Programming instructions

NC Programming 17VRS Tool Corrections
5-35
DOK-MTC200-NC**PRO*V17-ANW1-EN-P
Example NC program - tool path compensation with G42
20
40
60
80
100
20 40 60 80 100
X
Y
120 140 160 180
Fig. 5-28: Tool path compensation, right of contour (G42)
(TOOL CHANGE: IDENT=SF D5)
T4 BSR .M6
G00 G54 G06 G08 X115 Y99.5 Z5 Motion commands, interpolation conditions
G01 Z2 F1000 S2000 M03 1st starting position
Z-10 F1200 Lower cutter into material
G42 X117.5 Y99.5 F1500 Establish tool path compensation
G02 X98 Y80 I98 J99.5 Traverse to contour with ¼ circle
G01 X45 Y80 Machine 1st section
G03 X40 Y75 I45 J75 Machine 1st ¼ circle
G01 X40 Y25 Machine 2nd section
G03 X45 Y20 I45 J25 Machine 2nd ¼ circle
G01 X135 Y20 Machine 3rd section
G03 X140 Y25 I135 J25 Machine 3rd ¼ circle
G01 X140 Y75 Machine 4th section
G03 X135 Y80 I135 J75 Machine 4th ¼ circle
G01 X90 Y80 Machine 5th section
G02 X73.5 Y96.5 I90 J96.5 Withdraw from contour with ¼ circle
G01 X73.5 Y99.5 End position of outer contour
G00 Z2 Z axis to safety distance
G40 X68 Y49.5 Starting position inside contour
G01 Z-10 F1000 Lower cutter into material
G42 X65.5 Y49.5 F1500 Establish tool path compensation
X65.5 Y50.5 Linear motion
G02 X90 Y75 I90 J50,5 Traverse to contour with ¼ circle
G01 X130 Y75 Machine 1st section
G02 X135 Y70 I130 J70 Machine 1st ¼ circle
G01 X135 Y30 Machine 2nd section
G02 X130 Y25 I130 J30 Machine 2nd ¼ circle
G01 X50 Y25 Machine 3rd section
G02 X45 Y30 I50 J30 Machine 3rd ¼ circle
G01 X45 Y70 Machine 4th section
G02 X50 Y75 I50 J70 Machine 4th ¼ circle
G01 X98 Y75 Machine 5th section
G02 X119.5 Y53.5 I98 J53.5 Withdraw from contour with ¼ circle
G01 X119.5 Y49.5 End position inside contour
G00 Z2 Z axis to safety distance
(TOOL CHANGE: Store last tool)
T0 BSR .M6
RET End of program
NC program using G42