HEIDENHAIN TNC 407 (280 580) ISO Programming User Manual
Page 232
8-12
8
Cycles
TNC 426/TNC 425/TNC 415 B/TNC 407
Y
X
15
30
80
100
90
100
10
10
10
1
2
Example: Slot milling
A horizontal slot (50 mm x 10 mm) and a vertical
slot (80 mm x 10 mm) are to be milled.
The tool radius in the length direction of the slot
is taken into account for the starting position.
Starting position, slot
1
:
X
= 76 mm
Y
= 15 mm
Starting position, slot
2
:
X
= 20 mm
Y
= 14 mm
SLOT DEPTH:
15 mm
Setup clearance:
2 mm
Milling depth:
15 mm
Pecking depth:
5 mm
Feed rate for pecking:
80 mm/min
1
2
Slot length
50 mm
80 mm
1st milling direction
–
+
Slot width:
10 mm
Feed rate:
120 mm/min
SLOT MILLING cycle in a part program
%S810I 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 G74 P01 –2 P02 –15 P03 –5 P04 80 P05 X–50
P06 Y+10 P07 120 * ................................................... Define slot parallel to X axis
N60 G00 G40 G90 Z+100 M06 * ............................... Retract in the infeed axis, insert tool
N70 X+76 Y+15 M03 * .............................................. Approach starting position, spindle ON
N80 Z+2 M99 * .......................................................... Pre-position in Z to setup clearance, cycle call
1
N90 G74 P01 –2 P02 –15 P03 –5 P04 80 P05 Y+80
P06 X+10 P07 120 * ................................................... Define slot parallel to Y axis
N100 X+20 Y+14 M99 * ............................................ Approach starting position, cycle call
2
N110 Z+100 M02 * .................................................... Retract in the infeed axis, end of program
N99999 %S810I G71 *