I've got a Puma 8S. I have production jobs for a 14 X 2.0 metric thread on 304 SS. I'm single pointing ID threads 1.75 inch deep. I have lots of chatter and am breaking inserts every 3 to 4 parts. Using a Horn brand carbide bar. What's the deal?

Phoodieman

what is your feed,speed and depth of cut/pass?

I was @ 267 RPM. .0784something for the tpi of course. I called the dealer and he recommended 1900 rpm with 25 passes. No spring passes. Chatter was a lot worse. It has to be in the setup. I swept the threading bar and I have avout 5 thou runout. It's a slant bed and the tool is running parallel to that so whats up.

phoodieman

is you tool holder on center?

I will check Monday. I'll make a face cut then bring the threading tool up to see if I'm on center. Thanks....

Check Center and keep bar as short as possible.

I changed over to a lay down 3 corner bar insert. I'm grinding clearance on the back side of the tip. It's a two inch deep ID thread. I tried several different settings in Master Cam. Offset left and right... cutting in the center...taking a lot of passes (32). Taking 8 passes. Spring passes, no spring passes. .001 thou last cut. Mind you this is 304 SS ID and I'm getting a lot of shavings packing up in the back. I've got .200 in the back of the hole, so the shavings pack up in there. I want try threading from ID out, but I would have to buy a new toolbar and inserts. I don't want a left handed thread. Lot of chatter and I'm getting pissed. I sweep the bar at X zero from the chuck. The holders are a little worn, but I'm within about two thou of center. It's a slant bed and as far as I know the insert should be parallel to the bed. I'm set up turret up so the bar is upside down.

Phoodieman

try slower rpm

I was cutting at 247 RPM. I called the manufacturer and they suggested 1900 RPM. I laughed out loud over the phone. I tried it anyway and it chattered like a mofo. I'll hit it again tomorrow and see what I can do.

Phoodieman

what size thread are you doing

is your spindle going in the right dircetion where you turned the tool upside down?

The tool's not upside down. (Well if you look at it it's turned away from you in the cutting position) It's turret up configured, so to answer your question the spindle is turning the right way. I started putting a lot more passes in and the chipping of the insert went away. When I went down to 150 RPM the chatter completely went away. In the part I'm making now small chatter is not an issue, so I sped it up to about 400 RPM to get the part out the door. The thread is a 14 X 2.0 metric. It's a long throw. 2 inches in a thru hole and the other part is 1.650 in a lind hole. Time is always an issue to the bottom line and if I get that part again, I need to tweak to get the cycle time down.

phoodieman

Why not try a high performance tap?Like Dormers MTX model?

one thing we've found to work pretty well is that sometimes letting the front screw closest to the tip "float"... just have one screw holding the bar tightly at the back. of course, this assumes that you have a good fit in the reducing sleeve. Also, adding some stops to remove chips every 4-5 passes helps - like this:
(1" - 8 Stub Acme ID thread, 360 SFM=1375 RPM, 17-4 ph SST)
N5G50X8.Z6.
G0G97S1375T0500M3
X.827Z1.T0505M8
Z.5
M76
G92X.927Z-2.47F.125
X.932
X.937
X.942
X.947
X.952
G0X.827Z2.M0
(GOT CHIPS?)
M8
M3
G4U1.
G0X.827Z.5
G92X.957Z-2.47F.125
X.962
X.967
X.972
X.977
X.982
G0X.827Z2.M0
(GOT CHIPS?)
M8
M3
G4U1.
G0X.827Z.5
G92X.987Z-2.47F.125
X.992
X.997
X1.000
X1.003
X1.006
G0X.827Z2.M0
(GOT CHIPS?)
M8
M3
G4U1.
G0X.827Z.5
G92X1.009Z-2.47F.125
X1.012
X1.015
X1.0175
X1.020
G0X.827Z.5M9
X8.Z6.T0500
M1

PDI-Curtis, what is the thinking behind floating the front screw? Just curious.

sometimes letting the bar float will help reduce chatter... not a guaranteed fix, but if the bar is allowed to flex a very small amount it often helps us when this problem comes up.

It lets the bar find its own center

have you tried a different approach to programing ?

G76P010060
G76X?Z?Q20P20F.07813

I'll give your screw float tip a try.

We are making some 3.5 - 4 ACME nuts right now, going 4" deep, with a 1-1/2" dia. Vardex laydown bar. The material is a low carbon structural grade, ASTM A572 Gr 50 (yuck).

The bar has been cut down of course and choked up in the bushing/holder so that there is just 0.1 clearance to the face of the part at max -z.

In this case more RPM helped with reducing chatter. We started at 250 RPM and kept bumping it up - the faster we went, the better it got. We stopped at 600 RPM (550 SFM) because we are not running coolant through the bar (does anyone out there re-drill & pipe tap thier boring/threading bars after cutting them off?) and got a little worried about the insert.

on acme the programming would be

G76P010029

if you are not using 2 line g76 it will not work. If you are using G92 then you are either going to have to calculate the z movefor each pass. What this does is load the tool on one side, it increases wear on that side, but it keeps the insert stable

rough out at about .05 away with m74 m33 then run another cycle to size with .004 depth of cut per side with same depth of cut for finish with m74 m32 then repeat again with m74 m34.

150 rpm is about right. I worked for a company where they had a problem running 304 stainless castings and would chip the inserts out and scrap castings. When I got there they were trying to run at 1250 rpm. This was way to fast for stainless. 150-200 rpm max is perfect with a lay-down insert. Your tool wear will be very acceptable as well.

