Need Help!- Turning 321 Stainless!!! (is a fail)

[PoiToi]

Hi all, I have a deceptively simple little part that I'm having a heck of a time getting to run well.

the part is out of 321 Stainless(contains a titanium stabilizer, so I've read). It's 1/2" OD, most of that is turned down to .200", except for a .020" wide "head" that's left at the stock size. it also has a cross hole (which is the one thing that seems to be working OK)

my major problem is that it's just eating tools. I've tried running it from 160 to almost 300 SFM, and feeds from .0004 to .002 per rev. if i go slow, the material is so gummy that the chip doesnt break, and wraps around the part messing up the x-drill. does anyone have reliable feeds and speeds for this stuff?

also, i'm running the .020 wide head out, as a good finish is needed on the face. this keeps getting bent outward when I turn the back end. i've done such stuff in 303 with no problems, so I imagine when I get the feeds and speeds right this may go away. any suggestions??

thanks in advance!!!

[tobyaxis]

321 SS is a pain. Try using Cermit Uncoated Inserts from Sandvik .004 TNR. These are what I used and they worked like a charm.

Just try not to pull the burred edge back through the guide bushing because it will chip the carbide seats on the bushing.

I did end up using a G71 Rough Turning Cycle though, which is why I mentioned the bur chipping the guide bushing seats.

I hope you have better luck than I did.

[PoiToi]

what sort of feeds and speeds did you end up with?? If i run one part and take the tool out, the edge is completely cratered away. (at least that what it looks like to me)

I should've mentioned i'm using Utilis tooling, and we dont have time or $ to try a whole lot else.
i will keep that in mind though if this ends up being a failure pile in a sadness bowl. =)


the back turning tool i'm using has a sharp corner, i'll put a little radius on it and see if that helps any. the face has a .008 TNR, and it looks great, except for the bending.

[tobyaxis]

Originally Posted by PoiToi what sort of feeds and speeds did you end up with?? I should've mentioned i'm using Utilis tooling, and we dont have time or $ to try a whole lot else. i will keep that in mind though if this ends up being a failure pile in a sadness bowl. =) the back turning tool i'm using has a sharp corner, i'll put a little radius on it and see if that helps any. the face has a .008 TNR, and it looks great, except for the bending.

This was like 10 years ago LOL. I just remember what I did to solve the problem of the material eating the tools.

I would say off the top of my head 2500 rpm @ .0005 ipr, Doc .05.

My parts were short with the max diameter of .7 with a 1/2-20 thread and in the center I had to put a 5/16 hex (used a sub program and indexed the C axis).

I tried doing the part in reverse with a back turning tool but because it was a 35 degree tool it broke down fast. So I flipped the part the other way to use an 80 degree. Then transferred the part to the sub spindle to do the rest. We had Sandvik Tool holders and Inserts. As luck would have it the Cermit insert we had was a sample from the sales guy. It was worth a try and it worked great.

It was a real PITA.

[beege]

I have a Carpenter Stainless reference book here. Says:
Turning, single point (HSS) @ 85-100 SFM compared to 303 @ 110-130, same feedrates , .007"-.015".
Drilling, 1/4" drill, 50-60 SFM compared with 303 @ 70-100, feedrates .004 IPR compared with 303 @ .006" IPR

I'm sure its not much help, though... maybe call their applications people (Carpenter)?

Edit:

On second look, you're almost definitely work-hardening at that slow a feed. Have to stay UNDER that work hardened layer, maybe >.004"/rev. I you have to take a finish pass (you shouldn't have to), use a dead-sharp tool, and slow it down. As far as breaking the chip, I use a G75 cycle to break the chip by backing away .002" for every .005-.010" of feed, but I don't know what luck you'd have with the work hardening.

[tobyaxis]

Originally Posted by beege I have a Carpenter Stainless reference book here. Says: Turning, single point (HSS) @ 85-100 SFM compared to 303 @ 110-130, same feedrates , .007"-.015". Drilling, 1/4" drill, 50-60 SFM compared with 303 @ 70-100, feedrates .004 IPR compared with 303 @ .006" IPR I'm sure its not much help, though... maybe call their applications people (Carpenter)? Edit: On second look, you're almost definitely work-hardening at that slow a feed. Have to stay UNDER that work hardened layer, maybe >.004"/rev. I you have to take a finish pass (you shouldn't have to), use a dead-sharp tool, and slow it down. As far as breaking the chip, I use a G75 cycle to break the chip by backing away .002" for every .005-.010" of feed, but I don't know what luck you'd have with the work hardening.

Swiss Feeds and Speeds are way different than conventional Lathes. On a swiss we have to take a Rough and Finish Cut in one pass because you can't pull the part all the way out the other side of the Guide Bushing.

In other words if there is a Bore in a part that is done first then the OD is turned. If there are any Grooves you can either include this in the OD turning or do the OD>Groove>OD>Groove Steps.

On a conventional CNC or Standard Engine Lathe your specifications stand true, but not on a Swiss.

This will give you an idea.

http://video.google.com/videoplay?docid=-4369614827229532702

[MikeMc]

We have turned a bunch of this exotic stuff, 321, Inconol, Hastaloy, A286, etc. It does sound like the material is work hardening as you turn it. There is NO WAY to substitute good tooling. We always use Iscar or Sandvik tooling for these types of jobs, I lean more towards Iscar, but the other is good as well. With the Cermet tooling, you have got to keep the speed up, or you will break down the tool very fast. If the material is work hardening, you will have to slow the speed, and increase the feed, there is no other way around this.

