Haas CNC | G65 Code | Macro Subprogram Call Option

In this article, we describe how to use G65 code to call CNC macro subprogram for Haas CNC machines and controllers with all details and examples.

0
891

Introduction

G65 is the command that calls a subprogram with the ability to pass arguments to it. The
format follows for Haas CNC controller:

G65 Code Format

G65 Pnnnnn [Lnnnn] [arguments] ;

Arguments italicized in square brackets are optional. See the Programming section for more details on macro arguments.

The G65 command requires a P address corresponding to a program number currently located in the control’s drive or path to a program. When the L address is used the macro call is repeated the specified number of times.

When a subprogram is called, the control looks for the subprogram on the active drive or the path to the program. If the subprogram cannot be located on the active drive, the control looks in the drive designated by Setting 251. Refer to the Setting Up Search Locations section for more information on subprogram searching. An alarm occurs if the control does not find the subprogram.

You may be interested also:
“Haas CNC | G02 and G03 Code | Circular Interpolation”

In Example 1, subprogram 1000 is called once without conditions passed to the subprogram. G65 calls are similar to, but not the same as, M98 calls. G65 calls can be nested up to 9 times for Haas CNC, which means, program 1 can call program 2, program 2 can call program 3 and program 3 can call program 4.

G65 Code Examples

G65 CNC Program Example – 1

%
G65 P1000 (Call subprogram O01000 as a macro) ;
M30 (Program stop) ;
O01000 (Macro Subprogram) ;

M99 (Return from Macro Subprogram) ;
%

G65 CNC Program Example – 2

In Example 2, the program LightHousing.nc is called using the path that it is in.

G65 P15 A1. B1.;
G65 (/Memory/LightHousing.nc) A1. B1.;

Note: Paths are case sensitive.

G65 CNC Program Example – 3

In Example 3, subprogram 9010 is designed to drill a sequence of holes along a line whose slope is determined by the X and Y arguments that are passed to it in the G65 command line. The Z drill depth is passed as Z, the feed rate is passed as F, and the number of holes to be drilled is passed as T. The line of holes is drilled starting from the current tool position when the macro subprogram is called.

Note: The subprogram program O09010 should reside on the active drive or on a drive designated by Setting 252.

%
G00 G90 X1.0 Y1.0 Z.05 S1000 M03 (Position tool) ;
G65 P9010 X.5 Y.25 Z.05 F10. T10 (Call O09010) ;
M30 ;

O09010 (Diagonal hole pattern) ;
F#9 (F=Feedrate) ;
WHILE [#20 GT 0] DO1 (Repeat T times) ;
G91 G81 Z#26 (Drill To Z depth) ;
#20=#20-1 (Decrement counter) ;
IF [#20 EQ 0] GOTO5 (All holes drilled) ;
G00 X#24 Y#25 (Move along slope) ;
N5 END1 ;
M99 (Return to caller) ;
%


Need to More?

Our volunteers have worked together and carefully prepared the articles published here in their native language without using machine translation. You can search the entire site for more information on the subject. You can start a discussion on CNCarea.com forums and join us to get support, ask questions, improve a published article or give your opinion.


Previous articleMitsubishi CNC | M70-M80 Series | Servo Motor Vibration and Noise Suppression
Next articleMitsubishi CNC | M70-M80 Series | Program Restart