HEIDENHAIN MANUALplus 4110 - Manual (Page 520)

520 9 Examples
9.7 DIN Pr
ogr
a
mming Example "Milling Cy
cle"
DIN program "face milling"
%2005.nc Program number of the DIN program
[Example of face milling] Program description
N1 M5 Spindle STOP
N2 G197 S3183 G195 F0.12 M103 Program the speed, feed rate
N3 T40 Call the milling tool
N4 M14 Activate the C axis
N5 G110 C0 Position the C axis
N6 G0 X80 Z2 Approach the workpiece
N7 G793 Z0 ZE-6 P3 U0.5 I1 K0.15 F0.1 E0.08
H0 Q0 "Contour milling, face" (roughing cycle)
N8 G100 XK20 YK5 Starting point of contour definition for cycle G793
N9 G101 XK50 B5 Contour definition
N10 G103 XK5 YK50 R50 Q1 B5
N11 G101 XK5 YK20 B5
N12 G102 XK20 YK5 R20 B5
N13 G80 End of contour definition
N14 M15 Deactivate the C axis
N15 G14 Q0 Retract the tool (approach the tool change position)
N16 M30 End of program
END