HEIDENHAIN SW 54843x-03 DIN Programming - Manual (Page 355)

HEIDENHAIN MANUALplus 620, CNC PILOT 640 355
4.26 Milling cy
cles
Area milling, face G797
Depending on Q, G797 mills surfaces, a polygon, or the figure defined
in the command following G797.
Parameters
ID
Milling contour—name of the contour to be milled
NS Block number—beginning of contour section
 Figures: Block number of the figure
 Free closed contour: First contour element (not starting
point)
X Limit diameter
ZS Milling top edge
ZE Milling floor
B Width across flats (omit for Q=0): B defines the remaining
material. For an even number of surfaces, you can program B
as an alternative to V.
 Q=1: B=residual depth
 Q>=2: B=width across flats
V Edge length (omitted for Q=0)
R Chamfer/rounding
A Inclination angle (reference: see help graphic)—omitted for
Q=0
Q Number of surfaces (default: 0): Range: 0 <= Q <= 127
 Q=0: G797 is followed by a figure definition (G301.. G307,
G80) or a closed contour definition (G100, G101 to G103,
G80)
 Q=1: One surface
 Q=2: Two surfaces offset by 180°
 Q=3: Triangle
 Q=4: Rectangle, square
 Q>4: Polygon
P Maximum approach (default: total depth in one infeed)
U Overlap factor (default: 0.5): Minimum overlap of milling paths
= U*milling diameter
I Contour-parallel oversize
K Oversize Z
F Infeed rate
E Reduced feed rate for circular elements (default: current feed
rate)
H Cutting direction (default: 0): The cutting direction can be
changed with H and the direction of tool rotation (see help
graphic)
 0: Up-cut milling
 1: Climb milling