Icp Drilling, C Axis Unit - HEIDENHAIN CNC PILOT 640 User Manual

smart.Turn units | Units – Drilling in C axis

ICP drilling, C axis unit

The unit machines a single hole or a hole pattern on the face or
lateral surface. Using ICP, you define the positions of the holes as
well as further details.
Unit name: G74_ICP_C / cycle: G74
Further information: "Deep boring G74", Page 378
Pattern form:
FK: No. of ICP finished part – name of contour to be machined
NS: Starting block no. of contour – beginning of contour
section
Cycle form:
E: Period of dwell at end of hole (default: 0)
D: Retraction type
0: Rapid traverse
1: Feed rate
V: Feed reduction
0: Without reduction
1: At end of the hole
2: At start of the hole
3: At start & end of hole
AB: Drilling lengths (default: 0)
P: 1. Boring depth
IB: Hole depth reduct. val – value by which the hole depth
decreases after every infeed.
JB: Minimum hole depth
If you have entered a hole depth reduction value, the hole depth
is reduced only to the value entered in JB.
B: Return distance – value by which the tool is retracted after
reaching the respective hole depth
RI: Safety clearance internal – distance for reapproach inside
the hole (default: Safety clearance SCK)
RB: Return plane (default: back to start position)
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
2
129