M Functions (M08, M09); Additional Functions; Program-Support Functions; Fixed Cycles (G90, G92, G94) - Siemens SINUMERIK 808D Programming And Operating Manual

3.3.5.8

M functions (M08, M09)

General M functions
The non-specific M functions are defined by the machine manufacturer. A representative example of the use of general M
functions is available under. Details are available in the documentation of your machine manufacturer. If an M command is
programmed with an axis motion in the same block, whether the M function is to be executed at the start or end of the block
on reaching the axis position depends on the machine data setting of the machine manufacturer. Details are available in the
documentation of your machine manufacturer.
M function Function
M08 Coolant ON
M09 Coolant OFF
Specification of several M functions in one block
A maximum of five M functions can be programmed in on block. Possible combinations of M functions and possible
restrictions are specified in the documentation of your machine manufacturer.
Additional auxiliary functions (B functions)
If B is not used as axis identifier, B can be used as extended auxiliary function. B functions are output to the PLC as auxiliary
functions (H functions with the address extension H1=).
Example: B1234 is output as H1=1234.
3.4

Additional functions

3.4.1

Program-support functions

3.4.1.1

Fixed cycles (G90, G92, G94)

Fixed cycles simplify it for the programmer to create new programs. Frequently occurring machining steps can be executed
with a G function; without fixed cycles several NC blocks must be programmed. In this way, with fixed cycles, the machining
program can be shortened and the memory space can be saved.
In the ISO Dialect a shell cycle is called, which uses the functionality of the standard Siemens cycle. Thus the addresses
programmed in the NC block are transferred to the shell cycle via the system variable. The shell cycle customizes these data
and calls a standard Siemens cycle.
A fixed cycle could be canceled only with G80 or a G code of G code Group 1 before the program can be continued with a
blockwise cycle.
Longitudinal turning cycle
Format
G.. X... Z... F... ;
G code system A
G90
With the commands "G... X(U)... Z(W)... F... ;", a longitudinal turning cycle is executed as per the sequence 1-4.
50
Remarks
These M functions are defined by the machine manufacturer.
G code system B
G77
G code system C
G20
Programming and Operating Manual (ISO Turning/Milling)
01/2017