Reading & Writing System Variables (Every Control)

Every CNC control keeps a live picture of itself in memory — where each axis is, which work and tool offsets are active, what the probe just touched, which G-codes are modal, how many parts have run, which alarms are set. System variables are the named or numbered handles a part program uses to reach that data: read one into a scratch variable, do arithmetic, and (where the variable allows it) write a new value back. This one mechanism is behind every probing routine, tool-breakage check, adaptive-feed macro, and part-family program ever written. The idea is universal; only the spelling changes from control to control. This article puts the seven common dialects side by side so you can translate a pattern you know into one you don't — and links each control’s own reference for the full list.

Read-Only vs Read/Write — the Universal Caveat

Reading is almost always allowed. Writing is gated. Variables that report machine state — live positions, modal codes, the clock, probe-trigger positions — are read-only on every control; assigning to them is either ignored or throws an error. Variables that hold a stored value — work offsets, tool offsets, general-purpose commons, part counters — are read/write. On top of that split, some writes are locked behind an option or by the machine builder (OEM/PLC territory). Getting this wrong is the most common source of “why won’t it write?” confusion.

Three per-control notes worth memorizing. Fanuc/Haas: positions are read-only, offsets are writable — the whole probing workflow depends on that asymmetry. Siemens: read/write status is per-$-variable and documented in the System Variables manual (in synchronized actions, an “SA” column marks read/write eligibility). Heidenhain: the direct write path FN 17: SYSWRITE is machine-builder territory, so a normal NC program changes offsets by writing a table (FN 27, TABDATA WRITE, or SQL) or by letting a touch-probe cycle write the preset table.

The Rosetta Stone — One Task, Seven Dialects

Each row is a job a machinist actually asks of a macro; each column is how that control spells it. Axis suffixes shown are for Z on a typical 3-axis mill (X = first, Y = second, Z = third). Verify against the linked per-control article before you run converted code — option gates and index ranges differ.

Okuma note: the OSP references in this wiki document the named offset variables (VZOFx, VTOFx) and Renishaw probe outputs (VS75–VS89), but do not document a bare numbered current-position or skip-position system variable equivalent to Fanuc’s #5041/#5063. On an Okuma the read-and-write pattern is normally driven off the probing-cycle outputs (below), not a raw position variable. Heidenhain note: FN 18: SYSREAD always returns metric values regardless of program units, and a real-time read should be preceded by FN 20: WAIT FOR SYNC to flush look-ahead.

The Canonical Task in Every Dialect

Here is the same job — probe the top of a part and store the measured height into the active work offset so the touched face becomes Z0 — written seven ways. It is the “touch off and set zero” pattern that underpins in-process setup. Read the skip/probe position, add it to the stored work offset, retract.

Fanuc / Haas

Feed down with G31 until the probe trips; #5063 latches the Z skip position in work coordinates; shift the G54 Z offset #5223.

(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)

Mitsubishi (M700/M70)

Near-identical to Fanuc — same G31, same #5063 skip variable, same #5221–#522n work-offset block. Only the block terminator (;) and the millisecond timers differ from Fanuc habits.

(TOUCH TOP OF PART, SET G54 Z0)
G90 G31 Z-25. F200 ;      (feed until the skip signal comes in)
#5223 = #5223 + #5063 ;   (#5063 = Z skip position, workpiece coords)
G00 Z25. ;                (retract)

Mazak (EIA/ISO)

Mazak’s EIA macro language reads captured positions from the same numbers (#5061–#5076 skip, #5221+ work offsets share Fanuc’s numbering). Real Mazak Renishaw programs read #5041/#5043 the same way.

(TOUCH TOP OF PART, SET G54 Z0)
G90 G31 Z-25. F50           ; skip move down until the probe input fires
#5223 = #5223 + #5063       ; #5063 = present skip-signal Z
G00 Z25.                    ; retract

Siemens (SINUMERIK)

A measuring move captures the trigger position into $AA_MW[Z] (workpiece coords); write it into the G54 frame $P_UIFR[1,Z,TR] and re-select G54 to activate the change. STOPRE ensures the measured value is available before the write.

MEAS=+1 G01 Z-25 F300      ; probe down, trigger on probe 1
STOPRE                     ; make the measured value current
$P_UIFR[1,Z,TR] = $P_UIFR[1,Z,TR] + $AA_MW[Z]  ; shift G54 Z to the face
G54                        ; re-select G54 to apply the new frame
G0 Z25                     ; retract

Heidenhain (TNC 640)

There is no FN 17 write to a live datum — a touch-probe cycle does the write itself, straight into the preset table. Q305 selects the preset-table row, Q303 selects transfer of the measured value into the preset table. (To store into a datum table instead, probe first, then push the value with FN 27: TABWRITE or SQL UPDATE.)

