Operation Manual

HEIDENHAIN CNC PILOT 640 241
4.5 Recessing cycles
Type of machining for technology database access: Recess turning
Cycle run
1 Calculate the proportioning of cuts
2 Approach the workpiece from starting point for first pass
3 Execute the first cut (recessing)
4 Machine perpendicularly to recessing direction (turning)
5 Repeat 3 to 4 until contour end point X2, Z2 is reached
6 Return to starting point on paraxial path
7 Move to the tool change point according to the G14 setting
Cycle parameters
X, Z Starting point
X2, Z2 Contour end point
P Infeed depth: Maximum infeed depth
O Recessing feed rate (default: active feed rate)
B Offset width (default: 0)
U Unidirectional turning (default: 0)
 0: Bidirectional
 1: Unidirectional
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