HEIDENHAIN CNC PILOT 640 - C-axis commands

DIN/ISO programming | C-axis commands
4
392
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
4.23 C-axis commands
Reference diameter G120
G120 determines the Reference diameter of the unrolled lateral
surface. Program G120 if you use CY for G110 to G113. G120 is a
modal function.
Parameters:
X: Diameter
Example: G120
. . .
N1 T7 G197 S1200 G195 F0.2 M104
N2 M14
N3 G120 X100
Reference diameter
N4 G110 C0
N5 G0 X110 Z5
N6 G41 Q2 H0
N7 G110 Z-20 CY0
N8 G111 Z-40
N9 G113 CY39.2699 K-40 J19.635
N10 G111 Z-20
N11 G113 CY0 K-20 J19.635
N12 G40
N13 G110 X105
N14 M15
. . .
Datum shift in C axis G152
G152 defines an absolute datum for the C axis (reference:
Reference point, C axis). The datum is valid until the end of the
program.
Parameters:
C: Angle – spindle position of new C-axis datum
Example: G152
. . .
N1 M5
N2 T7 G197 S1010 G193 F0.08 M104
N3 M14
N4 G152 C30
C-axis datum
N5 G110 C0
N6 G0 X122 Z-50
N7 G71 X100
N8 M15
. . .