Thread tapping without compensating chuck

With this method of thread tapping (G63), the spindle is slaved synchronously to the contouring motion by the CNC. The spindle and the axes participating in the feed motion are exactly coordinated dynamically. Therefore, there is no need for a compensating chuck. The programmed feed rate must match the chosen spindle speed and the pitch of the drill, and is calculated as follows:

Feed rate F [mm/min] = speed S [rpm] * pitch [mm/rev]

The spindle must be at standstill when G63 is called up.

Cutting of a left-hand thread or movement out of a thread hole is programmed with a negative S value.

G63 is cancelled by selecting a different type of interpolation (e.g. G00, G01, G02, G03).

G63 F.. S.. Z..

Example:

A thread with a pitch of 1.25 mm and a depth of 50 mm is drilled. At a spindle speed S of 200 rpm, this results in a feed rate of:

F = 200*1.25 = 250 mm/min

G63 Z-50 F250 S200 Thread tapping

Z50 S-200 Moving out of thread hole

G01 F100 X100 ... Thread tapping cancelled, linear interpolation