[CharlieM]

So I write myself a program for milling 72 thread per inch. I will use a .25 Dia thread milling cutter. I want to mill a thread inside a .687 bore, the thread will go down about .06 in, and the spindle will return to home. I discover the thread is too small. I want the thread to be .010 in larger. I put (G41 .005) in the second line of code.

That don't work for me!!!

How do I cut this thread to the size I need, without re-writing the intire code?

N01 G00 X.0000 Y.0000 Z-.2000
N02 G02 X.0000 Y.2500 I.0000 J.12500 F3
N03 G02 X.2500 Y.0000 I.0000 J.0000 Z-.2035
N04 G02 X.0000 Y-.250 I.0000 J.0000 Z-.2069
N05 G02 X-.250 Y.0000 I.0000 J.0000 Z-.2104
N06 G02 X.0000 Y.2500 I.0000 J.0000 Z-.2139
N07 G02 X.2500 Y.0000 I.0000 J.0000 Z-.2174
N08 G02 X.0000 Y-.250 I.0000 J.0000 Z-.2208
N09 G02 X-.250 Y.0000 I.0000 J.0000 Z-.2243
N10 G02 X.0000 Y.2500 I.0000 J.0000 Z-.2278
N11 G02 X.2500 Y.0000 I.0000 J.0000 Z-.2312
N12 G02 X.0000 Y-.250 I.0000 J.0000 Z-.2347
N13 G02 X-.250 Y.0000 I.0000 J.0000 Z-.2382
N14 G02 X.0000 Y.2500 I.0000 J.0000 Z-.2417
N15 G02 X.2500 Y.0000 I.0000 J.0000 Z-.2451
N16 G02 X.0000 Y-.250 I.0000 J.0000 Z-.2486
N17 G02 X-.250 Y.0000 I.0000 J.0000 Z-.2521
N18 G02 X.0000 Y.2500 I.0000 J.0000 Z-.2555
N19 G02 X.2500 Y.0000 I.0000 J.0000 Z-.2590
N20 G02 X.0000 Y-.250 I.0000 J.0000 Z-.2625
N21 G02 X-.250 Y.0000 I.0000 J.0000 Z-.2660
N22 G02 X.0000 Y.2500 I.0000 J.0000 Z-.2694
N23 G02 X.0000 Y.0000 I.0000 J.1250 Z-.2694
N24 G00 X.0000 Y.0000 Z.0000

[Geof]

You seem to have a lot more code than I would write. But to adjust the size you need to use tool compensation. You would have the tool diameter entered into the diameter compensation for the tool # and then the code would be something like this using the center of the hole for the work zero and the top surface for Z tool length offset. This is for right hand thread.

G00 X0. Y0. Z.1 Move into position with Z clear
Z-.06 Move down to thread depth
G41 D01 G01 Y(OD/2) F1. Move out to the thread OD using the radius
G91 G03 I0. J-(OD/2) Z.0139 L5 Helically interpolate up out of the hole
G40 G00 X0. Y0. Z1. Cancel tool comp and move clear in Z

Now you adjust the size with the diameter wear on the offset page.

There are additional things that can be included such as doing a tangential entry into the cut but that is not really needed with such a fine thread.

Of course if your machine cannot handle the incremental helix you have to program every G03 in absolute but you do not need X Y values on the G03 line just the I J and Z

[CharlieM]

Well, Mr Geof, That's a hell of a lot better than what I am trying to do, especially since I can not cut a thread to size.

Me and you gonna cut that thread some day. After I get back from "Vacation".

Thanks for your response.

Charlie