HEIDENHAIN CNC PILOT 640 User Manual page 599

DIN/ISO Programming for the Y axis | Milling cycles for the Y axis
G845 (Y axis)—Milling
You can change the cutting direction with the Direction H, the
machining direction Q and the direction of tool rotation.
Program only the parameters given in the following table.
More information:
G845—Fundamentals:
roughing G845 (Y axis)", Page 597
G845—Calculating hole positions:
(Y axis)—calculating hole positions", Page 598
Parameters:
ID: Milling contour – name of the milling contour
NS: Starting block no. of contour – beginning of contour
section
Figures: Block number of the figure
Free closed contour: First contour element (not starting
point)
B: Milling depth (default: hole depth from the contour definition)
P: Max. approach (default: Milling in one infeed)
XS: Millg. top edge lateral surface (replaces the reference plane
from the contour definition)
ZS: Millg. top edge face (replaces the reference plane from the
contour definition)
I: O-size X
K: O-size Z
U: Overlap factor – defines the overlap of milling paths (default:
0.5) (range: 0 to 0.99)
Overlap = U * milling diameter
V: Overrun factor – defines the distance by which the tool
should pass the outside radius of the workpiece (default: 0.5)
0: The defined contour is milled completely
0 < V <= 1: Overrun = V * milling diameter
H: Mill cutting direction
0: Up-cut
1: Climb
F: Approach feed for plunging (default: active feed rate)
E: Reduced feed for circular elements (default: active feed rate)
RB: Return plane (default: back to start position)
XY plane: Retraction position in Z direction
YZ plane: Return position in X direction (diameter)
Q: Mach. direction (default: 0)
0: From the inside out
1: From the outside in
A: (Mill=0/PredrillPos=1) (default: 0)
NF: Position mark – reference at which the cycle stores the
hole positions (range: 1 to 127)
O: Plunging behavior (default: 0)
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
Further information: "Pocket milling -
Further information: "G845
6
599