Pocket Milling - Finishing G846 - HEIDENHAIN CNC PILOT 640 User Manual

DIN/ISO programming | Milling cycles

Pocket milling - finishing G846

G846 finish-machines closed contours.
If the pocket consists of multiple sections, G846 takes all the
sections of the pocket into account.
You can change the cutting direction with the 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 (no effect with C-axis machining)
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)
Front or rear face: Return position in Z direction
Lateral surface: Return position in X direction (diameter)
Q: Mach. direction (default: 0)
0: From the inside out
1: From the outside in
O: Plunging behavior (default: 0)
O=0 (plunge vertically): The cycle moves the tool to the
starting point; the tool plunges and finishes the pocket
O=1 (approaching arc with depth feed): When machining
the upper milling planes, the tool advances to the milling
plane and then approaches on an arc. When machining the
bottom milling plane, the tool plunges to the milling depth
while moving on the approaching arc (three-dimensional
approaching arc). You can use this approach behavior only in
conjunction with an approaching arc R. The precondition is
machining from the outside toward the inside (O=1)
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
4
431