PDA

View Full Version : Need Help! Turning 321 Stainless!!! (is a fail)



PoiToi
03-17-2009, 04:50 PM
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
03-17-2009, 04:57 PM
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
03-17-2009, 05:16 PM
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
03-17-2009, 05:32 PM
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
03-17-2009, 06:27 PM
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
03-17-2009, 09:05 PM
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.

Tsugami BA26L CNC automatic lathe

MikeMc
03-18-2009, 09:51 AM
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
03-18-2009, 05:06 PM
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
03-18-2009, 11:35 PM
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
03-19-2009, 12:55 PM
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
03-19-2009, 03:16 PM
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
03-19-2009, 07:35 PM
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.

tobyaxis
03-19-2009, 10:41 PM
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.

>_<

I used Cermit for Inconel X750. The insert is going to turn black. This is ok as long as you still have the tip and there isn't a notch at the DOC.

Post your Text Program if you can. I'll take look to see if there is a way to help. Without actually seeing the geometry it is tough to give any direction.

You can't post a proprietary part print, but G-Code is a Machinists Print:)

PoiToi
03-20-2009, 01:26 PM
there actually HAS been notching at the DOC.... i;ve got an insert to last at least a full bar with this program though!

G99
M123
M52
M6
G50Z.287
G0Z-.02
X.35

T3434(FACE)
M24S3200
G0X-.6
A-.02
G199A0.0F.002
G199X0.0F.002

M241
M25
M16
M10U.5
M72
M241
M73

T1212(CERMET FRONT TURN)
M03S1200
G00X.520Z-.03
G01X.32F.01
G01Z.395F.001
G01X.49F.01
X.52Z.51F.001
G00Z-.03

M03S1600
G01X0.0F.002
G41
Z0.0F.002
G01X.120F.004
G02X.200Z.040R.040F.001
G01Z.400F.001
G01X.485F.004
X.495Z.405F.001
Z.430F.0016
G40
G00X.54

M28S0
G04U.2
T1717(SPOT DRILL)
M80S2800
G50W-.2953
G0X.25Z.092
X.22
G98
G01X.14F2.0
X.13F1.0
G00X.22
M28S180
G01X.14F2.0
X.13F1.0
G00X.4

T1616(.060 DRILL)
G00X.22
G01X-.15F3.5
G00X.22
M28S0
G01X-.1F3.5
G00X.5
G50W.2953
Z.42
M82
M20

M72
G97M03S1600
T1111(LH CUTOFF.078)
M123
G99
G50W-.375
G97M03S1000
M24S1000
G00X.51Z.400
G01X.47Z.420F.001
G00X.49
M240A-.1
G98G01A.3F2000
M15
M73
G99G01X-.08F.0016
M241
G50W.375
M25
M7
G04U.2
G0X-.08Z.287T0
M56
M2



Like I said, it's a "simple" little part....

tobyaxis
03-20-2009, 02:43 PM
G99
M123
M52
M6
G50Z.287
G0Z-.02
X.35

T3434(FACE)
M24S3200
G0X-.6
A-.02
G199A0.0F.002
G199X0.0F.002

M241
M25
M16
M10U.5
M72
M241
M73

T1212(CERMET FRONT TURN)
M03S1500
G0X.520Z-.03
G1X.32
Z.395F.0015
X.49
X.52Z.51
G0Z-.03

G01X0.0F.01
G41
Z0.0F.001
G1X.12
G2X.2Z.04R.04F.0005 <Change feeds on radii to half linear feeds
G1Z.4F.001
X.485
X.495Z.405
Z.430
G40
G00X.54

M28S0
G04U.2
T1717(SPOT DRILL)
M80S2800
G50W-.2953
G0X.25Z.092
X.22
G98
G01X.14F2.0
X.13F1.0
G00X.22
M28S180
G01X.14F2.0
X.13F1.0
G00X.4

T1616(.060 DRILL)
G00X.22
G01X-.15F3.5
G00X.22
M28S0
G01X-.1F3.5
G00X.5
G50W.2953
Z.42
M82
M20

M72
G97M03S1600
T1111(LH CUTOFF.078)
M123
G99
G50W-.375
G97M03S1000
M24S1000
G00X.51Z.400
G01X.47Z.420F.001
G00X.49
M240A-.1
G98G01A.3F2000
M15
M73
G99G01X-.08F.0016
M241
G50W.375
M25
M7
G04U.2
G0X-.08Z.287T0
M56
M2

Being that this part is short you can use another tool to finish the OD and Face. Leave .002 on the OD and about .001 on the Face for finish. Try not to rip the tool out of the cut with 321ss. The burr will quickly destroy the tool tip. Also as a rule I always use half the feed of linear interpolations on radii. Facing can be tricky. Though you get a better finish going from the center out I usually start at the outside with exotic materials. Starting from the center as you are your damaging the tool tip on initial entry in 321SS. Make sure all your tools are center so there is no tiny point (You probably know this but for others reading this post). I found the parts I made from 321SS last night in a old tool box.

Notice the one with the broached 5/16 hex. That was the first. It was done originally with back turn tooling and a in house ground form tool for the radius blend. The tools were being eaten so I flipped it to Face, Spot, Drill, Bore, Broach, Turn, Form, Thread, Transfer to Sub-Spindle then Face, Break Edge, Bore the 45 degree with a larger circle tool B-Bar.

Next was the longer part. That remained a Back Turning because of the Internal Bores, Counter Bores, and Grooves. What a PITA.

The largest of the three I did on a standard cnc lathe but it too is 321SS.

I will see if I can locate that Program but it is pretty deep in the back ups and may even be on 3.5 Floppy.

PoiToi
03-20-2009, 04:32 PM
damn, those are nice lookin parts :)

we also dont have hi-pressure coolant, so i have to stop the machine every 25-50 parts and clear the birds next out of the way...

one other thing, i tried to face the front of the part from the OD like you recommended, but i cant seem to get it right.

I tired putting in:

T1212(CERMET FRONT TURN)
M03S1500
G0X.520Z-.03
G1X.32
Z.395F.0015
X.49
X.52Z.51
G42 <---------here
G0Z0.0

G01X-.02F.001
G41
G1X.12
G2X.2Z.04R.04F.0005

but that just made the part shorter by the Nose radius....
this seems to be right??

tobyaxis
03-20-2009, 04:46 PM
damn, those are nice lookin parts :)

we also dont have hi-pressure coolant, so i have to stop the machine every 25-50 parts and clear the birds next out of the way...

one other thing, i tried to face the front of the part from the OD like you recommended, but i cant seem to get it right.

I tired putting in:

T1212(CERMET FRONT TURN)
M03S1500
G0X.520Z-.03
G1X.32
Z.395F.0015
X.49
X.52Z.51
G0 X.55Z-.05
G41G1X.505Z0.0<<<<<<<<<<G41 for face
X0.0
Z-.05
G40G0X.55

G01X-.02F.001
G42>>>>>>>>>>>>>>>>>>>>>G42 for turning
G1X.12
G2X.2Z.04R.04F.0005

but that just made the part shorter by the Nose radius....
this seems to be right??

One thing I forgot to mention is that you should call tool nose radius compensation in a linear move. Rapid within 1.5 times the nose radius, then call comp in a single linear move (just X or just Z). If you have a book look at the TNRC (Tool Nose Radius Compensation) designation for the KEY MAP. G41/G42 may be different on your Machine Tool Configuration.