1.750 deep isn't that deep especially with a carbide bar. For an excellent insert try the iscar IC908 laydown series inserts with 3 corners. I run pre hardened 4140 with 12" long threads and the inserts hold up for at least 25 pc orders. I reccommend this insert for your stainless as well.

So snub up your bar from your turret to 1 7/8 and chuck up on your piece as much as possible if you can. You can also set your first block of G76 cycle to

G76P000060

This will not allow a finishing pass in the cycle which will sometimes reduce the chatter because you will still allow tool pressure all the way to minor or major diameter.

Bryan

Was you using a G76 cycle ?

What's the dia of the bar. You're going into a half inch hole or so, 2 inches deep. I;m guessing the length to bar dia ratio is about 5 or 6 to one??? You gotta go slow to kill the chatter. This a mild steel bar? You may need to get something more rigid, or live with the fact that it's slow

150 rpm is about right. I worked for a company where they had a problem running 304 stainless castings and would chip the inserts out and scrap castings. When I got there they were trying to run at 1250 rpm. This was way to fast for stainless. 150-200 rpm max is perfect with a lay-down insert. Your tool wear will be very acceptable as well.

1.750 deep isn't that deep especially with a carbide bar. For an excellent insert try the iscar IC908 laydown series inserts with 3 corners. I run pre hardened 4140 with 12" long threads and the inserts hold up for at least 25 pc orders. I reccommend this insert for your stainless as well.

So snub up your bar from your turret to 1 7/8 and chuck up on your piece as much as possible if you can. You can also set your first block of G76 cycle to

G76P000060

This will not allow a finishing pass in the cycle which will sometimes reduce the chatter because you will still allow tool pressure all the way to minor or major diameter.

Bryan

He has to be hanging out at least 5 times the diameter. He is using a carbide threading bar and I can tell you that is a lot for an I.D. of that size. A blind hole plus threading to within .2 of the bottom means the insert will be cutting chips. Not good.

150 RPM at that diameter is not "just about right." 100 SFM would be on the low end even for a 'soft' carbide insert such as a KC720 or BXC from Carmex. That works out to about 700 RPM. Don't know what diameter you are threading those castings at, but it should be about 2-3/16 inches at S175 using 100 SFM. We use CP500 a lot and thread 316 SS at 365 SFM (over S2500 at 14mm dia.). 99.99% of our threading is done with a laydown insert.

We currently have four 316 SS casting jobs running, all I.D. threads, ranging from S1200 for a 3/8-NPT to a 15/16-26UNF at S1450. One 15/16-26UNF job is running at S1000 because of chatter (doesn't have good support). Just finished a 1-3/16-18UN O.D. thread at S1200 in SS casting. I much prefer O.D. threads to I.D. because most of our parts are small with no place for the chips to go.

PDI-Curtis' idea of stopping every few passes isn't a bad one, but threading without any compound infeed is. His example is cutting equal amounts of material on both sides of the insert. Not only does this create more tool pressure, but the strongest chip possible. Neither is desirable in your case (especially the chip), although some load is usually needed to eliminate chatter.

Sometimes the excessively slow RPMs are the only way to avoid chatter. This is hard on an insert. Material wants to stick to the insert. The insert often chips at withdrawal or at the start (more likely) of the next cut. If it doesn't chip, the material stuck on the insert will cause the thread sides to not be nice and clean because the stuck on material will cause scoring.

This much I can tell you: Slower RPM makes chatter look worse. Higher RPM shortens the distance between the chatter marks. Usually I have to slow down until it disappears. However. I did have one O.D. thread (small diameter) that cleaned up beautifully at an RPM that was 170% faster than what the machine manufacture said the limit was for threading (120 IPM). Guess Hardinge lathes are built with a little leeway. :)

When I first start programming lathes, they were threading 303 SS at 500 to 700 RPM and 19 to 21 passes. This was for both 3/4-28UNF and 15/16-26UNF threads. Inserts didn't hold up well, and often had problem with chatter. I went to S1400 and 5 or 6 passes. Couldn't go faster because of the need to get close to a shoulder. No chatter. Excellent tool life. Figured the savings on just this one machine paid for my wages for the year. And this didn't take anything into account except the reduction in cycle time.

just went through a similar scenario. threading 1.875"-12 i.d. in 304SS, 2.00" deep in a blind hole. ended up with a vardex 3 sided 12 pitch vtx or vkx grade - both worked well. used 2 degree modifed infeed, 10 passes at 510 rpm. after success with this method, i switched to a pull thread, naturally i just needed to get the new anvil or shim, whichever you prefer to call it, and i couldn't get much more out of it in ways of rpm or less passes...just helped with the chips not packing in the back. had the luxury of being able to drill deeper as i was doing a bar push operation.

Id threads: On the 304ss in a 14mm dia on production Id use an OSG tap in a VC10 grade. It is not recomended for ss in the book BUT Iv ran parts for weeks and weeks in 304 ,17-4 ,and 15-5. The chips flow out of the hole. the VC10 grade is the only tap iv found that works in almost any ss. Good luck

Id threads: On the 304ss in a 14mm dia on production Id use an OSG tap in a VC10 grade. It is not recomended for ss in the book BUT Iv ran parts for weeks and weeks in 304 ,17-4 ,and 15-5. The chips flow out of the hole. the VC10 grade is the only tap iv found that works in almost any ss. Good luck

Thanks for the tip on VC10 grade. We do use some OSG taps, but I never paid any attention to the grade. Usually the purchasing agent orders the cheapest ones he can find unless instructed to order something else. The more money he can save on tools, the bigger his bonus. Course we don't get a bonus for getting the work done regardless of tooling, but hey....