HEIDENHAIN CNC PILOT 640 User Manual page 421

DIN/ISO programming | Milling cycles
O: Plunging behavior (default: 0)
O=0: Vertical plunging
O=1: With predrilling
If NF is programmed: The cycle positions the milling cutter
above the first hole position saved in NF, then plunges and
mills the first section. If applicable, the cycle positions the
tool to the next pre-drilled hole and mills the next section,
etc.
If NF is not programmed: The tool plunges at the current
position and mills the section. If required, repeat this
operation for the next section, etc.
Approach and departure: For closed contours, the point of the surface
normal from the tool position to the first contour element is the
point of approach and departure. If no surface normal intersects
the tool position, the starting point of the first element is the point
of approach and departure. For figures, use D and V to select the
approach/departure element.
Cycle run:
1 Starting position (X, Z, C) is the position before the cycle begins
2 Calculates the milling depth infeeds
3 Approaches to safety clearance:
If O=0: Infeed to the first milling depth
If O=1: Plunges to the first milling depth
4 Mills the contour
5 Infeeds:
For open contour and slots with slot width equal to the cutter
diameter: Moves at feed rate to the next milling depth, or
plunges at rapid to the next milling depth and mills the contour
in reverse direction
For closed contours and slots: Lifts off by the safety clearance,
moves forward and approaches to the next milling depth, or
plunges to the next milling depth
6 Repeats steps 4 and 5 until the complete contour is milled
7 Returns to Return plane RB
You can change the machining direction and the cutter radius
compensation (TRC) with the cycle type Q, the cutting direction H
and the rotational direction of the tool. Program only the parameters
given in the following table.
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
4
421