HEIDENHAIN CNC PILOT 640 - Chamfer Cycle G88 - Simple Turning Cycles; Radius Cycle G87 - Simple Turning Cycles

DIN/ISO programming | G codes from previous controls
4
504
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
Radius cycle G87 – simple turning cycles
G87 machines transition radii at orthogonal, paraxial inside and
outside corners. The direction is taken from the position of the
machining direction of the tool.
Parameters:
X: Edge (diameter value)
Z: Edge
B: Radius
E: Reduced feed
A preceding longitudinal or transverse element is machined if the
tool is located at the X or Z coordinate of the corner before the
cycle is executed.
The tool radius compensation is active
An oversize is not taken into account
Example: G87
. . .
N1 T3 G95 F0.25 G96 S200 M3
N2 G0 X70 Z2
N3 G1 Z0
N4 G87 X84 Z0 B2
Radius
Chamfer cycle G88 – simple turning cycles
G88 machines chamfers at orthogonal, paraxial outside corners.
The direction is taken from the position of the machining direction
of the tool.
Parameters:
X: Edge (diameter value)
Z: Edge
B: Cham. width
E: Reduced feed
A preceding longitudinal or transverse element is machined if the
tool is located at the X or Z coordinate of the corner before the
cycle is executed.
The tool radius compensation is active
An oversize is not taken into account
Example: G88
. . .
N1 T3 G95 F0.25 G96 S200 M3
N2 G0 X70 Z2
N3 G1 Z0
N4 G88 X84 Z0 B2
Chamfer