Thread Milling 3/8-18 NPT

[shawn]

Does anyone have an incremental program for a 3/8-18 NPT using a multi tooth threading tool. The diameter of my tool is .371". I am using a Tool Flo tool.

[ajl6549]

Try this...BE CARFUL! this is for a .31 dia. thrd mill but should work if you add .035" to cutter comp offset #1 (D1)

%
O151
(NO TOOL RADIUS COMPENSATION D1=0)
(ADJ. D1 PLUS .035 AND WORK TO SIZE)
N1 T1 M6
G90 G0 G54 G17 X0.0000 Y0.0000 S???? M03
G43 H1 Z1.
Z0
G01 G91 Z-0.4149 F200. M08
G01 G41 D1 X0.0839 Y-0.0839 F??
G03 X0.0839 Y0.0839 Z0.0069 I0.00000 J0.08390 F??
G03 X-0.1678 Y0.1682 Z0.0139 I-0.16823 J0.00000
G03 X-0.1687 Y-0.1682 Z0.0139 I0.00000 J-0.16866
G03 X0.1687 Y-0.1691 Z0.0139 I0.16909 J0.00000
G03 X0.1695 Y0.1691 Z0.0139 I0.00000 J0.16953
G03 X-0.0848 Y0.0848 Z0.0069 I-0.08476 J0.00000
G01 G40 X-0.0848 Y-0.0848 F200.
G01 Z0.5417
X0.0000 Y0.0000 Z1.
M30
%

[shawn]

Thank you very much worked perfect. I ended up at .021 in the offset but it worked great. My only question would be the depth? .4149 seems kind of Shallow. I run my 1/4-18 NPT@ z-.522? Since the program is incremental could I drop the Z lower and just increase my D offset to compensate?

[ajl6549]

Yes, by all means , if you need more thrds. do exactly that. BTW, that came from a cd-rom I got from my Iscar rep. if you have one in your area he/she should be able to set you up with one. Its "geared" for there product line but, I've found it works well for others as well

[shawn]

Oh ok. Thanks again. We dont deal much with them but I will give it a shot.

[ajl6549]

One other thing, the cutting length of your tool would be the determining factor as to how deep you can thrd. mill. I have a prog. for a 1-11.5 NPT that cuts the hole with a .625 dia bull nose e.m. using virtual axis interpolation to put a chamfer on the tappered hole before thrd. milling it. Note speed and feed on the bull mill it has cut at least 350 holes and shows no signs of wear!

M1
M6
G90 B90000 M42
T76 S5000 M3
(TOOL-94 = .625 BULL MULTI MASTER)
(B90 DEG/ G54)
G0 G90 G17 G95 G54 X-2.75 Y-3.5
Z1. M8
Z.1
G91 G1 G95 F.02 Y.5488
G3.1 X0 Y-.2713 J-.5488 Z-.3 P10
G3.1 X0 Y-.0375 J-.2775 Z-.65 P18
G3 J-.2485
G1 Y-.2485
G90 G0 Z1.
X-4.75 Y0
Z.1
G91 G1 G95 Y.5488
G3.1 X0 Y-.2713 J-.5488 Z-.3 P10
G3.1 X0 Y-.0375 J-.2775 Z-1. P18
G3 J-.24
G1 Y-.24
G90 G0 Z1.
G91 G30 Z0
G30 X0 Y0
M1
(TOOL-95 = ISCAR THRD MILL .625 DIA./.08696 PITCH)
M6
G90 G0 G54 X-2.75 Y-3.5 Z1.9685 S3033 M03
Z1. M8
Z0
G01 G91 Z-0.7339 F196.8 M08
G91 G94 G01 G41 D1 X0.3067 Y-0.3067 F56.5
G03 X0.3067 Y0.3067 Z0.0109 I0.00000 J0.30674 F38
G03 X-0.6135 Y0.6142 Z0.0217 I-0.61417 J0.00000
G03 X-0.6148 Y-0.6142 Z0.0217 I0.00000 J-0.61484
G03 X0.6148 Y-0.6155 Z0.0217 I0.61552 J0.00000
G03 X0.6162 Y0.6155 Z0.0217 I0.00000 J0.61620
G03 X-0.3081 Y0.3081 Z0.0109 I-0.3081 J0.00000
G01 G40 X-0.3081 Y-0.3081 F196.8
G00 G90 Z1.
G90 G0 Z1.
G91 G30 Z0
G30 X0 Y0

[shawn]

Wow that’s pretty impressive. What material are you cutting? We specialize in plastic so we never even cut a taper for an NPT thread on the mills. We just use the recommended size on a drill chart. But like I said that’s plastic. Now on a lathe it’s different we always turn or bore the correct taper.

[ajl6549]

Class 30 gray iron. We rarely taper ream either, I was just learn'in/play'in with the G3.1 virtual axis function on our new Mazak FH8800 machining ctr.

[shawn]

yeah you threw me for a loop I had never even seen a G3.1 before Mazak has their own controls right? We use Fanuc we have a couple of Haas' a Fadal and a couple of older smaller machinig centers.

[Kiwi]

Is boring the tapered hole a problem if you don't have a reamer?

I have a program that can generate a helix path to cut the taper. If a chamfer is required this can be generated and added.
The program is listed here.

http://www.cnczone.com/forums/showth...404#post190404
Just ask if more info required.

[ajl6549]

Originally Posted by shawn yeah you threw me for a loop I had never even seen a G3.1 before Mazak has their own controls right? We use Fanuc we have a couple of Haas' a Fadal and a couple of older smaller machinig centers.

Mazak does have their own controls but as an option they can use "G-code" as well. If I'm not mistaken Fanuc has somthing like G3.1 probably an option though

[ajl6549]

Originally Posted by Kiwi Is boring the tapered hole a problem if you don't have a reamer? I have a program that can generate a helix path to cut the taper. If a chamfer is required this can be generated and added. The program is listed here. http://www.cnczone.com/forums/showth...404#post190404 Just ask if more info required.

Cool prog. how do tell it different dia. tools or do you just use cutter comp.?