HEIDENHAIN CNC PILOT 640 - 4.14 Oversizes; Axis-Parallel Oversize G57; Switching off Oversize G50

DIN/ISO programming | Oversizes
4
308
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
4.14 Oversizes
Switching off oversize G50
G50 switches off Ov.size defined with G52 Geo for the following
cycle. Program G50 before the cycle.
To ensure compatibility, the G52 code is also supported for switching
off the oversizes. HEIDENHAIN recommends using G50 for new NC
programs.
Axis-parallel oversize G57
G57 defines different oversizes for X and Z. Program G57 before
the cycle call.
Parameters:
X: O-size X (only positive values; diameter value)
Z: O-size Z (only positive values)
G57 is effective differently in the following cycles:
After cycle run, the oversizes are deleted with G810, G820,
G830, G835, G860, G869, G890
After cycle run the oversizes are not deleted with G81, G82,
G83
If the oversizes are programmed with G57 and in the
cycle itself, the cycle oversizes apply.
Example: G57
. . .
N1 T3 G95 F0.25 G96 S200 M3
N2 G0 X120 Z2
N3 G57 X0.2 Z0.5
Paraxial oversize
N4 G810 NS7 NE12 P5
. . .