Siemens SINUMERIK 840D sl Programming Manual page 255

Example 4: Turning
Program code
N5 G0 G53 X280 Z380 D0
N10 TRANS X0 Z250
N15 LIMS=4000
N20 G96 S250 M3
N25 G90 T1 D1 M8
N30 G0 G42 X-1.5 Z1
N35 G1 X0 Z0 F0.25
N40 G3 X16 Z-4 I0 K-10
N45 G1 Z-12
N50 G2 X22 Z-15 CR=3
N55 G1 X24
N60 G3 X30 Z-18 I0 K-3
N65 G1 Z-20
N70 X35 Z-40
N75 Z-57
N80 G2 X41 Z-60 CR=3
N85 G1 X46
N90 X52 Z-63
N95 G0 G40 G97 X100 Z50 M9
N100 T2 D2
NC programming
Programming Manual, 12/2019, 6FC5398-2EP40-0BA0
2.10 Tool radius compensation
Comment
; Starting point.
; Work offset.
; Speed limitation (G96).
; Select constant feedrate
; Select tool selection and offset.
; Set tool with tool radius compensation.
; Turn radius 10.
; Turn radius 3.
; Turn radius 3.
; Turn radius 3.
; Deselect tool radius compensation and
approach tool change location.
; Call tool and select offset.
Fundamentals
255