FAQ.md

# Easy G-Code Plot FAQ

Updated for **2.9.0**: external CLI integration, alongside iTNC position patterns, pocket and thread-milling cycles, classic SINUMERIK milling cycles, native rotary/TCP input and bounded XZ turning.

This document is the detailed user and developer reference for Easy G-Code Plot. It reflects the current working tree and explains the GUI, the shared CNC execution kernel, supported FANUC, SINUMERIK native/ISO-M milling and native/ISO-T turning, and HEIDENHAIN iTNC 530 Klartext semantics, Macro B runtime, turning and milling cycles, rotary and TCP behavior, diagnostics, CLI, batch analysis and export behavior.

The same FAQ can be packaged for offline use in **Help → FAQ**.

<details>
  <summary><h2>Contents</h2></summary>

- [Easy G-Code Plot FAQ](#easy-g-code-plot-faq)
  - [Project scope and execution model](#project-scope-and-execution-model)
    - [What is Easy G-Code Plot?](#what-is-easy-g-code-plot)
    - [What is the authoritative data flow?](#what-is-the-authoritative-data-flow)
    - [Is the OpenGL plot the CNC model?](#is-the-opengl-plot-the-cnc-model)
    - [Is the program a machine simulator?](#is-the-program-a-machine-simulator)
    - [Can I visualize SINUMERIK CAM five-axis programs?](#can-i-visualize-sinumerik-cam-five-axis-programs)
    - [What does deterministic mean in this project?](#what-does-deterministic-mean-in-this-project)
  - [Getting started](#getting-started)
    - [How do I install it?](#how-do-i-install-it)
    - [What is the normal GUI workflow?](#what-is-the-normal-gui-workflow)
    - [How do I work with multiple documents?](#how-do-i-work-with-multiple-documents)
    - [Which settings are per document and which are shared?](#which-settings-are-per-document-and-which-are-shared)
    - [What happens to dialogs and playback when I switch documents?](#what-happens-to-dialogs-and-playback-when-i-switch-documents)
    - [How do Close and Close All handle unsaved changes?](#how-do-close-and-close-all-handle-unsaved-changes)
    - [How do I compare programs?](#how-do-i-compare-programs)
    - [What does the iTNC-code source type do?](#what-does-the-itnc-code-source-type-do)
    - [Which input encodings are supported?](#which-input-encodings-are-supported)
    - [Are compact FANUC blocks accepted?](#are-compact-fanuc-blocks-accepted)
    - [Which comment forms are understood?](#which-comment-forms-are-understood)
    - [How do optional `/` Block Skip lines work?](#how-do-optional--block-skip-lines-work)
  - [Diagnostics and fail-closed behavior](#diagnostics-and-fail-closed-behavior)
    - [What are `ok` and `complete`?](#what-are-ok-and-complete)
    - [What diagnostic information is stored?](#what-diagnostic-information-is-stored)
    - [What happens after unsupported position-changing semantics?](#what-happens-after-unsupported-position-changing-semantics)
    - [How are unsupported turning G-codes classified?](#how-are-unsupported-turning-g-codes-classified)
    - [What about unsupported M-codes?](#what-about-unsupported-m-codes)
    - [Are conflicting modal codes detected?](#are-conflicting-modal-codes-detected)
    - [Are there execution resource limits?](#are-there-execution-resource-limits)
  - [FANUC Macro B and program flow](#fanuc-macro-b-and-program-flow)
    - [How complete is Macro B support?](#how-complete-is-macro-b-support)
    - [Which variable forms are supported?](#which-variable-forms-are-supported)
    - [What is special about `#0`?](#what-is-special-about-0)
    - [What happens when an undefined variable is used numerically?](#what-happens-when-an-undefined-variable-is-used-numerically)
    - [Which arithmetic and relational operators are supported?](#which-arithmetic-and-relational-operators-are-supported)
    - [Which Macro B functions are implemented?](#which-macro-b-functions-are-implemented)
    - [Are assignments supported on labeled blocks?](#are-assignments-supported-on-labeled-blocks)
    - [Is unconditional `GOTO` supported?](#is-unconditional-goto-supported)
    - [Is `IF [...] GOTO` supported?](#is-if--goto-supported)
    - [Are `WHILE / DO / END` loops supported?](#are-while--do--end-loops-supported)
    - [Are real Macro B milling programs exercised by the tests?](#are-real-macro-b-milling-programs-exercised-by-the-tests)
    - [Is `G65` supported?](#is-g65-supported)
    - [How are G65 Type I arguments mapped?](#how-are-g65-type-i-arguments-mapped)
    - [How are repeated I/J/K G65 arguments handled?](#how-are-repeated-ijk-g65-arguments-handled)
    - [Do G65 argument words also perform machine actions?](#do-g65-argument-words-also-perform-machine-actions)
    - [What happens to `#1..#33` when a G65 macro returns?](#what-happens-to-133-when-a-g65-macro-returns)
    - [What does `G65 ... L...` do?](#what-does-g65--l-do)
    - [How deeply can G65 macros nest?](#how-deeply-can-g65-macros-nest)
    - [How does M98 behave inside a G65 macro?](#how-does-m98-behave-inside-a-g65-macro)
    - [Are M98/M99 subprograms supported outside Macro B?](#are-m98m99-subprograms-supported-outside-macro-b)
    - [Is `M99 P...` supported?](#is-m99-p-supported)
    - [Are Macro B variable values stored per execution step?](#are-macro-b-variable-values-stored-per-execution-step)
    - [Does Expanded Execution export keep Macro B statements?](#does-expanded-execution-export-keep-macro-b-statements)
  - [FANUC turning](#fanuc-turning)
    - [Main differences between Type A and Type B](#main-differences-between-type-a-and-type-b)
    - [What is the turning coordinate model?](#what-is-the-turning-coordinate-model)
    - [How do X/U and Z/W behave?](#how-do-xu-and-zw-behave)
    - [How are G20 and G21 handled?](#how-are-g20-and-g21-handled)
    - [Which turning arc formats are supported?](#which-turning-arc-formats-are-supported)
    - [Why can G2/G3 direction look inverted in an XZ plot?](#why-can-g2g3-direction-look-inverted-in-an-xz-plot)
    - [Is direct A-angle turning programming supported?](#is-direct-a-angle-turning-programming-supported)
    - [Are C chamfers and corner R fillets supported?](#are-c-chamfers-and-corner-r-fillets-supported)
    - [Are G32 and G33 threading motions supported?](#are-g32-and-g33-threading-motions-supported)
    - [What are the turning feed modes?](#what-are-the-turning-feed-modes)
    - [Are G96 and G97 modeled?](#are-g96-and-g97-modeled)
    - [What does G50 S do in turning?](#what-does-g50-s-do-in-turning)
    - [Are spindle start/stop signals tracked?](#are-spindle-startstop-signals-tracked)
    - [Which WCS features work in turning?](#which-wcs-features-work-in-turning)
    - [Is G53 supported in turning?](#is-g53-supported-in-turning)
    - [How does G28 work?](#how-does-g28-work)
    - [Is G30 the same as G28?](#is-g30-the-same-as-g28)
    - [How does tool-nose compensation work?](#how-does-tool-nose-compensation-work)
  - [Turning cycles](#turning-cycles)
    - [Which turning cycles are modeled?](#which-turning-cycles-are-modeled)
    - [Do cycle motions remember where they came from?](#do-cycle-motions-remember-where-they-came-from)
    - [How are cycle profiles selected by P and Q?](#how-are-cycle-profiles-selected-by-p-and-q)
    - [Do G71/G72/G73 profile blocks support lines and arcs?](#do-g71g72g73-profile-blocks-support-lines-and-arcs)
    - [How does G70 work?](#how-does-g70-work)
    - [What form of G71 is supported?](#what-form-of-g71-is-supported)
    - [How is G71 depth interpreted?](#how-is-g71-depth-interpreted)
    - [How are G71 U/W finish allowances handled?](#how-are-g71-uw-finish-allowances-handled)
    - [How does G71 distinguish OD and ID roughing?](#how-does-g71-distinguish-od-and-id-roughing)
    - [What is G71 Type I behavior?](#what-is-g71-type-i-behavior)
    - [Is G71 Type II supported?](#is-g71-type-ii-supported)
    - [How does G72 work?](#how-does-g72-work)
    - [Is G72 Type II fully generic?](#is-g72-type-ii-fully-generic)
    - [How does G73 work?](#how-does-g73-work)
    - [How does G74 work?](#how-does-g74-work)
    - [How does G75 work?](#how-does-g75-work)
    - [How is turning peck motion represented?](#how-is-turning-peck-motion-represented)
    - [How does two-line G76 work?](#how-does-two-line-g76-work)
    - [How are G76 P/Q integer increments interpreted?](#how-are-g76-pq-integer-increments-interpreted)
    - [How is G76 pass depth generated?](#how-is-g76-pass-depth-generated)
    - [What do the packed G76 P digits mean here?](#what-do-the-packed-g76-p-digits-mean-here)
    - [Which G76 tool angles are modeled?](#which-g76-tool-angles-are-modeled)
    - [How is G76 chamfer modeled?](#how-is-g76-chamfer-modeled)
    - [Is G92 a modal threading cycle?](#is-g92-a-modal-threading-cycle)
    - [Is G90 a modal turning cycle?](#is-g90-a-modal-turning-cycle)
    - [Is G94 a modal facing cycle?](#is-g94-a-modal-facing-cycle)
    - [What cancels G90/G92/G94?](#what-cancels-g90g92g94)
    - [Are turning G83 and G84 modal?](#are-turning-g83-and-g84-modal)
    - [How does turning G83 behave?](#how-does-turning-g83-behave)
    - [How does turning G84 behave?](#how-does-turning-g84-behave)
    - [Does P dwell in turning G83/G84 create geometry?](#does-p-dwell-in-turning-g83g84-create-geometry)
    - [What happens if a modal drilling/tapping cycle is left in an invalid state?](#what-happens-if-a-modal-drillingtapping-cycle-is-left-in-an-invalid-state)
  - [FANUC milling](#fanuc-milling)
    - [Which milling G functions are recognized?](#which-milling-g-functions-are-recognized)
    - [Which milling M functions are recognized?](#which-milling-m-functions-are-recognized)
    - [What basic milling motion is modeled?](#what-basic-milling-motion-is-modeled)
    - [How is indexed rotary milling handled?](#how-is-indexed-rotary-milling-handled)
    - [Which rotary profiles have been checked?](#which-rotary-profiles-have-been-checked)
    - [What happens when indexed geometry cannot be resolved?](#what-happens-when-indexed-geometry-cannot-be-resolved)
    - [Which milling canned cycles are modeled?](#which-milling-canned-cycles-are-modeled)
    - [What is the difference between G73 and G83 milling peck cycles?](#what-is-the-difference-between-g73-and-g83-milling-peck-cycles)
    - [How is G82 dwell represented?](#how-is-g82-dwell-represented)
    - [How is milling G84 represented?](#how-is-milling-g84-represented)
    - [How is milling G86 represented?](#how-is-milling-g86-represented)
    - [What do milling G98/G99 mean?](#what-do-milling-g98g99-mean)
    - [What are milling feed modes?](#what-are-milling-feed-modes)
    - [Which work coordinate systems are supported?](#which-work-coordinate-systems-are-supported)
    - [How does G10 behave under G91 in milling?](#how-does-g10-behave-under-g91-in-milling)
    - [How does G52 work?](#how-does-g52-work)
    - [How do G68 and G69 work?](#how-do-g68-and-g69-work)
    - [How does G51/G50 scaling work?](#how-does-g51g50-scaling-work)
    - [Is G53 supported in milling?](#is-g53-supported-in-milling)
    - [Is G28 supported in milling?](#is-g28-supported-in-milling)
    - [Is continuous five-axis TCP (`G43.4`) supported?](#is-continuous-five-axis-tcp-g434-supported)
    - [How are milling arcs programmed?](#how-are-milling-arcs-programmed)
    - [What does Arc Type autodetection do?](#what-does-arc-type-autodetection-do)
    - [Can one program mix R arcs with IJK arcs?](#can-one-program-mix-r-arcs-with-ijk-arcs)
    - [Are full circles supported?](#are-full-circles-supported)
    - [Is helical interpolation supported?](#is-helical-interpolation-supported)
    - [What does G16/G15 polar programming do?](#what-does-g16g15-polar-programming-do)
    - [How does polar G90 work?](#how-does-polar-g90-work)
    - [How does polar G91 work?](#how-does-polar-g91-work)
    - [Do G20/G21 scale the polar angle?](#do-g20g21-scale-the-polar-angle)
    - [Are polar G2/G3 arcs supported?](#are-polar-g2g3-arcs-supported)
    - [Is G12.1/G13.1 polar interpolation supported?](#is-g121g131-polar-interpolation-supported)
    - [How does milling cutter compensation work?](#how-does-milling-cutter-compensation-work)
    - [What does `UNVERIFIED_CUTTER_COMPENSATION` mean?](#what-does-unverified_cutter_compensation-mean)
    - [Is G43 tool-length geometry applied?](#is-g43-tool-length-geometry-applied)
  - [Tool libraries and tool discovery](#tool-libraries-and-tool-discovery)
    - [Where are persistent tools stored?](#where-are-persistent-tools-stored)
    - [What is the difference between Current Program and Saved Library?](#what-is-the-difference-between-current-program-and-saved-library)
    - [Does opening a program write discovered tools to the database?](#does-opening-a-program-write-discovered-tools-to-the-database)
    - [How are turning tool numbers represented?](#how-are-turning-tool-numbers-represented)
    - [Can comments describe tool geometry?](#can-comments-describe-tool-geometry)
    - [What happens when no explicit type hint is present?](#what-happens-when-no-explicit-type-hint-is-present)
    - [Are macro T expressions discovered as literal tools?](#are-macro-t-expressions-discovered-as-literal-tools)
    - [Which turning tool geometries are stored?](#which-turning-tool-geometries-are-stored)
    - [Which milling tools can be previewed?](#which-milling-tools-can-be-previewed)
    - [How are milling tool lengths defined?](#how-are-milling-tool-lengths-defined)
    - [Does CLI execution load the GUI Saved Library?](#does-cli-execution-load-the-gui-saved-library)
  - [Interface, editor and playback](#interface-editor-and-playback)
    - [How do I measure geometry in the plot?](#how-do-i-measure-geometry-in-the-plot)
    - [How do I insert the calculated stock into STL Objects?](#how-do-i-insert-the-calculated-stock-into-stl-objects)
    - [What are the two main GUI panels?](#what-are-the-two-main-gui-panels)
    - [How does an imported STL affect toolpath visibility?](#how-does-an-imported-stl-affect-toolpath-visibility)
    - [How do I use the STL Objects panel?](#how-do-i-use-the-stl-objects-panel)
      - [How do I import and select STL models?](#how-do-i-import-and-select-stl-models)
      - [What do Undo, Redo, Statistics and Delete do?](#what-do-undo-redo-statistics-and-delete-do)
      - [How do STL base points and bounding-box picks work?](#how-do-stl-base-points-and-bounding-box-picks-work)
      - [How do I position and transform an STL model?](#how-do-i-position-and-transform-an-stl-model)
      - [How do STL arrays work?](#how-do-stl-arrays-work)
      - [How do I make a 3D section through an STL model?](#how-do-i-make-a-3d-section-through-an-stl-model)
      - [What does STL Statistics report, and how do I display inches?](#what-does-stl-statistics-report-and-how-do-i-display-inches)
    - [How do I change letter case or mark optional blocks?](#how-do-i-change-letter-case-or-mark-optional-blocks)
    - [How do I print the plot?](#how-do-i-print-the-plot)
    - [Which fixed views are available?](#which-fixed-views-are-available)
    - [How does playback relate to the kernel?](#how-does-playback-relate-to-the-kernel)
    - [What do Step Backward and Step Forward do?](#what-do-step-backward-and-step-forward-do)
    - [Why can many playback motions map to one source line?](#why-can-many-playback-motions-map-to-one-source-line)
    - [How do I customize toolbar buttons?](#how-do-i-customize-toolbar-buttons)
    - [How do I locate a plotted move in the editor?](#how-do-i-locate-a-plotted-move-in-the-editor)
    - [Does automatic refresh move the editor caret?](#does-automatic-refresh-move-the-editor-caret)
    - [What happens when Auto Update is too expensive?](#what-happens-when-auto-update-is-too-expensive)
    - [What does Cancel stop?](#what-does-cancel-stop)
    - [What CNC editing assistants are included?](#what-cnc-editing-assistants-are-included)
    - [What does Hole Calculator generate?](#what-does-hole-calculator-generate)
    - [What does Pocket Calculator generate?](#what-does-pocket-calculator-generate)
    - [Where are snippets stored?](#where-are-snippets-stored)
  - [Options and scene configuration](#options-and-scene-configuration)
    - [Where can I read execution errors and warnings?](#where-can-i-read-execution-errors-and-warnings)
    - [How do I change the interface language?](#how-do-i-change-the-interface-language)
    - [How do I change the theme?](#how-do-i-change-the-theme)
    - [How do I change the current-line highlight color?](#how-do-i-change-the-current-line-highlight-color)
    - [Where do I set work coordinate systems and home values?](#where-do-i-set-work-coordinate-systems-and-home-values)
    - [How do I set turning stock dimensions?](#how-do-i-set-turning-stock-dimensions)
    - [Is Stock Removal available for milling?](#is-stock-removal-available-for-milling)
  - [Milling Stock Removal](#milling-stock-removal)
    - [How do I start milling stock simulation?](#how-do-i-start-milling-stock-simulation)
    - [How do milling stock bounds and allowance work?](#how-do-milling-stock-bounds-and-allowance-work)
    - [Which milling cutters and movements are supported?](#which-milling-cutters-and-movements-are-supported)
    - [What does milling Accuracy control?](#what-does-milling-accuracy-control)
    - [How do playback and tool edits affect the stock?](#how-do-playback-and-tool-edits-affect-the-stock)
    - [What do the stock colors and box faces represent?](#what-do-the-stock-colors-and-box-faces-represent)
    - [How do I export the simulated milling stock?](#how-do-i-export-the-simulated-milling-stock)
    - [How does the GPU stock engine work?](#how-does-the-gpu-stock-engine-work)
    - [What are the milling stock requirements and limits?](#what-are-the-milling-stock-requirements-and-limits)
  - [Turning Stock Removal](#turning-stock-removal)
    - [What is Turning Stock Removal?](#what-is-turning-stock-removal)
    - [How is automatic stock estimated?](#how-is-automatic-stock-estimated)
    - [Can stock dimensions be overridden manually?](#can-stock-dimensions-be-overridden-manually)
    - [Which tools remove material?](#which-tools-remove-material)
    - [How are threads represented in Stock Removal?](#how-are-threads-represented-in-stock-removal)
    - [Does Stock Removal detect machine collisions?](#does-stock-removal-detect-machine-collisions)
  - [Statistics and Tokens/Variables](#statistics-and-tokensvariables)
    - [What does Toolpath Statistics contain?](#what-does-toolpath-statistics-contain)
    - [Why can machining time be UNKNOWN?](#why-can-machining-time-be-unknown)
    - [What is the Tokens tab?](#what-is-the-tokens-tab)
    - [What is the Variables tab?](#what-is-the-variables-tab)
    - [Why can Variables be unavailable?](#why-can-variables-be-unavailable)
  - [Export](#export)
    - [Which GUI export families exist?](#which-gui-export-families-exist)
    - [Are exporters separate G-code interpreters?](#are-exporters-separate-g-code-interpreters)
    - [What does Full Program mean?](#what-does-full-program-mean)
    - [What does Expanded Execution mean?](#what-does-expanded-execution-mean)
    - [What does Auto (source controller) mean?](#what-does-auto-source-controller-mean)
    - [How do I manage user postprocessors in the GUI?](#how-do-i-manage-user-postprocessors-in-the-gui)
    - [How does Modal Feed work?](#how-does-modal-feed-work)
    - [Can I choose formatting options when converting to a specific controller?](#can-i-choose-formatting-options-when-converting-to-a-specific-controller)
    - [What does DXF contain?](#what-does-dxf-contain)
    - [Does DXF parse the G-code again?](#does-dxf-parse-the-g-code-again)
    - [Which NC formatting options exist?](#which-nc-formatting-options-exist)
    - [How does a post profile control word order and mandatory addresses?](#how-does-a-post-profile-control-word-order-and-mandatory-addresses)
    - [Which milling Expanded arc output modes exist?](#which-milling-expanded-arc-output-modes-exist)
    - [What happens when a full circle is exported in R mode?](#what-happens-when-a-full-circle-is-exported-in-r-mode)
    - [Can Expanded NC be converted between millimetres and inches?](#can-expanded-nc-be-converted-between-millimetres-and-inches)
    - [Can Full Program be forced to mm or inch?](#can-full-program-be-forced-to-mm-or-inch)
    - [What units does DXF use?](#what-units-does-dxf-use)
    - [Can comments be removed from export?](#can-comments-be-removed-from-export)
    - [Are exports written atomically by the CLI service?](#are-exports-written-atomically-by-the-cli-service)
    - [Can CLI export overwrite the source file?](#can-cli-export-overwrite-the-source-file)
    - [Can CLI export be compared directly with an expected NC file?](#can-cli-export-be-compared-directly-with-an-expected-nc-file)
  - [SINUMERIK 840D input](#sinumerik-840d-input)
    - [What SINUMERIK support is included?](#what-sinumerik-support-is-included)
    - [How are MPF and SPF files detected?](#how-are-mpf-and-spf-files-detected)
    - [Can FANUC milling programs be converted to SINUMERIK?](#can-fanuc-milling-programs-be-converted-to-sinumerik)
    - [Can SINUMERIK native milling programs be converted to FANUC?](#can-sinumerik-native-milling-programs-be-converted-to-fanuc)
    - [How do Full Program and Expanded Execution differ?](#how-do-full-program-and-expanded-execution-differ)
    - [Is SINUMERIK lathe supported?](#is-sinumerik-lathe-supported)
  - [HEIDENHAIN iTNC 530 input](#heidenhain-itnc-530-input)
    - [What HEIDENHAIN support is included?](#what-heidenhain-support-is-included)
    - [Which pocket and thread-milling cycles are supported?](#which-pocket-and-thread-milling-cycles-are-supported)
    - [How do position-pattern cycles 220 and 221 execute?](#how-do-position-pattern-cycles-220-and-221-execute)
    - [How are Klartext source, parameters and diagnostics represented?](#how-are-klartext-source-parameters-and-diagnostics-represented)
    - [Which iTNC editor tools and exports are available?](#which-itnc-editor-tools-and-exports-are-available)
    - [How is the iTNC implementation verified?](#how-is-the-itnc-implementation-verified)
  - [CLI](#cli)
    - [Does the CLI use the same kernel as the GUI?](#does-the-cli-use-the-same-kernel-as-the-gui)
    - [Which commands exist?](#which-commands-exist)
    - [What does `parse` do?](#what-does-parse-do)
    - [What does `trace` do?](#what-does-trace-do)
    - [What does `analyze` do?](#what-does-analyze-do)
    - [What does `batch` do?](#what-does-batch-do)
    - [What does `export` do?](#what-does-export-do)
    - [What does `batch-export` do?](#what-does-batch-export-do)
    - [Are single export and batch export different exporters?](#are-single-export-and-batch-export-different-exporters)
    - [Which dialect names are used?](#which-dialect-names-are-used)
    - [What are the exit codes?](#what-are-the-exit-codes)
    - [How do I see every option and default?](#how-do-i-see-every-option-and-default)
  - [Batch analysis](#batch-analysis)
    - [What does batch analysis validate?](#what-does-batch-analysis-validate)
    - [Which batch statuses exist?](#which-batch-statuses-exist)
    - [Which extensions are scanned by default?](#which-extensions-are-scanned-by-default)
    - [Can files without a normal NC extension be discovered?](#can-files-without-a-normal-nc-extension-be-discovered)
    - [Is discovery deterministic?](#is-discovery-deterministic)
    - [Can I restrict extensions?](#can-i-restrict-extensions)
    - [What is aggregated in the batch summary?](#what-is-aggregated-in-the-batch-summary)
    - [What files are written?](#what-files-are-written)
    - [Does a bad input file stop the whole batch?](#does-a-bad-input-file-stop-the-whole-batch)
    - [Are there preset batch scripts?](#are-there-preset-batch-scripts)
  - [Batch export](#batch-export)
    - [What problem does batch export solve?](#what-problem-does-batch-export-solve)
    - [Does batch export modify the input files?](#does-batch-export-modify-the-input-files)
    - [Is the source directory hierarchy preserved?](#is-the-source-directory-hierarchy-preserved)
    - [What happens if two source names map to one output name?](#what-happens-if-two-source-names-map-to-one-output-name)
    - [Does one export error stop every file?](#does-one-export-error-stop-every-file)
    - [What files describe the batch export?](#what-files-describe-the-batch-export)
    - [What are batch-export statuses?](#what-are-batch-export-statuses)
    - [Which export modes are available from the CLI?](#which-export-modes-are-available-from-the-cli)
    - [Which options are intentionally rejected in Full Program mode?](#which-options-are-intentionally-rejected-in-full-program-mode)
    - [Can sequence start/increment be supplied without sequence numbers?](#can-sequence-startincrement-be-supplied-without-sequence-numbers)
    - [Are there preset batch-export scripts?](#are-there-preset-batch-export-scripts)
  - [Configuration](#configuration)
    - [Where is application configuration stored on Windows?](#where-is-application-configuration-stored-on-windows)
    - [What is stored in `config.ini`?](#what-is-stored-in-configini)
    - [Is `tools.db` replaceable by old JSON values in config.ini?](#is-toolsdb-replaceable-by-old-json-values-in-configini)
    - [Where is the log file?](#where-is-the-log-file)
    - [What does DEBUG logging add?](#what-does-debug-logging-add)
  - [Troubleshooting](#troubleshooting)
    - [The plot is empty](#the-plot-is-empty)
    - [Macro B motion is missing](#macro-b-motion-is-missing)
    - [My G65 M/S/T words did not start spindle/coolant/change tool](#my-g65-mst-words-did-not-start-spindlecoolantchange-tool)
    - [Cutter compensation is not visible](#cutter-compensation-is-not-visible)
    - [G43 appears in the source but the plotted Z does not include tool length](#g43-appears-in-the-source-but-the-plotted-z-does-not-include-tool-length)
    - [G71 leaves material on the wrong side](#g71-leaves-material-on-the-wrong-side)
    - [G72 Type II reports an error](#g72-type-ii-reports-an-error)
    - [G76 reports `UNSUPPORTED_G76_TOOL_ANGLE`](#g76-reports-unsupported_g76_tool_angle)
    - [Batch shows `UNSUPPORTED_M_CODE` but the geometry looks correct](#batch-shows-unsupported_m_code-but-the-geometry-looks-correct)
    - [Export unit conversion is refused](#export-unit-conversion-is-refused)
    - [Batch-export says the output directory is invalid](#batch-export-says-the-output-directory-is-invalid)
    - [A large program does not update while typing](#a-large-program-does-not-update-while-typing)
    - [The GUI says the current execution is stale](#the-gui-says-the-current-execution-is-stale)
  - [Development and architecture](#development-and-architecture)
    - [How is the CNC kernel organized?](#how-is-the-cnc-kernel-organized)
    - [What belongs in `frontend/`?](#what-belongs-in-frontend)
    - [What belongs in `runtime/`?](#what-belongs-in-runtime)
    - [Why are turning cycles separate files?](#why-are-turning-cycles-separate-files)
    - [What belongs in `milling/`?](#what-belongs-in-milling)
    - [What belongs in `compensation/`?](#what-belongs-in-compensation)
    - [What belongs in `app/gcode/export/`?](#what-belongs-in-appgcodeexport)
    - [What does `execution/program.py` do?](#what-does-executionprogrampy-do)
    - [What does `batch/analysis.py` do?](#what-does-batchanalysispy-do)
    - [What does `batch/export.py` do?](#what-does-batchexportpy-do)
    - [Which native components exist?](#which-native-components-exist)
    - [How are execution results represented publicly?](#how-are-execution-results-represented-publicly)
    - [What is an `ExecutionStep`?](#what-is-an-executionstep)
    - [What is an `ExecutionEvent`?](#what-is-an-executionevent)
    - [How are tests organized?](#how-are-tests-organized)
    - [How do I run the main checks?](#how-do-i-run-the-main-checks)
    - [How do I run the daily GUI smoke test with a visible window?](#how-do-i-run-the-daily-gui-smoke-test-with-a-visible-window)
    - [Are generated Qt Python files edited manually?](#are-generated-qt-python-files-edited-manually)
  - [Build and release](#build-and-release)
    - [How do I build on Windows?](#how-do-i-build-on-windows)
    - [How do I build on Linux?](#how-do-i-build-on-linux)
    - [Does the project use a separate build environment?](#does-the-project-use-a-separate-build-environment)
    - [How are releases validated in CI?](#how-are-releases-validated-in-ci)
    - [Does a Linux executable run as a Windows `.exe`?](#does-a-linux-executable-run-as-a-windows-exe)
  - [License](#license)

