HEIDENHAIN TNC 360 ISO Programming - Manual (Page 163)

8-10
8 Cycles
TNC 360
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 starting position takes into account the tool
radius in the longitudinal direction of the slot.
Starting position slot 1 :
X = 76 mm Y = 15 mm
Starting position slot 2 :
X = 20 mm Y = 14 mm
SLOT DEPTHS: 15 mm
Setup clearances: 2 mm
Milling depths: 15 mm
Pecking depths: 5 mm
Feed rate for pecking: 80 mm/min
1 2
Slot length 50 mm 80 mm
1st milling direction – +
Slot widths: 10 mm
Feed rate: 120 mm/min
SLOT MILLING cycle in a part program
%S810I 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 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 the spindle, insert the tool
N70 X+76 Y+15 M03 * .............................................. Move to starting position, spindle ON
N80 Z+2 M99 * .......................................................... Pre-positioning in Z to setup clearance, cycle call
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 * ............................................ Move to starting position, cycle call
N110 Z+100 M02 * .................................................... Retract tool and end program
N9999 %S810I G71 *
8.2 Simple Fixed Cycles
Y
X
15 30 80 100
90
100
10
10
10
1
2
1
2