Bore Milling G75 - HEIDENHAIN CNC PILOT 640 User Manual

DIN/ISO programming | Drilling cycles

Bore milling G75

G75 is used for machining or deburring axial and radial bore holes
or hole patterns with a milling cutter. The milling cutter can also be
used to machine counterbores or enlarge holes.
Parameters:
ID: Hole dimensions – name of the hole definition
NS: Starting block no. of contour – beginning of contour
section
Reference to the contour of the hole (G49-Geo, G300-
Geo,G310-Geo, G71 or G73)
No input: single hole without contour description
O: Machining operation:
0: Roughing
1: Finishing
2: Roughing and finishing
3: Deburring
B: Milling depth (default: hole depth from the contour definition)
P: Max. approach (default: Milling in one infeed)
U: Overlap factor – overlap of milling paths = U*milling
diameter (default: 0.5)
H: Direction
0: Up-cut
1: Climb
I: O-size X
K: O-size Z
F: Approach feed for plunging (default: active feed rate)
RB: Return plane (default: retract to starting position or to
safety clearance; diameter value with radial holes and holes in
the YZ plane)
W: Plunging angle in infeed direction
WB: Diameter of the helix
Programming notes:
Only the contour description (ICP) for the C axis or Y
axis is used for bore milling.
NS refers to the hole contour, and not the definition
of the pattern.
If this cycle is used with the C axis, it machines
funnel-shaped oval contours on the lateral surface,
and not circles. Circles are machined when the Y axis
is used.
Further information:
Page 207
An active mirror function does not influence the type
of milling defined in the cycle.
Note that if the infeed distance is too large, the tool
or the workpiece may be damaged.
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
"ICP bore milling, Y axis units",
4
381