Yx z – HEIDENHAIN TNC 407 (280 580) ISO Programming User Manual
Page 236
8-16
8
Cycles
TNC 426/TNC 425/TNC 415 B/TNC 407
60
50
35
12
Y
X
Z
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 cycle in a part program
%S814I G71 * ............................................................ Start of 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 * .............................................. Define tool
N40 T1 G17 S2000 * .................................................. Call tool
N50 G77 P01 –2 P02 –12 P03 –6 P04 80 P05 35
P06 100 * ................................................................... Define circular pocket milling cycle
N60 G00 G40 G90 Z+100 M06 * ............................... Retract in the infeed axis, insert tool
N70 X+60 Y+50 M03 * .............................................. Approach the starting position (center of pocket), spindle ON
N80 Z+2 M99 * .......................................................... Pre-position in Z to setup clearance, cycle call
N90 Z+100 M02 * ...................................................... Retract in the infeed axis, end of program
N99999 %S814I G71 *