HEIDENHAIN CNC PILOT 640 User Manual page 414

4
Programming:
The cycle calculates the milling depth from ZS and
ZE, taking the oversizes into account
Surfaces and figures defined with G797 (Q>0) are
symmetric with respect to the center. A figure
defined in the following command can be outside the
center.
G797 Q0 .. is followed by:
The figure to be milled with:
Contour definition of the figure (G301 to G307)
Further information:
Conclusion of contour definition (G80)
The free contour with:
Starting point of milling contour (G100)
Milling contour (G101, G102, G103)
Conclusion of milling contour (G80)
Example: G797
%797.nc
N1 T9 G197 S1200 G195 F0.2 M104
N2 M14
N3 G110 C0
N4 G0 X100 Z2
N5 G797 X100 Z0 ZE-5 B50 R2 A0 Q4 P2 U0.5
N6 G100 Z2
N7 M15
END
Example: G797 / G304
%304_G305.nc
N1 T7 G197 S1200 G195 F0.2 M104
N2 M14
N3 G110 C0
N4 G0 X100 Z2
N5 G797 X100 ZS0 ZE-5 Q0 P2 F0.15
N6 G304 XK20 YK5 R20
N7 G80
N4 G0 X100 Z2
N5 G797 X100 ZS0 ZE-5 Q0 P2 F0.15
N6 G305 XK20 YK5 R6 B30 K45 A20
N7 G80
N8 M15
END
414
"Front/Rear face contours", Page 277
DIN/ISO programming | Milling cycles
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017