HEIDENHAIN CNC PILOT 640 User Manual page 427

DIN/ISO programming | Milling cycles
G845 – milling
You can change the cutting direction with the cutting direction
H, the machining direction Q and the direction of tool rotation.
Program only the parameters given in the following table.
See also:
G845—Fundamentals
Further information:
G845—Calculating hole positions
Further information:
Page 426
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 (no effect with C-axis machining)
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)
Front or rear face: Return position in Z direction
Lateral surface: 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)
NF: Position mark – reference at which the cycle stores the
hole positions (range: 1 to 127)
O: Plunging behavior (default: 0)
O=0 (vertical plunging): The cycle moves the tool to the
starting point; the tool plunges at the feed rate for infeed and
mills the pocket
O=1 (plunge at pre-drilled position):
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
"G845 – fundamentals", Page 425
"G845 – calculating hole positions",
4
427