Siemens SINUMERIK 808D ADVANCED Programming And Operating Manual page 143

N10 G90 G0 T11 D1 S500 M3
N20 G17 X35 Y35 Z60
N30 G1 F200
N40 CYCLE840(20,0,3,-15,,1,4,3,1,6,,3)
N50 M02
Programming example: Tapping with encoder
In this program, a thread is tapped with encoder at position X35 Y35 in the XY plane. The drilling axis is the Z axis. The lead
parameter must be defined, automatic reversal of the direction of rotation is programmed. A compensating chuck is used in
machining.
N10 G90 G0 T11 D1 S500 M4
N20 G17 X35 Y35 Z60
N30 CYCLE840(20,0,3,-15,,1,3,4,1,6,,3)
N40 M02
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA1, 01/2014
; Specification of technology values
; Approach drilling position
; Setting the path feedrate
Cycle call, dwell time 1 s, direction of
rotation for retraction M4, direction of
rotation after cycle M3, no safety
clearance, parameters MPIT and PIT have
been omitted
; End of program
; Specification of technology values
; Approach drilling position
; Cycle call, without safety clearance,
with absolute depth specification
; End of program
143