Fanuc Series 15i/150i-MA (Programming) Operators Manual

B-63324EN/03 PROGRAMMING 17.CUSTOM MACRO
- 639 -
17.6.4 Macro Call Using G Code
By setting a G code number used to call a macro program in a
parameter, the macro program can be called in the same way as for a
simple call (G65).
Explanation
By setting a G code number from -999 to 999 used to call a custom
macro program (O9010 to O9019) in the corresponding parameter
(N0.7050 to No.7059), the macro program can be called in the same
way as with G65.
If a call is to be made with a G code with the decimal point, custom
macroprogram O9040 to O9049 can be called by setting the code for
parameter No. 7060 to 7069. The G code, for which the number of
decimal positions is 1, must be multiplied by 10.
[Example] When 234 is set for parameter No. 7060, O9040 is
called with G23.4.
If a negative G code is set, the call is regarded as being modal. In this
case, whether the G code is equivalent to G66 or G66.1 can be specified
using parameter MGE (bit 3 of No. 7000).
For example, when a parameter is set so that macro program O9010 can
be called with G81, a user-specific cycle created using a custom macro
can be called without modifying the machining program.
- Correspondence between parameter numbers and program numbers
G code without the decimal point G code with the decimal point
Program
number
Parameter
number
Program
number
Parameter
number
O9010
O9011
O9012
O9013
O9014
O9015
O9016
O9017
O9018
O9019
7050
7051
7052
7053
7054
7055
7056
7057
7058
7059
O9040
O9041
O9042
O9043
O9044
O9045
O9046
O9047
O9048
O9049
7060
7061
7062
7063
7064
7065
7066
7067
7068
7069
- Repetition
As with a simple call, a number of repetitions from 1 to 999999999 can
be specified at address L.
O0001 ;
:
G81 X10.0 Y20.0 Z-10.0 ;
:
M30 ;
O9010 ;
:
:
:
N9 M99 ;
Parameter @No.7050=81

Leave a Reply

Your email address will not be published. Required fields are marked *