Programmable Data Input (G10); Changing The Tool Offset Value; M Function For Calling Subroutines (M98, M99) - Siemens SINUMERIK 808D Programming And Operating Manual

4.4.2

Programmable data input (G10)

4.4.2.1

Changing the tool offset value

Existing tool offsets can be overwritten via G10. It is not possible to create new tool offsets.
Format
G10 L10 P... R... ; Tool length compensation, geometry
G10 L11 P... R... ; Tool length compensation, wear and tear
G10 L12 P... R... ; Tool radius compensation, geometry
G10 L13 P... R... ; Tool radius compensation, wear and tear
P: Number of tool offset memory
R: Value statement
L1 can also be programmed instead of L11.
4.4.2.2

M function for calling subroutines (M98, M99)

This function can be used if subroutines are stored in the part program memory. Subroutines that are registered in the
memory and whose program numbers are assigned can be called and executed any number of times.
Commands
The following M functions are used to call subroutines.
M function
M98
M99
Subroutine call (M98)
● M98 Pnnnnmmmm
m: Program no. (max. 4 digits)
n: No. of repetitions (max. 4 digits)
Before using program M98 Pnnnnmmmm to call a program, name the program correctly, that is, add the program
number always to 4 digits with 0.
● If for example, M98 P21 is programmed, the part program memory is browsed by program name 21.mpf and the
subroutine is executed once. To call the subroutine three times, one must program M98 P30021. An alarm is output if the
specified program no. is not found.
● A nesting of subroutines is possible, up to 16 subroutines are allowed. An alarm is output if more subroutine levels are
assigned than is allowed.
End of subroutine (M99)
A subroutine is ended with the command M99 Pxxxx and program processing is continued in Block No. Nxxxx. The control
system first searches forward for the block number (from the subroutine call up to the end of the program). If no matching
block number is found, the part program is eventually searched in the reverse direction (in the direction of the part start of
program).
If M99 is without a block number (Pxxxx) in a main program, the control goes to the start of the main program and the main
program is processed afresh. In case of M99 with navigation to the block number in the main program (M99xxxx), the block
number is always searched from the start of program.
148
Function
Subprogram call
End of subroutine
Programming and Operating Manual (ISO Turning/Milling)
01/2017