HEIDENHAIN CNC PILOT 640 User Manual page 600

6
O=0 (vertical plunging): The cycle moves the tool to the
starting point; the tool plunges at the feed rate for infeed and
mills the pocket
O=1 (plunge at pre-drilled position):
If NF is programmed: The cycle positions the milling
cutter above the first pre-drilled hole; the tool plunges and
mills the first area. If applicable, the cycle positions the
tool to the next pre-drilled hole and mills the next area,
etc.
If NF is not programmed: The cycle plunges at the current
position and mills the area. If applicable, position the tool
to the next pre-drilled hole and mill the next area, etc.
O=2 or 3 (plunge in a helical motion): The tool plunges at the
angle W and mills full circles with the diameter WB. As soon
as it reaches the milling depth P, the cycle switches to face
milling
O=2—manually: The cycle plunges at the current position
and machines the area that can be reached from this
position
O=3—automatically: The cycle calculates the plunging
position, plunges and machines this area. The plunging
motion ends at the starting point of the first milling path,
if possible. If the pocket consists of multiple areas, the
cycle successively machines all the areas
O=4 or 5 (reciprocating linear plunge): The tool plunges at
the angle W and mills a linear path of length WB. You can
define the orientation angle in WE. 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
O=4—manually: The cycle plunges at the current position
and machines the area that can be reached from this
position
O=5—automatically: The cycle calculates the plunging
position, plunges and machines this area. The plunging
motion ends at the starting point of the first milling path,
if possible. If the pocket consists of multiple areas, the
cycle successively machines all the areas. The plunging
position is determined from the type of figure and from Q
as follows:
Q0 (from the inside toward the outside):
Linear slot, rectangle, polygon: Reference point of
the figure
Circle: Circle center
Circular slot, free contour: Starting point of the
innermost milling path
Q1 (from the outside toward the inside):
Linear slot: Starting point of the slot
Circular slot, circle: Not machined
Rectangle, polygon: Starting point of the first linear
element
Free contour: Starting point of the first linear
element (at least one linear element must exist)
600
DIN/ISO Programming for the Y axis | Milling cycles for the Y axis
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017