HEIDENHAIN CNC PILOT 640 User Manual page 135

smart.Turn units | Units – Drilling in C axis
ICP bore milling, C 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.
This cycle produces oval contours on the lateral surface,
and not circles.
Circles are machined when the Y axis is used.
Further information:
Page 207
Unit name: G75_BF_ICP_C_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
"ICP bore milling, Y axis units",
2
135