Tapping With Compensating Chuck: G63 - Siemens SINUMERIK 808D User Manual

N o te
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
N10 G54 G0 G90 X10 Y10 Z5 S600 M3
N20 G33 Z-25 K0.8
N40 Z5 K0.8 M4
N50 G0 X30 Y30 Z20
N60 M30
Axi s 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 fe e drate F is not relevant. It is, however, stored. However, the maximum axis velocity (rapid traverse)
defined in the machine data cannot be exceeded. This will result in an alarm.
N o te
Ove rride switch
The spindle speed override switch must remain unchanged for thread machining.
•
The feedrate override switch has no meaning in this block.
•
11.5.2

Tapping with compensating chuck: G63

Fu n ctionality
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.]
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.
R i ght-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 109)").
102
; metric thread 5,
; pitch as per table: 0.8 mm/rev., hole already
premachined
; Approach starting point, clockwise spindle rota-
tion
; Tapping, end point -25 mm
; Retraction, counter-clockwise spindle rotation
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017