</details>

---

## Project scope and execution model

### What is Easy G-Code Plot?

Easy G-Code Plot is a CNC editor, deterministic program executor, analyzer, backplotter and exporter for FANUC turning/milling, SINUMERIK 840D milling and bounded XZ turning, and HEIDENHAIN iTNC 530 Klartext milling programs. Supported native SINUMERIK input includes bounded R expressions and WHILE/GOTO/IF flow, plus CAM-oriented indexed 3+2 and continuous five-axis trajectories on configured rotary profiles; ISO Dialect M is also supported within its documented subset.

Native HEIDENHAIN input covers the documented subset of Klartext contours, Q parameters, drilling cycles, position patterns 220/221, pocket cycles 251/252 and thread milling 262; unsupported commands produce explicit diagnostics.

Checked CAM examples include programs generated in Autodesk Fusion 360 and Siemens NX 2312 using postprocessors for SINUMERIK 840D and FANUC. Coverage applies to the tested commands and configured kinematics described in this FAQ.

The project has two user-facing entry points:

- a PyQt6 desktop GUI;
- a standalone CLI executable.

Both use the same CNC kernel and the same resolved `ExecutionResult`. The GUI is not a second interpreter, and the CLI does not contain a simplified parser of its own.

### What is the authoritative data flow?

The core data flow is:

```text
G-code source
    |
    `--> Parser / controller frontend
           |- native Cython parser
           `- per-block Python fallback where required
                |
                v
             Program / AST
                |
                v
          Program tool setup
          (AST operation hints, library lookup, manual overrides)
                |- source comments / dimensions: Cython scanner
                `- Python scanner fallback
                |
                v
          CNC execution kernel
          (flow, cycles, compensation, geometry)
                |
                v
           ExecutionResult
                |
                +--> GUI rendering / playback
                +--> statistics
                +--> batch / CLI trace
                `--> NC / DXF export
```

`ExecutionResult` contains the resolved logical motion trace plus diagnostics, execution steps, signals, structural events, WCS state and execution completeness.

### Is the OpenGL plot the CNC model?

No. Rendering consumes the resolved trace produced by the kernel. The renderer does not independently reinterpret G-code.

This separation is intentional: the same resolved geometry is used by playback, statistics, export and analysis.

### Is the program a machine simulator?

No. Easy G-Code Plot models supported FANUC turning/milling, SINUMERIK 840D milling/native XZ turning and HEIDENHAIN iTNC 530 Klartext milling program semantics and toolpath geometry, including the supported native SINUMERIK CAM 3+2/five-axis subset. It does not model a complete physical CNC machine, servo dynamics, acceleration, spindle inertia, fixtures, machine envelopes or all controller parameters.

A clean result means the modeled program was executed without a known error inside the supported contract. It is not a substitute for machine verification.

### Can I visualize SINUMERIK CAM five-axis programs?

Yes, within the supported native milling subset. `CYCLE800` resolves supported static working frames and 3+2 indexing, while `TRAORI` / `TRAFOOF` resolves supported continuous TCP motion on **5Ax Table AC Angled** and **5Ax Table BC Angled**. Configured rotary axes, XYZ geometry and resolved tool orientations reach the same GUI, CLI and trace consumers.

Select Milling mode, open the native program as `.mpf` / `.spf`, and choose the matching rotary profile. The bundled `5ax_test.mpf` and `impeller.mpf` CAM examples are covered by execution tests through program completion.

Read diagnostics when checking the plot: some native commands are accepted with `UNMODELED_SINUMERIK_NATIVE` warnings and their effects are not modeled, so completion through `M30` alone does not establish verified geometry. Exact cycle/frame/TCP limits are listed under [SINUMERIK 840D input](#sinumerik-840d-input). EXPANDED export has its own limits. Supported G68.2/G53.1 and CYCLE800 indexed AC/BC frames can be converted experimentally through the bundled multiaxis posts; other frame combinations remain rejected.

### What does deterministic mean in this project?

For supported input, execution is intended to produce the same logical trace and diagnostics from the same source and configuration. The kernel avoids guessing controller-dependent behavior when the required semantics are not known.

Where the program cannot be resolved safely, the preferred behavior is an explicit diagnostic or incomplete result rather than invented geometry.

---

## Getting started

### How do I install it?

Release builds provide separate GUI and CLI executables for Windows and a Linux x64 archive containing both executables. A Python installation is not required for packaged builds.

For a source checkout, the project requires Python 3.13+, `uv` and a compiler for the native extensions.

```bash
git clone https://github.com/MaestroFusion360/easy_gcode_plot.git
cd easy_gcode_plot
uv sync --no-dev
uv run --no-dev python main.py
```

### What is the normal GUI workflow?

1. Open or drag a CNC program into the application.
2. Select **Lathe Mode** for turning or leave it disabled for milling.
3. Configure WCS, home and tools when the program requires them.
4. Refresh the execution result.
5. Inspect the trajectory, playback, diagnostics and statistics.
6. Export FULL, EXPANDED or DXF when required.

Menu locations in 2.7.0:

| Command | Menu path |
| --- | --- |
| Application options | Settings → Options |
| Stock, WCS and saved tools | Settings → Stock / WCS / Tool Library |
| STL object panel | View → STL Objects |
| Compare and execution reports | CNC Functions → Compare / Statistics / Tool List / Tokens/Variables |
| Measurements and generators | CNC Functions → Measure / Hole Calculator / Pocket Calculator |
| Document closing | File → Close / Close All |
| Toolbar button selection | Right-click a toolbar → Customize Toolbars |

### How do I work with multiple documents?

The application starts with **one empty milling document**, even if the previous session used Lathe Mode. Use **+** or **File → New** to create another document. **Open**, recent files and drag-and-drop open CNC programs without replacing a nonempty active document. Opening an ordinary CNC file into an empty, unmodified unnamed buffer fills that buffer and keeps its selected machine mode. HEIDENHAIN `.h`/`.H` files are an exception: they always select native Klartext and milling, even when the empty buffer was in Lathe Mode. SINUMERIK `.mpf/.spf` with unambiguous native turning signatures also select turning automatically. Opening a file that is already open selects its existing document.

Use the **document-list arrow** at the upper right of the menu bar to select an open document. The check mark identifies the active document; `*` marks unsaved text. **Save**, **Save As**, editor commands, export and calculation operate on the active document. Save As cannot overwrite a file that is open in another document. Open documents are retained in memory for the current session; the next launch starts with one empty document rather than restoring the list.

Save As provides NC, SINUMERIK `.mpf/.spf` and HEIDENHAIN `.h/.H` filters. Existing native filenames select their filter; an extensionless name receives `.mpf` or `.h` for the selected native group. Save/Save As writes source text without controller conversion.

### Which settings are per document and which are shared?

Each document keeps its text, undo/redo history, caret, selection, scroll position, file path and detected encoding. Its machine mode, source dialect/comment and arc overrides, current-program tool assignments, execution result, view direction and playback position are restored when selected. Stock dimensions and manual/automatic choices, STL objects, section and STL undo/redo history also belong to that document. A new document uses the active document's machine mode, with an empty scene and fresh program-tool assignments. STL edits are session state; saving the CNC source does not embed its STL scene.

**Options**, interface language/theme, editor appearance, shortcuts, toolbar layout, playback speed, export preferences, saved tool libraries, **WCS/Home offsets** and the selected rotary profile are shared application settings. If shared CNC inputs or arc-sampling settings change, an inactive document's old cached result becomes **STALE** when selected. Auto Update recalculates it when enabled; otherwise use **Refresh** before relying on its trajectory or exporting it. Switching documents does not undo shared preference changes.

### What happens to dialogs and playback when I switch documents?

Finish or cancel an open **Export**, **Renumber**, **WCS**, **Options**, **Stock**, **Tool Library**, **Hole/Pocket Calculator** or **Snippets** dialog before creating, switching or closing documents. This prevents pending edits from being applied to a different CNC program. Find/Replace continues to act on the active editor. The visible Tokens/Variables inspector refreshes for the selected document; the previous Statistics report is hidden, and Statistics can be opened again for the active program.

Switching pauses playback, removes the previous stock simulation and restores the selected document's saved playback position and scene. Start Play again to rebuild stock removal for that document. Switching/closing is blocked during CNC calculation or stock export, and waits for cancelled stock-preparation workers to stop.

### How do Close and Close All handle unsaved changes?

Use the **×** control, **File → Close**, or the default **Ctrl+W** shortcut to close the active document. **Close All** and closing the application check each modified document for Save, Discard or Cancel. Cancel or a failed/cancelled save stops closing and keeps the unsaved document open; documents already closed by Close All remain closed. Closing the last document leaves one empty milling editor. Opening or creating another document does not discard unsaved text. Close and Close All are available in the configurable hotkeys list.

### How do I compare programs?

Choose **CNC Functions → Compare** or its toolbar button. Select open documents (including unsaved buffers) or browse for external files independently on either side. The read-only panes align matching lines: yellow marks changes, green additions and red deletions. Vertical and horizontal scrolling are synchronized. **Refresh** rereads selected disk sources and current MDI buffers without replacing editor documents; a read error keeps the previous comparison. Copying is available, but editing, merging and saving/printing diff reports are not. This is a text comparison, not a comparison of CNC semantics or trajectories.

### What does the iTNC-code source type do?

The toolbar source chooser and **Settings → Options → General → Default file type** offer Text, ISO G-code and **iTNC-code**. The default persists across restarts. iTNC-code highlights native Klartext motions and comments. Opening `.h`/`.H` selects the HEIDENHAIN source dialect and milling mode automatically; unnamed text is recognized by `BEGIN PGM ... MM/INCH`. The native AST and milling runtime execute straight and circular motion, polar/helical `LP/CP`, `CC/C/CR/CT`, `APPR/DEP` transitions, `TOOL CALL`, feeds, spindle controls, `M91`, Q parameters, label flow and drilling/boring/tapping cycles 1/2 and 200–209/240/241, position patterns 220/221, pocket cycles 251/252 and thread milling 262 within the limits described below. Cycle 32 retains metadata without simulating controller smoothing. `RND`/`CHF` construct planar rounding/chamfers before existing RL/RR compensation, with block-local feeds. Rotary indexing, PLANE and AC/BC table TCP use configured kinematics; tool offsets DL/DR, auxiliary axes and `M120` remain unsupported. Unsupported execution stops with a source diagnostic. See [HEIDENHAIN iTNC 530 input and execution coverage](#heidenhain-itnc-530-input) below.

