GSK GSK928TE, Руководство пользователя

Страница: 129 / 187

Programming Chapter Four Programming Rules
124
N0000 G00 X50 Z11
； set a workpiece coordinate system
N0010 M3 S2
；
start the spindle, set the spindle speed to No.2 gear
N0020 M8
；
cooling ON
N0030 T11
；
execute No. 1 tool change and execute its tool
compensation
N0040 G00 Z0 X35 ； tool approaches the workpiece
N0050 G01 X0 F60
；
cut the end face with 60mm/min
N0060 G00 W2
；
tool leaves the end face of workpiece
N0070 X24 ； tool approaches the workpiece
N0080 G01 Z-78 F60
；
turn outer Φ 24 and reserve the cut width
N0090 G00 X26 ； tool leaves the workpiece surface
N0100 Z0
；
tool approaches the workpiece
N0110 X24
；
N0120 G90 X21 Z-50 F100 ； turn outer Φ 16mm with cylindrical surface cycle
command
N0130 X18
；
tool infeed 3mm and cycle again
N0140 X15.9
；
tool infeed 2.1mm and cycle again, outer is less than
0.1mm
N0150 G01 X14 Z0 ； tool positions to the starting point of chamfer
N0160 X16 W-1
；
cut a chamfer
N0170 G00 X50 Z50
；
retract the tool to safety position
N0180 T44 ； change No.4 thread tool
N0190 S2
；
set the spindle to high speed(the speed is not more
than 800n/min)
N0200 G00 X19 Z2
；
position to the thread starting point of the first tool
N0220 G92 X15 Z-50 P1.5 K2
；
machine the thread, length of run out of thread 2mm
N0230 X14.2 ； tool infeed 0.8mm to the 2
nd
thread machining
N0240 X13.8
；
tool infeed 0.4mm to the 3
rd
thread machinng
N0250 X13.6
；
tool infeed 0.2mm to the 4
th
thread machining
N0260 G00 X60 Z50
；
retract the tool to the safety position
N0270 T33
；
change No. 3 tool with its width 3mm
N0280 G00 X26 Z-78 ； position to the cut point
N0290 G01 X0 F50
；
cut
N0300 G26
；
X, Z returns to the starting point of machining
N0310 M9
；
cooling OFF
N0320 M5
；
close the spindle
N0330 M2 ； end of program
Example 3
：
Cut the multiple threads with M98, M99 subprogram call and its return instruction.
Fig. 35a: metric multiple thread. Fig. 35b: inch multiple thread. Example: the
cutting of 3 threads is as follows: