What's new
What's new

316 stainless parting problem

ezduzit

Hot Rolled
Joined
Jun 27, 2013
Location
Marina del Rey, California
Need advice on 316 parting issue.

Bar stock is 3" OD. About 0.9" length of working end has been turned to 2.70" dia. 2.00" dia hole has been bored to a depth of ~2.00". After turning the features of 1 piece into the working end I tried parting using a (MSC/Chinese) 3/32" thick x 1/2" wide HSS parting blade in my Aloris AXA holder. Speed seemed about right, but blade dulled after producing about 1/16" depth of cut. After resharpening I could not make any progress as the material most certainly had work hardened.

I would have used my other Aloris parting tool with 3/4" wide blade (Aloris #SGIH 19-3) with 1/8" thick replaceable carbide insert, but the installed insert felt dulled from previous use and I could not find spare inserts. Lathe is 12" x 35" Logan. Thought of dressing the 1 insert on a diamond wheel, just so I can finish the job. But don't mind ordering the right stuff, even though it would delay completion.

The bar stock must not be removed from the chuck, as I would never get things concentric again, and I have 3 more parts to get out of this setup. All the other machining so far has gone well, using brazed and insert carbide. But I messed up attempting to part with the HSS blade.

Photo shows an aluminum bar chucked in the tailstock to catch the parted off workpiece. The barely started parting groove can be seen in the third largest of the stepped bar OD.

What are my options on how to proceed with parting the work hardened material so I can save the work that's already been done? All comments welcome.

 
Carbide is certianly the way to go, as you might have learned already. The wider the insert, the more force you will put on the part, for no real gain. The slower the feed, the quicker the part will work harden. Too fast of feed, and of course you'll get breakage, and/or shift your part. In our CNC's we go with a .093-.125 cutoff tool. Kennametal M45 or Iscar IC807 grade, and flood with coolant. Consistant feed at 150sfm approx. without any issues. At home in my lathe, I use Aloris as well. The cutoff blade works like crap, so I understand your perspective. At home, I'll make my part, band saw it off, and face the length into spec. It's only three parts.
 
Let's see, you're trying to part a 3" dia piece of 316 in a 12" lathe. Problems, I see lots of them.

My 15" lathe is barely big enough for a project like that, and I've done several. You just don't have enough rigidity in that lathe for that sort of a cut.

You certainly don't have the rigidity for carbide, it takes too much cutting force. I use a "T" type HSS parting tool for jobs like that with OIL and lots of it. You have to make a cut in 316, you can't let it rub or it will work harden before you get the tool out. IMHO, you should be using an 1/8" HSS tool with a good cutting oil at 80 or less RPM. Even with that, you're going to watch your lathe or it will be dancing across the floor. If you get chatter, drop the RPM and don't power feed, you can't feel a thing.

Have you thought about changing material?
JR
 
I would try a live center in the tail stock to steady up the part, if nothing else a slug of metal center drilled to fit live center and cover end of part. When you get close, you will just have to tolerate the finish. Keep the HSS sharp, slow speed, firm feed with oil. Best of luck.

please edit: when getting "close" to cutting thru, back off center and the chatter will be what it will be.

this will work: if you goof up how true the part is running in the chuck, or if you go band saw method, use 4 jaw chuck to true part again. if you only get part the way thru with parting tool, pull out just as much blade as necessary, from tool holder, as you go. best of luck.
 
Last edited:
Thanks fellas.

The depth of cut for parting is 0.35" (2.00" ID and 2.70" OD). The lathe feels up to this job. If you look closely at the photo you'll see the parting groove leaves a 0.050" thick flange and a 0.050" wall protruding cylinder. It would be desirable to not have to try to hold such a flimsy part, for a secondary cleanup operation, if I can successfully part it cleanly. And, if I remove the bar from the chuck, to bandsaw it off, I will lose my concentricity for the remaining parts. And I'd prefer to save the time I already have in this.

316 stainless is being used because it is up to the rigors of a saltwater environment and is what I have in my inventory. The (replacement) parts are mating bearing races for a cruising sailboat's obsolete roller-furler, which is under great pressure, but operates at very slow speed.
 
I think I see the problem...

:) You're right. The math isn't that hard to do. I'm embarrassed to say that I don't know the RPM, just that the results of all the other machining seemed OK, though the rest was done using carbide. The lathe has the variable speed drive and I must admit to simply eyeballing the results.

Some time ago I bought a cheap little digital tach just for this purpose, but that I've never tried. Maybe now is the time to press it into service. Picked up the lathe and mill a few years ago and, at 74, I'm still trying to teach myself machining. Appreciate patience and the help fellas.

Just got off the phone with MSC; ordered some inserts for the 1/8" wide parting blade, also a 3/32" wide blade with inserts for the Aloris holder and some inserts for a 3/4" boring bar. Supposed to be here Monday.

I'm going to try parting with a fresh insert and see if I can get through the work hardened surface OK. Don't have a coolant pump but have had some small successes previously using the squeeze bottle with soluble oil & water, but on smaller parts.
 
OK, first thing is to fix your location. State is required, it's the rules.

Second, new parting blades aren't going to help you if it's already work-hardened. That thing will sing like a bird and you'll crank on the handle so hard that you'll probably move the part.

Face off what you've done and start over. Go down to the big box store and buy a gallon of Rigid pipe threading oil and put it in your squeed bottle. I've machined litterally tons of 316. Not my favorite, but lots easier than any high nickal stuff.
JR

BTW, if you've got a 4 jaw chuck, switch to that. I'm also guessing that your 3 jaw is worn and only gripping at the back.
 
The oil is easy to obtain. Hope I don't have to hacksaw the thing off! Same with anything that involves changing the setup, like replacing the 3-jaw chuck, which is a POS and is grabbing only at the back. Hope JR is wrong about the new parting blades not working! :(

Not sure why the location wasn't there.
 
You will end up,with a nasty burr on the inside Bore so the job will need a second op of some sort to clean that up, I would consider making the job a little longer and cleaning up the face after parting off.
With the situation as is, I would get your new parting tip and lots of straight oil lubricant, hydraulic oil will do, move the tool about 3/4 of the groove width towards the chuck, set the speed to 100 feet per min and make a new cut down to and deeper than the existing depth,don't let the tool rub and lots of oil, back the tool out and move across to original position and finish the part off. In this way the amoun of work hardened metal,is limited.
 
You need to talk to Curtis.

latheinserts.com

He will fix you light up...no guessing...MSC sucks in that regard...they are just good at selling stuff.
 
...move the tool about 3/4 of the groove width towards the chuck, set the speed to 100 feet per min and make a new cut down to and deeper than the existing depth,don't let the tool rub and lots of oil, back the tool out and move across to original position and finish the part off. In this way the amoun of work hardened metal,is limited.

Ooooo, this sounds doable.
 








 
Back
Top