Siemens SINUMERIK 840D sl Programming Manual page 58

Fundamentals
2.3 Creating an NC program
Program code
N130 G1 G40 Y-72 F3000
N140 G0 Z200 M5 M9
N150 T="SF10"
N160 M6
N170 S2800 M3 M8
N180 G90 G64 G54 G17 G0 X0 Y0
N190 G0 Z2
N200 POCKET4(2,0,1,-5,15,0,0,0,0,0,800,1300,0,21,5,,,2,0.5)
N210 G0 Z200 M5 M9
N220 T="ZB6"
N230 M6
N240 S5000 M3 M8
N250 G90 G60 G54 G17 X25 Y0
N260 G0 Z2
N270 MCALL CYCLE82(2,0,1,-2.6,,0)
N280 POSITION:
N290 HOLES2(0,0,25,0,45,6)
N300 ENDLABEL:
N310 MCALL
N320 G0 Z200 M5 M9
N330 T="SPB5"
N340 M6
N350 S2600 M3 M8
N360 G90 G60 G54 G17 X25 Y0
N370 MCALL CYCLE82(2,0,1,-13.5,,0)
N380 REPEAT POSITION
N390 MCALL
N400 G0 Z200 M5 M9
N410 M30
58
Comment
; Deselection of the milling tool radius
compensation.
; Retraction of the milling tool, spin-
dle + cooling off.
; Preselection of the tool with name
SF10.
; Load the tool into the spindle.
; Speed, direction of rotation, cooling
on.
; Basic settings for the geometry and
approach starting point.
; Call pocket milling cycle.
; Retraction of the milling tool, spin-
dle + cooling off.
; Call 6 mm centering drill.
; Exact stop G60 for exact positioning.
; Modal call of the drilling cycle.
; Jump mark for repetition.
; Position pattern for drilling.
; End delimiter for repetition.
; Reset modal call.
; Call D 5 mm drill.
; Modal call of the drilling cycle.
; Repetition of the position descrip-
tion from centering.
; Resetting of the drilling cycle.
; End of program.
Programming Manual, 12/2019, 6FC5398-2EP40-0BA0
NC programming