HEIDENHAIN CNC PILOT 640 - Interrupted Feed G64

DIN/ISO programming | Feed rate, shaft speed
4
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
297
Interrupted feed G64
G64 interrupts the programmed feed for a short period of time.
G64 is a modal function.
Parameters:
E: Interval time in seconds (range: 0.01 < E < 99.99)
F: Feed period in seconds (range: 0.01 < E < 99.99)
Example: G64
. . .
N1 T3 G95 F0.25 G96 S200 M3
N2 G64 E0.1 F1
Interrupted feed on
N3 G0 X0 Z2
N4 G42
N5 G1 Z0
N6 G1 X20 B-0.5
N7 G1 Z-12
N8 G1 Z-24 A20
N9 G1 X48 B6
N10 G1 Z-52 B8
N11 G1 X80 B4 E0.08
N12 G1 Z-60
N13 G1 X82 G40
N14 G64
Interrupted feed off
. . .