Siemens SINUMERIK 840D Programming Manual page 296

4
Turning Cycles
4.5 Stock removal cycle – CYCLE95
FAL, FALZ and FALX (final machining allowance)
The final machining allowance for the roughing operation
is either defined in parameters FALZ and FALX if you
wish to enter different final machining allowances for
each axis or in parameter FAL if you wish to enter a final
machining allowance that follows a contour. In this case,
this value is used for the final machining allowance in
both axes.
The programmed values are not subjected to a
plausibility check. If all three parameters are assigned
values, all the final machining allowances are calculated
by the cycle. It is, however, advisable to decide on one or
the other form of final machining allowance definition.
Roughing is always performed to these final machining
allowances. After each paraxial roughing operation the
resulting residual corners are immediately cut parallel to
the contour so that these do not have to be removed after
the roughing operation is completed. If no final machining
allowances have been programmed, roughing is
performed to the final contour.
The finish cut machining mode does not consider
programmed values. Turning always takes place down
to finishing dimension.
FF1, FF2 and FF3 (feedrate)
You can define different feedrates for the different
machining steps as is shown in the figure on the
right.
4-296
X
FF1
X
FF3
SINUMERIK 840D/840Di/810D Programming Guide Cycles (PGZ) – 11.02 Edition
4
03.96
10.00
G1/G2/G3
G0
Roughing
FF2
FF1
Z
Finishing
Z
© Siemens AG, 2002. All rights reserved