checks.md

Checks

The Problems panel lists every mistake GlossCode finds in a program, with the worst ones first on each line. Click a problem (or press F8) to jump to its line. Each problem also shows as a red, amber or blue mark in the margin.

The checks are split in two:

• Data in data/gcode-rules.json: the message, severity and explanation for every rule, plus the per-control tables the rules read (modal groups, canned cycle words, codes that mean something else on that control, number formats, limits).
• Logic in the core (checks.c, still to be written; the mockup's checkProgram() is the reference). It makes one pass over the program in the order the machine runs it, following subprogram calls, and carries the machine state as it goes: units, absolute or incremental, feed mode and rate, spindle, tool, length offset, cutter comp, the active canned cycle and the tool position.

Adding a control or fixing a cycle's word list is a data change. Adding a new kind of check is a code change plus a new entry in rules.

Severities

Severity	Meaning
error	The control will alarm, or the program will cut something different from what it says.
warning	Very likely a mistake, but some shops do it on purpose.
info	Worth a look. Often fine.

A machine definition file will be able to change any rule's severity or turn it off; see machine-definitions.md.

Rules

Rule id	Severity	What it catches
dup-address	error	The same letter twice in one line, like Y2. Y3. (G and M are exempt)
empty-value	error	A letter with no number, like X on its own
unbalanced-brackets	error	An expression whose [ and ] don't pair up, like V58=[[V50+V51]/2+V52
modal-group-clash	error	Two codes from one group on one line, like G90 G91 or G00 G01
m-conflict	error	M-codes that contradict each other, like M03 M05 or M08 M09
foreign-code	warning or error	A code that means something else on this control, like G54 on an Okuma (X-axis length offset) or M97 on a Fanuc
cycle-missing-word	error	A canned cycle without a word it needs, like G81 with no R
cycle-missing-choice	error	A cycle that needs one of several words, like Haas G83 with no Q and no I/J/K
code-missing-word	error	A code with words of its own missing one it needs, like a Fagor 8055 G60 pattern with only K, or a G66 pocket with no S and E profile labels
cycle-call-no-def	error	Heidenhain Klartext: CYCL CALL, M99 or M89 before any CYCL DEF
pgm-name-mismatch	warning	Heidenhain Klartext: END PGM names another program than BEGIN PGM
block-number-order	info	Heidenhain Klartext: a block number that isn't higher than the one before
pattern-no-cycle	warning	A Fagor 8055 multiple machining pattern (G60 to G65) with no canned cycle or (MCALL) active to repeat at its points
cycle-needs-feed-per-min	error	Fagor 8065 lathe: a live tool cycle (G160 to G163) in G95 with no G94 feed programmed before it
cycle-stray-word	info	A word the cycle doesn't use, like Q on a G81
missing-label	error	M97 P, a lathe cycle's P/Q, or a Fagor 8055 G66 label (S, E, D, H, R, I, F, K), pointing to an N number that isn't in the file; on Heidenhain Klartext, a CALL LBL or FN 9 to 12 jump to an LBL that isn't in the file
no-feed-rate	error	A G01/G02/G03 move or feed cycle before any F
feed-mode-changed	warning	F set under G94 and then used under G95 (or the reverse), which turns 10 ipm into 10 ipr
feed-plausibility	info	A per-rev feed that's large (over 0.05 in or 1.5 mm) or a per-minute feed that's tiny
spindle-off-feed	warning	A cutting move with the spindle stopped or never started (Haas taps start the spindle themselves, so they're exempt)
no-speed	warning	M03/M04, or a tapping cycle, with no S set
torch-off-cut	warning	Plasma: a feed move with the torch off or never turned on. Takes the place of spindle-off-feed on controls whose cut on and cut off codes are known
torch-on-at-end	warning	Plasma: the program ends with the torch still on
missing-decimal	warning	A distance word with no decimal point. X1 is 0.0001 in on a Fanuc-style control
arc-no-center	error	G02/G03 with no R and no I/J/K
arc-r-and-ijk	warning	An arc with both R and I/J/K
arc-full-circle-r	error	A full circle written with R
arc-radius-mismatch	warning	The arc's end point isn't the same distance from the center as its start
comp-start-on-arc	error	G41/G42 turned on during an arc
comp-no-d	warning	G41/G42 with no D offset given
tlo-missing	warning	A Z move after a tool change before G43 H (G56 H on Okuma)
tlo-h-mismatch	info	T3 with H04
cycle-left-on	warning	A canned cycle still active at a tool change or the program end
comp-left-on	warning	Cutter comp still on at a tool change or the program end
g28-absolute	warning	G28 Z0. under G90, which moves through work Z0 on the way home
css-no-clamp	warning	G96 on a lathe before any max RPM (G50 S, or G92 S on controls that clamp with G92)
dwell-no-time	error	G04 with no time
dwell-milliseconds	info	G04 P500 on a control that reads a whole-number P as milliseconds (set by dwellNoDecimal in the dialect; Haas controls, old and NGC, do)
m-per-block	error	More M-codes on one line than the control allows (set by mPerBlock; Haas allows one, Okuma P200L lathes eight)
rapid-below-zero	info	A G00 to a negative Z (assuming Z0 is the top of the part)
no-program-end	warning	No M30 or M02
unknown-word	info	A code that isn't in the dictionary or this machine's file

CHECKS_DEMO.nc and LATHE_CHECKS.nc in the mockup have one of these mistakes on almost every line.

