Custom G/M Cycles

Custom G-Code Assignment

Parameters 6050-6059 map custom G-codes to programs O9010-O9019. When the control reads the custom G-code, it executes the mapped O9xxx program with G65-style argument passing. The program O9010-O9019 must exist in the CNC memory (usually in protected memory).

G-code numbers should use numbers not already assigned to standard functions. Typically G100+, G200+, or G500+ are safe ranges.

Custom G-Code Numbering Rules

Selecting the right G-code number is critical. You cannot reuse numbers already assigned to standard Fanuc functions.

Custom M-Code Macros

M-codes can also trigger macro programs through parameters, just like custom G-codes. Parameters 6080-6089 map M-codes to macro programs O9020-O9029, called with G65-style argument passing. Parameters 6071-6079 map M-codes to subprogram calls of O9001-O9009 (M98-style, no arguments).

Argument Passing

Custom G-codes use the same argument system as G65 macro calls. Argument style 1 maps all letters A-Z (except G, L, N, O, P) to local variables in the called program.

Example Call

G100 A1.5 B2.0 X10.0 Y20.0 Z-5.0
(Passes values to O9010:)
(  #1 = 1.5   from A)
(  #2 = 2.0   from B)
(  #24 = 10.0 from X)
(  #25 = 20.0 from Y)
(  #26 = -5.0 from Z)

The argument style (1 or 2) is determined automatically by the control from the letters used in the call. Argument style 1 is the most common and maps single letters to variables. Argument style 2 allows multi-use of certain letters (I, J, K) for additional data sets. On 30i-era controls, bit 7 (IJK) of parameter 6008 can force I, J, and K to always use style 1.

Designing a Custom Cycle

Follow these steps to create a reliable custom G-code cycle.

Best Practices

Always validate arguments with #3000 alarms so the operator gets a clear error message instead of unexpected behavior. Document all inputs and outputs in the program header comments. Save and restore the modal state (#3003, #3004, G90/G91) so the calling program is not affected. Use M99 to return from the macro.

Worked Example - Custom Probing Cycle

This example creates a custom G100 single-surface probing cycle. It validates all required arguments, sets defaults where appropriate, and stores the measured Z position in #500.

(O9010 - CUSTOM SINGLE SURFACE PROBE G100)
(G100 X_ Y_ Z_ F_ H_)
(X,Y = APPROACH POSITION)
(Z = PROBE DEPTH)
(F = PROBE FEED RATE - DEFAULT 200)
(H = TOOL LENGTH OFFSET NUMBER)
(OUTPUT: #500=MEASURED Z)
(-----------------------------------)
IF [#24 EQ #0] THEN #3000=100(X POSITION REQUIRED)
IF [#25 EQ #0] THEN #3000=101(Y POSITION REQUIRED)
IF [#26 EQ #0] THEN #3000=102(Z DEPTH REQUIRED)
IF [#9 EQ #0] THEN #9=200. (DEFAULT FEED)
IF [#11 EQ #0] THEN #3000=103(H OFFSET REQUIRED)
(-----------------------------------)
#3003=1 (DISABLE SINGLE BLOCK)
G90 G00 X#24 Y#25
G43 Z10.0 H#11
G31 Z#26 F#9 (PROBE MOVE)
#500=#5063 (STORE Z AT SKIP SIGNAL)
G90 G00 Z10.0
#3003=0
M99

See also: Macro Structure for G65 vs G66 macro call details, Fanuc Parameters for parameter 6050-6059 setup, and Argument Variables for letter-to-variable mapping.

▶ Open the Macro Playground — write and run macros like these in your browser, with live variable values as the program executes.

References

• Peter Smid, Fanuc CNC Custom Macros, Industrial Press, 2004.
• Fanuc, Operator’s Manual / Parameter Manual, FANUC Corporation.
• Fanuc, Series 30i/31i/32i-MODEL B Plus Operator’s Manual (Common), B-64724EN/01, FANUC Corporation.