Tool Life Control" Function; Macro Programs; Differences With Subroutines; Macro Program Call (G65, G66, G67) - Siemens SINUMERIK 808D Programming And Operating Manual

G31 is an absolute command for 2 axes:
4.4.5.2

"Tool life control" function

Tool life monitoring and workpiece count can be undertaken with Siemens Tool Management.
4.4.6

Macro programs

Macros may consist of several part program blocks that are completed with M99. In principle, macros are subroutines that
are called with G65 Pxx or G66 Pxx in the part program.
Macros that are called with G65 are non-modal. Macros that are called with G66 are modal and are deselected again with
G67.
4.4.6.1

Differences with subroutines

Macro programs (G65, G66) can be used to specify parameters that can be evaluated in the macro programs. No
parameters can be specified in subroutine calls (M98).
4.4.6.2

Macro program call (G65, G66, G67)

Macro programs are generally executed immediately after their call.
The procedure of calling a macro program is described in the table below.
Call method
Simple call
Modal call (a)
Simple call (G65):
Format
G65 P_ L_ ;
A macro program to which a program number was assigned with "P" is called and executed "L" times by specifying "G65 P ...
L... <Argument>; ".
The required parameters must be programmed in the same block (with G65).
Explanation
In a part program block containing G65 or G66, the address Pxx is interpreted as program number of the subroutine in which
the macro functionality is programmed. The number of passes of the macro can be defined with the address Lxx. All other
addresses in this part program block are interpreted as transfer parameters and their programmed values are stored in the
system variables $C_A to $C_Z. These system variables can be read in the subroutine and evaluated for the macro
152
Command code
G65
G66
Remarks
Deselection through G67
Programming and Operating Manual (ISO Turning/Milling)
01/2017