The Home Machinist!

motion repetition is not something supported by all software or controls.

If I recall, I think I had to put the repetitious code in a subroutine and call that. Have to look it up. Mach was doing some strange things with cutter comp until I added a Y motion. I never tried that feature before so need to look into it. I might actually try cutting some threads before January now

SOME controls, when activating G41/G42 and going directly into a series of more than 2 arcs (as you are here) at a sharp included corner, 'loose track' of where they need to begin without having a Y component in the initiation line.

It is better (for the general control case), to initialize cutter comp on a short line, then have a small TANGENT ARC that joins the G41 line to the thread milling arc series...

If you do this, you will RARELY find a control that chokes on the code.

I could not figure it out because the tool would follow most of the initial small arc, but get closer to the edge and finally cross before it got to the large arc. Then, it fully reversed direction to pick up the large arc where it would cross at the left side...here is a figure I recreated from memory.

And not intending to derail the thread into a discussion about mach, but at least it's somewhat thread related. I figured I'd try to change the lead in and small arc to be tangent, so only 1/4 of a circle lead-in, especially since I'd expect my cutters to be closer to the hole diameter. Proposed paths shown in the figure, right side. My goal is to set up an Excel spreadsheet that takes the cutter diameter, hole diameter, and thread pitch and will produce the g-code. I could either rely on mach's cutter comp, or build it into my spreadsheet. My spreadsheet would produce a result as shown in the image. Mach will likely steer the cutter up (Y) from the lead in at the start to observe compensation on that path.

This is a case of the control not knowing what to do with cutter comp as described earlier.

You might find it easier tp use G42 and put in a negative value for the offset. Some controls will handle it better.

Another way to handle this is to break it into quadrants..some controls handle the LOOK AHEAD better if you do.

This is just a sample, It works with my Mach3

%
O0
G17 G40 G80 G90
T1 M6
S2500 M3
G0 G90 G54 X0 Y0
G43 Z1. H1 M8
G0 Z-0.9833
G1 Z-1.0833 F30.
X0.0003
G41 X0.0002 D1
G3 X0.9496 Y-0.0287 I0.4747 J-0.0143 F21.509
Z-1. I-0.9496 J0.0287
Z-0.9167 I-0.9496 J0.0287
Z-0.8334 I-0.9496 J0.0287
Z-0.7501 I-0.9496 J0.0287
Z-0.6668 I-0.9496 J0.0287
Z-0.5835 I-0.9496 J0.0287
Z-0.5002 I-0.9496 J0.0287
Z-0.4169 I-0.9496 J0.0287
Z-0.3336 I-0.9496 J0.0287
Z-0.2503 I-0.9496 J0.0287
Z-0.167 I-0.9496 J0.0287
Z-0.0837 I-0.9496 J0.0287
Z-0.0004 I-0.9496 J0.0287
Z0.0829 I-0.9496 J0.0287
X0.95 Y0 Z0.0833 I-0.9496 J0.0287
X0.0002 I-0.4749 J0
G1 G40 X0.0003
G0 Z0
Z1.
M9
G28 G91 Z0
M30
%




CTWO

That's a good example of tangencies...but care that you wear offset cannot exceed 0.0001 -> which may not be enough

A short video of this in use would be super cool.

I don’t have a video cutting the part.
Here’s the simulation and finished parts

https://www.youtube.com/watch?v=WWC3AjgiFd4

I'm liking thread milling a lot for stainless 1/8 NTP.
The next time I'm tinkering with it I'll shorten it up a thread or two and adjust the diameter accordingly.

I have done many internal threads by milling .
I started in the early days by hand grinding a single flute carbide Router bit and putting a relieved 'V" in the bottom.
Worked fine, but now I buy single point thread cutters .
I like centering on the hole and going to the bottom first and doing a relief groove. Then I climb mill in the helix coming out of the hole.
This means I don't have to contend with swarf from the cut, and eliminates a possible crash because I went too deep.
Buying a commercial cutter means you can see your maximum depth and plan accordingly
Here is the type of cutter I am referring to.
https://www.mscdirect.com/product/details/05252036
The commercial (multi-thread endmill)) cutters or insert cutters are pretty pricey for me and these do a bang up job, plus they will do verry small holes, where as the inserts are at a disadvantage

Rich

I have done thread milling pretty much like Rich stated above. Done both with CAM (G-code) and by conversational programming on my Hurco which has a Helix feature.
Only difference than what Rich does is I use a single profile cutter in place of a single point cutter like he does.
https://www.mscdirect.com/product/details/57568883