Siemens SINUMERIK 840D sl Programming Manual page 51

Program example 2
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
N105 G96 S210 M3
N110 G0 G42 X50 Z-60 M8
N115 G1 Z-70 F0.12
N120 G2 X50 Z-80 I6.245 K-5
N125 G0 G40 X100 Z50 M9
N130 G0 G53 X280 Z380 D0 M5
N135 M30
Fundamentals
Programming Manual, 09/2011, 6FC5398-1BP40-2BA0
Comment
; Starting point
; Zero offset
; Speed limitation (G96)
; Select constant cutting rate
; 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
; Select constant cutting rate
; Set tool with tool radius compensation
; Turn diameter 50
; Turn radius 8
; Retract tool and deselect tool radius
compensation
; Approach tool change location
; End of program
Creating an NC program
3.4 Program examples
51