Operation Manual

HEIDENHAIN CNC PILOT 640 191
4.4 Turning cycles
Cut, ICP contour-parallel, longitudinal
Select cut, longitudinal/transverse
Select ICP contour-parallel, longitudinal
The cycle roughs the defined area on contour-parallel paths.
 The cycle roughs contour parallel depending on the
workpiece blank oversize J and the type of cutting
lines H:
 J=0: The area defined by X, Z and the ICP contour,
taking the oversizes into account.
 J>0: The area defined by the ICP contour (plus
oversizes) and the workpiece blank oversize J.
 The tool plunges with the maximum possible angle,
leaving material remaining.
Danger of collision!
Workpiece blank oversize J>0: Set the infeed depth P to
the smaller infeed, if the maximum infeed differs for the
longitudinal and transverse directions due to the cutting
geometry.
Cycle parameters
X, Z Starting point
FK ICP finished part: Name of the contour to be machined
P Infeed depth—is determined taking J into account
 J=0: P is the maximum infeed depth. The cycle reduces
the infeed depth if the programmed infeed is not
possible in the transverse or longitudinal direction due to
the cutting geometry.
 J>0: P is the infeed depth. This infeed is used in the
longitudinal and transverse directions.
H Type of cutting lines—the cycle machines
 0: with constant cutting depth
 1: with equidistant cutting lines
I, K Oversize X, Z
J Workpiece blank oversize—the cycle machines
 J=0: From the current tool position
 J>0: The area defined by the workpiece blank oversize