Siemens SINUMERIK 808D ADVANCED Programming And Operating Manual page 172

Examples:
_KNAME="CONTOUR_1"
_KNAME="PIECE245:PIECE245E"
_LP1, _LP2 (length, radius)
Use the parameter _LP1 to program the approach travel or approach radius (distance from the tool external edge to the
contour starting point), and the parameter _LP2 to program the retraction travel or retraction radius (distance from the tool
external edge to the contour end point).
Parameters _LP1 and _LP2 must be set to >0. In the case of zero, error 61116 "Approach or retraction path=0" is output.
Note
When using G40, the approach or retraction travel is the distance from the tool center point to the start or end point of the
contour.
_VARI (machining type)
Use the parameter _VARI to define the machining type.
If a different value is programmed for the parameter _VARI, the cycle is aborted after output of alarm 61002 "Machining type
defined incorrectly".
_RL (bypassing the contour)
With the parameter _RL, you program the traveling around the contour centrally, to the right or to the left with G40, G41 or
G42.
_AS1, _AS2 (approach direction/path, retraction direction/path)
Use the parameter _AS1 to program the specification of the approach path and _AS2 to program that of the retraction path.
If _AS2 is not programmed, then the behavior of the retraction path is analogous to that of the approach path.
Smooth approach of the contour along a spatial path (helix or straight line) should only be programmed if the tool is not yet
being used or is suitable for this type of approach.
172
The milling contour is the complete
program CONTOUR_1.
The milling contour is defined as a
section in the calling program, which
starts from the block containing label
PIECE245 to the block containing label
PIECE245E.
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA1, 01/2014