Turning 4130 steel?

[Pontiff51]

Hello all. My problem is turning a tube 35" long, .812 ID with a .077 wall thickness. I worked with the machine seller over 6 weeks to finally get it running without chatter. The machine is a brand new Daewoo 2500 dual turret. I'm using a steady rest, hydraulic and self centering. RPM is 1350 Feed is .0085 IPR and depth of cut is .060 roughing and .015 finish. The finish is pretty good but I can't get the chips to break during roughing or finish cut. I get 8 to 12 inch long chips that are like springs. I have thousands of parts to mfg. and I know it's only a matter of time before the steady rest tangles one up. I am machining these parts on a hardened arbor. When I ship a few hundred parts to my customer I'll be able to shave some time off these parts (right now 19min) by doing some R+D with inserts and speeds and feeds. If anyone has machined 4130 before and has any ideas how to break a chip, I hope you'll post your ideas. Thanks.

Similar Threads:

• turning 4130, 4140
• Questions about 4130 chromoly steel
• Need Help!- Milling 4130 Steel
• RFQ: 4130 turning work
• 4130 Steel

[WOLOG]

Change your roughing insert to a positive geometry rather than a negative geometry. Negative inserts are not good for thin walled parts due to push off and such. Play around with your feeds and speeds to get a tight little chip. I cut 4140 HT all day long but you have to push hard to get a chip. The positive insert will shear the material rather than rub it raw which leads to stringy shavings. How do you like the 2500? Is it the TL or the TT? I am thinking about buying a TL2500.

[HuFlungDung]

If you are still in an experimenting mood, I'd recommend that you try the Iscar cutgrip tooling. In my experience, it does not necessarily break the chip, however, they can roll the chip into a nice smooth, tight coil about 3/16 to 1/4" diameter, and the coil may break when about 6" long.

Do the cut in one pass. The Iscar cutgrip is capable of excellent finish at a feedrate of .01 but be aware that setting of the tool is critical to prevent chatter. The cutgrip insert leans ever so slightly away from the cut direction due to the force of cutting, and this creates the insert clearance. So the tool must be set so that this tipping of the insert does not cause it to hog in along the broad nose. Only the corner does the cutting.

I used to turn .350 dia 304 stainless tubing down to .245 OD, leaving a .005" wall thickness with these inserts, one pass only. I also used a mandrel inside the tube for support. Turned length was 5.5", and cnc made it possible to program a gentle arc to counteract the flex of the part, as I had no steady nor follower for this process. I turned several hundred of these, finally I got smart and had tubing custom made for the application

[Pontiff51]

thanks guys, i'm going to check out iscar's tooling this week. my customer is our uncle sam, he ain't changin' nuten'. i'm using a TL it's pretty good. hydraulics on demand is nice and quiet.

[rhundl]

I would use a #1 radius tool for chatter problems. 4130 is a little more gummy than 4140, I would probably try a .008-.01ipr feedrate. Also I would try to keep the two cuts equal depth to maintain a chipload on the tool. At .015 finish, I would assume that it wouldnt break a chip very well at all. As far as rpm I would try around 400-600 sfpm. This is where I would start but might end up right where you are. Hope this helps

[The Wolf!]

i know this is a hella old thread, but bring this one back, verses starting a new one. have problems getting good finish on face of part. i have followed suggestions from here, and im close. ok details. using Haas st30, iscar wnmg 431-tf ic3028(i know, not the best, but my general steel insert). im running about as fast rpm as im willing to go. have tryed changing how much i leave on the face to with no luck.

here is the program:
N1 T202 (WNMG)
G54
G50 S2700
G96 S750 M03
M03
M08
G18
G00 X1.78 Z0.085
G71 P17 Q26 U0.025 W0.01 D0.05 F0.01
N17 G00 X0.
G01 Z0. F0.006
X1.2485
X1.2752
G03 X1.2902 Z-0.002 R0.015
G01 X1.595 Z-0.09
G03 X1.61 Z-0.103 R0.015
G01 Z-0.265
Z-0.365
N26 X1.78
G70 P17 Q26
M09
G00 X10. Z10.
T200
M01

thanks in advance

[MetalCarpenter]

i would try finishing the face feeding down from big dia to small dia,then reposition tool and come back and finish the od turn.id say leave about .015 for od finish and .002 for face finish.feed @.0053.this has worked well for me.check out mepro too.itll help get in the ballpark for finish requirements.

[The Wolf!]

bump for help

[The Wolf!]

i would try finishing the face feeding down from big dia to small dia,then reposition tool and come back and finish the od turn.id say leave about .015 for od finish and .002 for face finish.feed @.0053.this has worked well for me.check out mepro too.itll help get in the ballpark for finish requirements.

thanks man, ill try that.

[jaimecasep]

Hi, I have been trying to leave a good fine finish in 4130 for 3 months. Last week I finally achieved the goal, my client requested 2 different parts. The first with OD 1.001 "+.0005 - 0 and ID 0.645 +0 -.008. The second with OD 1.373" +.008 -0 and ID 1.007 "+0 -.0005; the surface finish was 100 - 110. I made the first tests with WNMG432 insert for external roughing with cuts of 0.030 "and 0.010" ipr feed. For exterior finishing use VNMG331 insert with cut of 0.003, 0.005, 0.008, 0.010 and different feeds, from 0.002 to 0.005 ipr but it was not possible that all were always with a good surface finish, some were scratched and others smooth. For the interior I used a 5/8 drill to make the first hole, then a 1/2 boring bar with DCMT21.51 insert for roughing with cuts of 0.030 and 0.010 ipr feed and for finishing cut of 0.025 and 0.005 ipr feed. The problem was that chips were accumulating at the end of the hole, since I was using the full 4130 bar to finish it complete in a single operation, which was causing the insert to break. Then change the boring bar to 1/2 bar with ccmt32.52 insert with similar cutting parameters, with which I managed to give a good finish, however after 3 or 4 parts the insert was broken, and I was not achieving the surface finish the customer asked for. After many tests I came to the conclusion that I was doing the wrong operations so I started all over again, first use my boring ring to machine 1 set of jaws at a diameter of 1,001” for the small part and 1 set of jaws at 1,373” for the large part. Then mount a new jaw set on the chuck and start machining the parts. For roughing, use WNMG432 insert with 0.030 cuts and 0.012 ipr feed. For the finish I decided to use a thread insert holder, it seemed a little crazy what I was trying to do, but I still tried, for this I used the thread insert (photographs attached) with a cut of 0.010 and 0.003 ipr feed. Which brings me a big surprise, the finish was very smooth and precise. For the interior, used the 5/8 bit for the first hole again. Then I cut the parts leaving material for face finishing (0.005). After finishing all the parts, small and large, changed the jaw set to the ones I had previously machined, lower the chuck pressure to 100psi to avoid deformation, then start the program with the face finish, then for inside used a 1/2 boring bar with DCMT21.51 insert, for roughing 0.030 "cuts and 0.005" feed, for finishing use 0.020” cut and 0.004" feed. The jaws previously machined, helped the chips were ejected from the back and did not accumulate, so that the insert is no longer broken, thus achieving an excellent smooth and precise finish (photos attached). Thus, we deliver the product to our client with the required specifications. I hope this can help you too.

Greetings from Ciudad Juarez, Mexico.