Programming and Operating Manual (Milling)
80
6FC5398-4DP10-0BA1, 01/2014
The drilling depth is specified by specifying one of the axes X, Y or Z; the thread pitch is specified via the relevant I, J or K.
G33 remains active until canceled by another instruction from this G group (G0, G1, G2, G3...).
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) - see Section
"Spindle movements (Page 87)"). To do this, the rotation value must be programmed under address S or a rotation speed
must be set.
Note
A complete cycle of tapping with compensating chuck is provided by the standard cycle CYCLE840.
See the following illustration for tapping using G33:
Programming example
; metric thread 5,
; pitch 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 G33 Z-25 K0.8
; Tapping, end point -25 mm
N40 Z5 K0.8 M4
; Retraction, counter-clockwise spindle rotation
N50 G0 X30 Y30 Z20
N60 M30
Axis velocity
With G33 threads, the velocity of the axis for the thread lengths is determined on the basis of the spindle speed and the
thread pitch. The feedrate F is not relevant. It is, however, stored. However, the maximum axis velocity (rapid traverse)
defined in the machine data can not be exceeded. This will result in an alarm.
Note
Override switch
●
The spindle speed override switch should remain unchanged for thread machining.
●
The feedrate override switch has no meaning in this block.
8.5.2
Tapping with compensating chuck: G63
Functionality
G63 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.]
