Programming Cycles - Siemens SINUMERIK 808D ADVANCED Programming And Operating Manual

CYCLE94: Undercut (DIN form E and F)
CYCLE95: Stock removal with relief cutting
CYCLE96: Thread undercut
CYCLE98: Thread chain
CYCLE99: Thread cutting
9.2

Programming cycles

A standard cycle is defined as a subroutine with name and parameter list.
Call and return conditions
The G functions effective prior to the cycle call and the programmable offsets remain active beyond the cycle.
The machining plane G17 for drilling cycles or G18 for turning cycles is defined before calling the cycle.
With drilling cycles, the drilling operation is carried out in the axis standing vertically to the current plane.
Messages output during execution of a cycle
During various cycles, messages that refer to the state of machining are displayed on the screen of the control system
during program execution.
These messages do not interrupt the program execution and continue to be displayed on the screen until the next message
appears.
The message texts and their meaning are listed together with the cycle to which they refer.
Block display during execution of a cycle
The cycle call is displayed in the current block display for the duration of the cycle.
Cycle call and parameter list
The defining parameters for the cycles can be transferred via the parameter list when the cycle is called.
Note
Cycle calls must always be programmed in a separate block.
Basic instructions with regard to the assignment of standard cycle parameters
Each defined parameter of a cycle has a certain data type. The parameter being used must be specified when the cycle is
called. The following can be transferred in the parameter list:
● R parameters (only numerical values)
● Constants
If R parameters are used in the parameter list, they must first be assigned values in the calling program. Proceed as follows
to call the cycles:
● with an incomplete parameter list
or
● by leaving out parameters.
If transfer parameters are omitted at the end of the parameter list, the parameter list must be prematurely ended with ")". If
any parameters are to be omitted within the list, a comma "..., ,..." must be written as a placeholder.
No plausibility checks are made for parameter values with a limited range of values unless an error response has been
specifically described for a cycle.
When calling the cycle, if the parameter list contains more entries than parameters are defined in the cycle, the general NC
alarm 12340 "Too many parameters" is displayed and the cycle is not executed.
Note
Axis-specific and channel-specific machine data of the spindle must be configured.
120
Programming and Operating Manual (Turning)
6FC5398-5DP10-0BA2, 06/2015