G92 NPT Thread Help

[p4th4ss]

I have only ever programmed using a G92 thread cycle in a cnc. I am trying to program a 2.0×11.5 npt thread and have never programmed tapered threads before. Could anyone write me a sample program using a g92 cycle for that thread size, AND EXPLAIN IT? Also when programming npt threads, is the bore tapered also, and if so, what degree taper? I'm completely confused at all of this Npt stuff.

 

[sinha]

An R address is used for tapered thread.
For NPT/BSPT, which have the same taper, R = L/32 where L is the TOTAL Z travel.
For external threads, if machining from right to left, R would be negative.
For internal threads, if machining from right to left, R would be positive.
The OD/Bore should have the same taper.

 

[aj]

NPT stands for National Pipe Taper. It's a standard from long ago for cutting pipe threads. The taper is 3/4" per foot, or 1/16 per inch or 3.5763 degrees. You didn't say what controller you're using, but when programming pipe threads on Fanuc with G92 you'll want to use the I variable. The I variable is the amount you want to add to your X dimension at the beginning of the pass.

Something like:
G92 X2.000 Z-1.000 Ixx where xx is the amount of taper from Z start position to Z finish position. If you're starting at Z0.300 and feeding to Z-0.800 the amount of taper will be plus or minus I0.0688 depending on if it's an internal or external thread. The 0.0688 comes from multiplying your total Z travel by 0.0625, or 1/16 per inch.

Vardex makes a pretty good thread calculator and it's a free download. I use it to get numbers for thread height and what-not. It'll get you close.

And yes, if you can bore the taper in the part first you'll make life a lot easier.

Speaking of making life easier, you should invest the time in learning G76. Two lines and done.

 

[angelw]

NPT stands for National Pipe Taper. It's a standard from long ago for cutting pipe threads. The taper is 3/4" per foot, or 1/16 per inch or 3.5763 degrees. You didn't say what controller you're using, but when programming pipe threads on Fanuc with G92 you'll want to use the I variable. The I variable is the amount you want to add to your X dimension at the beginning of the pass.

Hello aj,
"You didn't say what controller you're using" is the operative phrase. If the control is pre FS16 an "I" address for the taper argument will be used. If later, an "R" address, as suggested by Sinha, is used. Then the exception to this is for the FS0 Series control (circa 80's); they also use the "R" address.

To the OP
It helps a lot to specify for the Forum, the model of the control being used.

Regards,

Bill

 

[aj]

Thanks, Bill. I'd hate to lead anyone astray. And this is why I've repeatedly seen the phrase "waiting for Bill to chime in".

 

[WABOOM]

Taper is usually about I-.032, put that on the G92 line.. it puts taper at the front of the thread.

On Mazak using EIA it is J code