Hidden parameters
The following parameters are hidden. They are pre-assigned fixed values or values that can
be adjusted using setting data.
Parameter
Description
Value
Can be set in SD
PL (only for G code) Machining plane
Defined in MD
52005
SC (only for G
code)
Safety clearance
1 mm
x
Reference point
Position of the reference point: Center
Machining
position
Mill slot at the programmed position (X0, Y0, Z0).
Single posi‐
tion
α0
Angle of rotation
0°
Machine manufacturer
Please refer to the machine manufacturer's specifications.
10.2.10
Long hole (LONGHOLE) - only for G code programs
Function
In contrast to the groove, the width of the elongated hole is determined by the tool diameter.
Internally in the cycle, an optimum traversing path of the tool is determined, ruling out
unnecessary idle passes. If several depth infeeds are required to machine an elongated hole,
the infeed is carried out alternately at the end points. The path to be traversed in the plane
along the longitudinal axis of the elongated hole changes its direction after each infeed. The
cycle searches for the shortest path when changing to the next elongated hole.
Note
The cycle requires a milling cutter with a "face tooth cutting over center" (DIN 844).
Approach/retraction
1. Using G0, the starting position for the cycle is approached. In both axes of the current plane,
the closest end point of the first elongated hole to be machined is approached at the level
of the retraction plane in the tool axis and then lowered to the reference point shifted by
the amount of the safety clearance.
2. Each elongated hole is milled in a reciprocating motion. The machining in the plane is
performed using G1 and the programmed feedrate. At each reversal point, the infeed to
the next machining depth calculated internally in the cycle is performed with G1 and the
feedrate, until the final depth is reached.
Programming technological functions (cycles)
10.2 Milling
Milling
Operating Manual, 08/2018, 6FC5398-7CP41-0BA0
469
