Hi guys, I don't know if anyone is still subscribing to this or not. I've recently had a revelation about this subject.
I believe the ACTUAL answer is no. You cannot CORRECTLY thread mill an NPT thread using the Planet function in Mazatrol. Even though I've been doing it that way for some years, I realized that it doesn't work perfectly.
Yes the thread mill is tapered to the correct angle. But your toolpath must follow a "reducing circle" as the thr'd mill works its way up to the next "pitch".
Lets say your making a 1" NPT. Lets call the very first tooth on your thrd mill T1 and the 2nd tooth T2 (clever heh?). The pitch is .08696"
You program the thread major diameter to 1.308" and the depth to .661". T1 will essentially mill a diameter at 1.267" because of the 3.566deg included angle of the thrd mill.
However, T2 is milling 1.2724" diameter. When the tool finish its tool path all the way back around to the starting point (360 degrees) and out by .08696", T1 is now where T2 had started. The problem is that T1 is still at 1.267" diameter, thus not perfectly blended or "meeting" up with where T2 created its cut. The result is about a .004-.005" step all the way up the milled thread.
Fortunately the customers receiving parts made this way must have been using sealant or tape, and the descrepancy has not created an issue. If these were dry seals (NPTF I believe), there may be some leaking resulting.
I was an honest mistake. Now I use a simple program general made in MS Excel that the guys at Threadmill USA created. It took some time to tweak the axis for Turn/Mill machines and tweak some of the G-Codes. But now I'm using the data provided and plugging them into Mazatrol Manual Programming Unit templates I created. The result is correct toolpath generation and no more step in the threads.
The real bonus is, the emulator has a 3 pass option, so I've been using this set for standard UNC threads in tough materials when I want to take additional passes.