### Which input encodings are supported?

The normal document encodings are UTF-8 and Windows-1251. The GUI opens `.ptp` files by default and tries Windows-1251 if UTF-8 decoding fails; saving preserves the detected encoding. The CLI exposes the supported encodings through `--encoding`.

### Are compact FANUC blocks accepted?

Yes. Words do not need spaces. Blocks such as:

```text
G18G21G40G54G80G99
G0X100Z5
```

are parsed as address words rather than relying on whitespace splitting.

### Which comment forms are understood?

Both common forms are recognized:

```text
(COMMENT)
; COMMENT
```

A persistent comment-style option controls generated text exports. Reading source programs is not limited to the selected output style.

Native iTNC uses `;` comments. With an iTNC document active, Options locks comment style to semicolons and disables ISO arc autodetection; ISO preferences are preserved. Changing the default file type affects new documents, while applying Options preserves the current editor mode. In Colors, Rapid move, Linear move and Circular move describe motion types for all controllers.

### How do optional `/` Block Skip lines work?

A source block beginning with `/` is marked as optional.

With **Ignore Block Skip** enabled, the complete block is excluded from execution, including:

- motion;
- Macro B assignments;
- signals;
- subprogram or macro calls.

With the option disabled, it executes normally.

---

## Diagnostics and fail-closed behavior

### What are `ok` and `complete`?

`ExecutionResult.ok` describes whether execution avoided a fatal modeled error. `ExecutionResult.complete` indicates whether the kernel considers the resulting execution trace complete enough for consumers such as export.

A program can therefore retain trustworthy motions before an unsupported or invalid block while still being marked incomplete.

### What diagnostic information is stored?

A diagnostic can contain:

- a stable code such as `UNSUPPORTED_G_CODE` or `UNDEFINED_MACRO`;
- a human-readable message;
- severity;
- status such as verified, unverified, unsupported, malformed or resource-limited;
- source line;
- offending raw block.

### What happens after unsupported position-changing semantics?

The kernel does not assume that the old position remains trustworthy. For turning, an unsupported position-changing command can create an unknown-axis gap. Trace publication resumes only after later absolute coordinates establish a known position again.

This prevents a misleading connector line from being drawn through an unknown region.

### How are unsupported turning G-codes classified?

An unsupported G-code that can affect geometry is treated more seriously than a non-geometric control code. For example, an unsupported code on a block containing X/Z/U/W can make the block unsupported rather than merely unverified.

Y-axis motion is not modeled in `fanuc_turn` and produces `UNSUPPORTED_AXIS`.

### What about unsupported M-codes?

The core tracks modeled program-control and machine signals. Unmodeled auxiliary M codes produce non-blocking `UNSUPPORTED_M_CODE` warnings in FANUC milling/turning and SINUMERIK native/ISO milling, including mixed motion blocks. SINUMERIK native/ISO-T turning instead rejects unmodeled M functions with an unsupported diagnostic. This rule applies to GUI execution and CLI/batch analysis. M2/M30 end programs. FANUC M98/M99 retain modeled call/return behavior; native SINUMERIK milling M17/M96/M97/M99 stop with unsupported-flow diagnostics. Native milling M66/M98 produce auxiliary warnings; M98 does not call a FANUC subprogram.

### Are conflicting modal codes detected?

Yes. Supported modal groups are checked for conflicts within one block. A conflict such as two mutually exclusive motion, plane, unit, compensation, feed, spindle or transform modes produces `MODAL_GROUP_CONFLICT` and the block is not silently interpreted using source-order luck.

### Are there execution resource limits?

Yes. The default execution budget protects against runaway macros, recursive calls and pathological cycles:

| Resource | GUI default |
| --- | ---: |
| Executed blocks | 500,000 |
| Subprogram/macro calls | 10,000 |
| Generated motions | 2,147,483,647 |
| Auto update max segments | 2,147,483,647 |
| Cycle iterations | 100,000 |
| Macro loop iterations | 100,000 |
| General call depth | 64 |

The kernel, GUI, CLI and batch execution share these default execution budgets. GUI segment limits apply to rendering, and explicitly configured execution limits still take precedence.

Cancellation is checked through the same budget mechanism. Resource exhaustion produces a structured `RESOURCE_LIMIT`-style result instead of an unbounded run.

---

## FANUC Macro B and program flow

### How complete is Macro B support?

Macro B is part of the execution runtime, not a text substitution preprocessor. Expressions are evaluated while the program executes, so loops, branches, subprogram calls and variable state affect the real logical motion trace.

The same Macro B runtime is used by turning and milling.

### Which variable forms are supported?

Numeric variables:

```text
#1
#100
#500
#13001
```

Named variables:

```text
#<NAME>
#<TOOL_RADIUS>
```

Indirect references:

```text
#[#1]
#[100+#2]
#[FUP[#[ROUND[#3]]]]
```

Indirect assignment is also supported:

```text
#1=100
#[#1]=5
#[#1+1]=#100+2
```

The indirect destination must resolve to an integer variable number.

### What is special about `#0`?

`#0` is permanently vacant.

It cannot be assigned:

```text
#0=123
```

produces `INVALID_MACRO_ASSIGNMENT`.

Vacant values are distinct from numeric zero for equality tests:

```text
IF[#1 EQ #0] GOTO10
```

is the normal way to detect an omitted/vacant local argument.

In arithmetic, a vacant value behaves as numeric zero. Assigning a vacant value clears the destination variable:

```text
#100=#0
```

After that assignment, `#100` is vacant rather than stored as numeric `0`.

### What happens when an undefined variable is used numerically?

A normal numeric reference to an undefined variable fails closed with `UNDEFINED_MACRO`.

The special null-aware comparison behavior is used where FANUC vacant semantics are required, such as comparisons to `#0`.

### Which arithmetic and relational operators are supported?

The expression evaluator supports ordinary arithmetic and FANUC-style relational/logical tokens used by the project fixtures, including:

```text
+  -  *  /
MOD
EQ  NE  GT  GE  LT  LE
AND  OR  XOR
```

Brackets may be nested:

```text
X[#100+5]
#10=[[#1+#2]*#3]
```

Compact expressions such as `#1LT#3` are accepted. AND/OR/XOR convert operands to integers and apply bitwise arithmetic; they do not use Python truthiness. Comparisons return numeric 0/1.

The evaluator rejects exponentiation (`**`), strings, bytes, containers and boolean constants. Limits are 4,096 source characters, 512 AST nodes and depth 64; expression arithmetic uses finite floating-point constants. LN requires a positive argument; EXP overflow produces an execution diagnostic. BIN/BCD/ADP remain explicitly unsupported because their controller-specific semantics were not verified against local references.

### Which Macro B functions are implemented?

The current evaluator includes:

```text
ABS
SQRT
SIN
COS
TAN
ATAN
FIX
FUP
ROUND
MIN
MAX
LN
EXP
```

Trigonometric arguments and results follow FANUC-style degree semantics.

Two-argument FANUC arctangent syntax is supported:

```text
ATAN[y]/[x]
```

For example:

```text
#119=ATAN[0.75]/[1.625]
```

`ROUND` uses FANUC-style nearest-integer rounding with `.5` away from zero.

### Are assignments supported on labeled blocks?

Yes. An `N` block label may precede a Macro B flow statement or assignment:

```text
N900 #151=7
```

Labels are indexed once for flow execution.

### Is unconditional `GOTO` supported?

Yes:

```text
GOTO100
...
N100 ...
```

A missing target produces `FLOW_TARGET_MISSING`.

### Is `IF [...] GOTO` supported?

Yes:

```text
IF[#1 EQ 2] GOTO900
IF[[#2*#11] GT 360] GOTO16
```

Conditions are evaluated at runtime using the current variable state.

### Are `WHILE / DO / END` loops supported?

Yes:

```text
#1=0
WHILE[#1 LT 3] DO1
#1=#1+1
G1 X#1 F100
END1
```

Nested loop IDs are indexed before execution. Missing `END`, unmatched `END`, runaway loops or an exhausted macro-iteration budget produce diagnostics rather than hanging the application.

### Are real Macro B milling programs exercised by the tests?

Yes. The regression corpus includes Macro B programs that generate:

- repeated boss milling;
- face milling;
- hole milling;
- thread milling;
- nested loops;
- large deterministic arc counts;
- indirect variable access.

These execute through the normal milling kernel rather than a separate test interpreter.

### Is `G65` supported?

Yes. `G65 P...` calls an `O` macro program and creates a proper macro-local scope.

Example:

```text
G65 P7700 X0 Y0 M48 S5. D1 R50. Z-70. Q4. V8. I860. A7.5 B15. H24. K1. E100. F200.
```

The called macro can then use the mapped local variables `#1..#33`.

### How are G65 Type I arguments mapped?

The current Type I mapping is:

| Address | Local variable |
| --- | ---: |
| A | #1 |
| B | #2 |
| C | #3 |
| I | #4 on first occurrence |
| J | #5 on first occurrence |
| K | #6 on first occurrence |
| D | #7 |
| E | #8 |
| F | #9 |
| H | #11 |
| M | #13 |
| Q | #17 |
| R | #18 |
| S | #19 |
| T | #20 |
| U | #21 |
| V | #22 |
| W | #23 |
| X | #24 |
| Y | #25 |
| Z | #26 |

`G`, `L`, `N`, `O` and `P` are control words and are not bound as ordinary local arguments.

### How are repeated I/J/K G65 arguments handled?

Repeated I/J/K words use FANUC Type II-style sequential local slots. Each occurrence advances by three:

```text
I -> #4,  #7,  #10, ...
J -> #5,  #8,  #11, ...
K -> #6,  #9,  #12, ...
```

Up to 10 occurrences of each I/J/K address are accepted in one G65 call.

### Do G65 argument words also perform machine actions?

No. On a G65 call, words such as `M`, `S`, `T`, `X`, `Y`, `Z` and `F` are macro arguments, not simultaneous spindle, tool, motion or feed commands.

For example, `T7` or `M8` inside a G65 argument list does not create a tool-change or coolant signal.

### What happens to `#1..#33` when a G65 macro returns?

Local variables are scoped.

On macro entry, the caller's local variables are saved and replaced by the call arguments. On `M99`, the caller's local values are restored. Common and named variables remain shared.

The Variables inspector reflects the active local scope while playback is inside the macro and shows the restored caller values after return.

### What does `G65 ... L...` do?

`L` repeats the macro call. The accepted range is `1..9999`.

Each repetition starts again with the original G65 local arguments. Changes made by the previous repetition to `#1..#33` do not leak into the next repetition.

### How deeply can G65 macros nest?

The current implementation allows four nested G65 local-variable levels. A deeper macro nesting request produces `CALL_DEPTH_EXCEEDED` rather than silently sharing a damaged local scope.

The wider M98/G65 call-stack budget is separately limited by the general call-depth setting.

### How does M98 behave inside a G65 macro?

An M98 subprogram call inside a G65 macro shares the current macro-local level. It does not create another G65 local scope by itself.

### Are M98/M99 subprograms supported outside Macro B?

Yes.

Typical form:

```text
M98 P2000
M98 P2000 L3
...
O2000
...
M99
```

`P` must identify an existing positive integer O-program number. `L` must be a positive integer. Missing targets and invalid values produce structured subprogram diagnostics.

### Is `M99 P...` supported?

No. `M99 P` is controller-profile dependent and currently produces `UNSUPPORTED_M99_P` rather than guessing its jump semantics.

### Are Macro B variable values stored per execution step?

Yes. `ExecutionStep.variables` contains an immutable snapshot of the variable state for that occurrence of a source block. Unchanged snapshots are internally reused rather than copied for every motion.

This is what allows the GUI Variables inspector to follow logical playback without re-running the CNC program.

### Does Expanded Execution export keep Macro B statements?

Expanded Execution follows the actual executed occurrence order. Macro flow and G65 calls are resolved into their resulting execution rather than exported as a second unevaluated macro program.

Subprogram/macro boundaries are preserved as execution events/comments where appropriate, while generated motion comes from the authoritative trace.

---

## FANUC turning

The turning interpreter supports FANUC Type A (default) and Type B. Select Type B in **Settings → Options → General → Source lathe G-code system**, or pass `--lathe-gcode-system B` to a CLI command. Type B uses G90/G91 for absolute/incremental X/Z, G33 for threading, G77/G78/G79 for simple cycles, and G94/G95 for feed per minute/revolution. Type C, G66/G67 modal macro calls and G68.2/G53.1 indexed-plane operations are outside the current turning language.

### Main differences between Type A and Type B

| Operation | Type A | Type B |
| --- | --- | --- |
| Rapid | G00 | G00 |
| Linear | G01 | G01 |
| Arc CW | G02 | G02 |
| Arc CCW | G03 | G03 |
| Dwell | G04 | G04 |
| Thread cutting | G32 | G33 |
| Coordinate system / spindle clamp | G50 | G92 |
| Finish cycle | G70 | G70 |
| Rough turning | G71 | G71 |
| Rough facing | G72 | G72 |
| Pattern repeating | G73 | G73 |
| Face peck drilling | G74 | G74 |
| OD/ID grooving | G75 | G75 |
| Multiple threading | G76 | G76 |
| Turning canned cycle | G90 | G77 |
| Threading canned cycle | G92 | G78 |
| Facing canned cycle | G94 | G79 |
| Feed per minute | G98 | G94 |
| Feed per revolution | G99 | G95 |

Type A uses absolute X/Z and incremental U/W. Type B uses G90/G91 to switch X/Z between absolute and incremental; U/W remain incremental.

### What is the turning coordinate model?

Turning uses X/Z geometry. Internally, physical X geometry is radial, while programmed X can follow diameter or radius programming.

The default turning state is diameter programming.

### How do X/U and Z/W behave?

- `X` and `Z` are absolute-axis words where the active mode requires absolute programming.
- `U` and `W` are incremental turning-axis words.
- X/U conversion respects diameter versus radius mode.

Cycle expansion uses the same conversion helpers rather than treating cycle X values differently from ordinary motion.

### How are G20 and G21 handled?

The kernel normalizes physical geometry to millimetres internally.

- `G20` sets inch input scaling;
- `G21` sets millimetre input scaling.

The selected unit mode is captured per execution step so playback, statistics and export can reconstruct the executed unit context.

### Which turning arc formats are supported?

Turning uses G18 XZ circular interpolation with:

- relative or absolute I/K center coordinates, selected by Arc Type or auto detection;
- R radius programming.

Resolved arcs store analytical center, radius, sweep and direction in physical geometry.

R-programmed profile arcs remain R arcs during G71/G72/G73 roughing and G70 finishing, regardless of the selected I/K interpretation. If an I/K arc in a P/Q profile is invalid in the manually selected mode, the associated cycle emits no partial trajectory and reports the source line.

### Why can G2/G3 direction look inverted in an XZ plot?

The physical G18 orientation and the visual X/Z plot orientation are not the same coordinate view. The kernel resolves the physical arc direction and the plotting layer uses the correct XZ convention rather than treating it as XY geometry.

### Is direct A-angle turning programming supported?

Yes. On ordinary G1 turning blocks, A-angle programming can resolve a missing X or Z endpoint using the previous contour direction and programmed angle.

### Are C chamfers and corner R fillets supported?

Yes. Ordinary G1 contour blocks can include:

- `C` corner chamfers;
- corner `R` fillets.

This is distinct from `G2/G3 R`, where R is the circular interpolation radius.

### Are G32 and G33 threading motions supported?

Yes. G32/G33 are represented as synchronized threading motions in the resolved trace. Threading state is preserved into export and Stock Removal where applicable.

### What are the turning feed modes?

For turning:

```text
G98 -> feed per minute
G99 -> feed per revolution
```

The default turning feed mode is per revolution.

Per-revolution machining time is only known when a trustworthy spindle speed is also available. Otherwise statistics report unknown time rather than inventing a feed rate.

### Are G96 and G97 modeled?

Yes.

```text
G96 -> constant surface speed (CSS)
G97 -> direct RPM mode
```

In CSS mode, the S value is stored as surface speed. In inch mode the source surface-speed value is converted to metres per minute internally.

### What does G50 S do in turning?

`G50 S...` is tracked as the spindle-speed limit used with the turning spindle model. It is not treated as the milling G50 scaling cancel operation.

### Are spindle start/stop signals tracked?

Yes. M3/M4 mark the spindle running and M5 marks it stopped. Machine signals such as spindle, coolant, dwell and program end are also published in `ExecutionResult.signals`.

### Which WCS features work in turning?

The kernel supports:

- `G54-G59`;
- `G54.1 P1-P99` extended offsets;
- `G10 L2` programming of G54-G59;
- `G10 L20` programming of G54.1 offsets.

Runtime G10 changes are returned in the execution result and do not silently write application settings.

### Is G53 supported in turning?

Yes, for non-modal machine-coordinate G0/G1 motion.

A turning `G53 G2/G3` cannot be modeled by the current contract and produces `UNSUPPORTED_G53_MOTION` instead of being executed as a WCS-relative arc.

### How does G28 work?

When configured reference-return emulation is enabled, G28 resolves the intermediate programmed point and then emits the configured machine-home motion. Reference-return events are also recorded structurally.

### Is G30 the same as G28?

No. The project does not silently reuse the configured G28 home as a second reference point for G30. A controller-specific G30 reference must not be invented from G28 configuration.

### How does tool-nose compensation work?

G40/G41/G42 state is tracked in turning. When a valid configured turning tool with usable nose geometry is available, the resolved trace can be compensated deterministically.

Tool geometry alone does not activate compensation. G71/G72/G73 profiles use nose compensation only when G41/G42 is explicitly active, including commands within the P-Q contour. Without G41/G42, changing the configured nose radius leaves the programmed trajectory unchanged; the cycle's U/W finishing allowances still apply.

The compensation layer works from executed motions and tool geometry rather than rewriting source text.

If the required geometry cannot be established safely, the result is not presented as verified compensated motion.

---

## Turning cycles

### Which turning cycles are modeled?

The current turning cycle layer includes:

| Type A | Type B | Purpose in the kernel |
| --- | --- | --- |
| G70 | G70 | P-Q finishing contour |
| G71 | G71 | Longitudinal roughing |
| G72 | G72 | Facing roughing |
| G73 | G73 | Pattern-repeat roughing |
| G74 | G74 | Z peck / face grooving |
| G75 | G75 | X peck / radial grooving |
| G76 | G76 | Two-line multipass threading |
| G83 | G83 | Axial peck drilling |
| G84 | G84 | Axial tapping |
| G90 | G77 | Modal longitudinal turning cycle |
| G92 | G78 | Modal threading cycle |
| G94 | G79 | Modal facing cycle |

Cycle geometry is expanded into ordinary logical motions. Those motions are then consumed by playback, statistics, Stock Removal and export.

### Do cycle motions remember where they came from?

Yes. Generated motions are marked as cycle-generated and retain source ownership such as the invoking block, source text and playback group where applicable.

This is why one source cycle block can own many logical playback motions without losing editor navigation.

### How are cycle profiles selected by P and Q?

P/Q contour cycles resolve N labels in the parsed program. The resolver handles repeated labels relative to the cycle call site rather than assuming every N label is globally unique.

For finishing, a preceding P-Q profile can be preferred where appropriate.

### Do G71/G72/G73 profile blocks support lines and arcs?

Yes. The P-Q contour is built as profile segments and can include supported linear and circular geometry. Analytical arc data is preserved where possible rather than converting every profile arc into a staircase.

### How does G70 work?

`G70 P... Q...` builds the referenced finish contour and approaches it from the actual G70 call position.

The finish path is based on the nominal P-Q profile, not the roughing-offset profile used by G71/G72/G73.

If tool-nose compensation is active and can be verified, the finishing contour uses the compensated profile.

After the finish group, the cycle returns to the saved call position using the project's deterministic turning return order.

### What form of G71 is supported?

The common two-line FANUC form is modeled:

```text
G71 U... R...
G71 P... Q... U... W... F...
```

The first line captures rough depth and retract. The second line supplies the P-Q profile, finishing allowances and feed.

