Yx z – HEIDENHAIN TNC 360 ISO Programming User Manual
Page 167
8-14
8
Cycles
TNC 360
Example: Milling a circular pocket
Pocket center coordinates:
X
= 60 mm
Y
=
50 mm
Setup clearance:
2
mm
Milling depth:
12
mm
Pecking depth:
6
mm
Feed rate for pecking:
80
mm/min
Circle radius:
35
mm
Milling feed rate:
100
mm/min
Direction of the cutter path:
–
CIRCULAR POCKET MILLING cycle in a part program
%S814I G71 * ............................................................ Begin program
N10 G30 G17 X+0 Y+0 Z–20 * ................................... Define workpiece blank
N20 G31 G90 X+100 Y+100 Z+0 *
N30 G99 T1 L+0 R+4 * .............................................. Tool definition
N40 T1 G17 S2000 * .................................................. Tool call
N50 G77 P01 –2 P02 –12 P03 –6 P04 80 P05 35
P06 100 * ................................................................... Cycle definition CIRCULAR POCKET MILLING
N60 G00 G40 G90 Z+100 M06 * ............................... Retract the spindle, insert the tool
N70 X+60 Y+50 M03 * .............................................. Move to starting position (pocket center), spindle ON
N80 Z+2 M99 * .......................................................... Pre-positioning in Z to setup clearance, cycle call
N90 Z+100 M02 * ...................................................... Retract tool and end program
N9999 %S814I G71 *
8.2
Simple Fixed Cycles
60
50
35
12
Y
X
Z