Siemens SINUMERIK 840DE Programming Manual page 166

Programming Motion Commands
4.18 Tapping with compensating chuck (G63)
Parameters
G63
X Y Z
Note
G63 is modal.
The last programmed interpolation command G0, G1, G2, etc., is reactivated after a block
with programmed G63.
Feedrate
Note
The programmed feed must match the ratio of the speed to the thread lead of the tap.
Thumb rule:
Feed F in mm/min = spindle speed S
in rpm x thread lead in mm/rev
Both the feed and the spindle speed override switch are set to 100% with G63.
Example 1
N10 SPOS[n]=0
N20 G0 X0 Y0 Z2
N30 G331 Z-50 K-4 S200
N40 G332 Z3 K-4
N50 G1 F1000 X100 Y100 Z100 S300 M3
N60 M30
Example 2
In this example, an M5 thread is to be drilled. The lead of an M5 thread is 0.8 (specified in
table).
With a selected speed of 200 rpm, the feed F is 160 mm/min.
4-60
Tapping with compensating chuck.
Drilling depth (end point) in a Cartesian coordinate
;Prepare tapping
;Approach starting point
;Tapping, drilling depth 50, lead K
;negative = direction of spindle rotation
counterclockwise
;Retract, automatic reversal of direction
;Spindle reverts to operation in spindle
mode
;End of program
Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1
Fundamentals