### How is G71 depth interpreted?

The first-line U depth is treated as a radial depth and converted consistently into programmed diameter motion when diameter programming is active.

An empty P-Q profile or zero first-line depth produces an explicit G71 diagnostic; no partial cycle trajectory is published.

### How are G71 U/W finish allowances handled?

The second-line U and W are applied to the roughing profile before rough passes are generated.

U is signed. This matters for OD versus ID work:

- positive U leaves outside material on an OD contour;
- negative U can leave material toward the bore interior on an ID contour.

The sign is not discarded by taking an unconditional absolute value.

### How does G71 distinguish OD and ID roughing?

The cycle compares the stock-side approach and profile geometry and selects boring versus outside behavior. The same P-Q contour engine is used, but pass direction and retract direction follow the selected material side.

### What is G71 Type I behavior?

Type I is treated as monotonic longitudinal roughing. Each rough pass is parallel to Z and terminates at the P-Q roughing profile.

After the roughing passes, the implementation adds one complete pass along the already allowance-offset roughing profile. It does not incorrectly reuse the nominal finishing contour at this stage.

### Is G71 Type II supported?

A Type II profile is detected when the first P block contains both an X/U component and a Z/W component.

The implementation can follow non-monotonic/pocketed profile geometry using clipped profile segments. Controller-dependent cases are handled conservatively; unsupported geometry is not silently simplified.

### How does G72 work?

G72 uses the same P-Q profile infrastructure as G71 but performs facing roughing in Z planes.

Typical two-line form:

```text
G72 W... R...
G72 P... Q... U... W... F...
```

The first line captures axial depth and retract. The second line references the profile and finishing allowances.

### Is G72 Type II fully generic?

No. Type II is supported where the facing plane resolves to a deterministic profile span. If one facing plane produces multiple disjoint material spans that require controller-specific interpretation, execution fails explicitly with:

```text
UNSUPPORTED_G72_TYPE_II_SPANS
```

instead of choosing an arbitrary span.

An empty profile, zero pass depth, or a lone interior crossing after a closed Type II span also produces an explicit diagnostic. No cuttable Type II facing span is reported as an error rather than an empty expansion.

Repeated intersections at the same endpoint of a closed contour count as one crossing. Distinct, disjoint spans still produce `UNSUPPORTED_G72_TYPE_II_SPANS`.

### How does G73 work?

G73 is implemented as repeated shifted copies of the roughing profile.

The first line captures the total U/W pattern displacement and the R pass count. The second line provides P/Q, finish allowances and feed.

The signs of programmed U/W are preserved. The cycle does not infer displacement direction from where the tool happened to approach the contour.

### How does G74 work?

G74 supports Z-direction peck behavior and face-grooving style repetition.

A first block containing R alone can establish the retract distance. The executing block can use X/U and Z/W plus P/Q/R/F parameters.

If no X target is supplied, G74 can operate as a drilling-style Z peck at the current X.

When X repetition is requested, P controls the X step and Q controls Z peck depth. The cycle returns to its saved start using an explicit Z-first return order.

### How does G75 work?

G75 performs X-direction peck/radial grooving.

P controls the radial peck step. Q can repeat grooves along Z. If Q is omitted, a programmed Z/W selects one groove location rather than being treated as an invalid zero-step repetition.

The R value from the setup block controls retract distance, and the executing-block R value is handled as the bottom allowance where applicable.

### How is turning peck motion represented?

The kernel emits actual feed and rapid primitives for each peck/retract sequence. It does not store G74/G75 as an opaque cycle that the renderer has to understand separately.

### How does two-line G76 work?

The modeled form is FANUC-style two-line G76:

```text
G76 P...... Q... R...
G76 X... Z... P... Q... R... F...
```

The first block stores:

- packed P control digits;
- minimum radial increment Q;
- optional finish allowance R.

The second block supplies:

- final thread X;
- final Z;
- thread height P;
- first cut Q;
- optional taper R;
- lead F.

### How are G76 P/Q integer increments interpreted?

The first-block Q and second-block P/Q are treated as integer least-input increments rather than ordinary floating length words.

For metric turning they are converted in thousandths of a millimetre. Inch mode uses the corresponding 0.0001-inch increment converted to physical millimetres.

### How is G76 pass depth generated?

The thread passes use a decreasing-depth / approximately constant-chip-area progression based on the first-cut depth and square-root pass relationship, while respecting the minimum radial increment and finish allowance.

The final commanded X is authoritative for the final thread diameter.

### What do the packed G76 P digits mean here?

The packed first-line P is decoded as:

```text
P(m)(r)(a)
```

where the fields represent:

- final/spring-pass count;
- chamfer amount in tenths of pitch;
- tool/thread angle.

### Which G76 tool angles are modeled?

The supported set is:

```text
0, 29, 30, 55, 60, 80 degrees
```

Other packed angles fail explicitly with:

```text
UNSUPPORTED_G76_TOOL_ANGLE
```

For supported nonzero angles, pass start/end Z is shifted to model FANUC-style single-edge flank infeed rather than ignoring the angle digits.

### How is G76 chamfer modeled?

The packed chamfer digits mark an axial interval based on thread lead. The current model splits the final part of the pass into collinear segments; it does not simulate an angled radial pull-out or the resulting physical chamfer. The controller's pull-out angle is not configured, and the tool angle in P is not a substitute for it. No universal 45-degree exit is assumed.

### Is G92 a modal threading cycle?

Yes.

Example:

```text
G92 X18 Z-10 F1.5
X17.5
X17.0
```

The initial G92 establishes the thread end and lead. Subsequent X/U-only blocks continue the active G92 cycle with new depths until another explicit motion/cycle mode cancels it.

Each pass expands to approach, synchronized longitudinal cutting, retract and return primitives.

### Is G90 a modal turning cycle?

Yes. G90 establishes a longitudinal rectangular turning cycle. Subsequent X/U-only blocks can continue the active cycle at new diameters until cancellation by another explicit motion/cycle code.

### Is G94 a modal facing cycle?

Yes. G94 establishes a facing rectangular cycle. Subsequent Z/W-only blocks can continue the active cycle at new face positions until cancellation.

### What cancels G90/G92/G94?

A non-motion modal code such as G96/G97 does not cancel the active cycle.

Another explicit motion or cycle code cancels the old modal turning cycle unless that same cycle is explicitly present in the block.

### Are turning G83 and G84 modal?

Yes. G83 and G84 remain active for subsequent eligible coordinate blocks until G80, another cycle state, or a tool change cancels them.

### How does turning G83 behave?

G83 is an axial Z drilling cycle.

- If Q is supplied, Z pecks are generated.
- If Q is absent, the kernel does not invent peck depth; it emits one feed stroke to depth and a rapid return.
- Optional X positioning is handled before the axial stroke and restored afterward.

### How does turning G84 behave?

G84 is an axial tapping cycle. The downstroke and return are synchronized feed motions; the return is not represented as a rapid move.

### Does P dwell in turning G83/G84 create geometry?

No. Dwell is a time/control event, not a spatial segment. The backplot geometry therefore does not invent a motion for the dwell itself.

### What happens if a modal drilling/tapping cycle is left in an invalid state?

The runtime can report an `UNCLOSED_CYCLE`-class execution error rather than silently carrying an impossible modal cycle to program end.

---

## FANUC milling

### Which milling G functions are recognized?

This table lists the G codes recognized by the `fanuc_mill` kernel. Details and limits are explained below.

| G code | Function in the kernel |
| --- | --- |
| G00 | Rapid positioning |
| G01 | Linear interpolation |
| G02 / G03 | Clockwise / counterclockwise circular interpolation |
| G04 | Dwell signal; no spatial motion |
| G10 | Program WCS offsets (`L2`, `L20`) |
| G15 / G16 | Cancel / enable polar coordinate programming |
| G17 / G18 / G19 | Select XY / XZ / YZ plane |
| G20 / G21 | Inch / millimetre input units |
| G28 | Reference return using the configured home |
| G40 / G41 / G42 | Cancel / left / right cutter-radius compensation |
| G43 / G49 | Track / cancel tool-length state; G43 does not apply H geometry to the plotted path |
| G43.4 | TCP G0/G1/G2/G3 motion for the angled AC/BC table profiles, including Cartesian arcs with rotary interpolation; combination with G68.2 is unsupported |
| G50 / G51 | Cancel / enable coordinate scaling |
| G52 | Local coordinate shift |
| G53 | Non-modal machine-coordinate motion |
| G54–G59 | Select work coordinate system |
| G54.1 P1–P99 | Parsed and selected; the GUI has no offset setting, so the offset is zero unless the program sets it with G10 L20 |
| G65 | Call a Macro B program |
| G68 / G69 | Enable / cancel coordinate rotation |
| G68.2 / G53.1 | Tilted working plane / tool-axis orientation (3+2, `fanuc_mill` with two-axis table-table, head-head or head-table kinematics) |
| G73 | High-speed peck drilling cycle |
| G80 | Cancel canned cycle |
| G81 | Drilling cycle |
| G82 | Drilling cycle with dwell |
| G83 | Full-retract peck drilling cycle |
| G84 | Tapping cycle |
| G85 | Boring cycle with feed return |
| G86 | Boring cycle with spindle-stop signal |
| G90 / G91 | Absolute / incremental programming |
| G93 | Inverse-time feed: each cutting block takes 1/F minutes; reprogram positive F when switching G93/G94/G95. Cycles and cutter compensation are unsupported in G93 |
| G94 / G95 | Feed per minute / feed per revolution |
| G98 / G99 | Return to initial / R plane in canned cycles |

### Which milling M functions are recognized?

| M code | Function in the kernel |
| --- | --- |
| M00 / M01 | Stop / optional-stop signal |
| M02 / M30 | End program |
| M03 / M04 / M05 | Spindle clockwise / counterclockwise / stop signals |
| M06 | Tool-change event for the selected T number |
| M07 | Recognized; no machine-specific coolant action is modeled |
| M08 / M09 | Coolant on / off signals |
| M19 | Spindle-orientation signal; S on this block is an angle, not spindle RPM |
| M29 | Prepare rigid tapping; S on this block sets spindle RPM for the following G84 |
| M98 / M99 | Call / return from subprogram |

Unknown auxiliary M codes produce `UNSUPPORTED_M_CODE` warnings and let execution continue in FANUC milling/turning and SINUMERIK native/ISO milling, including mixed motion blocks. SINUMERIK native/ISO-T turning instead rejects unmodeled M functions with an unsupported diagnostic. M0/M1 record machine-stop signals without stopping the trace; M2/M30 end programs; FANUC M98/M99 model call/return. Native SINUMERIK milling M17/M96/M97/M99 stop with unsupported-flow diagnostics, while native milling M66/M98 produce auxiliary warnings without subprogram dispatch. Recognized M codes describe trace signals and program flow; they do not simulate machine hardware.

`M29 S500` followed by `G84` marks rigid tapping in the trace. With `G95`, `F1.5` is 1.5 mm per revolution in metric mode; with `G94`, the equivalent feed at 500 RPM is `F750` mm/min. `G80` clears the rigid-tapping preparation. M29 syntax and whether it is required depend on the machine configuration. The kernel records synchronization semantics but does not simulate an encoder or spindle acceleration.

### What basic milling motion is modeled?

The milling kernel supports XYZ rapid, linear and circular/helical motion in the active G17/G18/G19 plane.

Resolved `TraceMotion` is full 3D geometry even though many CNC constructs are planar.

### How is indexed rotary milling handled?

If calculation stops because no rotary profile is selected or the selected profile lacks an axis, a persistent notice appears above the plot. It lists detected A/B/C motion addresses, including zero angles, and the stopping source line. **Choose kinematics...** opens the existing profile menu; **Go to line** moves the editor to that block. The failed result remains available after Auto Update even when it produced no motions. The notice follows the active MDI document and disappears after a successful calculation. Address detection excludes comments and G65 macro arguments; it does not infer table/head ownership, rotary order, signs or pivots, so a machine profile is not selected automatically.

Select a profile in **Settings → Rotary kinematics** or pass `--kinematics PROFILE_ID` with `--lang fanuc_mill` in the CLI. The GUI selection is stored as `CNC/ROTARY_KINEMATICS`. The profile maps programmed A/B/C addresses to signed rotary axes. G90 assigns an absolute rotary angle; G91 adds an increment. For the checked table profiles, later XYZ motions, resolved arcs and milling cycles are transformed into the fixed WCS display frame, and playback orients the tool preview at the resolved tool-tip point. WCS axes themselves do not rotate.

G28 reference return and non-modal G53 use machine-axis coordinates first, including repeated returns and G91 increments, then map their trace points into the indexed display frame. The active WCS remains selected after G53. An A/B index records an event and changes subsequent geometry; the kernel does not currently generate a sampled tool-tip sweep during the rotary movement. The plot omits a connector across that position change.

For the checked **4-axis Table C** profile, concurrent X/C feed blocks and C-only blocks map their endpoints into the fixed XY plane. Here X is the programmed radius and C is the angle about Z; the source program provides the contour sampling. These blocks record `ROTARY_MOTION` rather than an index event.

### Which rotary profiles have been checked?

The **4Ax Table A** and **4Ax Table B** profiles have been compared with the programs in `tests/fixtures/milling/fanuc/indexed_table_a.nc` and `tests/fixtures/milling/fanuc/indexed_table_b.nc`. The **4-axis Table C** profile is checked against `tests/fixtures/milling/fanuc/indexed_table_c.nc`: its X/C contour overlays the program's first XY contour within 0.05 mm at the sampled endpoints. The fixture files are reference inputs, not definitions of a machine. Automated checks also cover A/B angle signs, G90/G91, and repeated G28/G53 behavior.

The complete installed catalog of 24 configurations is available in **Settings → Options → Rotary Kinematics**. This includes Head A/B/C, orthogonal AC/BC, mixed table/head and angled profiles. **Enabled**, in the profile settings, controls whether a profile appears in **Settings → Rotary kinematics**. Built-in visibility preferences are stored separately in user settings; installed definitions and their historical `enabled` flags remain unchanged. Hidden profiles remain in Options so they can be enabled again. Visibility changes take effect with **OK** and are discarded by **Cancel**. Hiding the active profile clears the active selection and refreshes execution. All built-in profiles are initially visible; user copies retain their own enabled state.

Each rotary joint in a user profile has optional **Min (deg)** and **Max (deg)** travel limits. Enter both finite values with Min <= Max, or leave both blank for an unrestricted (continuous) axis. Installed profiles have no limits; create a copy to add them. An executed angle outside the inclusive range produces a **ROTARY_AXIS_LIMIT_EXCEEDED** warning in Tokens/Variables on the source line, without stopping execution or blocking export. Only changed axes are checked; angles are compared as executed, without wrapping. Limits do not change geometry or select a different TWP/TCP solution.

Only the five profiles **4Ax Table A**, **4Ax Table B**, **4-axis Table C**, **5Ax Table AC Angled** and **5Ax Table BC Angled** have the previously documented practical program verification. The other profiles and user copies are available but **unverified**; the Options status label makes this distinction. Synthetic checks of direction vectors and rotation order prove those parameters reach the kernel, not that an arbitrary NC program matches a physical machine. **None** remains the default active selection.

The Options tab displays built-in profiles read-only. **Create copy** creates a user profile whose name, enabled state, table/head ownership, addresses, direction vectors and rotation order can be edited. Axis 1 precedes Axis 2 within each branch. The sidebar and action icons match Postprocessors; Add asks for the new copy name, and Rename renames a user profile. **Save profile** stages the edit; **OK** writes user copies atomically to `rotary_profiles.json` beside `config.ini`, while **Cancel** discards pending edits and deletions. Editing a disabled copy keeps it disabled unless its checkbox is explicitly changed. Browsing, copying and saving do not activate a profile: use the existing Settings menu, which persists the selection and refreshes execution. User copies can be deleted; installed profiles cannot be edited or deleted.

A selected profile defines the table/head axis and sign explicitly; the software cannot infer those properties from an A, B or C word. Direction and order changes feed the existing rotation matrices used by trajectory and tool orientation calculations. TCP requires an A/B table tilt followed by a vertical C table spin; planar continuous-C requires a single vertical C table joint. Unsupported layouts retain indexed behavior and reject unsupported continuous/TCP commands. Execution steps retain the selected WCS and configured angles. G10 L2 and WCS changes preserve the current machine position after a table index. This remains Rotary Axis Kinematics with a stationary workpiece, without machine dimensions, pivots or physical machine simulation.

Old overrides of built-in IDs are loaded as separate user copies; saved GUI selections follow the migrated copy. Reading leaves the original file untouched. The first subsequent save preserves its exact original bytes in a neighboring `rotary_profiles.json.invalid-*.bak` file before writing the migrated user catalog. Malformed individual entries are logged and skipped independently, leaving the installed catalog and other valid copies available. Completely unreadable user files are logged and ignored by default in both GUI and kernel/CLI, so built-in profiles remain usable. Saving a valid user copy recovers the file with the same backup protection. Internal callers can request strict file validation with `load_catalog(ignore_user_errors=False)`.

### What happens when indexed geometry cannot be resolved?

A changed A/B/C address without a selected profile or an address absent from the selected profile stops milling execution with an explicit diagnostic. Simultaneous rotary/XYZ movement and non-rapid rotary interpolation also stop for the indexed A/B profiles; the checked **4-axis Table C** planar X/C feed contour is the exception. This is the current implementation, not a general FANUC restriction. A/B/C with an unsupported position-changing G-code also stops execution. Unknown M-codes and G41/G42 that cannot be verified because of missing tool or unsupported contour data produce warnings and let execution continue. G30 is not modeled as G28: its controller-specific second reference point is not inferred from the configured G28 home.

For **4-axis Table C**, G41/G42 cutter compensation is unsupported. Execution continues, but the X/C plot shows the programmed tool-tip path without cutter-radius offset and reports `UNSUPPORTED_TABLE_C_CUTTER_COMPENSATION`. G40 cancels the modal request. Do not treat this plot as a verified compensated contour.

A selected profile makes the calculation repeatable; it does not by itself prove that the profile matches a physical machine. Inspect diagnostics and the supported contract before using `ok` or `complete` as an export decision.

### Which milling canned cycles are modeled?

The current set includes:

```text
G73
G80
G81
G82
G83
G84
G85
G86
```

The common cycle runtime returns generated geometry, modal updates, signals and final position as one outcome.

### What is the difference between G73 and G83 milling peck cycles?

G73 is high-speed peck drilling with short intermediate retract behavior. G83 returns to R between pecks, then rapidly re-enters at clearance d above the previous depth before continuing at feed. Reentry is limited to the R plane. The kernel option `milling_g83_clearance` sets d in millimetres, including inch programs; it must be finite and non-negative. The default 1.0 mm is a modeling assumption because the controller setting cannot be read from the program. This changes G83 feed distance and cycle-time statistics; turning G83 and native SINUMERIK CYCLE83 keep their separate behavior.

For milling drilling cycles, a depth above R reports `INVALID_DRILLING_DEPTH`. Z equal to R remains valid and produces no drilling feed stroke.

### How is G82 dwell represented?

G82 includes its dwell semantics, but dwell itself does not create spatial geometry.

### How is milling G84 represented?

G84 tapping returns from depth as synchronized feed motion rather than rapid motion.

### How is milling G86 represented?

The cycle models spindle-stop semantics together with its drilling motion/return behavior.

### What do milling G98/G99 mean?

For milling canned cycles, G98/G99 select cycle return behavior. They are not the turning feed-mode meanings of G98/G99.

### What are milling feed modes?

For milling:

```text
G94 -> feed per minute
G95 -> feed per revolution
```

Statistics only compute trustworthy machining time where the required feed/spindle information is known.

### Which work coordinate systems are supported?

The kernel supports:

- `G54-G59`;
- `G54.1 P1-P99`;
- runtime `G10 L2`;
- runtime `G10 L20`.

