HEIDENHAIN CNC PILOT 640 User Manual page 601

DIN/ISO Programming for the Y axis | Milling cycles for the Y axis
O=6 or 7 (reciprocating circular plunge): The tool plunges at
the plunging angle W and mills a circular arc of 90°. The cycle
then mills along this path in the opposite direction. As soon
as it reaches the milling depth P, the cycle switches to face
milling. WE defines the arc center, WB the arc radius
O=6—manually: The tool position corresponds to the
center of the circular arc. The tool moves to the arc
starting point and plunges
O=7—automatically (only permitted for circular slots and
circles): The cycle calculates the plunging position on the
basis of Q:
Q0 (from the inside toward the outside):
Circular slot: The circular arc lies on the curvature
radius of the slot
Circle: Not permitted
Q1 (from the outside toward the inside): Circular slot,
circle: The circular arc lies on the outermost milling
path
W: Plunging angle in infeed direction
WE: Position angle of the milling path/circular arc
Reference axis:
Front or rear face: Positive XK axis
Lateral surface: Positive Z axis
Default orientation angle, depending on O:
O=4: WE=0°
O=5 and
Linear slot, rectangle, polygon: WE = orientation angle of
the figure
Circular slot, circle: WE=0°
Free contour and Q0 (from the inside toward the outside):
WE=0°
Free contour and Q1 (from the outside toward the inside):
Orientation angle of the starting element
WB: Diameter rework (default: 1.5 * milling diameter)
Cutting direction, machining direction and direction of tool rotation.
For the machining direction
toward the inside), please note:
The contour must start with a linear element
If the starting element is < WB, WB is reduced to the
length of the starting element
The length of the starting element must not be less
than 1.5 times the diameter of the milling cutter
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
(from the outside
Q=1
6
601