Siemens SINUMERIK 840D sl Programming Manual page 266

Motion commands
9.13 Tapping with compensating chuck (G63)
Feedrate
Note
The programmed feed must match the ratio of the speed to the thread lead of the tap.
Thumb rule:
Feedrate F in mm/min = spindle speed S in rpm * thread lead in mm/rev
Not only the feedrate, but also the spindle speed override switch are set to 100% with G63.
Example
In this example, an M5 thread is to be drilled. The lead of an M5 thread is 0.8 (according to
the table).
With a selected speed of 200 rpm, the feed F = 160 mm/min.
Program code
N10 G1 X0 Y0 Z2 S200 F1000 M3
N20 G63 Z-50 F160
N30 G63 Z3 M4
N40 M30
266
Comment
; Approach starting point, activate spindle.
; Tapping, drilling depth 50.
; Retraction, programmed reversal of direction.
; End of program.
Programming Manual, 09/2011, 6FC5398-1BP40-2BA0
Fundamentals