### How does G10 behave under G91 in milling?

For runtime work-offset programming, incremental mode updates the existing selected offset instead of silently replacing it with the raw incremental value.

### How does G52 work?

`G52 X/Y/Z` sets a local coordinate-system shift for subsequent motion. The G52 control block itself does not move the tool.

### How do G68 and G69 work?

G68 enables coordinate rotation around the programmed center in the active plane. G69 cancels the rotation.

In SINUMERIK ISO-M mode (`G291`), the modeled `G68` subset requires `G90` and has no `I/J/K` vector. `G68` with `G91` angle semantics or with any `I/J/K` 3D rotation vector is recognized but unsupported. `G69` remains supported.

The active transform applies to later endpoints and I/J/K arc vectors. Enabling or cancelling the transform does not itself create a motion segment.

G68.2 X/Y/Z I/J/K defines a 3+2 tilted working plane with Z-X-Z Euler angles. Select a kinematics profile with two distinct rotary axes first; supported topologies include table-table, head-head and head-table. G53.1 must be the next standalone block: it solves the selected profile's rotary angles to align the physical tool axis with functional +Z. An unreachable orientation stops with a diagnostic. G69 cancels the plane while retaining the indexed rotary position. This model applies only to `fanuc_mill`. Explicit A/B/C addresses during the tilted plane and simultaneous G68 rotation are unsupported. G53 and G28 reference motions use machine coordinates. Supported G68.2/G53.1 and CYCLE800 indexed AC/BC frames can be converted experimentally through the bundled multiaxis posts; other frame combinations remain rejected. Full Program preserves the source.

### How does G51/G50 scaling work?

Milling G51 supports:

- uniform scaling with P, where `P1000` means factor 1.0;
- per-axis factors through I/J/K.

G50 cancels milling scaling.

For SINUMERIK ISO-M, `G51` uses the modeled 0.001 scale-factor weighting (`P2000` means a factor of 2.0). Machine-specific alternative weighting is not modeled.

The scaling center is interpreted as absolute coordinates even under G91, and omitted center axes use the current position.

Axis-specific scaling of an arc can turn a circle into non-circular geometry. The kernel reports that unsupported case instead of approximating it as a circle.

### Is G53 supported in milling?

Yes. G53 is non-modal machine-coordinate motion. It does not overwrite the active WCS for later ordinary work-coordinate blocks. An absolute zero axis target such as `G53 Z0` resolves to the configured machine home on that axis; non-zero absolute and incremental targets retain their machine-coordinate meanings.

### Is G28 supported in milling?

Yes. The configured reference-return path is resolved through the execution kernel rather than handled only by the GUI. For indexed milling, the intermediate and home targets are resolved on machine axes before their trace points are transformed for display. `G91 G28 Z0` returns the Z axis to the configured home Z.

With 4/5-axis table kinematics, G28/G53 use the current table orientation without resetting ABC. For example, with home Z=500 and zero WCS offset, a B-table return targets global Z=500 at B0 and Z=-500 at B180. A Z-only reference segment that crosses the WCS centre plane stops execution with an error; check machine home Z and the WCS offset. This check does not detect collisions with a part model.

After G28/G53 in a 4/5-axis program, the next approach can start a separate trace segment in the new table orientation. No connecting line is drawn between those segments. Ordinary three-axis paths remain continuous, including reference returns.

### Is continuous five-axis TCP (`G43.4`) supported?

For `fanuc_mill`, continuous `G0/G1` tool-center motion with simultaneous linear and rotary axes is supported on the angled AC and BC table profiles. Activating TCP preserves the current physical point in the plotted trace. With TCP off, indexing retains programmed XYZ and changes the displayed table frame. `G2/G3` TCP arcs may interpolate configured rotary axes while programmed XYZ remains the authoritative tool-center path; start/end tool orientations and rotary events are retained. Combining TCP with `G68.2` remains unsupported. This is toolpath interpretation, not a complete machine or collision simulation.

### How are milling arcs programmed?

Milling supports:

- relative IJK center offsets;
- absolute IJK center coordinates;
- R radius programming.

The selected source interpretation is resolved into one analytical arc center/radius/sweep representation.

### What does Arc Type autodetection do?

When enabled, the kernel examines milling or turning IJK arcs in source occurrence order before final geometry resolution. Turning X and I values are converted from diameter coordinates to physical radial coordinates for this comparison.

For each IJK arc it compares relative and absolute-center interpretations using the configured arc tolerance. The first unambiguous candidate fixes the IJK mode for that execution.

R-only arcs are ignored during detection because they do not distinguish IJK conventions.

If every candidate is ambiguous, the selected fallback mode is used. GUI, CLI parse/trace/analysis and file/batch export enable detection by default for both milling and turning; CLI uses relative IJK as the fallback. Shared application execution uses the GUI's default 0.01 mm arc tolerance. Direct kernel calls retain explicit mode/tolerance controls and a 0.001 mm default for turning.

Selecting an Arc Type in the GUI manually overrides auto detection for the current document. The Auto Detect setting remains enabled for the next opened document. In turning, an I/K arc interpreted with the wrong center mode reports `INVALID_TURNING_ARC_CENTER`; selecting Radius mode for an arc without an R word reports `TURNING_ARC_REQUIRES_R`.

### Can one program mix R arcs with IJK arcs?

Yes. Arc-type detection determines the IJK interpretation. An R-only block remains an R arc regardless of that decision.

### Are full circles supported?

Yes. Analytical full circles are represented directly by the kernel.

When Expanded Execution is asked to emit R-format arcs, a full circle is exported as two exact R semicircles because one R block cannot uniquely represent a full circle.

### Is helical interpolation supported?

Yes. Circular interpolation can include motion along the axis normal to the active plane where the supported geometry contract permits it.

### What does G16/G15 polar programming do?

`G16` enables milling polar-coordinate endpoint programming and `G15` returns to ordinary Cartesian programming.

The active G17/G18/G19 plane determines the polar plane:

- first in-plane axis = radius;
- second in-plane axis = angle in degrees.

### How does polar G90 work?

In absolute mode, the active work/local origin is used as the pole. Programmed polar radius and angle are absolute polar values.

### How does polar G91 work?

When entering `G91 G16`, the current position becomes the pole. Later G91 polar words increment modal radius or angle, and omitted components retain their previous polar value.

### Do G20/G21 scale the polar angle?

No. The radius is a length and follows units. The angle remains degrees.

### Are polar G2/G3 arcs supported?

The implemented polar circular contract requires R radius programming. I/J/K center programming while G16 polar mode is active is rejected with an explicit diagnostic rather than guessed.

### Is G12.1/G13.1 polar interpolation supported?

No.

### How does milling cutter compensation work?

G40/G41/G42 uses configured milling tool diameter and works on supported line, arc and compatible helical contours.

Supported cutters include Flat, Bull, Ball, Face, Slot and Chamfer Mill. Compensation uses half the configured diameter; for Chamfer Mill this is the nominal cutter radius, without calculating a depth-dependent contact radius. Tap previews have a flat front face in both milling and turning.

For indexed table A/B milling, the offset is calculated in the local programmed working plane before the completed geometry is transformed into the fixed WCS plot. Execution continues when the tool or contour cannot be verified, with `UNVERIFIED_CUTTER_COMPENSATION` reported. The 3D view uses left drag to pan and middle drag to orbit around the cursor, as in CNCEditor; the table B 3D/ISO preset shows +Y vertically upward, +X upward-right and +Z downward-right while table A keeps the vertical mill preset.

For **4-axis Table C**, G41/G42 is not resolved. The trace retains the programmed X/C tool-tip coordinates and emits `UNSUPPORTED_TABLE_C_CUTTER_COMPENSATION`; G40 ends the modal request. This limit is specific to the current C-table implementation.

The compensation engine resolves:

- entry transitions;
- steady offset geometry;
- line/arc and arc/line joins;
- corners;
- G40 exit transitions.

Inserted transition motions preserve execution-step ownership so editor navigation and export remain coherent.

### What does `UNVERIFIED_CUTTER_COMPENSATION` mean?

The source requested G41/G42, but the kernel could not prove a valid compensated path with the available tool/configuration/geometry.

The system marks that state explicitly rather than presenting uncompensated geometry as verified compensation.

### Is G43 tool-length geometry applied?

No. G43/G49 and H values are tracked for execution/export context, but H-offset geometry is not currently applied to the resolved toolpath.

That limitation is intentional and should not be interpreted as a simulated tool-length-compensated machine position.

---

## Tool libraries and tool discovery

### Where are persistent tools stored?

Turning and milling tools are stored in:

```text
%LOCALAPPDATA%\easy-gcode-plot\tools.db
```

This SQLite database is authoritative for Saved Library tools.

### What is the difference between Current Program and Saved Library?

Current Program tool export accepts only `.json` filenames (case-insensitive). Other extensions, including `.nc` and `.mpf`, and filenames without an extension are rejected before writing; existing files remain intact.

**Current Program** is temporary state for the open CNC program. Literal T selections can be discovered from source and assigned geometry without modifying the persistent library.

**Import** and **Export** below Current Program exchange the current milling or turning setup as JSON, independently of Saved Library and `tools.db`. Export saves all current tools, regardless of the selected row. Import validates the entire file first, replaces matching T slots, keeps other current tools unchanged and reports unused imported numbers. The file retains geometry, controller identities, offsets and custom metadata; dimensions are in millimetres. Imported assignments, Edit Geometry and library assignments stay pending until **OK**. **Cancel** discards them without recalculating the simulation.

Simulation settings in **Options**, **Tool Library**, **WCS** and **Stock** take effect only after **OK**. Editing controls, browsing rotary profiles or resetting stock to automatic bounds does not regenerate 3D milling or 2D turning stock. **Cancel** keeps the active simulation unchanged; **OK** without simulation changes does not rebuild it. User profile edits made in Options are also pending until its **OK**. Activating kinematics through the Settings menu takes effect immediately.

The operation identifies the fallback tool type first. A matching T number in the corresponding Saved Library then supplies the actual geometry, including its saved type and dimensions. If no valid matching record exists, discovery uses source comment dimensions and the operation-based default. Milling `T02` matches `T2`; turning `T202` matches `T0202`, while different packed offsets remain distinct. Manual Current Program edits take priority on subsequent recalculations.

**Saved Library** is persistent and is committed to `tools.db` only when the Tool Library window is accepted.

Import does not work in an empty NC program: it updates tool slots already found in the source. First add a tool selection/change with a number present in the JSON, for example `T1 M6` for FANUC milling or `T0101` for FANUC turning. Refresh the program analysis or reopen Current Program so the tool appears in the list, then import the file. At least one tool number must match.

### Does opening a program write discovered tools to the database?

No. Tool discovery is temporary.

### How are turning tool numbers represented?

Turning selections retain the packed tool/offset form such as:

```text
T0909
```

Milling selections use the tool number, for example `T03` becomes tool key `T3`.

### Can comments describe tool geometry?

Yes. Tool discovery recognizes useful inline and nearby comments, for example:

```text
(T3 D=6. CR=0. - FLAT END MILL)
(OD ROUGH R0.8)
(ID ROUGH R0.8)
(GROOVE H4)
(DRILL)
(TAP)
(THREAD)
(BALL)
(FACE MILL)
(CHAMFER)
```

Dimensions are interpreted using the units active at the tool selection.

### What happens when no explicit type hint is present?

Operation context supplies a practical temporary default where possible:

- milling G81-G83 -> drill;
- milling G84 -> tap;
- native SINUMERIK CYCLE81/CYCLE82/CYCLE83 -> drill;
- native SINUMERIK CYCLE84 -> tap;
- turning G32/G33/G76/G92 -> thread tool;
- otherwise standard milling or turning fallback geometry.

Native cycle classification uses the controller AST, including modal MCALL, cancellation and tool changes. Cycle names in comments or MSG text do not classify an operation. An operation's type takes priority over a conflicting comment type hint; an automatically matched saved tool keeps its own geometry. The preliminary scan does not execute macros or infer physical dimensions from a toolpath. CLI/API callers can supply a library snapshot through `execute_program(..., library_tools=...)`; execution does not load a local SQLite library implicitly.

Shared GUI/CLI execution builds Program/AST once, resolves tools from that same object before motion execution, and then calculates the trace. Discovery does not run another frontend pass. The Cython/Python scanner still extracts source comments and literal tool candidates; it does not independently execute controller operations.

Finding a saved tool or assigning a default does not guarantee verified compensation. `UNVERIFIED` describes an unproven compensated path, not merely an unknown tool. G41/G42 can remain unverified with missing geometry, an unsupported tool or an invalid entry/path, including native SINUMERIK named tools without matching numeric geometry. Operation-based defaults existed before automatic library lookup.

### Are macro T expressions discovered as literal tools?

No. Discovery intentionally does not evaluate `T#1` or `T[expr]`. Literal tool discovery and full CNC execution are separate concerns.

### Which turning tool geometries are stored?

The turning library uses nine canonical geometry types:

- Diamond 80;
- Diamond 35;
- Square;
- Round;
- Triangle;
- Groove;
- Thread;
- Drill;
- Tap.

OD, ID and Face are UI filters for available tracing orientations, rather than different geometry classes. They do not choose the material-removal side or change Stock Removal results for the same trace and physical geometry.

### Which milling tools can be previewed?

The milling tool model includes flat, bull-nose, ball, tapered ball, face, slot, chamfer, drill and tap geometry.

### How are milling tool lengths defined?

The milling editor stores two metric lengths:

- `fluteLength`: cutting length measured from the tip; must be greater than zero.
- `bodyLength`: non-cutting length from the end of the cutting portion to the holder; may be zero.

Length to holder is `fluteLength + bodyLength` and is read-only in the editor. The compatibility field `length` is derived from this sum; there is no `shaftLength`. The Inches switch changes display units; SQLite and JSON/CSV exports retain millimetres.

For face and slot mills, `fluteLength` sets the cutting head height; `cuttingHeight` is retained only for legacy records. For tapered ball mills, the taper ends at `fluteLength`, followed by a cylindrical body extending to the holder. Both library and playback previews use this geometry.

The library preview shows the cutting part in gold and the non-cutting body in gray. In 3D, the default cutting color is yellow; the body is near-white in the dark theme and dark gray in the light theme to distinguish it from gray STL models. The tool color option changes only the cutting part. Tools without an explicit length split use one color.

Existing tools with only `length` keep their total and preview without an inferred split. The editor identifies these records as legacy. Editing unrelated fields keeps the unsplit record; entering cutting/body lengths defines the new partition. Loading the library does not rewrite the database.

Tool comments can supply both dimensions, for example `(FLAT END MILL D10 FL25 BL15)`. Comment dimensions follow the units active at tool selection. A comment providing only `L`/`LENGTH` retains an unsplit total. Automatically discovered tools without length dimensions use editable defaults, not measured dimensions.

### Does CLI execution load the GUI Saved Library?

No. CLI runs use the same temporary source-based tool discovery used for a newly opened program. GUI manual Current Program assignments and the Saved Library are not silently loaded into the CLI execution.

This matters for G41/G42 verification: inferred tool dimensions should be reviewed before treating a compensated CLI trace as authoritative.

---

## Interface, editor and playback

### How do I measure geometry in the plot?

Choose **Top (XY)**, **Front (XZ)**, **Left (YZ)** or **Lathe View**, then enable **CNC Functions → Measure**. Click a toolpath point, STL edge or STL facet to set the first point. Move the mouse to preview the blue ruler; click a second geometry point to fix the result. The next click starts a new measurement. **Reset** or **Esc** in the plot clears the measurement; closing the nonmodal Measure dialog turns the ruler off. Free 3D views do not support Measure.

The dialog shows From/To XYZ coordinates, signed coordinate differences, the distance projected onto the current view plane, and the full 3D distance. Rows are **From**, **To** and **Difference**, with **X/Y/Z** columns. Double-click a From or To cell to enter coordinates; Difference is calculated automatically. **Inches** converts coordinates and distances without moving the physical points or changing application units. In Lathe View, **X (D)** coordinates and X differences are diametral; both distances use physical radius coordinates. With **Grid** enabled, the ruler also snaps to visible grid crossings near the cursor, using the currently drawn adaptive or manual spacing. Geometry picks take precedence; hidden grids do not snap. Ruler clicks do not move the editor caret or playback slider. Ctrl+drag still pans; zoom remains available.

STL picking uses the currently displayed transformed facets, including transparent objects and active clipped sections. Hidden objects are excluded. Toolpath measurements follow the sampled geometry displayed in the plot; stock-mesh measurements retain the resolution of the simulated surface.

### How do I insert the calculated stock into STL Objects?

Pause three-axis **Stock Removal** at the required playback/TrackBar position. Right-click the plot and choose **Insert Mesh into Plot View**. Wait for the selected stock frame to finish displaying before inserting. The application reads that calculated GPU state and builds an independent mesh in memory, without exporting or reading an STL file.

The new **Stock snapshot** appears in **STL Objects**, aligned with the program in physical coordinates. Subsequent playback does not change it. Use the normal object transforms, sections and Measure tool; leaving Stock Removal keeps the inserted object in the plot. Mesh construction is cancellable, does not refine or coarsen the simulated surface, and rejects meshes over the plot's two-million-triangle limit.

### What are the two main GUI panels?

The left side is a QScintilla editor with syntax highlighting, line numbers, search/replace and cleanup functions. The right side is an OpenGL trajectory view with axes, grid, camera controls, trajectory picking and playback.

The milling 3D view uses an orthographic CAD projection. Rotating from Top, Front or Left keeps parallel lines parallel and preserves apparent size across depth.

### How does an imported STL affect toolpath visibility?

In solid mode, the STL surface hides toolpath segments behind it. The feature-edge wireframe has no solid surface to occlude those segments. This changes only visibility in the plot, not the resolved trajectory geometry. Manage imported models in **View → STL Objects**; the guide below covers transforms, sections, picking and measurements.

### How do I use the STL Objects panel?

The **View → STL Objects** dock edits imported STL scene objects without changing the G-code program. Import a model with **File → Import STL**. The dock lists each imported model; select a row before applying an operation. Choose **Base point**, **Position**, **Transform**, **Circular array**, **Rectangular array** or **Section** from the operation selector. The four compact buttons at the top apply Undo, Redo, Statistics and Delete to the STL scene.

#### How do I import and select STL models?

Use **File → Import STL** to load an ASCII or binary mesh. **File → Recent STL** reopens a recent model. Each import appears as a separate row in the dock; selecting a row makes it the target of the operation controls and statistics. **Delete** removes the selected model. **File → Clear STL** removes all STL models. These commands affect imported scene objects, not the editor contents or G-code trajectory.

#### What do Undo, Redo, Statistics and Delete do?

The STL **Undo** and **Redo** history is separate from text-editor undo. It records scene edits such as adding another model, changing a base point, moving, rotating, mirroring, scaling, creating arrays, applying or clearing a section, and deleting an object. The first imported model establishes the scene baseline, so Undo does not close the panel or remove that first model. **Statistics** opens copyable measurements for the selected object. **Delete** removes only the selected row; use **File → Clear STL** to remove the complete STL scene.

#### How do STL base points and bounding-box picks work?

The **Base point** selector chooses the point used as the pivot for rotation, mirroring and scaling:

- **Center** sets it to the center of the source mesh's bounding box.
- **Bounding-box corner** sets it to the source mesh's minimum X, Y and Z corner and displays the transformed object's axis-aligned bounding box in the Base Point color.
- **Origin** sets the point to model coordinates `(0, 0, 0)`.
- **Custom** enables the X/Y/Z fields; enter coordinates in model space and press **Set base point**.

When the bounding box is displayed, its eight corners are picking points. Hold **Shift** and left-click a corner in the 3D plot to move the base point there. The picked point becomes larger and cyan; the other seven corner markers remain in the Base Point color. Picking changes the base point to a custom point, while keeping the box visible so another corner can be picked. Choosing Center or Origin exits bounding-box picking.

