[phoodieman]

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

[lakeside]

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

[phoodieman]

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

[lakeside]

is you tool holder on center?

[phoodieman]

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

[cseely]

Check Center and keep bar as short as possible.

[phoodieman]

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

[lakeside]

try slower rpm

[phoodieman]

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

[lakeside]

what size thread are you doing

[lakeside]

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

[phoodieman]

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

[M-man]

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

[PDI-Curtis]

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

[pdoherty]

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

[PDI-Curtis]

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.

[mtlmnchr]

It lets the bar find its own center

[mtlmnchr]

have you tried a different approach to programing ?

G76P010060
G76X?Z?Q20P20F.07813

[pdoherty]

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.

[mtlmnchr]

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