Siemens SINUMERIK 840D sl Programming Manual page 53

Program example 3
Program code
N10 T="PF60"
N20 M6
N30 S2000 M3 M8
N40 G90 G64 G54 G17 G0 X-72 Y-72
N50 G0 Z2
N60 G450 CFTCP
N70 G1 Z-10 F3000
N80 G1 G41 X-40
N90 G1 X-40 Y30 RND=10 F1200
N100 G1 X40 Y30 CHR=10
N110 G1 X40 Y-30
N120 G1 X-41 Y-30
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)
Fundamentals
Programming Manual, 09/2011, 6FC5398-1BP40-2BA0
Creating an NC program
3.4 Program examples
Comment
; Preselection of the tool with
name PF60.
; Load the tool into the
spindle.
; Speed, direction of rotation,
cooling on.
; Basic settings of the
geometry and approach
starting point.
; Z axis at safety clearance.
; Behavior with active G41/G42.
; Milling tool at working depth
with feedrate = 3000 mm/min.
; Activation of the milling
tool radius compensation.
; Travel to the contour with
feedrate = 1200 mm/min.
; Deselection of the milling
tool radius compensation.
; Retraction of the milling
tool, spindle + cooling off.
; Preselection of the tool with
name SF10.
; Load the tool into the
spindle.
; Speed, direction of rotation,
cooling on.
; Basic settings of the
geometry and approach
starting point.
; Call of the pocket milling
cycle.
; Retraction of the milling
tool, spindle + cooling off.
; Call center drill 6 mm.
; Exact stop G60 for exact
positioning.
; Modal call of the drilling
cycle.
53