The **Position** page shows the current base point's world position. Enter a target X/Y/Z there and use **Move base point here** to place the pivot at those world coordinates. Moving changes the object's transform while preserving its shape.

#### How do I position and transform an STL model?

On **Transform**, select an axis and angle to rotate around the current base point. **Mirror** reflects the object across the plane whose normal is the selected X, Y or Z axis, passing through the base point. **Scale** applies a uniform factor around that point. These operations preserve the source STL and update the scene object's transform; they do not modify the original file on disk.

#### How do STL arrays work?

**Circular array** creates the requested number of copies around a selected axis and center, spread over the total angle. With **Rotate copies** enabled, each copy rotates with its position. When disabled, each copy keeps its orientation and distributes the current base point around the circle. A full 360-degree array spaces copies evenly without duplicating the first copy at the end.

**Rectangular array** creates copies along X, Y and Z. Set the copy count and step for each axis; the resulting array includes the original object. Array creation is one STL history action and can be undone.

#### How do I make a 3D section through an STL model?

On **Section**, choose X, Y or Z for the cutting plane, enter its coordinate and choose which side to keep. The initial coordinate is the midpoint of the selected model's world-space bounding box along that axis. **Apply section** clips the solid in 3D and closes the cut where the mesh produces a closed contour; the cut model remains visible over the source toolpath. **Clear section** restores the full STL. Applying and clearing a section are undoable STL scene actions.

#### What does STL Statistics report, and how do I display inches?

**Statistics** reports surface area, volume, center of mass, world-space coordinate bounds and per-axis lengths. Bounds are written explicitly as `Xmin`, `Xmax` and `Length` (and likewise for Y and Z). The **Inches** checkbox at the lower left of the dialog converts all reported lengths, coordinates, area and volume while leaving the mesh unchanged. Unchecked values display in millimetres; checked values use inches, square inches and cubic inches.

STL files do not encode a unit system, so these labels are display units and do not determine the source model's real-world scale. Surface area and bounding box are available for open meshes. Volume and center of mass require a closed mesh with consistently oriented faces; otherwise the dialog reports them as undefined.

### How do I change letter case or mark optional blocks?

Use **Edit → Uppercase** (`Ctrl+Shift+U`) or **Edit → Lowercase** (`Ctrl+U`), or their optional toolbar buttons enabled in Customize Toolbars, to convert selected text. With no selection, they convert the entire editor document. Their shortcuts can be changed in Options.

Select one or more blocks and press **Ctrl+/** to add `/` at the start of each selected nonempty block. Press **Ctrl+Shift+/** to remove one leading `/` from each selected block. Without a selection, these commands do nothing. Both shortcuts are fixed and cannot be assigned to another command. The slash is the FANUC optional block skip marker; whether such blocks execute depends on the Block Skip setting.

### How do I print the plot?

Use **File → Print** (`Ctrl+P`) or enable its optional File-toolbar button through Customize Toolbars. The app prints sharp vector lines in the current camera orientation, fitted to a landscape page. Printing ignores the playback slider and does not hide lines behind an imported STL. In **Settings → Options → Plot**, you can show or hide rapid moves, render them dashed or solid, and color all moves by tool; Print follows those choices. **FAQ** opens with `F3`, and **Grid** toggles with `F4` by default.

### Which fixed views are available?

Top, Front and Left are orthographic views. The milling ISO/3D view also uses parallel projection; free orbit retains it.

**View → Rotate view** rotates the current fixed milling view around model X, Y or Z through the current center of the view. Enter a signed angle (default 90°) and select the model axis. Positive angles follow the right-hand rule. Rotations accumulate; the camera center, scale and calculated trajectory are preserved, without CNC recalculation. For example, 180° around X turns Top into the opposite bottom view; 180° around Z turns Front into Back and Left into Right.

The same command and icon are available in the plot context menu, View toolbar, Hotkeys and Customize Toolbars. Existing saved toolbar choices remain respected; enable the command there if needed. It is disabled in ISO/3D and turning. Top/Front/Left restore their standard orientations. Each MDI document retains its rotated camera.

When the rotated camera faces XY, XZ or YZ, the grid and ruler follow that actual plane. At arbitrary oblique angles, planar grid and measurement are disabled until the camera returns to a coordinate plane. Toolpath selection remains available. Camera rotation does not transform program coordinates, stock, STL objects or machine kinematics.

### How does playback relate to the kernel?

Playback advances through resolved logical motions from the current `ExecutionResult`. It does not re-parse each source line as the slider moves.

During ordinary trace playback, supported analytical arcs and helices with a fixed tool orientation animate through intermediate cursor and milling-tool positions. This includes full-circle moves repeated by Macro B WHILE loops. The slider remains on one logical-motion step during these visual frames and advances once for the next motion; render quality does not change its range. Even at the fastest speed, circles retain intermediate positions instead of jumping between two opposite points. Turning Stock Removal uses its own playback timeline.

The Play button shows the Pause icon while running. Click it again to pause; stopping or completing playback restores the Play icon.

### What do Step Backward and Step Forward do?

They move by one logical motion, including generated motions from cycles and Macro B-expanded execution.

### Why can many playback motions map to one source line?

One source block can emit many motions. Examples include:

- turning cycles;
- milling canned cycles;
- Macro B loops that execute the same source line repeatedly;
- compensated transition geometry.

Playback tracks execution occurrence and source ownership separately.

### How do I customize toolbar buttons?

Right-click a toolbar and choose **Customize Toolbars**. Check the buttons you want on each panel; search filters the list without changing your choices. **OK** applies and saves the selection, **Cancel** discards it, and **Restore Defaults** stages the compact default button set. The toolbar context menu also lets you hide whole panels or reset their layout and buttons. Menu commands and shortcuts remain available even when a button is hidden. Static CNC Functions and Tool Library/WCS/Stock/Tokens commands are available; Recent Files and rotary-profile lists remain in menus. Source-type and playback-speed widgets are retained.

The 2.6.0 default keeps grouped file operations, undo/redo/search, view controls, toolchange navigation, Compare/statistics/measurement and playback. Clipboard buttons, case conversion, cleanup, Save As, Print, tool-list export, snippets and calculators are optional. Existing saved choices remain unchanged until you explicitly restore defaults.

### How do I locate a plotted move in the editor?

Use Shift+left-click near a trajectory line or arc, including in the milling 3D view. The application selects the owning source block and moves the playback slider to the corresponding executed movement. Overlapping 3D segments are selected by camera depth; hidden rapid moves are excluded.

**Settings → Options → General → Cimco Like Picking** is off by default. Enable it to select with a left-click and pan by dragging the right mouse button in milling views. A right-click without dragging opens the context menu; dragging does not. With the option off, left-button dragging pans and Shift+left-click selects. Middle-button rotation and wheel zoom remain available. The setting takes effect on OK; Cancel discards the change. Turning controls are unchanged.

### Does automatic refresh move the editor caret?

Normal execution/plot refresh is intended to update the result without using editor caret movement as a side effect. Playback/navigation can intentionally select source locations.

### What happens when Auto Update is too expensive?

Auto Update has a sampled-segment limit. Large edits may be left pending until explicit Refresh so typing remains responsive.

If source changes while a refresh is running, the stale calculation is cancelled/ignored and a new refresh is queued.

**Settings → Options** also exposes arc tolerance, arc sampling preset, maximum/minimum circular radius and minimum chord length. Sampling controls change the GUI trace representation without changing the resolved CNC geometry. General settings include the maximum generated motions, automatic sampled-segment limit and toolbar icon size. Explicit Refresh is cancellable.

### What does Cancel stop?

The execution dialog covers the expensive source-to-result pipeline, including reading, parsing, execution, tool discovery, trace sampling and final plot publication. Cancellation is cooperative and checked throughout the execution budget.

### What CNC editing assistants are included?

The GUI contains:

- Hole Calculator;
- Pocket Calculator;
- Snippets.

Hole and Pocket Calculator are milling-only. Snippets is available in both machine modes.

### What does Hole Calculator generate?

It generates coordinate blocks for circular or rectangular/grid hole patterns. It does not invent the complete surrounding drilling-cycle safety logic.

### What does Pocket Calculator generate?

It can generate circular or rectangular milling fragments with configurable stepover, depths, safe/reference Z, feed, direction, clearing strategy, helical entry and finishing pass.

The generated fragment is a starting point, not a machine-safety certification.

### Where are snippets stored?

On Windows, the SQLite library is normally stored in:

```text
%LOCALAPPDATA%\easy-gcode-plot\snippets.db
```

The **Controller** selector separates **Fanuc**, **Sinumerik**, **Heidenhain**, **Fanuc Lathe** and **Sinumerik Lathe**. Each space has independent names, text and ordering. Opening Snippets selects the active document's controller and machine mode; selecting another space changes only the snippet list. Before switching snippets/controllers or closing the manager, unsaved text and picture changes can be saved, discarded or kept by cancelling the action.

Each space includes **Program Start**, **Toolchange**, **Toolchange (Drill)**, **Program End**, **Retract Home Z**, **Comment**, **Rapid Move**, **Linear Move**, **Circular Move** and **Drilling**. Turning also includes G71/CYCLE95 roughing and G76/CYCLE97 threading. FANUC Lathe examples use G-code system A and diameter X programming.

Milling templates also include FANUC G73/G74/G76/G81–G87/G89, SINUMERIK CYCLE81/82/84–87/89/90, HOLES1/2 and POCKET3/4, and HEIDENHAIN cycles 200–209, 220/221, 240/241, 251/252 and 262. HEIDENHAIN coordinates and numeric Q parameters retain explicit `+`/`-` signs. Patterns 220/221 require a previously defined machining cycle; pockets and thread milling require a configured cutter. POCKET3/4 templates expose VARI=1/2/11/12; other entry strategies need additional parameters. CYCLE84 uses the entered SST for cutting and retraction, matching the project's supported cycle subset.

**Toolchange** collects the tool number, offset, spindle speed/direction and clearance coordinates. Its inserted comment includes the tool type and diameter for milling, or the tool type, insert designation and nose radius for turning. HEIDENHAIN uses the selected tool-table entry. **Toolchange (Drill)** instead collects diameter and point angle, without insert fields. Coordinates, feeds and cycle arguments also have their own input fields; numeric ranges, integers, allowed choices and dependent limits are validated. G76's packed P word is entered as three separate two-digit values: finishing passes, pull-out and tool angle.

Set up units, coordinates, the tool and the starting position in the surrounding program. FANUC uses milling G83 or axial turning G74; SINUMERIK milling uses **MCALL CYCLE83**, so add the required hole-position blocks and cancel with **MCALL** after them. SINUMERIK turning uses CYCLE83; HEIDENHAIN uses CYCL DEF 203 and CYCL CALL. G71/CYCLE95 require an existing contour. Default SINUMERIK drilling uses DAM=0 and VARI=1; HEIDENHAIN Q208 defaults to 500. Circular Move defines an endpoint/radius/feed and assumes a suitable starting point; it does not add clearance moves.

Edit the source directly in the compact manager and use **Insert** to open the parameter form. It contains input fields, an attached read-only picture when present, and OK/Cancel. There is no text preview or Preview tab. Invalid input disables OK; Cancel inserts nothing. The successful insertion is one editor undo action, and the Snippets manager stays open. Templates without input fields insert directly. The **View → Snippets** side panel filters templates by group and name and uses the same insertion workflow.

| Literal | Result |
| --- | --- |
| `{{?D=10}}` | Declare input D with default 10; `{{?Name}}` requires a value |
| `{{?D=10\|number\|gt=0}}` | Require a positive numeric diameter |
| `{{?Tool=1\|int\|min=0}}` | Require a nonnegative integer tool number |
| `{{?ReturnMode=98\|int\|choices=98,99}}` | Offer an allowed-value combo |
| `{{?RPM=\|int\|optional\|min=1\|prefix=S}}` | Optional positive RPM; omit the S address when empty |
| `{{?Z=-20\|number\|lt=ReturnZ}}` | Check a limit against another parameter |
| `{{D}}` | Reuse an input without another field |
| `{{?X=10:+\|number}}`, `{{X:+}}` | Include the plus sign for nonnegative values, as in Klartext |
| `{{=1000*Vc/(PI*D):0}}` | Calculate RPM with zero decimal places |
| `{{=(D/2)/TAN(Angle/2):4}}` | Drill-point height with four decimal places |
| `{{=TO_INCH(D):4}}`, `{{=TO_MM(Inches):3}}` | Convert mm to inches or inches to mm |
| `{{date}}`, `{{time}}`, `{{datetime}}` | Local date/time captured together for the insertion |
| `{{date:DD.MM.YYYY}}`, `{{time:HH:mm}}` | Formatted date/time |
| `{{file.name}}`, `{{file.stem}}` | Current saved document name, with or without extension |
| `{{file.path}}`, `{{file.dir}}` | Absolute file path or parent folder; the file must exist |
| `{{selection}}`, `{{cursor}}` | Selected editor text; final cursor position after insertion |

Field metadata follows `|` separators. Types are `text`, `number`, `int` and `contour` (START:END labels). `min`/`max` are inclusive; `gt`/`lt` are strict. Limits may reference other numeric fields. `optional` allows an empty field, `oneof=Other` requires an alternative when it is empty, `width=2` pads integers, and `prefix`/`suffix` apply only to nonempty values. An optional display label can precede the type.

Arithmetic supports `+ - * / % ^`, parentheses and `PI`. Functions: `SIN`, `COS`, `TAN`, `ASIN`, `ACOS`, `ATAN`, `ATAN2(y,x)`, `ABS`, `SQRT`, `ROUND`, `MIN`, `MAX`, `TO_MM`, `TO_INCH`, `TO_RAD`, `TO_DEG`. Trigonometry uses degrees. `:0` through `:12` controls displayed decimals; intermediate calculations retain precision. Numeric fields accept a decimal comma and insert a decimal point. FANUC `#`, SINUMERIK `R` and HEIDENHAIN `Q` retain their ordinary CNC syntax.

Every controller includes **Spindle speed (formula)**, **Drill point (formula)**, **MM to INCHES**, **INCHES to MM**, **Trigonometry (formula)** and **Document header**. Each unit-conversion entry has exactly one input. Formula examples insert their calculated results into the snippet text; the conversion entries produce comments.

In the manager, **Picture → Load Picture... / Paste Picture / Remove Picture** attaches, replaces or removes the selected snippet's PNG/JPEG/BMP/WebP/SVG. **Save** stores text and picture together; editing only text preserves the saved image. The adjacent status reports whether a picture is attached and whether its change is unsaved. Images are limited to 10 MB and 4096 × 4096 pixels. Insert displays the attachment read-only, with click-to-enlarge and zoom; the picture area is hidden when absent. There is no picture editing or drag-and-drop in Insert. Pictures stay in SQLite and are never inserted into NC text. Rapid, Linear and Circular Move and Drill point have bundled diagrams, with separate X/Z motion diagrams for turning.

Defaults come from `app/gcode/snippet_defaults.py` and the formula entries in `app/gcode/snippet_examples.py`. A new library is seeded once; reopening it does not automatically replace text or restore deleted entries. **Update Defaults** restores **all standard snippets for the selected controller**, including deleted entries, and fills missing bundled pictures. It replaces changed standard text, so save personal variants under a different name first. Custom names, existing record order/IDs and attached pictures are retained; other controller spaces are unaffected. The button is disabled when all standard texts and bundled pictures are present and current. Deleting a snippet deletes its picture; restoring a standard snippet restores its bundled diagram, not a previously deleted custom image. Back up `snippets.db` to preserve all five spaces and their pictures.

Older text-file snippets can still be imported once without deleting their originals. Invalid UTF-8 files are skipped with a log warning; valid files are imported. This import is separate from Update Defaults.

---

## Options and scene configuration

### How do I hide the tool in Plot?

Enable **Settings → Options → Plot → Hide Tool**. It is off by default and hides the tool only in the regular plot; Stock Removal simulation keeps displaying its tool.

### Where can I read execution errors and warnings?

The Status Bar shows one compact diagnostic count, such as **Warnings: 2** or **Errors: 1**. Hover over it for the complete messages and affected source-line numbers; **Tokens** also shows execution diagnostics. Equal messages from different source lines remain separate records. **READY**, **UPDATING** and **STALE** indicate calculation state. Long temporary notifications are shortened with an ellipsis within the available space; hover over the Status Bar to read the full notification. Resizing does not extend its timeout.

### How do I change the interface language?

Open **Settings → Options → General**. In **Language**, choose **English** or **Russian**, then press **OK**. Restart Easy G-Code Plot to apply the language change; the application displays a restart notice. This setting changes the interface language, not the CNC dialect used to execute a program.

### How do I change the theme?

Open **Settings → Options → General**, select **Light** or **Dark** in **Theme**, and press **OK**. The theme is applied immediately without restarting. Language and theme choices are saved in the application configuration.

### How do I change the current-line highlight color?

Open **Settings → Options → Colors**. The **Editor** group contains separate current-line colors for the light and dark themes: `#e8e8ff` and `#2a2d2e` by default. Click the color swatch for the native color picker or enter `#RRGGBB`, then press **OK**. Both colors are saved independently; changing themes or the editor file type preserves custom values. **Cancel** leaves the saved colors unchanged, and **Restore Defaults** resets both. The **Plot** group contains trajectory, tool, background and STL colors.

Enable or disable the highlight in **Settings → Options → Editor → Highlight current line**.

### Where do I set work coordinate systems and home values?

Open **Settings → WCS**. This is a separate dialog from Options.

| Setting | How to use it |
| --- | --- |
| G54–G59 | Enter the X/Y/Z work offsets for each system. The program selects the active system with its G54–G59 command; editing a row does not insert that command into the program. |
| Home (G28) | Enter the configured reference-return coordinates and use the home configuration checkbox to indicate whether they are configured. These values are used by the modeled G28 return. |
| Turning X/Z | In turning mode, X fields use diameter values; Y fields are disabled. Z is an axial coordinate. |
| Milling X/Y/Z | In milling mode, all three coordinate fields are available and X is a linear coordinate. |
| Inches | Switch the displayed and entered lengths between millimetres and inches. Existing physical values are converted rather than reinterpreted as another unit. |

Press **OK** to apply the values and recalculate the program. **Cancel** leaves the stored values unchanged. G54.1 extended offsets have no fields in this dialog; they remain zero unless set by supported program commands such as G10 L20.

### How do I set turning stock dimensions?

In turning mode, open **Settings → Stock**. Enter the initial blank dimensions before starting Stock Removal.

| Control | Meaning |
| --- | --- |
| Outside diameter | Initial outside diameter of the blank. |
| Inside diameter | Initial bore diameter; use zero for a solid blank. |
| Length | Axial length of the blank. |
| Stock front Z | Absolute Z coordinate of the front face. The rear face is at `front Z − length`; this field is not just an allowance thickness. |
| Accuracy | Stock-model resolution. Higher accuracy gives a finer model and requires more processing time. |
| Inches | Display and enter dimensions in inches instead of millimetres, preserving their physical size. |
| Run Stock Removal when Play is pressed | Enable material-removal playback when pressing Play. |
| Reset to Auto | Return to dimensions estimated from the current program's cutting trace. |

Press **OK** to apply manual dimensions; **Cancel** discards the dialog edits. Manual dimensions remain active until **Reset to Auto**, **New**, or opening another program restores automatic sizing. Stock Removal requires a calculated, complete turning program and configured tool geometry. See [Turning Stock Removal](#turning-stock-removal) for automatic sizing and supported tools.

### Is Stock Removal available for milling?

Yes. **3D milling stock removal on the GPU is the main addition in 2.0.0.** It shows the material remaining throughout a three-axis program and exports the current machining stage as STL. See the [milling stock guide](#milling-stock-removal) below. The turning simulator remains separate.

