Pocket Milling - Finishing G846 (Y Axis) - HEIDENHAIN CNC PILOT 640 User Manual

DIN/ISO Programming for the Y axis | Milling cycles for the Y axis

Pocket milling - finishing G846 (Y axis)

G846 finishes closed contours defined in the XY or YZ plane in the
program sections:
FRONT Y
REAR SIDE Y
SURFACE Y
You can change the cutting direction with the Mill cutting direction
H, the Machining direction Q and the direction of tool rotation.
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)
B: Milling depth (default: hole depth from the contour definition)
P: Max. approach (default: Milling in one infeed)
XS: Millg. top edge lateral surface (replaces the reference plane
from the contour definition)
ZS: Millg. top edge face (replaces the reference plane from the
contour definition)
R: Apprch angle (default: 0)
R=0: Contour element is approached directly. Feed to the
starting point above the milling plane, then vertical plunge
R>0: Tool moves on approaching/departing arc that connects
tangentially to the contour element
U: Overlap factor – defines the overlap of milling paths (default:
0.5) (range: 0 to 0.99)
Overlap = U * milling diameter
V: Overrun factor – defines the distance by which the tool
should pass the outside radius of the workpiece (default: 0.5)
Overrun = V * milling diameter
H: Mill cutting direction
0: Up-cut
1: Climb
F: Approach feed for plunging (default: active feed rate)
E: Reduced feed for circular elements (default: active feed rate)
RB: Return plane (default: back to start position)
XY plane: Retraction position in Z direction
YZ plane: Return position in X direction (diameter)
Q: Mach. direction (default: 0)
0: From the inside out
1: From the outside in
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
6
603