Contour And Figure Milling Cycle On Front Face G793 - HEIDENHAIN CNC PILOT 640 User Manual

4

Contour and figure milling cycle on front face G793

G793 mills figures or (open or closed) free contours.
G793 is followed by:
The figure to be milled with:
Contour definition of the figure (G301 to G307)
Further information:
Conclusion of milling contour (G80)
The free contour with:
Starting point of milling contour (G100)
Milling contour (G101, G102, G103)
Conclusion of milling contour (G80)
Preferentially use ICP and the G840, G845 and G846
cycles to program the contour description in the geometry
section.
Parameters:
ZS: Millg. top edge
ZE: Milling floor
P: Max. approach (default: Milling in one infeed)
U: Overlap factor – contour milling or pocket milling (default: 0)
U = 0: Contour milling
U > 0: Pocket milling—minimum overlap of milling paths =
U*milling diameter
R: Apprch angle (default: 0)
R = 0: Contour element is approached directly; infeed to
starting point above the milling plane—then vertical plunge
R > 0: Tool moves on approaching/departing arc that connects
tangentially to the contour element
R < 0 for inside corners: Tool moves on approaching/departing
arc that connects tangentially to the contour element
R < 0 for outside corners: Length of linear approaching/
departing element; contour element is approached/departed
tangentially
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: Up-cut
1: Climb
408
"Front/Rear face contours", Page 277
DIN/ISO programming | Milling cycles
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017