---

## Milling Stock Removal

### How do I start milling stock simulation?

1. Open a three-axis milling program and calculate it successfully through completion.
2. Check **Tool Library / Current Program**. Assign the cutter types and dimensions used by the program; the cut depends on that geometry.
3. Open **Settings → Stock**, select the milling tab and configure the box and **Accuracy**.
4. Confirm the settings and enable **Stock Removal** on the toolbar. Use Play/Pause, step controls or the playback slider to inspect the stock at different machining stages.
5. Rotate the scene to inspect the machined surface, outer walls and underside. Save the current state with **Save stock as STL** in the Plot context menu when needed.

Stock simulation consumes the already resolved execution trace, including cycle expansion and program flow. It does not interpret a second copy of the G-code. If a tool has not been configured, check the missing-tool warning: substituted geometry can give an inaccurate result.

### How do milling stock bounds and allowance work?

The initial milling blank is a rectangular box. Automatic sizing uses cutting-motion bounds, cutter radius and machining allowance; its top is at the selected WCS Z0. The lower Z bound extends below the cutting trace. The allowance applies to the automatic suggestion; it does not add material above the WCS zero automatically.

Manual sizing exposes X−/X+, Y−/Y+ and Z−/Z+ relative to the selected WCS origin. Set a positive Z+ to include material above zero for a facing operation. Each maximum must exceed its corresponding minimum. Manual dimensions are saved independently of turning stock settings. **Use automatic bounds** returns the dialog to the trajectory-derived suggestion. Inch display converts the dimensions; internal geometry uses millimetres.

### Which milling cutters and movements are supported?

The swept cut uses the configured axial/radial cutter profile. Supported profiles include flat end mills, face mills, ball mills, corner-radius mills and tapered-ball mills. Diameter, tip shape, corner radius and taper affect the result where applicable. Changing only a tool's display name is not a substitute for assigning its physical geometry.

The simulator follows resolved three-axis linear, arc and helical motion, including movements generated by supported cycles and macros. Straight sweeps and constant-Z XY arcs have analytical GPU handling; other curved trajectories are prepared within the selected contour tolerance. Rapid movement through stock also removes intersected material and records rapid damage.

### What does milling Accuracy control?

GPU textures have a **4 GiB maximum**, including power-of-two padding and all hierarchy levels. Available GPU memory and the device texture-size limit may impose a lower limit. If resources are insufficient, a warning explains the failure and simulation stops; Accuracy is preserved. Choose a smaller stock or lower Accuracy and retry.

Steep walls use smoothed lighting normals and a soft fill light to suppress grid stripes. This affects shading only; it does not change the calculated stock, intersection depth or exported STL.

Zoom remains available during playback. GPU ray traversal advances through the grid in one direction and has a finite bound derived from its dimensions, preventing repeated visits to shared boundaries when zoom changes floating-point rounding. This does not lower Accuracy.

The slider has five fixed levels. Moving toward higher accuracy makes the XY height grid finer and tightens curved-trajectory preparation. It increases GPU memory use and processing work. The selected level stays fixed at every playback speed and for large programs; it is not reduced in response to frame time.

The current implementation uses these internal presets, in millimetres:

| Level, left to right | Curved-trajectory contour tolerance | Grid spacing limit parameter |
| --- | ---: | ---: |
| 1 | 0.20 | 0.50 |
| 2 | 0.10 | 0.25 |
| 3 | 0.05 | 0.15 |
| 4 | 0.02 | 0.08 |
| 5 | 0.01 | 0.05 |

Actual XY node spacing is no greater than the grid parameter divided by √2, adjusted to cover the box boundaries. These are discretization settings, not a certified bound on total machining error. The displayed surface interpolates the stored heights with bilinear patches. Increasing Accuracy rebuilds the stock at the current playback position; it can reveal detail that the coarser grid could not represent.

### How do playback and tool edits affect the stock?

Play/Pause, stepping and seeking use the same logical-motion position as the tool display. Forward playback adds the new cutter sweeps to the existing GPU stock. Rewinding clears and replays the required prefix to reconstruct the earlier material state. A quality change also reconstructs the current state at the new resolution.

Editing or assigning current-program tool geometry rebuilds the active simulation while restoring its playback position. Background frame preparation coalesces seek requests and discards superseded work. Leaving simulation or closing the window cancels outstanding milling work. Turning retains its own stock engine and replay behavior.

### What do the stock colors and box faces represent?

Options provides separate stock-material and machined-surface colors. Untouched stock retains the stock color; the cut surface uses the machined color and surface lighting. Rapid cuts carry damage coloring. This identifies intersections with the configured stock, rather than checking an entire machine for collisions.

The box has visible outside walls and a bottom wherever material remains. Through removal does not leave an artificial bottom cap. You can inspect the underside by rotating the scene. The GPU computes normals for the interpolated top surface and uses the corresponding plane normals for the outside box faces.

### How do I export the simulated milling stock?

During milling simulation, open the Plot context menu and choose **Save stock as STL**. Export captures the actual GPU material state at the current playback position, so an intermediate operation can be saved as well as the completed result. Select the simulation Accuracy you need before saving.

| Export setting | Current effect |
| --- | --- |
| Length units | Writes coordinates in millimetres or inches. |
| Use calculated stock without mesh refinement | Enabled by default. Saves the displayed GPU state without replay or additional subdivision. Constant-height regions are merged exactly to reduce file size. |
| Maximum edge length | Starts from simulation Accuracy. Applies only when additional mesh refinement is enabled. |
| Linear/angular deviation | Linear deviation starts from simulation Accuracy. Simulation has no separate angular tolerance. Optional refinement follows the captured bilinear heightfield, without recalculating material removal. |

GPU readback uses the thread owning the OpenGL context and is reused until the GPU stock changes. Mesh serialization runs on a cancellable worker and replaces the destination only after successful completion. Export time depends on the remaining surface complexity and file size; smaller output edges cannot recover detail absent from the simulation.

### How does the GPU stock engine work?

The engine keeps remaining height and rapid-damage state in a GPU texture. OpenGL 4.3 compute shaders apply the cutter sweeps to their affected XY rectangles. Forward updates retain the existing material texture and update the changed regions and their maximum-height hierarchy.

The display shader traverses that hierarchy and intersects viewing rays with bilinear height patches, deriving their surface normals and writing scene depth. There is no repeated CPU construction and upload of a display triangle mesh. CPU responsibilities include CNC execution, cutter/trajectory preparation and STL serialization. A background worker prepares immutable trajectory frames; GPU removal, drawing and readback run on the OpenGL context thread.

Relevant implementation files are `app/gcode/stock/milling_stock.py`, `milling_stock_sweep.py`, and `app/ui/plot/milling_stock_gpu.py`, `milling_stock_shaders.py`, `milling_stock_overlay.py`. CPU triangle generation remains for STL export of GPU readback.

### What are the milling stock requirements and limits?

- **OpenGL 4.3** and a working graphics driver are required. There is no CPU milling-removal fallback.
- The model stores one remaining height per XY node above the box base. It supports vertical cutters and three-axis work; rotary/TCP motion, tilted cutters and undercuts are outside its scope.
- Imported STL meshes remain reference geometry. Stock removal operates on the configured box, not arbitrary STL solids.
- Resolution is limited by the device's maximum texture dimensions and available GPU memory. Exceeding the texture-size limit reports an explicit error rather than lowering Accuracy silently.
- Runtime depends on the GPU, box dimensions, selected Accuracy and cutter sweeps. No fixed speed multiplier is promised.

If the blank appears misplaced, check the selected WCS and the six stock bounds. If the cut has the wrong width or shape, check the active tool geometry. For missing fine detail, increase Accuracy. If initialization reports an OpenGL or texture-size error, check the graphics driver and the requested box/resolution.

---

## Turning Stock Removal

### What is Turning Stock Removal?

It is an axisymmetric material-removal preview based on the resolved turning trace and configured cutter geometry.

It is not a machine simulation.

### How is automatic stock estimated?

The resolved G1/G2/G3 cutting trace provides the minimum outside diameter and length. Rapid G0 outliers are ignored, cycle-generated cutting motions are included, and G18 arc extrema are evaluated analytically.

### Can stock dimensions be overridden manually?

Yes. **Settings → Stock** allows explicit outside diameter, inside diameter, stock length, absolute front-face Z and accuracy/resolution. See [How do I set turning stock dimensions?](#how-do-i-set-turning-stock-dimensions) for the fields and playback setting.

Manual values persist until Reset to Auto, New or opening another program returns the stock model to program-derived sizing.

### Which tools remove material?

The supported turning tool geometries include the nine canonical tool-library types. Stock Removal follows the resolved trace, tracing orientation and physical cutter geometry. OD/ID/Face checkboxes only filter the tracing choices in the tool editor; changing these filters does not change removal for the same trace and cutter geometry.

The cutter's bounded swept footprint removes only the material it intersects. Separate remaining material rings are retained, including the outside wall during G71 boring. Stepping backward and replaying the same motions restores the same stock section. For grooves, **Groove geometry** selects radial or face geometry independently of these checkboxes.

### How are threads represented in Stock Removal?

Synchronized G32/G33, modal G92 and G76 cutting motions use a deterministic longitudinal thread-section model rather than sweeping the complete insert body as a generic solid.

The programmed X defines root depth, F defines pitch/lead, and configured thread geometry shapes the section.

The displayed thread insert is a separate fixed silhouette shared by Tool Library and the Stock Removal overlay: a triangular body with three small 60-degree cutting teeth and recessed shoulders. Its active tracing point is anchored to the programmed tool position. In the standard lathe view, the external P8 vertex points down and the internal P6 vertex points up.

Only the insert diameter scales this silhouette. The reference contour is D12; entering D20 scales every coordinate by `20 / 12`, approximately 1.667. EX, RC and the thread profile angle do not deform the displayed body. The angle remains part of the removal calculation but is hidden in the editor; the library summary shows the tracing orientation. These display changes do not rewrite SQLite tool records.

### Does Stock Removal detect machine collisions?

Turning CPU Stock Removal detects intersections of the existing tool silhouette with remaining stock throughout G0 movements. The intersected material is marked red without being removed. Marks persist after the tool leaves, disappear where later G1/G2/G3 machining removes the affected material, and follow playback/TrackBar history. Already removed material, bores and gaps remain clear; boundary-only contact is ignored. A new simulation starts with no marks.

This check covers the configured cutting tool and the sampled turning stock section. It does not model holders, chuck, turret, fixtures, acceleration or full machine geometry. Milling GPU Stock Removal is unchanged.

---

## Statistics and Tokens/Variables

### What does Toolpath Statistics contain?

Open **CNC Functions → Statistics**. The inspector is under **CNC Functions → Tokens/Variables**; it is no longer in Settings.

Statistics are derived from the resolved trace and include:

- logical motion counts;
- length breakdown;
- known and unknown machining time;
- average feed;
- assumed rapid speed;
- XYZ bounds;
- per-tool sections.

The Statistics window displays an HTML summary. Use the tool selector to switch between the whole program and one tool. Export HTML saves the summary and all tool sections with the same selector and the current display units. Only the exported report adds a static SVG projection below the table: XY for milling, XZ for turning. The tool selector also filters the drawing. The GUI export uses the same prepared geometry, page fitting and line styles as Print. Every motion is included. The NC source is not embedded.

The Inches display switch converts displayed values without changing stored physical geometry. CLI equivalent: `python -m app analyze program.nc --html statistics.html` (add `--inches` for imperial display).

### Why can machining time be UNKNOWN?

The kernel avoids fabricating a physical feed rate. A common case is feed-per-revolution motion without a known spindle RPM.

### What is the Tokens tab?

Tokens displays parsed/evaluated words, source position, execution status and diagnostics. Warning rows are orange and error rows are red. Double-click a diagnostic row to read the full source block and message in a dialog; rows without diagnostics do not open it. The table can also be exported to CSV.

The leading columns are **Ln, Raw, Support, Action, Valid**; the remaining columns retain their previous order. Support and diagnostics are therefore beside the source instead of beyond the token/address columns. Native Klartext words and Siemens parameter assignments are displayed directly, without converting them into FANUC tokens. CSV follows the same column order.

Above the table, **All / Warnings / Errors** selects row severity. The **Rows: shown / total** counter is in the lower-left footer, aligned with the buttons. The search field on the right matches source text, words and diagnostics, for example `T1 M6`, ignoring case and repeated whitespace. It keeps matching rows rather than the entire machining section for that tool. Both filters operate on the loaded table without recalculating the program. Clear the search with its clear button; copying and CSV export include visible rows only. **Refresh** reloads the current document analysis and preserves the chosen filters.

Opening Tokens, switching back to its tab and pressing Refresh reuse the active document's existing execution result when the source and calculation settings are current. A new analysis is requested only when there is no current result or it is stale. Opening the inspector during an active calculation does not start another calculation or cancel the running one. Variables continues to use playback snapshots.

### What is the Variables tab?

Variables displays the captured variable state at the current logical playback position for the active controller:

- **FANUC Lathe/Mill:** numbered `#1` variables and named `#<NAME>` variables, including recorded G65 local scopes and caller restoration after M99.
- **SINUMERIK:** `R0`, `R1`, etc. and supported declared/named variables; Macro B identifiers in mixed input remain explicitly prefixed with `#`.
- **HEIDENHAIN iTNC 530:** `Q`, `QL` and `QR` identifiers as captured by native execution, without FANUC prefixes.

The context above the table identifies the dialect, physical source line and execution occurrence. Numbered families sort numerically, so Q2 precedes Q10. Columns are **Variable / Value**, and CSV uses the displayed controller-specific identifiers. At program end the final captured state is shown; an assignment-only program can show its last executed state even without toolpath motions. Undefined captured values are labeled explicitly. These are recorded values from the supported executor, not live controller memory or a claim of full controller-variable coverage.

The inspector uses existing execution snapshots and does not re-run the CNC program while the playback slider moves.

### Why can Variables be unavailable?

If no execution result exists, there is no variable history to show. If the source or execution settings have changed, update the toolpath first; Refresh only rereads the variable snapshots. A valid position without recorded variables is reported explicitly rather than displaying unrelated values from another dialect or document.

---

## Export

**Five-axis FANUC ↔ SINUMERIK conversion is supported experimentally and may contain errors. Use the generated NC program entirely at your own risk.** Successful export or a clean Tokens table does not guarantee correct or collision-free machining. Before running on a machine, independently verify the target controller/post, machine kinematics, WCS, tool numbers and length offsets, compensation, rotary branches, and approach/retract moves; check the output in a suitable machine simulation and perform a controlled dry run. OEM CYCLE800 retract paths and a complete physical machine are not modeled.

Indexed 3+2 frame conversion covers **5Ax Table AC**, **5Ax Table BC**, **5Ax Table AC Angled** and **5Ax Table BC Angled** with `fanuc_mill_multiaxis` / `sinumerik_840d_multiaxis`, using absolute output. Supported TCP conversion uses the configured AC/BC subset. Tilted-plane output retains G54–G59 selection and lists required work offsets in comments; configure the same offsets on the target. Named SINUMERIK tools retain their source identities; the GUI asks for distinct FANUC T1–T99 slots and emits the mapping in comments. Verify the corresponding H offsets in the target tool table. Explicit nonzero G53/SUPA targets remain explicit. Unverified geometry and unsupported combinations still reject.

**G41/G42 cutter-radius compensation:** EXPANDED does not output G41/G42 commands; bundled milling posts output G40. Before five-axis conversion, disable cutter compensation in **Options** to avoid compensation calculation/export errors. With compensation disabled, the exported path is the contour without cutter-radius compensation, not a compensated tool-center path; check the machining result independently. This instruction concerns radius compensation, not tool-length H/D offsets. Correct output for five-axis conversion with cutter compensation enabled is not guaranteed.

### Which GUI export families exist?

The program has three NC/geometry export families:

- **FULL** — source-preserving NC normalization;
- **EXPANDED** — resolved geometry/state through a controller post profile;
- **DXF** — toolpath geometry.

Tool List and Statistics reports are separate report exports, not NC export modes.

### Are exporters separate G-code interpreters?

No. FULL uses the exact source together with its authoritative execution map. EXPANDED and DXF consume resolved execution geometry/state. None of them runs a second CNC interpreter.

### What does Full Program mean?

FULL preserves ordinary source blocks, comments, modal commands, controller dialect and supported cycles. FANUC flow/label-dependent constructs are unfolded from the execution map before renumbering: evaluated Macro B, IF/GOTO/WHILE, G65 and M98/M99 calls, and turning G70–G76. Supported native SINUMERIK milling expressions and WHILE/GOTO/IF flow remain in the source; numeric jump labels are preserved and sequence renumbering is rejected for programs with native jumps. HEIDENHAIN and SINUMERIK turning FULL normalization are unsupported; use Save/Save As to retain those sources. FULL does not convert the program to another controller.

### What does Expanded Execution mean?

EXPANDED is the controller-conversion path. One generic postprocessor emits resolved geometry and machine state through a JSON profile. Cycles, variables and subprogram flow have already been executed. Target profiles define syntax, mandatory frames, capabilities and defaults; they do not disable user output options.

Bundled profiles are `fanuc_mill`, `fanuc_mill_multiaxis`, `fanuc_lathe_a`, `fanuc_lathe_b`, `sinumerik_iso`, `sinumerik_840d`, `sinumerik_840d_multiaxis` and `heidenhain_itnc530`; an external JSON path can be supplied with `--post-profile`. The `*_multiaxis` profiles declare `supports.axes` `X/Y/Z/A/B/C` and emit explicit resolved rotary coordinates; the three-axis profiles stay XYZ-only and still reject rotary geometry.

Supported tilted-plane output retains G54–G59 and requires matching target offsets; other displaced-WCS indexed cases remain rejected as `UNSUPPORTED_INDEXED_WCS_EXPANDED_EXPORT`. TCP arc subdivision distributes ABC with XYZ; G91 rotary output avoids cumulative rounding drift. With a custom G93-capable profile, subdivision preserves the original block duration and restores the source feed for later motions. Unverified compensation and ignored native geometry-changing commands return `UNSUPPORTED_UNVERIFIED_GEOMETRY_EXPANDED_EXPORT`, including the concrete execution diagnostic codes.

### What does Auto (source controller) mean?

`Auto (source controller)` is not a separate capability mode. FANUC turning uses the selected Type A/B lathe profile, FANUC milling uses `fanuc_mill`, SINUMERIK ISO-M milling uses `sinumerik_iso`, native SINUMERIK milling uses `sinumerik_840d`, and HEIDENHAIN uses `heidenhain_itnc530`. SINUMERIK turning currently falls back to the selected FANUC Type A/B lathe post because no Siemens turning output post is bundled; it does not preserve the source controller. EXPANDED always re-serializes the resolved execution and remains subject to export preflight restrictions.

### How do I manage user postprocessors in the GUI?

Open **Settings / Postprocessors** to create or edit a post. The list is on the left and the editor is embedded on the right. The buttons below the list add a copy, save, rename and delete. Built-in profiles are read-only. A new copy stays in memory until **Save** or settings **OK**; **Cancel** discards unsaved changes. Switching profiles offers Save, Discard and Cancel.

The editor contains **Source**, **Output**, **Format**, **Sequencing**, **Motions**, **Home**, **Cycles**, **Commands**, **Program** and **Supports**. Format controls general number settings. In Sequencing, drag address tiles to change output order and select a tile to set its precision, sign and repetition. Custom arc split angles, including 5400 degrees, are displayed without substitution.

**Save** validates the whole post through the same loader used by CLI export and atomically replaces its managed JSON. Errors leave the editor open and preserve the previous file. Profile saves take effect independently of the outer Settings dialog's OK/Cancel.

In **Export Options / EXPANDED EXECUTION**, choose **Target CNC** or use **Add ready…** to import a validated JSON for the current machine type. Import copies it into the configuration directory’s `post-profiles` folder and preserves the original. Profile editing and management stay in Settings; renaming retains the path and controller `id`.

