turning 13-8 stainless

[revan555]

I am turning and milling 13-8 on a tsugami and not having much luck. i've always been able to cut everything in one pass but this shaft is going from 1" diameter to .4" so I don't think it will be an option. I've tried deep cut shallow cut slow feed(.006) and high feed (.013) and the chip is the same. It mills great though, i'm thinking about using an endmill with the main spindle turning and possible milling it down then finish turning. anyone done this?

[gizmo_454]

I am turning and milling 13-8 on a tsugami and not having much luck. i've always been able to cut everything in one pass but this shaft is going from 1" diameter to .4" so I don't think it will be an option

I thought that swiss type machines were supposed to be able to cut materials down like this in one pass. I am confused...

I've tried deep cut shallow cut slow feed(.006) and high feed (.013) and the chip is the same.

0.006" feed is "slow"? 0.013" is "high"? Did somebody slip a 30HP spindle and drive in your Tsugami? Our E32 Citizen grunts with a 0.004" feed with a 0.150" deep cut in 304 Stainless. And that has a 7.5 HP main spindle. Our lathe with a 15 HP spindle would be pushing it to handle 0.006-0.008" feed at that depth of cut. I certainly wouldn't think of trying to push our swiss to 0.013" feed in stainless!

Did you try a different insert, grade, and/or chipbreaker?

Mike

[MCImes]

I agree with gizmo that .006-.013 ipr is a very high feed for a swiss.

I was turning aluminum from .75 to .312 in one pass. My spindle load was maxed and I found that lowering my RPMs lowered spindle load much more than lowering feed, so try turning slower. Also my main spindle on a 19mm machine maxes out around .004 per rev before I hit 90% load, so try lower rpms and feed.

The highest feed ive ever used was .008 and that was in a 32mm machine with soft steel...

also if you have stringy chip problems try using the custom macro chip breaker I posted here: http://www.cnczone.com/forums/fanuc/...tom_macro.html

it works like a charm and you can have any size chip you want. It might not work too well if you have to hold <.0005 total tolerance, but its worth a shot.

[revan555]

thanks guys, and i should have mentioned when i was feeding that fast i was taking a very low doc, i will try these suggestions. thanks again

[lukehonor]

On my Tsugamis, BE20 and SS32, i've taken .150" depth of cut moving at .006" per rev with no problems on 304 S.S. I had 1250 PSI of good cutting oil right at the edge and I flew at around 4000RPMS (don't remember exactly). With the SS32, on soft steels and non-ferrous, I've machined .300" depth of cut at 900 SFM at .01" per rev. THis is done daily on our machines.

I just finished running a job on our SS32. We were machining 416 S.S. I used a DCMT 32.52 roughing insert at 900 SFM. I was feeding at .009" per rev. I took the stock down from About 1.110" to .517" in 2 passes. This is standard operating procedure for me on 416 S.S. or any other "soft" steel.

I've been machining like that for a long time and have never phased out a machine or pushed the spindle too hard. You can push sliding headstock machines MUCH harder than a fixed headstock lathe.

Your 13-8 PH is going to be a problem, though. When I've machined it, the cutting changed from bar to bar and stock lot was a HUGE difference. We ended up using Sandvik WNMG 432 1115 to rough and WNMG 1025 to finish turn. We cut at .05" DOC. Slow surface footage and high feed rate was how we turned the part. We were never able to acquire good chip control.

Good luck to you!