Discrete ManufacturingFree referencePDF, Excel, Word exportMachining

Fanuc Macro B System Variables Reference

Custom Macro B turns a Fanuc program into a small programming language with variables, loops and probing logic. The hard part is remembering which variable number reads what. This lookup lists the commonly used system variables for offsets, position, timers, alarms and counters.

Download:

Variable	Area	Meaning	Access	Example
#0	Null	Always empty, cannot be written	Read only	IF [#1 EQ #0] GOTO10
#1 to #33	Local	Local variables used inside a macro call or main program	Read/write	#1=5.0
#100 to #199	Common	Common variables, cleared on power off on most controls	Read/write	#100=#100+1
#500 to #999	Common (retained)	Persistent common variables kept after power off	Read/write	#500=12.5
#3000	Alarm	Raises a macro alarm, number plus message text	Write	#3000=1 (TOOL MISSING)
#3001	Timer	Millisecond timer that runs while power is on	Read/write	#101=#3001
#3002	Timer	Timer in hours that runs while the cycle start lamp is on	Read/write	#102=#3002
#3003	Control	Single block suppression and cycle start wait	Read/write	#3003=1
#3004	Control	Feed hold, feed override and exact stop control	Read/write	#3004=7
#3006	Message	Stops the program and displays a message to the operator	Write	#3006=1 (CHECK CLAMP)
#3011	Clock	Current date as YYYYMMDD	Read only	#103=#3011
#3012	Clock	Current time as HHMMSS	Read only	#104=#3012
#3901	Parts	Number of parts required	Read/write	#3901=100
#3902	Parts	Number of parts machined	Read/write	#3902=#3902+1
#4001 to #4022	Modal	Modal G code groups from the previous block	Read only	IF [#4003 EQ 90] GOTO20
#5001 to #5003	Position	End point of previous block, X Y Z in the workpiece system	Read only	#105=#5001
#5021 to #5023	Position	Current position in the machine coordinate system, X Y Z	Read only	#106=#5023
#5041 to #5043	Position	Current position in the workpiece coordinate system, X Y Z	Read only	#107=#5041
#5201 to #5203	Work offset	External workpiece offset X Y Z	Read/write	#5201=0
#5221 to #5223	Work offset	G54 work offset X Y Z	Read/write	#5221=-350.0
#5241 to #5243	Work offset	G55 work offset X Y Z	Read/write	#5241=-120.5
#5261 to #5263	Work offset	G56 work offset X Y Z	Read/write	#5263=-410.0
#5281 to #5283	Work offset	G57 work offset X Y Z	Read/write	#5281=0
#5301 to #5303	Work offset	G58 work offset X Y Z	Read/write	#5301=0
#5321 to #5323	Work offset	G59 work offset X Y Z	Read/write	#5321=0

Variable ranges, options and write access vary by control model (0i, 30i, 31i and others) and by machine tool builder parameters. Tool offset variables use different numbers depending on the memory type, so check the macro section of your control's programming manual before relying on any value.

Make CNC programs searchable

Optional: a short discussion on linking NC programs and macros to parts, routings and revisions in your ERP.

Optional. The tool and every export work without this. No spam.

How to use the table

Search for a variable number or a keyword such as G54, timer or alarm. The access column tells you whether a macro can write the value or only read it. Examples are written in the standard macro syntax where square brackets enclose expressions. Export the list to keep with your macro library.

Local, common and persistent variables

Local variables #1 to #33 exist only inside the current macro level, and argument letters in a G65 call map onto them. Common variables #100 to #199 are shared across programs and cleared on power off on most controls, while #500 to #999 survive power cycles and are the safe place for counters and calibration values.

Reading and writing work offsets

Work offsets are readable and writable through the #5221 series, with each additional work coordinate system 20 higher: G54 at 5221, G55 at 5241, and so on. This is how probing macros update G54 after finding a part edge. Always write offsets in the correct units and confirm that the offset write option is enabled.

G54 starts at #5221, G55 at #5241
The X, Y, Z axes are consecutive numbers
Writing offsets needs the correct control option and parameters
Test in single block with the machine locked first

Common mistakes

Programmers often write to a variable that is read only, store a counter in a common variable that clears at power off, or assume a variable number from one control exists on another. Another frequent problem is forgetting that #3006 stops the program for operator action, so it should not be used for routine logging.

Frequently Asked Questions

What is the difference between #100 and #500 variables?

Both are common variables shared between programs. On most Fanuc controls the #100 to #199 range is cleared when power is turned off, while #500 to #999 is retained. Use the retained range for counters and stored measurements.

How do I stop a program with a message?

Set variable #3006 to a number and put the message in parentheses, for example #3006=1 (CHECK PART CLAMPED). The control stops and shows the message to the operator. Use #3000 instead to raise a full macro alarm.

Which variable holds the G54 X offset?

G54 X is in #5221, Y in #5222 and Z in #5223. G55 starts at #5241, G56 at #5261, G57 at #5281, G58 at #5301 and G59 at #5321. External offsets begin at #5201.

Do Haas and Okuma use the same variables?

Haas macros are similar in style, but system variable numbers and options differ, and Okuma uses its own user task language. Treat this table as Fanuc specific and check the manual for other controls.

If your CNC programs and macro libraries are stored in file shares, we can show how they could be made searchable and linked to part and routing records.

Talk to an Expert Explore More Free Tools

Related Tools

Developer Tools

More Discrete Manufacturing tools

See all

Back to All Tools