Siemens CNC Milling | G63 Code | Tapping with Compensating Chuck

G63 Code Introduction

G63 code can be used for tapping with compensating chuck. The programmed feedrate F must match with the spindle speed S (programmed under the address “S” or specified speed) and with the thread pitch of the drill:

F [mm/min] = S [rpm] x thread pitch [mm/rev.]

The compensating chuck compensates the resulting path differences to a certain limited degree.

The drill is retracted using G63, too, but with the spindle rotating in the opposite direction M3 <-> M4.

G63 is non-modal. In the block after G63, the previous G command of the “Interpolation type” group (G0, G1,G2, …) is active again.

Right-hand or left-hand Thread

Right-hand or left-hand thread is set with the rotation direction of the spindle (M3 right (CW), M4 left (CCW).

Note: The standard cycle CYCLE840 provides a complete tapping cycle with compensating chuck (but with G33 and the relevant prerequisites).

You may be interested also:

“Siemens CNC | CYCLE840 | Tapping with Compensating Chuck”

G63 Code Example

See the following illustration for tapping using G63:

; metric thread 5,
; lead as per table: 0.8 mm/rev., hole already premachined

N10 G54 G0 G90 X10 Y10 Z5 S600 M3 ; Approach starting point, clockwise spindle rotation
N20 G63 Z-25 F480 ; Tapping, end point -25 mm
N40 G63 Z5 M4 ; Retraction, counter-clockwise spindle rotation
N50 X30 Y30 Z20
M30