G-code & M-code Reference by Operation: LinuxCNC, GRBL, Centroid, FANUC, Mach 3, Mach 4

A cross-control G-code and M-code reference, organized by operation — what you actually want the machine to do — rather than by code number. Each row is one operation (a feed move, an arc, a probe, a drilling cycle, a work-offset select…) and each control's column shows the exact code that control uses for it.

Covers LinuxCNC, GRBL (1.1), Centroid (CNC12 — Acorn / Allin1DC / Oak; mill unless called out), FANUC (0i / 30i, mill-focused with lathe specifics flagged), Mach 3 (Mill Rev 1.84-A2), and Mach 4 (Mill v1.0).

How to read the tables:

• A cell shows the code(s) that control uses for the operation — e.g. the "probe toward work" row reads G38.2 for LinuxCNC, G31 for FANUC, and M115/M116 for Centroid.
• — means the control has no equivalent code for that operation.
• A code with a dotted underline has a control-specific caveat; the full note is in that row's Notes column (and on hover).
• Use the control filter at the top of the tables to hide every column but your own.

Sources used for fact-checking are listed at the bottom of this doc.

#Codes by operation

#False friends — same number, different meaning

The operation tables above already handle the "different code, same job" case — each row lists every control's spelling, so you can't miss it. This section is about the opposite and more dangerous case: the same number does fundamentally different things on different controls or modes. A program that runs cleanly on one will produce wrong output — or crash — on another.

If you're porting G-code between platforms, this is the section to read twice.

#M100 / M101 — PLC-bit wait vs user-script slot

A FANUC-trained operator and a Centroid-trained operator will write M100 for two completely incompatible reasons.

Portability impact: A Centroid program using M100 /5000 to wait on a vacuum-ready PLC signal will, on LinuxCNC, try to execute an external script literally named M100 — completely different runtime. On a stock Mach3 install with no M100.M1S written, the same line silently does nothing. Always rewrite explicit PLC waits when moving between controls.

#G98 / G99 — canned-cycle return (mill) vs feed mode (FANUC lathe)

The single biggest mill-vs-lathe trap on FANUC.

Portability impact: A FANUC T-series lathe program that sets G98 expecting feed-per-minute will, on every other platform here, be parsed as a canned-cycle return-mode change. The lathe-feed-mode interpretation is FANUC-T-series-exclusive.

#G50 — three completely different meanings depending on platform/mode

Portability impact: A FANUC lathe program that issues G50 S3000 to cap a CSS-driven spindle will be a no-op or error on mill controls, because the mill-side G50 takes no S word.

#G74 — counter-tapping (mill) vs face grooving (FANUC lathe)

Portability impact: Same code, same control vendor (FANUC), totally different machining operation depending on whether the control is a mill or a lathe. Posts targeting a lathe always assume the FANUC lathe meaning.

#G76 — fine boring (mill) vs threading (FANUC lathe)

Portability impact: A lathe-threading G76 block has a completely different argument list than a mill-boring G76 block. They are not interchangeable.

#G5 / G5.1 / G5.4 — different high-speed look-ahead implementations

Portability impact: Same number, completely different math. A LinuxCNC G5 block defines a spline curve through control points; a FANUC G05 toggles a look-ahead acceleration mode. Output is unrelated.

#Quick differences cheat sheet

GRBL intentionally omits canned cycles, cutter comp, polar coords, scaling, rotation, macros, and subprograms. CAM posts targeting GRBL expand cycles into raw G01 moves and skip G41/G42 entirely.

FANUC is the lineage everyone else copies, but it's where most divergence happens at the high end. The single biggest cross-control trap: G98/G99 are canned-cycle return modes on the mill, but feed-mode modes on the lathe. G50, G70–G76 also reassign on lathe. High-speed machining options (G05.1, G05.4, G08, G64 tuning) vary by controller generation and machine builder.

LinuxCNC is closest to a clean superset of standard RS-274/NGC. It adds first-class probing variants (G38.2–G38.5), digital/analog HAL I/O M-codes (M62–M68), user-defined M100–M199 scripts, and uses O-codes for subroutines rather than FANUC-style M98/M99.

Centroid (CNC12) is mostly FANUC-compatible for the canonical drill, bore, and macro codes. Macro programming uses #-variables with IF/THEN/ELSE and block-number GOTO branching — it does not have WHILE/DO loops. Probing is done with M-codes (M105/M106, M115/M116/M125/M126), not G31/G38. Extended work offsets use G54 Pn (no decimal), not G59.1+ or G54.1. G70–G76 lathe cycles only apply on T-series. The canonical mill canned-cycle set is G81–G85 + G89; G86/G87/G88 back-bore and modal-macro G66/G67 are not in the CNC12 manual.

Mach 3 is the lowest-feature commercial control here — no G65 macros (custom M-codes are VBScript .M1S files instead), no polar coordinates, no extended fixture offsets beyond G59.3, no G31 multi-probe. M62–M66 typically need OEM scripts rather than working natively. Subroutines via M98/M99 work.

Mach 4 is a substantial superset of Mach 3: adds G65 macros (with .nc macro-file extension required), G54.1 P1–P248 extended fixtures, G31.0–G31.3 multi-probe, G12/G13 full-circle, polar coords, G84.2/G84.3 rigid tap, G40.1/G40.2 cutter-comp corner styles, native M62–M68 I/O, and an M200–M228 family. Lua replaces VBScript for custom M-codes — Mach3 macros do not port directly.