Numbers and units in the gloss line

• The gloss line always shows a decimal point: X1. reads X1.0, and X.25 reads X0.25.
• A distance word (X, Y, Z, U, W, I, J, K, R, Q) written without a decimal point is shown the way the control reads it. On Fanuc and Haas that's the smallest increment (Okuma is assumed to match until checked), so X1 reads X0.0001 in orange under G20, or X0.001 under G21, and missing-decimal flags it. The per-control setting is numbers in the rules file, so a control set up to read whole numbers as units can turn this off.
• F and S keep their letter, followed by a small unit: F12.0 ipm, F0.008 ipr, F300.0 mmpm, S2500 rpm, S400 sfm, S120 smm. The unit follows the active G94/G95 (G98/G99 on Fanuc-style lathes), G96/G97 and G20/G21.

How the rules file is laid out

{
  "rules": {
    "cycle-missing-word": { "severity": "error", "title": "...", "message": "{cycle} ({name}) needs {word}: {meaning}." }
  },
  "dialects": {
    "fanuc": { "mill": { "modalGroups": {...}, "cycles": {...}, "foreign": {...} }, "lathe": {...} },
    "haas":  { "inherits": "fanuc", "mill": { "cycles": { "G83": {...}, "G87": null } } },
    "okuma": { "inherits": "fanuc", "verified": false, ... }
  }
}

A dialect inherits from another and overrides by key. Objects like cycles and foreign merge one entry at a time, and null removes an inherited entry (Haas has no G87 back bore; it uses G77). Each cycle entry lists requires, optional, choices (one of several sets), labels (words that name N numbers), and flags: feed (uses F as a feed rate), leadF (F is the thread lead), speed (needs S), spindle (needs the spindle running), startsSpindle (the cycle starts it) and modal (false for one-shot lathe cycles).

Other dialect keys the checks read: unitCodes (the codes that switch inch and metric; null when units come from a parameter, as on Okuma lathes where G20 and G21 are home returns), leadCodes (motion codes whose F is a thread lead, so the feed checks skip it), mPerBlock and dwellNoDecimal. A cycle can carry meaning to say what a required word does in that cycle, for the missing-word message.

Word hints

wordHints lists the words other codes need, so the editor can show them as grey hint text after the code (G02 shows R## or I## J##). An entry is either { "arc": true } (R, or the two centers for the active plane: I/J under G17, I/K under G18, J/K under G19) or { "requires": [...] }. Canned cycles don't need entries here: their hints come from requires and choices in cycles, G04 uses dwellWords, and subprogram calls use subCalls, so the hints always match the checks. Once a line uses any word from one choice, the other choices' hints go away.

Cycle help

cycleHelp (beside dialects) feeds the canned cycle guide (F1). It's keyed mill and lathe for the Fanuc-style base, with haas.mill, haas.lathe and so on overriding by cycle. Each cycle has about (what it does), sketch (which drawing to use), optional labels (letters on the drawing, since Fanuc G76 calls the thread height P where Haas calls it K) and words. A word entry is [example value, what it does] or [example value, what it does, English word]. The English word, when given, is what the editor shows for that letter while the cycle is active, so Haas G76 ... A60 reads ANGLE60 instead of an unknown word. common holds words shared by every cycle of that type (X, Y, Z, R, F on a mill).

The word list in the guide (and whether each word is required, one of a choice, or optional) comes from the dialect's cycles table, not from cycleHelp.

Plasma and other machine types

machineTypes (beside dialects) lists the machine types. mill and lathe are the original two. plasma has "base": "mill": a plasma machine starts from its control's mill tables along the whole inherits chain, then the control's plasma tables go on top, and a word not in <control>.plasma falls back to <control>.mill and the mill meaning in the dictionary. fanuc.plasma is the shared plasma base. It turns off canned cycles, tool changes, tool length offsets and spindle speed modes, and lays out the columns with a Torch column (the control's cut codes) and a Kerf column (D). A control with no mill tables, like Hypertherm, has only its plasma table.

A plasma table's process names the torch: on and off are the cut on and cut off codes, which replace the spindle checks (spindle-off-feed and no-speed don't run on plasma), and changes lists codes that change the process or material, which the timeline marks. Controls whose cut codes aren't verified leave on empty, which turns the torch checks off. timeline in machineTypes lists what the timeline can plot for that type, the first being the default.

