Siemens SINUMERIK 840D Programming Manual page 160

Milling Cycles
3
3.11 Face milling - CYCLE71
_FDP1 (overrun travel)
By means of this parameter an overrun travel in the
direction of the plane infeed may be defined (_MIDA)
allowing the deviation between the current cutter radius
and the cutting edge (e.g. tool nose radius or inclined
cutting tips) to be compensated. The last cutter center
point path therefore always corresponds to _LENG (or
_WID) + _FDP1 tool radius (from correction table).
_FALD (final machining allowance)
During roughing, the depth finishing allowance used
is defined by this parameter.
The residual material designated as the finishing
allowance must always be specified for finish cutting
so as to ensure that the tool can be lifted and
inserted at the starting point of the next cut without
risk of collision.
_VARI (machining mode)
You can define the type of machining with parameter
_VARI.
Possible values are:
Units digit:
1=Roughing to final machining allowance
2=Finishing
Tens digit:
• 1=Parallel to the abscissa, in one direction
• 2=Parallel to the ordinate, in one direction
• 3=Parallel to the abscissa, with changing direction
• 4=Parallel to the ordinate, with changing direction
If another value has been programmed for
parameter _VARI, the cycle is aborted after alarm
61002 "Machining type incorrectly defined" is output.
Further notes
A tool offset must be activated before the cycle is
called. Otherwise the cycle is aborted and alarm
61000 "No tool offset active" is output.
3-160
Mill diameter from tool table
SINUMERIK 840D/840Di/810D/FM-NC Programming Guide, Cycles (PGZ) - 04.00 Edition
03.96
12.98
_FDP1
Surface
 Siemens AG 2000 All rights reserved.
3