HEIDENHAIN SW 548328-05 DIN Programming - Manual (Page 510)

510
DIN programming for the Y axis
6.7 Milling cy
cles f
o
r the Y axis
G845 (Y axis)—Milling
You can change the cutting direction with the "cutting direction H,"
the "machining direction Q" and the direction of tool rotation (see table
G845 in the User's Manual). Program only the parameters given in the
following table.
See also:
 G845—Fundamentals: Page 508
 G845—Calculating hole positions: Page 509
Parameters—Milling
ID Milling contour—name of the contour to be milled
NS Starting block no. of contour
 Figures: Block number of the figure
 Free closed contour: A contour element (not starting point)
B Milling depth (default: depth from the contour description)
P Maximum infeed (default: milling in one infeed)
XS Milling top edge in YZ plane (replaces the reference diameter
from the contour description)
ZS Milling top edge in XY plane (replaces the reference plane from
the contour description)
I Oversize in X direction (radius)
K Oversize in Z direction
U (Minimum) overlap factor. Defines the overlap of milling paths
(default: 0.5).
Overlap = U*milling diameter
V Overrun factor (default: 0.5). Defines the distance by which the
tool should pass the outside radius of the workpiece.
 0: The defined contour is milled completely
 0< V <= 1: Overrun = V*milling diameter
H Cutting direction (default: 0)
 0: Up-cut milling
 1: Climb milling
F Feed rate for infeed (default: active feed rate)
E Reduced feed rate for circular elements (default: current feed
rate)
RB Retraction plane (default: back to starting position)
 XY plane: Retraction position in Z direction
 YZ plane: Retraction position in X direction (diameter)
Q Machining direction (default: 0)
 0: From the inside out (from the inside towards the outside)
 1: From the outside in (from the outside towards the inside)
A Sequence for "Milling": A=0 (default=0)
NF Position mark—reference from which the cycle reads the hole
positions [1 to 127].