Contour And Figure Milling Cycle On Lateral Surface G794 - HEIDENHAIN CNC PILOT 640 User Manual

4
Contour and figure milling cycle on lateral surface
G794
G794 mills figures or (open or closed) free contours.
G794 is followed by:
The figure to be milled with:
Contour definition of the figure (G311 to G317)
Further information:
Conclusion of contour definition (G80)
The free contour with:
Starting point (G110)
Contour definition (G111, G112, G113)
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:
XS: Upper edge of milling
XE: 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
K: Contour-parallel oversize
I: O-size X
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
410
"Lateral surface contours", Page 284
DIN/ISO programming | Milling cycles
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017