Siemens SINUMERIK 840D Programming Manual page 199

03.96
08.99
3
3.15 Pocket milling with islands - CYCLE73, CYCLE74, CYCLE75
_RAD (center-point path or insertion angle)
Parameter _RAD defines the radius of the helical path
(referred to tool center point path) or the maximum
insertion angle for oscillation.
_DP1 (insertion depth for helical path)
With the parameter _DP1 you define the infeed
depth for insertion on the helical path.
Further notes
Name for pocket machining (NAME)
Pockets are generally machined in several
technological machining steps. However, the contours
defining the pocket geometries are defined only once.
To ensure that contours can be automatically assigned
to the appropriate machining step in the program, the
contour definition is marked with labels and this
program section then repeated later with the REPEAT
instruction.
When programs are written using the cycles support
function, a name for the pocket machining program is
therefore entered in the respective screen forms.
name length is restricted to 8 characters.
In sample program 2, this is, for example
"ACCEPTANCE4".
The T number contains the milling tool for all machining
technologies. When residual material is machined more
than once, the tool used beforehand must always be
entered in the T number.
Explanation of the cycle structure
Cycle CYCLE73 is used to solve very complex
problems associated with solid machining of pockets
with islands which require a high level of computing
capacity in the control. For optimum timing, the
calculation is carried out in the MMC.
The calculation is started from the cycle. Its result
contains programs with traversing blocks for drilling or
milling operations which are stored in the file system of
the control. These are then called by the cycle and
executed.
 Siemens AG 2000 All rights reserved.
SINUMERIK 840D/840Di/810D/FM-NC Programming Guide, Cycles (PGZ) - 04.00 Edition
.
The
Milling Cycles
3
3-199