Stainless 316 - Yikes!

First real bout with Stainess 316 today. What a disaster! Rat chewed finish at all speeds and feeds (manually fed, with speeds varying from 100 rpm to about

4000 -- VFD's rock when coupled with a manual speed changer).

Carbide Tool Holder: Set first at dead center, experimented with a bit over and a bit under, many different speeds... No positive results.

Lathe/Crossslide/Chuck: Everything tight, lined up and on center, etc. A remote possibility is that one of the balls in the front bearings might be getting ready to eat itself (when I put the earphones to the front main bearing I get an occasional "hick"). Six jaw chuck zeroed, etc. Everything else, good to go.

I got alot of pretty good curly brown-blue chips going once the front surface of the work was "smooth", and all you could hear was the shhhhhhhhh of the metal parting as the carbide went through it. BUT -- the finish still sucked. It sucked less than when it *sounded* like it was getting chewed, but not by less.

Ultimately toasted an entire box of carbite insert bits, both sides for a grand total of 20 ruined tools. Best finish was with a HSS hand ground tool bit. Go figure.

Now, before everyone says 303 or even 304, I need the welding properties of the

316. I can't use the HSS bits because the steel will imbed and ultimately rust and ruin the finish (you know, the one I cant' get in the first place).

Anyone have any suggestions? I've seen some newer alloys that promise equal welding qualities and easy machining, but they aren't sold at the "small amount" shops like Online Metals.

Thanks..... As always, all help appreciated.

(same question also posted at HSM&MW BBS)

Reply to
Enders Epilogue
Loading thread data ...

Cutting 316 is a matter of experience. First, a light weight machine doesn't work well. Second, 316 is sticky, you need lots of relief to ease dragging. Third, you should use a slow speed and a high feed. Fourth, the tool nose should be 2 feed revolutions wide. High speed steel with cobalt 5% or more works very well. Carbide tools induce a lot of drag. If you must use carbide, use a negative holder to increase relief. The use of a HSS tool will not contaminate the weld. The use of a coolant also helps, but use an oil, not the water soluble type. You want to use something that lowers the chip friction. Even diesel fuel works well applied by brush. Steve

Reply to
Steve Lusardi

You didn't mention the grade of carbide you used. Machining stainless is ultra critical regards insert life. If you used a C5 or similar grade, you screwed up big time. C2 is highly recommended for stainless (Carboloy

883, for example, is a great choice).

You'll have better luck with tougher grades of stainless if you allow the machine to take a lighter feed and use considerable positive rake, but even that's a delicate balance. It's often a recipe for tool failure, too. For the most part, anything but 303 is a bitch, and nothing makes it much better. Negative rake works fine if you have the power to pull the cut, but if you don't stop at the right point, the usual result is a broken insert.


Reply to
Harold & Susan Vordos

Unless you are either facing to the center, or cutting a taper or profile, you should give the tool greater relief by setting it .005 to .010 from center. For turning and facing set the tool below center. For boring set the tool above center. The rule is - Turn below, bore above.

This is your clue that the rough finish has something to do with the cutting tool geometry. Perhaps you have a smaller nose radius on the HSS tool which is reducing the cutting force. Are you getting any vibration or ringing?

304 welds fine, as easy as 316. It is 303 that is not recommended. As a side note- it is 303 that cuts with a very rough finish as though the material was tearing. It almost sounds like you are cutting 303 instead of 316. It is carbide that causes corrosion from being embedded in the surface. Passivation will remove the carbide particles.
Reply to

I've read what the others have written, and I cannot specifically comment on stainless.

However, hand feeding an indexable tool sounds like a bad idea unless the tool is specifically made for low horse machines (sharp). What's the horsepower of your lathe? Heavy feed usually means heavier than you can reasonably push with your hand, especially at a reliable rate. I can't imagine getting my hands in line with a cut at the correct feed and speed to get many indexable cutters to work correctly. (500+ SFPM, feed at .010"+/rev in mild steel).




Reply to
Robin S.

I don't have much (hardly any) experience turning stainless, but I wanted to make some small parts out of 1/2" round 316 a while ago. Using a 12x20 Chinese machine and hand ground HSS cutting tools with a significant top rake angles worked well. The best finish I achieved was using lanolin for cutting lube. I got 2 ounce (weight) tubes of it from Enco for about $5 each.

The parts also needed to be knurled and drilled and tapped 3/8-24 and #6-32, and Lenox Pro Tool Lube was used for these operations. The parts turned out well and there weren't any cutting tool failures. My metalworking tasks are for enjoyment, not for production schedules.

WB ...........

Reply to
Wild Bill

316 is just plain nasty to work. High chromium, keep the speeds low, treat it like a hardened steel. Don't let the cut stop once it's started, you might not get it started again. Feeds, depending on how you're holding your tongue, and the way the tool is sharpened can work from very light to heavy. If you can get away with heavy, so much the better. No light cuts, that .005" finish cut will only eat the tip off your tool, leave at least .010" per side. Lube, I use plain old thread cutting oil, high sulfur, the boss uses another, he swears by his, I swear my mine. Rough finish, in my case, has always been chip scarring, use more top rake. HSS works as well as anything, and allows more freedom with angles. Keep the tool sharp, I use the diamond wheel to just polish the edge, seems to help. Sometimes, not always, grinding to a sharp point, then break the point .015" to .020" helps, more depends on the tool angles. 316 isn't fun to work.
Reply to
Lennie the Lurker

What sort of carbide bits? The best are uncoated bits designed for non ferrous applications which have much sharper edges than most others. I can get a good finish with light cuts on anything from aluminium to stainless steel engine valves with those.

Reply to
Dave Baker

PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.