Haas System Variables

Haas system variables are the #-numbers a macro uses to read and write the control’s state — tool offsets, work offsets, live positions, probe results, timers, pallet data, even settings and parameters. Haas follows the Fanuc Macro B model closely, then extends it: the Next Generation Control (NGC) adds five-digit variable ranges that mirror settings (#20000+), parameters (#30000+), and the full tool table (#50001+), making a Haas unusually transparent to a macro programmer.

NGC vs Legacy Numbering

The Classic Haas Control (CHC) used the traditional three-digit macro ranges (#100–#999). The NGC moved general-purpose storage into five-digit ranges (#10000–#10999) and kept the legacy numbers working as aliases into the same storage — #100 and #10100 are two addresses for the same variable on an NGC machine. Programs written for a classic control run unchanged; new programs get much more room (plus ranges that have no legacy equivalent at all). The table below shows both addresses side by side.

Reading & Writing System Variables in a Macro

Probe a surface and write the result to a work offset. The core “touch off and set zero” chain on a Haas: feed with G31 until the probe trips, read the latched skip position, write it into the offset. On Haas the skip block is #5061–#5069 in axis order X, Y, Z, A, B, C, U, V, W — so Z is #5063:

(TOUCH TOP OF PART, SET IT AS G54 Z0)
G90 G31 Z-25. F50.        (feed down until the probe trips)
#5223 = #5223 + #5063     (shift G54 Z so the touched face = Z0)
G00 Z25.                  (retract)

Write an additional work offset (G154 P). The NGC exposes G154 P1–P99 at #14001+ (each P block is 20 apart); the legacy #7001+ block only reaches P20. Setting the G154 P5 X offset:

#101 = 5                       (which G154 P offset)
#[14001 + [[#101 - 1] * 20]] = #5061   (G154 P5 X = probed X position)

Track cycle counts across power-off. Haas retains the general-purpose ranges through power-off, so a retained variable makes a free parts/maintenance counter alongside the built-in #3901/#3902 M30 counters:

#10800 = #10800 + 1            (survives power-off)
IF [#10800 LT 500] GOTO 99
#3006 = 1 (500 PARTS - CHECK FIXTURE CLAMPS)
#10800 = 0
N99 M30

Read machine state for logging or adaptive decisions — the NGC exposes far more than Fanuc does by default:

#100 = #3026    (tool currently in the spindle)
#101 = #3027    (spindle RPM right now)
#102 = #1064    (max X-axis load seen)
#103 = #20009   (Setting 9: dimensioning - branch inch vs metric)

Gotchas Worth Knowing

• Settings and parameters are read-only mirrors. #20000+ and #30000+ let a macro read any setting or parameter, but writes are rejected — change offsets through their own writable variables (or G10), and change settings on the Settings page.
• Legacy and NGC numbers are the same storage. #500 and #10500 are one variable, not two. When porting a classic-control program, don’t “migrate” values between the two ranges — there is nothing to migrate.
• Probe ranges are only meaningful with probing installed. #10150–#10199 (outputs) and #10550–#10599 (calibration) belong to the Renishaw/WIPS macros when the option is present; without it they are just more general-purpose storage.
• #6001–#6999 is reserved. Classic Fanuc habits sometimes park data there; on a Haas, don’t.
• Read positions with the axes stopped. As on Fanuc, #5021+/#5041+ are only trustworthy after motion completes — except the skip variables #5061+, which are latched at the instant the G31 input trips.

▶ Try these in the Macro Playground — pick the Haas control, set the system-variable inputs (like #5063), and watch the values update live as the macro runs.

See also: Haas Programming & Macros for the language itself, Settings & Parameters for what #20000+ is mirroring, Renishaw Inspection Plus for the full probing system, and Reading & Writing System Variables for the same patterns on every control.

References

• Haas, Operator’s Manual / NGC Programming Guide, Haas Automation, Inc.