[Manishpwn]

G90 G94 G17 G49 G40 G80
G21
G28 G91 Z0.
G90
T01 M06
S3308 M03
G54
G00 X0 Y0
G43 Z5. H01
G90
Z-12.354
G01 Z-13.854 F500.
G41 X-3.782 Y-0.77 D01 [B](Here alarm shows interference G41/G42)
G03 X5. Y0 Z-13.5 I4.357 J0.77 F69.

Z-12.0 I-5.0 F122.
X-3.782 Y0.77 Z-11.646 I-4.425 F69.
G40 G01 X0 Y0 F500.
G00 Z5.

G28 G91 Z0.
G28 G91 X0. Y0.
M30

[Jfrahm]

What value is D01?

[the_gentlegiant]

I see you're double posting this. You're trying to threadmill. That explains a lot.

What is the thread you're trying to create. (size and pitch)
What size is your tool?
Are you using a single point tool or one that can do multiple threads at the same time?
What material are you cutting? Need to know this to determine how many passes to take.
Right hand or left hand thread?
FYI - It's generally best to threadmill in Incremental Mode (G91) Not so much if you're only doing a single hole.

More info gets better feedback.

[Manishpwn]

D01 -1.245
M10x1.5 Tapping with 7.7 Thread Mill
Steel Material

[the_gentlegiant]

Hi Manishpawn,

Here you go. This should work. Fanuc based. (Single block it above your part to check first) I don't normally program in Metric so the Feeds and Speeds I leave up to you. Mine are wild-ish guesses. Adjust as you see fit. Adjust D1 until your thread gauge checks properly. When thread milling you really need a thread gauge to check. I used D21 for the roughing comp setting. Use any unused offset number you want.

The threading part of this programming is in incremental. You can take everything between M8 and M9 and put it in a sub, position your tool centered above any pre-drilled hole and run the sub. That's one of the benefits of running thread mills in incremental.

The startup Cutter Comp move will place the side of your tool right next to the wall of the 8.5mm pre-existing hole. The next two moves will gradually move you into the material. Then at the end, the last three moves will gradually move you out and back to the hole center for retracting out of the hole.

O100(THREAD MILL 10 X 1.5)

(T01 THREAD MILL DIA 7.7MM LOC 18MM)

(PROGRAM ZERO IS FIXED)
(JAW AND LEFT EDGE)

(Z ZERO IS TOP OF PART)

(ASSUME 8.5MM EXISTING HOLE)

(START D01 AT 3.850 FINISH)
(START D21 AT 3.980 ROUGH)

T1M6 (MULTI POINT THREAD MILL)
G17G21G40G49G54G80G90G98

G0X0.Y0.
G43Z3.H1S4430M3
M8
G1Z-18.F250.
G91
G1G41Y-4.D21F110.(ROUGH)
X1.Z0.058
G3X4.Y4.I0.J4.Z0.317
I-5.J0.Z1.5
X-4.Y4.I-4.J0.Z0.317
G1X-1.Z0.058
G40Y-4.
G90
Z-18.F250.
G91
G41Y-4.D1F110.(FINISH)
X1.Z0.058
G3X4.Y4.I0.J4.Z0.317
I-5.J0.Z1.5
X-4.Y4.I-4.J0.Z0.317
G1X-1.Z0.058
G40Y-4.
G90
G0Z5.
M9
G53Z0.Y0.M5
M30

(SINGLE POINT THREAD MILL VERSION)

T1M6 (SINGLE POINT THREAD MILL)
G17G21G40G49G54G80G90G98

G0X0.Y0.
G43Z3.H1S4430M3
M8
G1Z-18.F250.
G91
G1G41Y-4.D21F110.(ROUGH)
X1.Z0.058
G3X4.Y4.I0.J4.Z0.317
I-5.J0.Z1.5
I-5.J0.Z1.5
I-5.J0.Z1.5
I-5.J0.Z1.5
I-5.J0.Z1.5
I-5.J0.Z1.5
I-5.J0.Z1.5
I-5.J0.Z1.5
I-5.J0.Z1.5
I-5.J0.Z1.5
I-5.J0.Z1.5
I-5.J0.Z1.5
I-5.J0.Z1.5
X-4.Y4.I-4.J0.Z0.317
G1X-1.Z0.058
G40Y-4.
G90
Z-18.F250.
G91
G41Y-4.D1F110.(FINISH)
X1.Z0.058
G3X4.Y4.I0.J4.Z0.317
I-5.J0.Z1.5
I-5.J0.Z1.5
I-5.J0.Z1.5
I-5.J0.Z1.5
I-5.J0.Z1.5
I-5.J0.Z1.5
I-5.J0.Z1.5
I-5.J0.Z1.5
I-5.J0.Z1.5
I-5.J0.Z1.5
I-5.J0.Z1.5
I-5.J0.Z1.5
I-5.J0.Z1.5
X-4.Y4.I-4.J0.Z0.317
G1X-1.Z0.058
G40Y-4.
G90
G0Z5.
M9
G53Z0.Y0.M5
M30

(OR USE A SUB)
(ADJUST L TO GET YOU OUT OF HOLE)

T1M6 (SINGLE POINT THREAD MILL)
G17G21G40G49G54G80G90G98

G0X0.Y0.
G43Z3.H1S4430M3
M8
G1Z-18.F250.
G91
G1G41Y-4.D21F110.(ROUGH)
X1.Z0.058
G3X4.Y4.I0.J4.Z0.317
M98P101L13
X-4.Y4.I-4.J0.Z0.317
G1X-1.Z0.058
G40Y-4.
G90
Z-18.F250.
G91
G41Y-4.D1F110.(FINISH)
X1.Z0.058
G3X4.Y4.I0.J4.Z0.317
M98P101L13
X-4.Y4.I-4.J0.Z0.317
G1X-1.Z0.058
G40Y-4.
G90
G0Z5.
M9
G53Z0.Y0.M5
M30
%

%
O101 (THREADMILL SUB)

G3I-5.J0.Z1.5
M99
%

Hope it helps. I got to get back to work...

[the_gentlegiant]

Hi Manishpwn... any luck on your thread milling yet?

[Manishpwn]

Thank you for your suggestion, It is only wear offset error. Now program running fine