Siemens SINUMERIK 808D ADVANCED Programming And Operating Manual page 186

NUM (number)
Use the parameter NUM to specify the number of long holes.
LENG (long hole length)
The length of the long hole is programmed under LENG.
If it is detected in the cycle that this length is smaller than the milling diameter, the cycle is aborted with alarm 61105 "Milling
radius is too large".
MID (infeed depth)
Use this parameter to define the maximum infeed depth.
The depth infeed is performed by the cycle in equally-sized infeed steps.
Using MID and the total depth, the cycle automatically calculates this infeed which lies between 0.5 x maximum infeed depth
and the maximum infeed depth. The minimum possible number of infeed steps is used as the basis. MID=0 means that the
cut to pocket depth is made with one feed.
The depth infeed starts from the reference plane brought forward by the safety clearance (depending on _ZSD[1]).
FFD and FFP1 (feedrate for depth and surface)
The feedrate FFP1 is active for all movements in the plane traversed at feedrate. FFD acts for infeeds vertically to this plane.
CPA, CPO and RAD (center point and radius)
You define the position of the circle in the machining plane by the center point (CPA, CPO) and the radius (RAD). Only
positive values are permitted for the radius.
STA1 and INDA (starting and incremental angle)
The arrangement of the long holes on the circle is defined by these parameters.
If INDA=0, the indexing angle is calculated from the number of long holes, so that they are equally distributed around the
circle.
Note
A tool compensation must be programmed before the cycle is called. Otherwise, the cycle is aborted and alarm 61000 "No
tool compensation active" is output.
If mutual contour violations of the slots result from incorrect values of the parameters that determine the arrangement and
the size of the slots, the cycle will not start the machining. The cycle is aborted and the error message 61104 "Contour
violation of slots/elongated holes" is output.
During the cycle, the workpiece coordinate system is offset and rotated. The values in the workpiece coordinate system are
shown on the actual value display such that the longitudinal axis of the long hole being machined is positioned on the first
axis of the current machining plane.
After the cycle has been completed, the workpiece coordinate system is in the same position again as it was before the
cycle was called.
Programming and Operating Manual (Milling)
186
6FC5398-4DP10-0BA1, 01/2014