Rockwell Automation 8520-GUM 9/Series CNC Grinder Operation and Programming Manual Documentation Set - Manual (Page 697)

Paramacros
Chapter 20
20-53
The G66.1 command is modal and is executed in the same manner as the
G66 with these exceptions:
The macro programmed by the P word in the G66 block is not executed
when the G66 block is read, whereas the macro programmed by the
G66.1 is executed when G66.1 is read.
The macro is executed in any and all blocks following the G66.1, not
just after motion blocks, except for paramacro command blocks such as
assignment, goto, etc.
Axis motion cannot be generated by normal program blocks. Axis
motion can be generated only in the program called by G66.1.
The following words, when programmed after the G66.1 block, are used
as argument assignments:
N: When programmed after a word other than N or O, it is used as
assignment #14.
G: The last G-code programmed in a block is used as an argument
statement for parameter #10. All other G-codes are interpreted as
normal.
L: Assigns value to parameter #12
P: Assigns value to parameter #16
All other argument assignments are interpreted as listed in Table 20.H
The L word or any optional argument statements following a G66.1 can
contain any valid mathematical expression. For example:
G66.1 P1002 L[#1+1] A[12*6] B[SIN[#101]];
Example 20.20 illustrates G66.1 macro operation.
Example 20.20
G66.1 Macro Operation
N0100G90G17G00;
N0110G66.1P9400;
Macro 9400 is executed.
N0120G91G18G01; G91 and G18 become effective, 01 is assigned to parameter
#10, macro 9400 is executed.
N0130G03X1.; 03 is assigned to parameter #10, 1. is assigned to parameter
#24, macro 9400 is executed.
N0135; Macro 9400 is executed.
N0140G67; Macro 9400 is deactivated.
N0150M30; Program end.