Siemens SINUMERIK 840D Programming Manual page 283

4
03.96
09.01
FAL1 and FAL2 (machining allowance)
You can program separate final machining allowances
for the groove base and the flanks. Roughing is
performed to this final machining allowance. Then, the
same tool is used to machine a contour-parallel cut
along the final contour.
IDEP (infeed depth)
By programming an infeed depth you can divide the
paraxial grooving action into several depth infeeds.
After every infeed, the tool is retracted for
chipbreaking by 1 mm or, from SW 6.2 or higher
onwards, by the distance programmed under _VRT.
Parameter IDEP, anyway, is to be programmed.
DTB (dwell time)
A dwell time at the base of the groove should be
chosen that allows at least one spindle revolution.
The dwell time is programmed in seconds.
VARI (type of processing)
The units digit of the VARI parameter determines the
type of processing for the groove. This parameter
can be assigned any of the values shown in the
figure.
The tens value of the VARI determines the type of
calculation for the chamfer.
VARI 1...8: Chamfers are calculated as CHF
VARI 11...18: Chamfers are calculated as CHF
Input of the ones position in cycle support is
distributed among three selection fields:
1. Field: longitudinal/plane
2. Field: external/internal
3. Field: starting point left/right (for longitudinal) or
top/bottom (for plane)
© Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Cycles (PGZ) – 11.02 Edition
4.3 Grooving cycle – CYCLE93
VARI
1/11
X
X
5/15
3/13
X
7/17
X
6/16
X
8/18
X
2/12
X
4/14
X
4
Turning Cycles
Final machining
allowance on
flanks, FAL2
Final machining
at base, FAL1
Selection of cycle support
longitudinal, external,
left
Z
longitudinal, external,
right
Z
longitudinal, internal,
left
Z
longitudinal, internal,
right
Z
plane, external, top
Z
plane, external, bottom
Z
plane, internal, top
Z
plane, internal, bottom
Z
4-283