Control	Cut on	Cut off	Notes
Hypertherm Phoenix / EDGE Connect (hypertherm)	M07 (or M03/M04 when code mapping makes them cut on)	M08 (or M05/M06)	G59 sets variables, G97/G98 start and end a loop, G04 X dwell, G94/G95 flagged as unsupported, G41/G42 D kerf
Centroid Acorn (centroid)	M61 touch off and pierce	M62 torch off and raise	M65 material profile; everything else as Centroid CNC12 mill
Tormach PathPilot (tormach)	not checked yet	not checked yet	G15 probe and G16 pierce instead of polar coordinates; M200–M213 aren't in the dictionary yet

See manual-reviews/plasma-hypertherm-tormach-centroid.md.

fileHints (beside dialects) suggests controls when a file with no default machine is opened. Each rule names controls, optional ext (lower case, with the dot) and content clues (re, optional flags, and why, the reason shown). A content clue counts 3 and an extension 2; the controls of the best-scoring rules go first in the picker. Only add clues that belong to one control family.

verified: false marks tables written from general knowledge that still need checking against the control's programming manual. The mockup shows a banner in the Problems panel for those.

How much Haas and Okuma support there is today

Control	Translation	Checks	Confidence
Haas mill (NGC)	Good for 2.5-axis work, plus gloss words for G12/G13, G47, G70–G72 bolt patterns, G110–G129 and G154 work offsets, M10–M13 brakes	All rules above, with Haas cycle words (I/J/K peck, J retract on taps, L repeats), M97 local subprograms, one M code per line, P without a decimal as milliseconds	High: checked against the 2025 and 2020 mill manuals (see manual-reviews/haas-ngc.md)
Haas lathe (NGC)	Good for turning, facing, grooving and threading, plus gloss words for work offsets G110–G129 and G154, live tool, chuck, tailstock and sub-spindle M codes, M88/M89 high-pressure coolant, G95 live-tool tap	All rules above, with Haas one-block G71/G72/G73/G76, G90/G92/G94 cycles, G50 S clamp, G84 starting the spindle, one M code per line, P without a decimal as milliseconds	High: checked against the 2020 and 2025 lathe manuals (see manual-reviews/haas-ngc.md and haas-ngc-lathe-2025.md)
Fanuc (0i/30i)	Same base as Haas	Same, with Fanuc cycle words and M97 flagged as Haas-only	High
Haas mill, 1995 control (haas1995)	Same as Haas mill, plus G87/G88 manual-retract bores, G110–G129 work offsets and M16	Haas rules with the 1995 cycle words (no P on G73/G83, no J on G74/G84), one M-code per line, P without a decimal as milliseconds, and G93/G95/G96/G154/M88/M89 flagged	High: checked against the June 1995 VF-Series Operator's Manual (see manual-reviews/haas-vf-1995.md)
Okuma mill (OSP)	G15 H work offsets, G56 H length offset, G53 offset cancel, CALL / RTS subprograms, M02	All the generic rules, plus Okuma's traps: G54–G59 (length offsets on Okuma), G43, G28, M97, M98, M99	Medium: first draft, not yet checked against an OSP manual
Okuma lathe (OSP)	G90/G91, G94/G95 feed modes, G20 home return, G28/G29 torque limit, G31–G35 thread cycles, LAP codes named	Generic rules, plus G71/G72 thread, G73/G74 grooving and G77/G78 tapping cycles, up to eight M codes per line, G54–G59 (info), G98/G99, G28 and M97/M98 flagged	Medium: lathe tables checked against the OSP-P200L manual (see manual-reviews/okuma-osp-p200l.md); LAP isn't checked yet

Not covered yet

Haas mill: checks for G12/G13 circular pockets, G150 pocketing, G70/G71/G72 bolt patterns and G47 engraving (they translate but their words aren't checked), G51/G68 scaling and rotation, 4th and 5th axis (A/B words, G93 inverse time, G234 TCPC, G254 DWO), and macros (# variables, IF, WHILE, GOTO, G65 calls). Macro lines are left alone rather than flagged.

Haas lathe: live tooling checks (C axis, G112 polar interpolation, Y axis, G95/G186/G195 live-tool taps, G242–G246), sub-spindle and tailstock codes, bar feeder, and tool nose comp checks.

Okuma, both: the parts of OSP that aren't Fanuc-shaped. These need their own parser support, not just table entries:

• Sequence names made of letters (NAT1, NLAP1) and program names like OSUB. The mockup only handles numeric N and O labels.
• User Task variables (VC1, V1, named variables) and IF [..] N.. / GOTO branches.
• Schedule programs and file types (.MIN, .SSB, .SDF).
• Okuma lathe LAP: the G85/G86/G87/G88 roughing and finishing cycles read a contour defined between G81/G82 and G80, named by a sequence name. Checking these needs the contour block support above.
• Okuma lathe 6-digit tool calls (T010101) and two-letter words (DA, SB, QA, SA).
• Twin-turret G13/G14 and the Okuma M-codes that differ from Fanuc.

To take Okuma past draft quality, the next step is a handful of real programs from each Okuma machine, plus the control model (P300, P500…) so the tables can be checked against its manual.