Cutting With Relief Cut - Cycle95 - Siemens sinumerik 808d Programming And Operating Manual

2.5.5

Cutting with relief cut - CYCLE95

Programming
CYCLE95(NPP, MID, FALZ, FALX, FAL, FF1, FF2, FF3, VARI, DT, DAM, _VRT)
Parameters
Parameter
NPP
MID
FALZ
FALX
FAL
FF1
FF2
FF3
VARI
TT
DAM
_VRT
Function
Using the rough turning cycle, you can produce a contour, which has been programmed in a
subroutine, from a blank by paraxial stock removal. The contour may contain relief cut
elements. It is possible to machine contours using longitudinal and face machining, both
externally and internally. The technology can be freely selected (roughing, finishing,
complete machining). When roughing the contour, paraxial cuts from the maximum
programmed infeed depth are programmed and burrs are also removed parallel to the
contour after an intersection point with the contour has been reached. Roughing is
performed up to the final machining allowance programmed.
Finishing is performed in the same direction as roughing. The tool radius compensation is
selected and deselected by the cycle automatically.
Turning Part 2: Programming (Siemens instructions)
Programming and Operating Manual, 05/2012, 6FC5398-5DP10-0BA0
Data type Description
STRING Name of contour subroutine
REAL Infeed depth (enter without sign)
REAL Finishing allowance in the longitudinal axis (enter without sign)
REAL Finishing allowance in the transverse axis (enter without sign)
REAL Finishing allowance according to the contour (enter without sign)
REAL Feedrate for roughing without undercut
REAL Feedrate for insertion into relief cut elements
REAL Feedrate for finishing
REAL Machining type
Range of values: 1 ... 12
REAL Dwell time fore chip breaking when roughing
REAL Path length after which each roughing step is interrupted for chip
breaking
REAL Lift-off distance from contour when roughing, incremental (to be
entered without sign)
Cycles
2.5 Turning cycles
161