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.
|You may be interested also:|
|“Siemens CNC Milling | CYCLE75 | Transfer Island Contour”|
|CYCLE74 (_KNAME, _LSANF, _LSEND)|
|_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.