I had done thread milling on my Tormach once in the past. It was for a left hand 16mm x 1.0mm thread in hardened stainless steel using a carbide thread mill. I wanted a tight fit to an existing (female) part so I selected a 2D contouring machining operation with cutter diameter compensation. In the "strategy" tab I set "Helical machining" to "Available" and in the "Parameters" I set the "Depth of Cut" to 1mm and a "Bottom Level" to 16mm (the length of the thread I wanted). By using "cutter diameter compensation" I was able to run the same program while varying the cutter diameter to get the fit I wanted. By inputting a cutter diameter (into the Tormach tool table) smaller than the actual cutter diameter (and working down in size) this allowed me to mill to the "minor diameter" I needed. You can calculate this if you just wanted to make one pass.
If you wanted to make multiple cuts to get to your final minor diameter you can set the "Roughing Step Parameters" in the "Strategy" tab to cut the thread in the depth increments you want.
I wasn't quit sure of the quality of the thread I would get at first but was extremely pleased with the result. I got a smooth, tight fit to the existing part. The part was a nozzle for a high pressure waterjet cutter (60,000 psi)
The code resembled:
T35 G43 H35 M6
(0.500" thread mill)
G0 X24. Y0. Z5. ('compensation switch out' lead in for cutter comp.)
G42 (turn cutter comp. on)
G1 Z0. F100 M8
G3 X8 Y0 Z-1. I-7.99999 J0.00001 F200 (start 1mm above part)
X8 Y0 Z-1. I-7.99999 J0.00001 (repeated 16 more times while "Z" increments 1mm each time)
G1 X24. ('compensation switch out' lead out for cutter comp.)
G40 (turn cutter comp. off)
I'm sure there are a half dozen ways to accomplish the same task in Sprutcam.