How to program thread milling?

[Vegabond]

Hello Superman!

Do you know, does iscar have that program?


Greetings from Robert.

[Superman]

Never seen it on ISCAR, & never suggested by their reps

The usage would be the same, no matter who supplied the application
just cut & paste into the NC program

[dpuch]

Bugger those 2, they can compare their nut sizes between themselves

Here is a link to a few wizards from SECO -- the threading wizard links are down the RH side

lol
That said I generally prefer climb cutting. There are reasons to conventional cut and/or single point from the top of the hole, but that would not be my general practice.

Thread milling really isn't that complex. In fact it is almost identical to milling a drilled hole out bigger but with a z move also.

Start at the center. A line move so you can activate cutter comp. Arc into the final diameter to minimize cutter shock and flex. A circle at the final diameter. Then lead out like you led into it.

if R = the radius of the final cut, and the center is at X0 Y0.
G0 X0 Y0
G1 Z(full hole depth)
G1 G41 X(1/2R) Y(1/2R)
G3 X(R) Y0 J(1/2R)
G3 I(-R)
G3 X(1/2R) Y(1/2R) I(-1/2R)
G1 G40 X0 Y0
G0 Z(clear)

Add your Z's to that and you have a thread mill path. I use 1 pitch in Z for the full arc, and 1/8 pitch for the lead in and out arcs.

G0 X0 Y0
G1 Z(full hole depth)
G1 G41 X(1/2R) Y(1/2R)
G3 X(R) Y0 Z(up 1/8P) J(1/2R)
G3 I(-R) Z(up 1P)
G3 X(1/2R) Y(1/2R) Z(up 1/8P) I(-1/2R)
G1 G40 X0 Y0
G0 Z(clear)

[Vegabond]

Thank you, im going to try that. Easy explaining, i like that


Greetings from Robert.

lol
That said I generally prefer climb cutting. There are reasons to conventional cut and/or single point from the top of the hole, but that would not be my general practice.

Thread milling really isn't that complex. In fact it is almost identical to milling a drilled hole out bigger but with a z move also.

Start at the center. A line move so you can activate cutter comp. Arc into the final diameter to minimize cutter shock and flex. A circle at the final diameter. Then lead out like you led into it.

if R = the radius of the final cut, and the center is at X0 Y0.
G0 X0 Y0
G1 Z(full hole depth)
G1 G41 X(1/2R) Y(1/2R)
G3 X(R) Y0 J(1/2R)
G3 I(-R)
G3 X(1/2R) Y(1/2R) I(-1/2R)
G1 G40 X0 Y0
G0 Z(clear)

Add your Z's to that and you have a thread mill path. I use 1 pitch in Z for the full arc, and 1/8 pitch for the lead in and out arcs.

G0 X0 Y0
G1 Z(full hole depth)
G1 G41 X(1/2R) Y(1/2R)
G3 X(R) Y0 Z(up 1/8P) J(1/2R)
G3 I(-R) Z(up 1P)
G3 X(1/2R) Y(1/2R) Z(up 1/8P) I(-1/2R)
G1 G40 X0 Y0
G0 Z(clear)

[Daleb]

I have thread milled thousands of parts mostly out of 316 st. st., Inconel and Hastaloy anywhere from 3/8" UN to 3/4" NPT thread depths yp to 4 diameters. I always start at the bottom of the hole, climb mill and I take two passes. the thread will not vary and the tools will not break. Depending on what manufactor I am milling with is the software that I use, just because it will give me the best tool for the application I am using at the time. They all will give you the software for free when you buy their tools.

[Maxter]

I have thread milled thousands of parts mostly out of 316 st. st., Inconel and Hastaloy anywhere from 3/8" UN to 3/4" NPT thread depths yp to 4 diameters. I always start at the bottom of the hole, climb mill and I take two passes. the thread will not vary and the tools will not break. Depending on what manufactor I am milling with is the software that I use, just because it will give me the best tool for the application I am using at the time. They all will give you the software for free when you buy their tools.

I have also started at the bottom and climb milled with the same exotics for over 20 years. Works for me. I might add that I prefer solid carbide thread mills vs insert thread mills. (works much better)