Siemens CNC Milling | G63 Code | Tapping with Compensating Chuck

In this article, we describe how to use G63 code for tapping with compensating chuck in Siemens CNC controlled milling (machine centre) machines with all details and examples.


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

Need to More?

Our volunteers have worked together and carefully prepared the articles published here in their native language without using machine translation. You can search the entire site for more information on the subject. You can start a discussion on forums and join us to get support, ask questions, improve a published article or give your opinion.

Previous articleSiemens CNC Milling | G02-G03-TURN | Helix Interpolation
Next articleSiemens CNC Milling | G331-G332 Codes | Thread interpolation


Comments are closed.