Can I thread mill NPT using mazatrol
we thread mill some different size threads using the cir mill tornado in mazatrol... does anyone know how to make a npt using mazatrol NOT an EIA
program. would need to use a single point threadmill
I cannot program my way out of a paper bag, however, wasnt the "Tornado" subroutine developed specifically for the Reime-Noris UNIversal threadmill, which will cut its own core hole into solid material and threadmill its way down, in one corkscrew pass, then retract?
If your'e doing NPT, unless the threadmill is designed for NPT, dont you need conical interpolation?
did you try to write G2.1 in conventional unit ?
not sure it works but maybe
G2.1 (G3.1) is conical interpolation code . look EIA / ISO manual.
If not , do a macro programm you call call as a sub with fixin some value ( diameter , pitch , depth, etc..)
If you are not able to do it , ask to your local Mazak application dept.
Yes you can. I just did a 1" NPT thread mill Thursday on our Matrix Controlled Nexus MSY machine. You can use the Tapping Unit w/ Planet option, HOWEVER, for an NPT it will not come out exactly correct. The thread will be out-of-round because this process does not compensate for the angle of the NPT as the tool cuts around the thread.
Threadmill USA has an excel spreadsheet that I used to generate the correct positions to constantly move "out" in the radial axis(s) while the tool moved out in the axial axis. I used the excel data, and plugged the numbers, into a Manual Program Unit, and its running great still today. You need a Y-Axis machine I believe. Contact me if you need some more details. I don't check in here too often.
Oh, I re-read you message. I used a multi-point 1" NPT specific threadmill. My impression of the tornado funtion is that it is an option to rough down into a circle mill. I certiainly suspose you could use it to produce a thread, but I've never tried it. On an NPT thread, Ferrous Antiquos is correct in that you need to interpolate in a "cone" fashion... even with a multi tooth, angled NPT specific tool.
I don't believe it is possible with a single point threadmill to threadmill NPT threads within Mazatrol. We use tapered threadmills from Xactform to create our NPT threads using Tornado mode.
JimmyB, we use Planet tapping for NPT threads on our Integrex Machines and they come out great. Like above though, we use tapered threadmills. My only problem with planet tapping is that you can't control the number of revolutions the tool makes. It's only designed for 1 revolution, so if you are using a skip-tooth threadmill, your pitch is doubled and you have to write a 2nd unit. Kind of a pain.
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.
LOL, I'm a dope. I re-read my early post at which time I guess I had already realized the information I just posted. Well anyways, theres a more detailed explanation.