#How this app handles non-supported codes

G54.APP's parser is permissive — unrecognized G or M codes are kept verbatim in the source and just don't affect the visualization. So a file written for FANUC with G68 rotation or M98 subprogram calls will render the linear/arc moves it does understand and silently skip the rest. Always sanity-check the simulation against the target control's expected behavior before cutting.

#Sources

These are the public references consulted while building this chart. Vendor manuals (FANUC, Centroid) ship with the controller and may not be publicly archived; where a vendor PDF was used, the URL is the one that served at the time of writing.

LinuxCNC (free, online):

• G-code quick reference — https://linuxcnc.org/docs/html/gcode/g-code.html
• M-code quick reference — https://linuxcnc.org/docs/html/gcode/m-code.html
• Main user manual — https://linuxcnc.org/docs/

GRBL 1.1 (open source):

• Supported commands wiki — https://github.com/gnea/grbl/wiki/Grbl-v1.1-Commands
• commands.md source-of-truth — https://github.com/gnea/grbl/blob/master/doc/markdown/commands.md

Centroid CNC12 (vendor PDFs):

• Macro Programming guide — https://www.centroidcnc.com/centroid_diy/downloads/acorn_documentation/centroid_cnc_macro_programming.pdf
• M-Series (Oak / Allin1DC) Operator's Manual v4.14 — https://www.centroidcnc.com/centroid_diy/downloads/CNC12-v414_operator_manuals/centroid-cnc12-oak-allin1dc-mill-operator-manual-v4.14.pdf
• v3.16 Mill Operator Manual — https://www.centroidcnc.com/downloads/centroid_v3.16_mill_operator_manual.pdf
• G and M codes extract — https://www.centroidcnc.com/centroid_diy/downloads/centroid_G_and_M_codes.pdf
• PLC + CNC Functions Programming Manual (CNC12 v5.x+) — https://www.centroidcnc.com/centroid_diy/downloads/centroid_plc_programming_manual.pdf
• Helman CNC mirror of Centroid Mill M-code list — https://www.helmancnc.com/centroid-m-code-cnc-mill/
• Centroid forum post on G10 P/R parameter-setting form — https://centroidcncforum.com/viewtopic.php?t=3429

FANUC (third-party aggregators of vendor manuals; vendor PDFs are generally not freely hosted):

• FanucWorld "Ultimate M-Code & G-Code List for Fanuc Controls" — https://content.fanucworld.com/m-code-g-code-list/
• REACO CNC FANUC Machining Center G/M codes — https://reacocnc.com/blogs/fanuc-g-code-m-code-list/g-code-m-code-machining-center
• REACO CNC FANUC CNC Lathe G/M codes — https://reacocnc.com/blogs/fanuc-g-code-m-code-list/g-code-m-code-lathe
• Helman CNC "Fanuc 31i G Codes Machining Center" — https://www.helmancnc.com/fanuc-31i-g-codes-machining-center-fanuc-30i-31i-32i/
• Cross-checked against: FANUC Series 0i-MD Operator's Manual, FANUC Series 30i/31i/32i-MODEL B Operator's Manual, FANUC Macro Compiler / Macro Executor Programming Manual (titles only — these are not openly hosted)

Mach 3 (ArtSoft / MachMotion):

• MachMotion "G and M-code Reference Using Mach3Mill Rev 1.84-A2" — https://machmotion.com/documentation/Software/Mach3/Mach3%20GCode%20Language%20Reference.pdf
• Mach3 G-Code Manual (MachMotion) — https://machmotion.com/documentation/Software/Mach3/Mach3%20G-Code%20Manual.pdf
• Mach3 V3.x Macro Programmer's Reference (ArtSoft) — https://www.machsupport.com/wp-content/uploads/2013/02/Mach3_V3.x_Macro_Prog_Ref.pdf
• Helman CNC "Mach3 Mill G Code List" — https://www.helmancnc.com/mach3-mill-g-code-list/
• CNCCookbook on Mach3 + G65 — https://www.cnccookbook.com/m98-m99-g-code-cnc-subprograms/

Mach 4 (ArtSoft / MachMotion):

• Mach4 Mill GCode Manual v1.0 (ArtSoft) — https://www.machsupport.com/wp-content/uploads/2014/05/Mach4%20Mill%20GCode%20Manual.pdf
• MachMotion Mach4 G & M Code Reference Manual — https://machmotion.com/documentation/Software/Mach4/Mach4-G-and-M-Code-Reference-Manual.pdf
• MachMotion BookStack Mach4 G/M Code Reference — https://support.machmotion.com/books/software/page/mach4-g-code-and-m-code-reference
• Mach4 Lathe Programming Guide — https://www.machsupport.com/wp-content/uploads/2014/05/Mach4%20Lathe%20GCode%20Manual.pdf
• Warp9 Mach3 vs Mach4 FAQ — https://www.warp9td.com/index.php/faq/faq-g-code-m-code

#Known unverifiable / uncertain entries

• FANUC G05.4 nano smoothing — present on some 30i-B variants, not universal across the 30i family.