HEIDENHAIN CNC PILOT 640 User Manual page 209

smart.Turn units for the Y axis | Units – Drilling in Y axis
ICP bore milling, Y axis, lateral surface unit
The unit machines a single hole or a hole pattern on the lateral
surface. Using ICP, you define the positions of the holes as well as
further details.
Only the contour description (ICP) for the C axis or Y
axis is used for bore milling.
Unit name: G75_BF_ICP_Y_MANT / cycle: G75
Further information: "Bore milling G75", Page 381
Contour form:
FK: Finished part contour – name of the contour to be
machined
NS: Starting block no. of contour – beginning of contour
section
FZ: Approach feed (default: active feed rate)
B: Milling depth (default: hole depth from the contour definition)
Cycle form:
QK: Machining operation
0: Roughing
1: Finishing
2: Roughing and finishing
H: Mill cutting direction
0: Up-cut
1: Climb
P: Max. approach (default: Milling in one infeed)
I: Contour-parallel oversize
K: Infeed-direction oversize
WB: Diameter of the helix
EW: Plunging angle
U: Overlap factor – overlap of milling paths = U*milling
diameter (default: 0.5)
RB: Return plane (default: retract to starting position or to
safety clearance; diameter value with radial holes and holes in
the YZ plane)
Further forms:
Further information: "smart.Turn unit", Page 78
Access to the technology database:
Machining operation: milling
Affected parameters: F, S, FZ, P
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
3
209