trouble with 304 stainless

Anyone have any advice on turning corners off of square 304? i am trying to turn down 1.25” 304 bar stock i am running a newer mazak cnc lathe and using a dnmg insert. tool life is very bad sometimes breaking the entire insert after just a few cycles. Any help at all will be appreciated because i can’t seem to find much info on doing an interrupted cut on 304.

I've done roughly the same operation several times and have had the most success running it dry on the roughing op.

I make a few families of parts that get interupted turning. We mill the corners off first. Live tooling or VMC.

Also get the toughest inserts. My Iscar guy recommended a "milling grade" That helped us a lot.

Big thing with interrupted cut is to keep the feed low, and nose in solid uninterrupted material when you can.
For roughing DNMG's aren't all that tough vs CNMG. I have a holder that uses the 100° side of CNMG's, that's pretty tough... then finish and do the corner with something else.
Sandvik's 2220 is pretty good, 1125 too.
In the end though, with interrupted cuts inserts simply aren't gonna last forever and tool life isn't all that predictable.

It really is helpful if you give us the parameters that are you are using
RIGHT NOW that aren't working. And the things you've tried that aren't
working.

No point in me or anybody else typing out a response and giving feeds and
speeds if its the same thing you are already doing that isn't working. Your
idea of "Not Working" might be the best you can get.


High depth, low feed. I mean LOW!!!! Already said, try and get your nose in
there, or at least really really close. 1.25" square to round is a .258ish DOC.
Getting the nose in there a bit stabilizes everything.

The dry interrupted cut is also a real thing.. Carbide can take heat.. It can
take a LOT OF HEAT.. What it can't take is a lot of rapid thermal cycling. Say
you are running 1000rpms, you are heating and cooling that insert 4000 times a
minute.. Carbide does not like that, it will take it for a while... And then
it won't.

I would use one tool with maybe a .200 to .230 DOC, DRY, and maybe .003 a rev,
maybe less. And then go to your rougher, and then finisher, which would be just
like turning round bar.

How long is the part you are machining eh?

I have a tendency to mill the corners off and make it an octagon. Or grind the corners as to have a smoother transition between cuts!

i haven’t tried running it dry i will see how that works out ty

i will have to try a cnmg i think i have one around here ty

anywhere from 4 feet to 18 feet but i’m only working about 6 inches at one end

If you are taking it down to a solid round profile then the best way is to take all the material in one pass so that your tool tip is in solid metal and doesnt have to make the interrupted cut. This was already suggested earlier. Otherwise take as much as you can in one pass but just dont expect the insert tip to last very long. Use a rougher and a finisher, I use VCMT inserts for the roughing and a CCMT for finishing. They peel the material better with the sharper rake but I only take 0.001 per rev on roughing. I also always use a center even when the stickout is short.

Good luck.
Charles

Low sfm and light roughing passes

If you can substitute 303 stainless (it is more expensive per pound), you will be amazed at how much better it machines.

ToolCat