0.005" per tooth, maybe even a bit higher if you have the torque available.

Also lose the coolant and go with a strong air blast. In addition to work hardening badly with a slow feed you are probably thermally shocking the inserts and get micro-chipping.

[DMF_TomB]

i am calculating a cutting force of 80% of 200 lbs or about 160 lbs.
.
a possibility is part vibration and chatter is hurting the carbide inserts. i would try a short length and smaller diameter end mill and a lower depth of cut

[SSMrob]

I cannot comment on the inserts because I am not familiar with them but I think the speed is a bit high and the feed a bit low. Machining stainless at 0.002" per tooth means each insert is cutting in the work hardened surface created by the preceding insert.

My approach would be to take the speed down to 200fpm and bump the feed to 0.005" per tooth, maybe even a bit higher if you have the torque available.

Also lose the coolant and go with a strong air blast. In addition to work hardening badly with a slow feed you are probably thermally shocking the inserts and get micro-chipping.

I agree with the above.. I found that actually getting rid of the coolant helped on stainless too..

Basically it was explained to me that when machining stainless the heat has to go somewhere and with coolant the heat goes back into the part, causing work hardening of the material, but more important, work hardening of the chips then the chips are actually what cause the damage to the tool edges. OTOH with cold air or misting the chips are hot and the part is not as much.

[neilw20]

Also climb milling,will help a lot, if it can be arranged.

S/S is quite a bad conductor of heat, and you want the heat to go into the chips. Either severe flooding, or lots of air. Just a dribble and you will end up with chipped inserts. Don't recut the chips.

Inserts designed for the grade of S/S used will make an enormous difference.

Touchy stuff until you get it all working, then it is easy.
Not too much speed. Aggressive feed and careful with intermittent cuts and approach paths.

[Delw]

No coolant forsure

Just out of curiosty does your inserts wear more on the part that is closest to the center?do you get any chatter?

Personally I thing the center isnt a good Idea for heavy cuts as it will chatter and wear your inserts faster than fast.
Build a A-frame for that end. the set up looks like it can flex to much

[RCaffin]

Looking at the pics, several thoughts came to mind:
Intermittent cutting - very rough on cutters
Flexible job support, especially at the tailstock end - rough on cutters
Cutting into the hardened surface and chips - ditto
Big overhang on cutter with that coupling - ouch

Smaller diameter cutter, much more solid mount for cutter, much more solid mount for parts, more aggresive cut seem like useful ideas.

Cheers

[Bada Bing]

looks like your setup needs to be more rigid, and agree with the speed and feed changes.

[neilw20]

Now I see the pictures, wow!! Not stiff enough.
If you can lift the jig easily, it is probably not stiff enough.
Just like the tailstock.
Use a smaller cutter.
If you can feel vibration, you have a problem. Do you have a lock on the rotary axis?

[Packers]

ghyman, what is your cutting tool distributor doing for you when you run into issues like this? I do not mean to criticize you but solving applications like this should be no problem.

[Bob La Londe]

All I can say is I commiserate. The first thing I ever made on my mini lathe was a stainless shoulder bolt and nut to replace a broken pivot pin on a pocket knife my son gave me for Father's Day. I destroyed two insert bits, two taps, and one die, but I fixed it. I used a $500 machine and detroyed $50 worth of tools, but I saved that $6.95 pocket knife my son gave me. I still have the knife. I may engrave it. LOL.

[PixMan]

You've got a couple of correctable issues there. One, the inserts you are using may well be the wrong grade for a tough austenitic stainless steel like that. Looking it up on the painfully slow Kyocera website, I see it's CVD-coated carbide insert, in a grade that is primarily meant for cast irons. While it should work and the numbers you have are right by Kyocera's published data, the grade clearly isn't working.

I don't like what I see in the cutter geometry either. The inserts are vitrually straight in-line with the rotational axis, which is fine for cast iron but the opposite of what you want in a tough stainless. You need some shearing action through a combination of top rake angle (which the insert does have) and shear angle (which it has little to none.) Even with those features in place you still need a grade that works.

BTW, your coolant salesman might be in love with you. I don't know what coolant you are using or if you are using a refractometer together with the right correction factor for the coolant of choice, but that really looks far too rich.

If you have any inclination to try something different, I believe I have a cutter that would kick ass in that job. It has the right inserts for that material in it, and it's available.

It's a 1-1/2" 6-insert cutter using 10mm (.39" depth per pass capable), on a 1/2" pilot shell mill mount. Ping me if interested.