This cycle is usually called the G92 threading cycle on Fanuc controls.
The Fanuc G92 threading cycle is very simple to program.
Fanuc G92 threading cycle does not have any special infeed methods, the only thread infeed method is a straight plunge type.
For better thread control like Infeed angle you might use CNC Fanuc G76 Threading Cycle
CNC Fanuc G92 Threading Cycle
Contents
1: Fanuc G92 Threading Cycle Format
N40 G92 X.. Z.. F..
where
X = Current diameter of the thread pass
Z = End position of the thread in Z-axis
F = Threading feedrate in in/rev (Thread Pitch)
2: Fanuc G92 Threading Cycle Passes
Fanuc G92 threading cycle gives the cnc machinist the flexibility to control every thread pass depth, so the following cnc program blocks will be the calculated diameters for each thread pass. For example
N50 X2.9520 N51 X2.9360 N52 X2.9230
3: Fanuc G92 Thread Cycle Completion
Fanuc G92 Threading cycle can be canceled only by another motion command. If G00 is missing in the program, the control system will expect that there are more threads to cut.
So the block after the last thread pass diameter block must be like this,
N110 GOO X12.O Z4.5 M09
CNC Fanuc G92 Threading Cycle Program Example
03802 N10 T0505 M42 N20 G20 G97 S450 M03 N30 G00 X3.2 Z0.25 M08 N40 G92 X2.972 Z-1.6 FO.0833 N50 X2.9520 N60 X2.9360 N70 X2.9230 N80 X2.9130 N90 X2.9040 N100 X2.8978 N110 GOO X12.O Z4.5 M09 N120 M30
