HEIDENHAIN TNC 360 ISO Programming - Manual (Page 160)

8-7
8 Cycles
TNC 360
8.2 Simple Fixed Cycles
Example: Tapping with a floating tap holder
Cutting an M6 thread at 100 rpm
Coordinates of the hole:
X = 50 mm Y = 20 mm
Pitch p = 1 mm
F = S x p ➞ F = 100 . 1 = 100 mm/min
Setup clearance: 3 mm
Thread depth: 20 mm
Dwell time: 0.4 s
Feed rate: 100 mm/min
TAPPING cycle in a part program
%S87I 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 S100 * .................................................... Tool call
N50 G84 P01 –5 P02 –20 P03 0.4 P04 100 * ............. Cycle definition TAPPING
N60 G00 G40 G90 Z+100 M06 * ............................... Retract the spindle, insert the tool
N70 X+50 Y+20 M03 * .............................................. Pre-positioning in the X/Y plane, spindle ON
N80 Z+3 M99 * .......................................................... Pre-positioning in Z to setup clearance, cycle call
N90 Z+100 M02 * ...................................................... Retract tool and end program
N9999 %S87I G71 *
Y
X
50
20