Siemens SINUMERIK 840D Programming Manual page 221

03.96
08.99
4
If the parameter is assigned another value, the cycle
is aborted and alarm 61002 "Machining type
incorrectly programmed".
The contour monitoring performed by the cycle
ensures that a realistic groove contour results. This
is not the case if the radii/chamfers touch each other
at the base of the groove or overlap or if an attempt
at face grooving is made on a section of the contour
that runs parallel to the longitudinal axis. The cycle is
then aborted and alarm 61603 "Groove form
incorrectly defined" is output.
Further notes
You must activate a double-edged tool before calling
the grooving cycle. You must enter the offset values
for the two tool edges in two successive D numbers
of the tool, the first of which must be activated before
the cycle is called. The cycle determines itself which
of the two tool offsets it requires for which machining
step and activates them automatically. After the
cycle is completed, the offset number programmed
before the cycle call becomes active again. If no D
number has been programmed for a tool offset when
the cycle is called, the cycle is aborted with alarm
61000 "No tool offset active" and the cycle is
aborted.
For SW 5.1 and higher, cycle setting data _ZSD[4]
can be used to influence the retraction after the 1st
groove.
_ZSD[4]=0 means retraction with G1 as before,
_ZSD[4]=1 means retraction with G0.
 Siemens AG 2000 All rights reserved.
SINUMERIK 840D/840Di/810D/FM-NC Programming Guide, Cycles (PGZ) - 04.00 Edition
4.3 Grooving cycle – CYCLE93
Turning Cycles
4
4-221