; Probe the top face in the tool axis and set it as the datum.
; The cycle writes PRESET.PR directly - no FN 17 SYSWRITE (OEM-locked).
5 TCH PROBE 417 DATUM IN TS AXIS ~
Q305=+0    ; preset-table row to update (0 = active preset)
Q303=+1    ; transfer the measured value into the preset table
6 CYCL CALL
; To verify afterward, read the active preset row back:
7 FN 18: SYSREAD Q1 = ID530 NR1      ; number of the active preset

Okuma (OSP)

A Renishaw single-surface cycle (O9811) probes the face and stores the measured Z in VS77; add that to the work-zero offset for offset set 1, VZOFZ[1]. (The protected cycle can also update the offset for you when given a work-offset argument; the manual read-then-write below shows the mechanism.)

(PROBE TOP FACE WITH RENISHAW SINGLE-SURFACE CYCLE)
CALL O9811                    (measured Z surface lands in VS77)
VZOFZ[1] = VZOFZ[1] + VS77    (shift work-offset set 1 in Z to the face)

Indirect & Computed Access

The real power of system variables is reaching one whose number or index is computed at run time — e.g. “the length offset for whatever tool is active” without hard-coding the tool.

Argument Passing — Getting Data Into a Macro

The flip side of reading control data is handing your own values to a subprogram. Each dialect does it differently:

• Fanuc / Haas / Mitsubishi / Mazak — G65 letter→variable. A macro call maps address letters to local variables: A→#1 B→#2 C→#3 D→#7 F→#9 H→#11 I→#4 R→#18 X→#24 Y→#25 Z→#26…. G65 P8010 A15. B40. H6 lands 15 in #1, 40 in #2, 6 in #11. A fresh local set is created per call level. See the Fanuc, Mitsubishi, and Mazak articles.
• Siemens — PROC with typed parameters. A subprogram declares its own signature: PROC DRILL(REAL DEPTH, INT COUNT), called as DRILL(-12.5, 6). R-parameters and GUD provide the shared, named alternative. See SINUMERIK R-Parameters & System Variables.
• Heidenhain — no positional arguments; Q parameters are global. CALL LBL "UP1" and CALL PGM … pass nothing directly — Q parameters remain globally effective across program calls, so you set Q1… before the call and the subprogram reads them. Local scratch uses QL parameters. See Klartext & Q-Parameters.
• Okuma — named local variables on CALL. CALL O1234 AA11=1.234 BB22=BB22 PC33=1 creates named locals in the subprogram; a leading P (PC33) marks an optional argument testable with EMPTY. See Okuma Argument & Local Variables.

Each Control’s Full Reference

• Fanuc System Variables & Modal & Position Data — the #-number reference the others map to.
• Haas System Variables — NGC and legacy variable mappings, with an explicit read/write column.
• Mitsubishi M700/M70 Programming & Macros — ~95% Fanuc Macro B, with the millisecond-timer gotcha.
• Mazak EIA/ISO Programming — Fanuc-like #-variables, but tool data by index and Mazak-specific numbers.
• SINUMERIK R-Parameters & System Variables & Synchronized Actions — the $-prefix decode and real-time reads/writes.
• Heidenhain TNC 640 Tables & System Data (FN 18 SYSREAD, FN 27, TABDATA) & Klartext & Q-Parameters.
• Okuma Variable Types (VS / VC / VZOF / VTOF) & Okuma Argument & Local Variables.

▶ Open the Macro Playground — read and write system variables interactively across seven controls.

References

• Fanuc, Operator’s Manual / Parameter Manual, FANUC Corporation.
• Haas, Operator’s Manual / NGC Programming Guide, Haas Automation, Inc.
• Mitsubishi Electric, CNC 700/70 Series Programming Manual (Machining Center System), IB-1500072.
• Yamazaki Mazak, Programming Manual (Machining Centers) — EIA/ISO, MAZATROL SmoothAi, H747PB1000E.
• Siemens, SINUMERIK System Variables Parameter Manual and Programming Guide: Job Planning, Siemens AG.
• HEIDENHAIN, TNC 640 Klartext Programming User’s Manual, NC software 34059x-11.
• Okuma, OSP Programming Manual, Okuma Corporation; Renishaw, Inspection Plus Programming Manual, Renishaw plc.