Area Milling On Front Face G797 - HEIDENHAIN CNC PILOT 640 User Manual

DIN/ISO programming | Milling cycles

Area milling on front 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 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)
X: Limit diameter
ZS: Millg. top edge
ZE: Milling floor
B: Width/Width across flats
Omit for Q=0: 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: Chamf./round. (default: 0)
A: Inclinat. ang. omitted for Q = 0 (reference: see help graphic)
Q: No. 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: Max. approach (default: Milling in one infeed)
U: Overlap factor – overlap of milling paths = U*milling
diameter (default: 0.5)
I: Contour-parallel oversize
K: O-size Z
F: Approach feed for plunging (default: active feed rate)
E: Reduced feed for circular elements (default: active feed rate)
H: Mill cutting direction
0: Roughing
1: Finishing
O: Roughing/Finish
0: Roughing
1: Finishing
J: Mill direction
0: Unidirectional
1: Bidirectional
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
4
413