I can't stress enough to you the importance of buying the very best in tooling for a job like this. They last 321 job we did needed a 0-80 crossed tapped hole, the taps alone (Emuge) cost $56.00 per tap, and we wnt through one in 100 parts. Any other tap I tried broke after two holes.

[PoiToi]

well, i've gotten a little bit further.
thanks for all of your suggestions! I'm still learning!

I got the bending problem to go away by turning the part around and picking it up with the subspindle .
also modified a toolholder we have that we have come cermet inserts for(Mitsubishi CCMT style) The first few turned out great. ran anywhere from the tool rep's recommended 375-400 SFM to 250 SFM.(at .0022/rev, taking 2 passes, rough at .09 DOC, finish at .06 DOC.) filled the whole damn shop with smoke either way (we just run old screw machine oil, i'm trying to change this as well.)...
and the cermet inserts lasted about 10 parts. Now i'm out and my boss is pissed. >_<

TiN coated .078 cutoff is also getting eaten alive. lasts maybe 4 freakin parts anywhere from 1200RPM at .0016 or 2200 rpm at .0022 while holding the part with the subspindle... I feel freakin useless.


any help?? We have like 10,000 of these damn things to make. If it would help, I will ask my boss if it'd be OK to post up a print.

at least the cross hole is still going strong! =)

[tobyaxis]

Your not useless!!!!! Mitsu's are ok cutting tools. Your DOC is too Deep for those inserts. They are only designed for .05 to .07 DOC and those Feeds are way too high. If this is what the guy told you too run he has no clue.

I hate to be this Brash, but realize this is not your fault. Your boss quoted the job, not you. He buys the Tools, Not you.

Try running the spindle slower and feed lighter than .0022 ipr.

Start at 1500 rpm and .001 ipr. See how it cuts then go from there. Never machine 321SS fast because you will burn out your tools before the job is finished. Titanium is nasty but everything can be cut.

I have a few questions for you.

1) What kind of tension do you have on your Guide Bushing? It should be set so that you can't push the material through by hand but with a brass hammer by a sharp tap.

2) What is the condition of the bar your machining?? It should be precision ground stock .0005 from one end to the other.

If these two conditions aren't met, your boss is just dreaming. You will continue to burn up and break tools.

What kind of training have you had on a swiss???

[PoiToi]

Originally Posted by tobyaxis Your not useless!!!!! Mitsu's are ok cutting tools. Your DOC is too Deep for those inserts. They are only designed for .05 to .07 DOC and those Feeds are way too high. If this is what the guy told you too run he has no clue. I hate to be this Brash, but realize this is not your fault. Your boss quoted the job, not you. He buys the Tools, Not you. Try running the spindle slower and feed lighter than .0022 ipr. Start at 1500 rpm and .001 ipr. See how it cuts then go from there. Never machine 321SS fast because you will burn out your tools before the job is finished. Titanium is nasty but everything can be cut. I have a few questions for you. 1) What kind of tension do you have on your Guide Bushing? It should be set so that you can't push the material through by hand but with a brass hammer by a sharp tap. 2) What is the condition of the bar your machining?? It should be precision ground stock .0005 from one end to the other. If these two conditions aren't met, your boss is just dreaming. You will continue to burn up and break tools. What kind of training have you had on a swiss???

Thanks for your input!! I was just trying to take as few passes as possible becuase the material work hardens so much, which is also why i was feeding so fast. it <i>seemed</i> like a good idea!
I'll try running it much slower and see how that goes. When i dropped the speed of the cermet downto 250SFM(still 4800RPM), it just seemed to last shorter. I'll go REALLY slow.

and yes, that's where my GB is set. I try to run everything like that, It works OK.
The material is good Ugine stuff, I jus tmic'd it and it varies about .001 end to end.... I've made do with much worse. =)

My training comsists mostly of teaching myself how to do it over the last 3 years here. It has worked out well, actually. I learn fast and have done lotsa things that my boss didnt think could be done on our basic machines. I klnow I'm not useless, I was just frustrated.

and i kinda DO buy the tooling. (at least, i tell my boss what I need and how to improve stuff around here, and he listens!) I've been slowly making the switch from ETCO to utilis tooling. Many here seemed to agree that Utilis was great stuff. THe only Mit. tools I have are the cermet ones, and until now thay have been kinda amazing. =)

thanks again!

[PoiToi]

Well.... 1500 RPM at .001 in 3 passes = 15 parts with the cermet.

the whole corner of the cermet for about .100 in each direction is black.... Still too much heat? WTF!!!

I'm totally at a loss here.
i should just swallow my pride and tell my boss to get it done somewhere else.

>_<

[citizencnc]

Hi there,
My shop is an Aerospace company, we have 6 swiss machines here and 3 of them running 347 ss 24/7(compare to 321 ss it's not much different as far as I know). I suggest that you should try Kennametal brand, DCGT xxxx HP or CCGT xxxx HP grade KC 5010. These are high possitive inserts designed for Aerospace high temp material. The bad thing is they don't come with "V" geometry(35 deg) if this is what you need. With these type of mat'l it's hard to break the chips, the way to get around it is create a macro path let's say feed in .010 then back up .002 with a feed rate of .001-.0015. I don't see any problem with running 150 to 300 SFM. Also coolant is a big factor of getting better tool life. We have high pressure coolant on every machine here so it help to blast the chips without any problem.
I hope this would help. Good luck.