Siemens sinumerik 808d Programming And Operating Manual page 154

Cycles
2.5 Turning cycles
VARI (machining type)
The machining type of the groove is defined with the units digit of the VARI parameter. It can
assume the values indicated in the illustration.
The tens digit of parameter VARI determines how the chamfers are taken into account.
VARI 1...8: Chamfers are calculated as CHF
VARI 11...18: Chamfers are calculated as CHR
If the parameter has a different value, the cycle will abort with alarm 61002 "Machining type
defined incorrectly".
The cycle carries out a contour monitoring such that a reasonable groove contour results.
This is not the case if the radii/chamfers come into contact or intersect at the groove base or
if you try to carry out a face grooving operation at a contour segment located parallel to the
longitudinal axis. In such cases, the cycle will abort with alarm 61603 "Groove form defined
incorrectly".
_VRT (variable retraction path)
The retraction path can be programmed in the _VRT parameter on the basis of the outside or
inside diameter of the groove.
For VRT=0 (parameter not programmed), the tool is retracted by 1 mm. The retraction path
is always measured according to the programmed system of units, inch or metric.
The same retraction path is also used for chip breaking after each depth infeed into the
groove.
Note
Before calling the grooving cycle, a double-edged tool must be enabled. The offset values for
the two cutting edges must be stored in two successive D numbers of the tool whereby the
first of which must be activated prior to the first cycle call. The cycle itself defines for which
machining step it will use which of the two tool compensation values and will also enable
them automatically. After completion of the cycle, the tool compensation number
programmed prior to the cycle call is active again. If no D number is programmed for a tool
compensation when the cycle is called, the execution of the cycle is aborted with the alarm
61000 "No tool compensation active".
154
Turning Part 2: Programming (Siemens instructions)
Programming and Operating Manual, 05/2012, 6FC5398-5DP10-0BA0