Siemens SINUMERIK 840D sl Programming Manual page 707

No. Param Param
mask internal
6 F FF1
FY FF2
7
8 FS FF3
9 VARI
10 DT DT
11 DI DAM
VRT _VRT
12
13 _GMODE
14 _DMODE
Job Planning
Programming Manual, 03/2013, 6FC5398-2BP40-3BA1
Explanation
Feedrate for roughing
Insertion feedrate, relief cuts
Finishing feedrate
Machining type
UNITS and TENS:
1 = Roughing, longitudinal, external
2 = Roughing, transverse, external
3 = Roughing, longitudinal, internal
4 = Roughing, transverse, internal
5 = Finishing, longitudinal, external
6 = Finishing, transverse, external
7 = Finishing, longitudinal, internal
8 = Finishing, transverse, internal
9 = Complete machining, longitudinal, external
10 = Complete machining, transverse, external
11 = Complete machining, longitudinal, internal
12 = Complete machining, transverse, internal
HUNDREDS:
0 = With rounding at the contour, without residual corners
1 = Without rounding at the contour
2 = Rounding only to previous intersection, residual corners can result
Dwell time at feed interruption
Distance for feed interruptions
Lift-off distance from the contour
0 = A lift-off distance of 1 mm is used internally regardless of the active system (inch or
metric)
> 0 = Lift-off distance
Geometrical mode (evaluation of programmed geometrical data)
UNITS: Evaluation of the infeed depth
0 = Infeed depth is calculated corresponding to the G group DIAMON/DIAMOF
1 = Infeed depth acts as radius value (independent of DIAMON/DIAMOF)
Display mode
UNITS: Machining plane G17/18/19
0 = Compatibility, the plane effective before cycle call remains active
1 = G17 (only active in the cycle)
2 = G18 (only active in the cycle)
3 = G19 (only active in the cycle)
THOUSANDS:
0 = Compatibility mode: Contour name is in NPP
1 = Contour name is programmed in CYCLE62 and transferred to _SC_CONT_NAME
Programming cycles externally
18.1 Technology cycles
707