Siemens CNC Milling | CYCLE74 | Transfer Pocket Edge Contour


CYCLE74 Introduction

Cycle CYCLE74 transfers the pocket edge contour to pocket milling cycle CYCLE73. This is achieved by creating a temporary internal file in the standard cycles directory and storing the transferred parameter values in it.

If a file of this type already exists, it is deleted and set up again. For this reason, a program sequence for milling pockets with islands must always begin with a call for this cycle.

CYCLE74 Format

CYCLE74 (_KNAME, _LSANF, _LSEND)

Parameters

_KNAME = Name of contour subroutine of pocket edge contour
_LSANF = Block number/label identifying start of contour definition
_LSEND = Block number/label identifying end of contour definition

Explanation of the Parameters

The edge contour can be programmed either in a separate program or in the main program that calls the routine. Transfer to the cycle takes place via the _KNAME parameter, the name of the program, and _LSANF, LSEND, identification of the program section from…to by block numbers or labels, whereby not all of these need to be programmed.

The following options are available for contour programming:

  • Contour is in its own program, in this case, only _KNAME must be programmed; e.g. CYCLE74 (“EDGE”,””,””)
  • Contour is in the calling program, in this case, only _LSANF and _LSEND must be programmed; e.g. CYCLE74 (“”,”N10″,”N160″)
  • The edge contour is a section of a program, but not of the program calling the cycle, in this case, all three parameters must be programmed. e.g. CYCLE74(“EDGE”,”LABEL_START”,”LABEL_END”)

The program name can be described by its path name and program type.

Example: _KNAME=”/N_WKS_DIR/_N_EXAMPLE3_WPD/_N_EDGE_MPF”