Siemens SINUMERIK 840D Programming Manual page 196

Milling Cycles
3
3.15 Pocket milling with islands - CYCLE73, CYCLE74, CYCLE75
_BNAME (name for drilling position program)
_PNAME (name for pocket milling program)
The pocket milling cycle generates programs with
traversing blocks required to rough drill or mill the
workpiece. These programs are stored in the same
directory as the calling program in the part program
memory, i.e. in the "part programs" directory (MPF.DIR) if
the cycle is called from there or in the corresponding
workpiece directory. The programs are always main
programs (type MPF).
The names of these programs are defined by parameters
_BNAME and _PNAME.
A drilling program name is needed only when
_VARI=XXX5.
Example:No drilling program name:
CYCLE73(1011,"",ACCEPTANCE4_MILL,...)
_TN (name of solid machining tool)
This parameter must be set to the solid machining tool.
Depending on whether the tool management function is
active or not, the parameter must be set to a tool name or
tool number.
Example:
• with tool management
CYCLE73(1015,"PART1_DRILL","PART1_MILL",
"MILL3",...)
• without tool management
CYCLE73(1015,"PART1_DRILL","PART1_MILL","3",
...)
Parameter _TN is defined as a compulsory parameter with
a maximum length of 16 characters. It must therefore be
assigned to the cutting tool in every subsequent CYCLE73
call. When the residual material machining operation is
used more than once, the tool from the last residual
material removal process must be used.
TOOL AND OFFSET:
It must be ensured that the tool offset is processed
exclusively by D1. Replacement tool strategies may not be
used.
3-196
SINUMERIK 840D/840Di/810D/FM-NC Programming Guide, Cycles (PGZ) - 04.00 Edition
03.96
08.99
3
 Siemens AG 2000 All rights reserved.