HEIDENHAIN MANUALPLUS 620 User Manual

HEIDENHAIN MANUALplus 620 289
4.21 Undercut Cycles
Blocks following the cycle call
Undercut type U G856
G856 machines an undercut and finishes the adjoining plane surface.
A chamfer or rounding (optional) can be machined.
Tool position at the end of the cycle: Cycle starting point
Blocks following the cycle call
N.. G853 FP.. I.. K.. W.. /Cycle call
N.. G0 X.. Z.. /Corner point of cylinder start chamfer
N.. G1 Z.. /Undercut corner
N.. G1 X.. /End point of plane surface
N.. G80 /End of contour definition
 Undercuts can only be executed in orthogonal, paraxial
contour corners along the longitudinal axis.
 Cutting radius compensation: Active.
 Oversizes: are not taken into account.
Example: G856
%856.nc
[G856]
N1 T3 G95 F0.23 G96 S248 M3
N2 G0 X60 Z2
N3 G856 I47 K7 B1
N4 G0 X50 Z-30
N5 G1 X60
N6 G80
END
Parameters
I Undercut depth (default: value from standard table)
K Undercut length (default: value from standard table)
B Chamfer/rounding:
 B>0: Radius of rounding
 B<0: Chamfer width
N.. G856 I.. K.. /Cycle call
N.. G0 X.. Z.. /Undercut corner
N.. G1 X.. /End point of plane surface
N.. G80 /End of contour definition
 Undercuts can only be executed in orthogonal, paraxial
contour corners along the longitudinal axis.
 Cutting radius compensation: Active.
 Oversizes: are not taken into account.
 If the cutting width of the tool is not defined, the control
assumes that the tool's cutting width equals K.

HEIDENHAIN MANUALPLUS 620 Specifications

General

Brand	HEIDENHAIN
Model	MANUALPLUS 620
Category	Control Systems
Language	English