Siemens SINUMERIK 840Di sl - Page 72

Fundamental Principles of NC Programming
2.5 Second programming example for milling application
Fundamentals
72 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
N070 SUPA G0 Z0 D0 M5 M9
;********************Tool change********************
N075 T2 M6
;d = 1 inch facing tool
MSG ("Side machining")
N080 G0 X-1 Y.25 S1200 M3 M8
N085 Z1 D1
N090 G1 Z-.5 F50
N095 G42 X.5 F30
N100 X5.5 RNDM=-.375
;Modal rounding. Radius=0.375
N105 Y3.625
N110 X.5
N115 Y.25
N120 X=IC(.375) RNDM=0
;Needed for edge rounding
N125 G40 G0 Y-1 M5 M9
;Rapid traverse to initial setting
N130 Z1
N135 X-1 Y0
N140 Z-.25
,********************Continue to use 1-inch mill****************
MSG ("Side Cut Top Boss")
N145 G01 G41 X1 Y2
N150 G2 X1.5476 Y3.375 CR=2
N155 G3 X4.4524 CR=3
N160 G2 Y.625 CR=2
N165 G3 X1.5476 CR=3
N170 G2 X1 Y2 CR=2
N175 G0 G40 X0
N180 SUPA G0 Z0 D0 M5 M9
;Z approaches tool change position
N185 SUPA X0 Y0
;X and Y to tool change position
;********************Tool change********************
N190 T3 M6
;27/64 drill
MSG ("Drill 3 holes")
N195 G0 X1.75 Y2 S1500 M3 M8
;Approach first drill hole
N200 Z1 D1
N205 MCALL CYCLE81 (1,0,.1,-.5,)
N207 X1.75
;Drill first hole
N210 X3
;Drill second hole
N215 X4.25
;Drill third hole
N220 MCALL
N221 SUPA Z0 D0 M5 M9
;Delete modal call. Z axis traverses to ;machine zero
N225 SUPA X0 Y0
MSG ()
N230 M30
;End of program