Yx z – HEIDENHAIN TNC 360 ISO Programming User Manual
Page 158
8-5
8
Cycles
TNC 360
Example: Pecking
Hole coordinates:
1
X
= 20 mm
Y
= 30 mm
2
X
= 80 mm
Y
= 50 mm
Hole diameter:
6
mm
Setup clearance:
2
mm
Total hole depth:
15
mm
Pecking depth:
10
mm
Dwell time:
1
s
Feed rate:
80
mm/min
PECKING cycle in a part program
%S85I 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+3 * .................................................... Tool definition
N40 T1 G17 S1200 * ........................................................ Tool call
N50 G83 P01 –2 P02 –15 P03 –10 P04 1 P05 80 * .......... Cycle definition PECKING
N60 G00 G40 G90 Z+100 M06 * ..................................... Retract the spindle, insert the tool
N70 X+20 Y+30 M03 * .................................................... Pre-positioning for first hole, spindle ON
N80 Z+2 M99 * ................................................................ Pre-positioning in Z to setup clearance, cycle call
N90 X+80 Y+50 M99 * .................................................... Move to second hole, cycle call
N100 Z+100 M02 * .......................................................... Retract tool and end program
N9999 %S85I G71 *
8.2
Simple Fixed Cycles
50
20
80
30
Y
X
Z
6
1
2