Siemens SINUMERIK 840D Programming Manual page 234

Turning Cycles 03.96
12.98
4 4
4.5 Stock removal cycle – CYCLE95
All the traversing blocks for the first two axes in the
current plane are preprocessed in the cycle as only
these axes are involved in the machining operation.
Movements for other axes can be included in the
contour subroutine but their travel paths are
suppressed during the cycle run.
The only geometry permitted in the contour are
straight line and circular programming with G0, G1,
G2 and G3. Commands for fillets and chamfers can
also be programmed. If any other motion commands
are programmed in the contour, it is aborted with
alarm 10930 "Illegal interpolation type in the
machining contour".
The first block containing a traversing movement in
the current machining plane must contain a travel
command G0, G1, G2 or G3, otherwise the cycle is
aborted with the alarm 15800 "Wrong starting
conditions for CONTPRON".
This alarm is also activated when G41/G42 is active.
The starting point of the contour is the first position
on the machining plane programmed in the contour
subroutine.
The maximum possible number of blocks for the
contour containing travel commands for the current
plane depends on the type of contour. In principle,
there is no limit to the possible number of relief cuts.
If a contour contains more contour elements than
the cycle memory can hold, the cycle is aborted with
the alarm 10934 "Overflow contour table".
 Siemens AG 2000 All rights reserved.
4-234
SINUMERIK 840D/840Di/810D/FM-NC Programming Guide, Cycles (PGZ) - 04.00 Edition