Operation Manual

HEIDENHAIN CNC PILOT 640 177
4.4 Turning cycles
Cut, transverse plunge
Select cut, longitudinal/transverse
Select plunge, transverse
The cycle roughs the area described by the contour starting point,,
contour end point and plunge angle.
Type of machining for technology database access: Roughing
 The tool plunges with the maximum possible angle,
leaving material remaining.
 The steeper the tool plunges into the material, the
greater the feed rate decrease (max. 50%).
Cycle parameters
X, Z Starting point
X1, Z1 Contour starting point
X2, Z2 Contour end point
P Infeed depth: Maximum infeed depth
H Contour smoothing
 0: With every cut
 1: With the last cut
 2: No finishing cut
A Plunge angle (range: 0° <= A < 90°; default: 0°)
W End angle—oblique cut at contour end
(range: 0° <= W < 90°)
G47 Safety clearance (siehe Seite 140)
G14 Tool change point (siehe Seite 140)
T Turret pocket number
ID Tool ID number
S Spindle speed/cutting speed
F Feed per revolution
MT M after T: M function that is executed after the tool call T.
MFS M at beginning: M function that is executed at the
beginning of the machining step.
MFE M at end: M function that is executed at the end of the
machining step.
WP Displays which workpiece spindle is used to process the
cycle (machine-dependent)
 Main drive
 Opposing spindle for rear-face machining