The bundled `heidenhain_itnc530` is an EXPANDED output target, separate from the native input parser and milling runtime. It emits `BEGIN/END PGM`, `TOOL CALL`, `L/FMAX`, `CR`, `CC` with `C/CP`, cycles 200/201/202/203/207 and rapid XYZ machine returns with `M91`. IPA and DR use matching signs; Q239 is negative for left-hand tapping. G85 uses cycle 201 with feed retraction, while G86 uses cycle 202 with stopped-spindle rapid retraction. Arcs outside the spindle plane in TOOL CALL are linearized at the export tolerance. Numeric sequence prefixes omit `N`. Unsupported rotary/TCP operations and cycles are rejected before writing. Export capabilities do not imply corresponding iTNC input execution coverage; see [the input coverage table](#what-heidenhain-support-is-included).

Export passes the selected JSON path through the same writer as CLI `--post-profile`, including its output extension. Selections persist by identifier/path. Missing, damaged or incompatible profiles require choosing Auto or another valid profile explicitly. Profile selection is disabled for FULL and DXF. Cancel in Export Options discards output options and the temporary selection; separately saved profiles remain available.

### How does Modal Feed work?

`Modal Feed` controls whether `F` is restated: **Yes** emits `F` only when the feed or feed mode changes, **No** restates `F` on every cutting motion.

### Can I choose formatting options when converting to a specific controller?

Yes. EXPANDED treats Target CNC as the target syntax/post profile, not as a capability switch. Coordinates (G90/G91), sequence numbers, delimiter, leading zero, modal feed, decimal precision, force decimal, plus sign, arc output and start/end program text remain available and are honored for FANUC → FANUC, FANUC → SINUMERIK ISO, FANUC → SINUMERIK native and SINUMERIK → FANUC. A profile default applies only when you did not choose a value. If a profile declares a mandatory prefix (for example `G290`/`G291`), that prefix stays physically first and your start text follows it. A profile is only consulted for genuine capability limits: rotary/TWP/TCP, a missing axis or an unsupported arc/feed state.

### What does DXF contain?

DXF contains the available resolved motion geometry. Rapid and cutting motions use separate layers. Turning uses the plot-aligned Z/X representation; milling writes 3D lines and analytical arcs/circles where representable, with sampled polylines for geometry that cannot be represented as one DXF arc.

### Does DXF parse the G-code again?

No. The DXF writer consumes motion geometry and does not interpret controller words or NC formatting options.

### Which NC formatting options exist?

Shared export options include:

- absolute/incremental coordinates where supported;
- sequence numbers;
- sequence start and increment;
- sequence-number spacing;
- spaces/no spaces between words;
- leading zeroes (`G01` versus `G1`);
- comments/no comments;
- safety line (the profile's declared safe restart block);
- decimal precision, force decimal and plus sign;
- start and end program text;
- milling arc representation.

For EXPANDED these options are user-owned: the target profile supplies syntax and a default only for values you do not set. A profile-defined mandatory frame stays first and your start text follows it.

### How does a post profile control word order and mandatory addresses?

The profile's `format.words` object gives every frame token an `order` and a `required` flag: `motion`, `X`, `Y`, `Z`, `A`, `B`, `C`, `I`, `J`, `K` and `R`. `required=true` emits the address whenever it has a resolved value (for example `Y0` instead of omitting zero `Y`); `required=false` allows the serializer's normal omission of an unchanged value. `motion.required=false` makes the motion code modal, so `G1` is restated only when the motion changes. Per-word `decimals`/`sign` are stored in the same object. An axis entry is only accepted when that axis is declared in `supports.axes`, and `F` is deliberately excluded because feed is controlled by Modal Feed. Address requiredness is a property of a specific post/controller, so it lives only in the profile and has no separate GUI/CLI switch.

The postprocessor editor exposes this ordered list on **Sequencing**. Drag the address tiles to change the stored order; selecting a tile opens its formatting controls below the sequence.

Additional arc controls live under `format`: `turnsWord`, `radiusSplitAngle`, `arcSplitAngle` and `fullCircle`. Capability declarations under `supports` include `axes`, `inverseTime`, `multiTurnArcs` and `absoluteArcCenters`. A request beyond the selected post's capabilities returns `UNSUPPORTED` instead of writing partial NC. Three-axis posts reject rotary/TWP/TCP geometry; select an appropriate multiaxis post for the supported indexed/TCP subset.

### Which milling Expanded arc output modes exist?

The CLI contract exposes:

```text
auto
ijk-relative
ijk-absolute
radius
linearized
```

`auto` uses the post profile convention. The four explicit modes are relative IJK, absolute IJK, radius and linearized. Source arc syntax has already been resolved before posting. Native SINUMERIK profiles render absolute centers as `I=AC(...)` / `J=AC(...)` / `K=AC(...)` and radius arcs as `CR=`.

### What happens when a full circle is exported in R mode?

It is emitted as two exact semicircular R arcs.

### Can Expanded NC be converted between millimetres and inches?

Yes. Unit conversion is applied to resolved geometry/state at the postprocessor boundary. Coordinates, arc geometry, I/J/K or radius output, feeds and supported controller state are emitted in the requested units and replay-tested by the export suite.

FULL remains source-preserving and therefore accepts only `--units auto`.

### Can Full Program be forced to mm or inch?

No. CLI Full Program export currently accepts only `--units auto`.

Semantic unit normalization is an Expanded Execution feature.

### What units does DXF use?

DXF can be emitted in millimetres or inches. `auto` keeps the current default DXF behavior, which is millimetres.

### Can comments be removed from export?

Yes. `--no-comments` removes source comments from FULL and suppresses source comments carried into EXPANDED. EXPANDED comment syntax comes from the selected post profile.

### Are exports written atomically by the CLI service?

Yes. The CLI export service writes to a temporary file in the output directory and then replaces the final output path. A failed write does not intentionally leave a partially written final file.

### Can CLI export overwrite the source file?

No. Source and output must be different paths.

### Can CLI export be compared directly with an expected NC file?

Yes. Add `--compare-with FILE` to single-file NC `export`, in either FULL or EXPANDED mode:

```powershell
.\easy_gcode_plot_cli.exe export source.nc --lang fanuc_mill --post-profile sinumerik_840d -o actual.mpf --compare-with expected.mpf
```

The CLI compares the actually generated output with the UTF-8 reference. LF and CRLF line endings are treated equally; spaces, comments and the final newline are compared. Exit code `0` means a match, `1` means a mismatch, and `2` means an export or file error. A mismatch prints a unified diff on stdout, with the reference first (`---`) and generated output second (`+++`), without timestamps. The generated file is retained; the reference cannot be the output destination and is never overwritten. This option is not available for DXF or `batch-export`.

This is a direct text regression check. Execution/replay tests remain the check for machining-semantic equivalence when different NC text can represent the same operation.

---

## SINUMERIK 840D input

**Options > General > 840D Extended cycles** selects the cycle interface for native input and native EXPANDED output. Checked (default): the Siemens 03/2009 interface, CYCLE81/82/83/84 with 9/9/20/24 parameters. Unchecked: the classic 01/2008 interface with 5/6/17/21 parameters. Short compatible calls remain accepted; 840D Extended cycles signatures in classic mode produce diagnostics. Changing the setting re-executes the current program. This selection does not change G290/G291 or the rotary-kinematics profile; the installed cycle package, rather than the platform name alone, determines compatibility. CLI uses `--sinumerik-cycles classic|sl`; native post JSON stores both sets in `cycleProfiles.classic_0108` and `cycleProfiles.sl_0309`.

The unchanged [ext_cycles.mpf](tests/fixtures/milling/sinumerik/ext_cycles.mpf) and [no_ext_cycles.mpf](tests/fixtures/milling/sinumerik/no_ext_cycles.mpf) now execute completely in their selected profiles, including deep/left tapping and CYCLE85/86/87/89. Native M19 emits a spindle-orientation signal.

Arc-center interpretation follows the executed controller mode: native and ISO-M (`G291`) use incremental IJK centers; native I=AC/J=AC/K=AC explicitly selects absolute centers. Mixed `G290/G291` input resolves each arc in its active mode; document arc settings and automatic detection do not override these semantics. Configured native rotary axes are supported by the bounded TCP/indexing subset; rotary A/B/C in G291 remains rejected.

Structured execution and CLI/batch reports include `source_dialect` (`fanuc` or `sinumerik`) independently of the shared `fanuc_mill` geometry language. This identifies the source family, not one controller mode for the entire mixed program. Unsupported SINUMERIK G/M diagnostics contribute concrete codes to batch summaries; unsupported syntax and features do not become fabricated G/M entries.

The SINUMERIK scope includes **native CAM trajectories and bounded parametric programs**: R arithmetic, WHILE/ENDWHILE and numeric-label GOTO/IF GOTO. This is a documented subset of the Siemens language; arrays, system variables and arbitrary subprogram calls remain unsupported. Executing subprograms from SDI mode is currently unavailable. Opening an SPF file is supported as a document, but arbitrary Siemens subprogram invocation is not.

MPF/SPF documents preserve the selected rotary profile. Settings and Options remain available. Native CYCLE800/TRAORI supports the angled AC/BC table profiles; incompatible profiles, axes and ISO-M rotary commands produce kernel diagnostics.

### What SINUMERIK support is included?

The application supports bounded native Siemens milling and turning subsets (`G290`, also the initial mode of MPF/SPF files). `G291` selects ISO Dialect M in milling and a bounded ISO Dialect T subset in turning. Both publish the shared resolved trace; see the turning coverage below.

The table and native/ISO-M transition, cycle and TCP rules below describe **milling**. Turning diameter modes, M-code policy and cycle restrictions are described in [SINUMERIK lathe coverage](#is-sinumerik-lathe-supported); milling capabilities do not carry over automatically.

| Native function | Current behavior |
| --- | --- |
| `G0/G1`, `G2/G3`, `G17/G18/G19` | XYZ positioning, linear moves and arcs in the selected plane; `CR=` radius arcs, including negative radius for a major arc |
| `G90/G91`, `G54`–`G59` | Absolute/incremental coordinates and work offsets |
| `G70/G71` | Inch/metric lengths; feed units remain unchanged |
| `G700/G710` | Inch/metric lengths and feed units; modal numeric F is retained |
| `G93` | Inverse-time feed: each cutting motion takes 1/F minutes, including rotary TCP motion; F must be positive. Reprogram F when switching G93/G94/G95. Cycles and cutter compensation are unsupported in G93 |
| `G40/G41/G42` | Modeled cutter-radius compensation using the configured tool |
| `DIAMON/DIAMOF/DIAM90` | Warning-only; all coordinates are executed with DIAMOF semantics |
| `CHR/RND` | Nonmodal chamfer side length / rounding radius between continuous planar G1 elements, before cutter compensation. Fixed rotary and tilted working planes use local coordinates; the selected profile alone does not change a three-axis contour. Adjacent elements must share their plane, tool and compensation mode |
| `CHF/RNDM/FRC/FRCM` | Parsed with warnings without geometry/feed changes. Modal rounding and corner feed are not simulated. RNDM=0 has no geometric effect; ignored-word warnings block resolved NC export |
| `G60/G64` | Exact-stop / continuous-path metadata; acceleration, stop time and blending are not simulated |
| `G500` | Modal work-offset deactivation with coordinate rebasing; zero G500/base frame by default, API `wcs_offsets[500]` can supply translation; OEM base-frame rotations, mirroring and scaling are not modeled |
| R assignments and address/cycle expressions | Bounded `+ - * /`, parentheses, comparisons and `SIN/COS/ABS/SQRT`; trigonometry in degrees; separate Siemens R state |
| `WHILE/ENDWHILE`, `GOTO N...`, `IF condition GOTO N...` | Nested loops and numeric-label jumps with shared execution/iteration limits and cancellation; invalid flow stops with source-line diagnostics |
| `M19` | Spindle-orientation signal without motion or a spindle-state change |
| `G96/G961`, `G97/G971` | CSS or RPM with per-revolution/per-minute feed respectively; CSS retains surface speed without inferring milling RPM |
| `ANG`, `SCALE/ASCALE`, `MIRROR/AMIRROR` | Recognized but geometry is unmodeled; execution stops before motion |
| `DEF REAL`, direct named-scalar assignments | Bounded underscore-named `DEF REAL` scalars used by CAM setup and direct numeric/R/scalar assignments are accepted; compound named-scalar assignments remain unsupported |
| `T`, `M6`, `D0..D12`, `S`, basic M codes | Tool change, modeled cutting-edge selection/cancellation, spindle and coolant signals; controller-specific offset tables are not simulated |
| Named tools with `M6` | Named tool changes are accepted; if cutter geometry is unavailable, `G41/G42` remains unverified rather than assuming a radius |
| `G0 SUPA ... D0` | Nonmodal absolute XYZ and configured A/B/C positioning, independent of G91. In the application's reference-coordinate model, zero XYZ addresses use the configured G28/SUPA return coordinates, as FANUC G53 does. WCS and the current rotary frame determine the displayed return. Rotary zero means A/B/C=0; `SUPA G0 B0 C0 D0` requires a compatible BC profile |
| `G64`, `MSG(...)`, `WORKPIECE(...)`, `;` comments | Path-control/display metadata and comments; no blending or stock geometry is generated from these declarations |
| `SETMS(1)`, `FNORM`, `COMPOF`, `CYCLE832` | Accepted CAM setup/control statements; `CYCLE832` is ignored without geometry or display events |
| `MCALL CYCLE81/82/83/84/85/86/87/89(...)` | Modal Z drilling/tapping in `G17/G40`, triggered by subsequent XY blocks; bare `MCALL` cancels the cycle |
| `CYCLE81/82` | Drilling and rapid return, with modeled seconds-based dwell for `CYCLE82`; safety plane is `RFP + SDIS`, return plane is `RTP`; the four-argument `CYCLE81` form is accepted |
| `CYCLE83` | Modeled first depth, amount degression, minimum peck depth, chip-breaking/full-retract options and reentry clearance |
| `CYCLE84` | Metric right/left tapping in G94, including VARI=1/2, DAM/VRT and balanced final pecks; explicit PIT and equal SST/SST1 matching S. SDAC=3/4/5 is retained. |
| `CYCLE85/86/87/89` | Separate reaming feeds; oriented fine-boring clearance; spindle/operator stop; feed-return boring with dwell. |
| `POCKET3/POCKET4` | Classic 01/2008 positional interface: 17–23 / 14–19 arguments; rectangular/circular pockets, roughing or finishing, allowances and supported VARI entry strategies. Preformed-blank AP1/AP2/AD variants and extended signatures are diagnosed |
| `HOLES1/HOLES2` | Six positional arguments; row/circle positions execute the active supported MCALL drilling cycle in G17 without TCP. HOLES1 starts from the nearer row end; HOLES2 accepts omitted/zero INDA for equal spacing |
| `CYCLE90` | Classic 13-argument thread milling; internal/external TYPTH variants, explicit pitch, G2/G3 direction and analytic multi-turn helices |
| `TRAORI` / `TRAFOOF` | GUI/CLI/kernel TCP via the common angled AC/BC table core; G0/G1/G2/G3 with configured numeric A/B/C and R references; incremental IC supported; `DC` selects the shortest absolute rotary approach, while an exactly 180-degree ambiguity is rejected |
| `CYCLE800` | GUI/CLI/kernel static frames: modes 57/54/39/27/30/45, ST0/1/200000/200001/220000/220001, DIR-1/0/1; 14/15/16-argument calls and legacy R_DATA setup are accepted; active-frame reset via empty/bare call or TC="0" |
| `CIP` | Spatial circle through the start, intermediate I1/J1/K1 and end points, independent of G17/G18/G19. G90/G91 and explicit AC/IC intermediate coordinates are supported. Fixed frames and G40 are required; concurrent rotary motion is rejected. Plot/Playback retain the circle; EXPANDED emits G1 chords within the configured linearization tolerance. |
| `TRANS/ATRANS`, `ROT/AROT`, `RPL=` | Programmable rigid frames: replacement/reset or composition in local axes, preserving physical tool position. Spatial rotation uses RPY (MD10600=1); RPL rotates in the active plane. Combination with active TWP/TCP, polar mode, cycles or cutter compensation is rejected |
| `G505`–`G599`, `G601/G641/G642/G645` | Parsed with unverified warnings; their controller-specific effects are not simulated |
| Unknown auxiliary M codes | Non-blocking `UNSUPPORTED_M_CODE` warnings; motion and known commands in the same block still execute. M2/M30 end programs. Native M17/M96/M97/M99 stop with unsupported-flow diagnostics; M66/M98 warn without subprogram dispatch |

POCKET3/4 and CYCLE90 require G17, G40, G80, feed per minute, no active MCALL and a configured milling cutter diameter through `milling_tools`/`tool_resolver`. TCP, polar and CIP combinations are outside this subset. These calls use the classic 01/2008 signatures regardless of the extended drilling-cycle selector; newer signatures are not silently reinterpreted. Short examples are in [`sinumerik/cycles/`](tests/fixtures/milling/sinumerik/cycles/). Their internal pass sequences have not been independently confirmed against a controller trace.

Unsaved editor text selects native SINUMERIK when executable commands such as SUPA, CIP, MCALL, TRANS or CYCLE800 are present. Comments and quoted strings do not select a dialect; Undo/Redo updates the selection. Named files retain their extension-based source contract.

`D0` cancels cutting-edge selection; `D1` through `D12` select an edge while retaining nominal tool geometry. Edges above D1 report `UNVERIFIED_SINUMERIK_EDGE_OFFSETS` because controller offset tables are unavailable. CYCLE800 ST220000/220001 computes a new/additive frame without indexing. The `DMG` frame-only data-set name is accepted on **5Ax Table BC Angled** with FR0; OEM indexing remains unsupported.

Programmable `TRANS`/`ATRANS` and `ROT`/`AROT` affect subsequent XYZ geometry relative to the active WCS. `TRANS` and `ROT` replace all programmable frame components; bare `TRANS` or `ROT` resets the frame. `ATRANS` adds a translation in the current local axes; `AROT` adds a local rotation and preserves translation. Changing the frame rebases program coordinates without moving the physical tool. Spatial XYZ angles use the default Siemens RPY order Z → Y′ → X″ (MD10600=1), regardless of address order in the block. Machines configured for Euler order are outside this policy. `RPL=` rotates in the active plane about +Z (G17), +Y (G18) or +X (G19). Each command requires a separate NC block and accepts numeric values, direct R references or supported named scalars; general expressions are not added. Active TWP/CYCLE800, TCP, polar mode, cycles and cutter compensation cannot be combined with these commands. SCALE/ASCALE and MIRROR/AMIRROR remain unsupported. FULL preserves frame commands; EXPANDED resolves their effect into output coordinates and linearizes arcs whose physical plane cannot be represented by the selected standard plane.

Native CR radius arcs require a SINUMERIK source document: use .mpf/.spf, or unnamed text detected by executable native commands. A named .nc document retains FANUC syntax. Native X/Y/Z=IC(...) is incremental independently of G90/G91. MSG() is accepted.

`CYCLE84` accepts the 24-argument CAM call and shortened numeric declarations. Depth uses `DP` or positive relative `DPR` in compatibility mode; absolute-depth `AMODE=2/1001002/1002002` requires `DP`. Metric right/left tapping and deep tapping (`VARI=1/2`, `DAM`, `VRT`) are modeled. `MPIT`/thread tables, nonmetric pitch units, spindle orientation/technology options and unequal entry/withdrawal speeds produce diagnostics. Spindle synchronization/reversal uses logical signals without angular spindle simulation. Parameters follow the [Siemens Cycles manual](https://cache.industry.siemens.com/dl/files/633/109443633/att_829767/v1/PGZ_1106_en.pdf). Paired fixtures verify tapping geometry and native trace replay.

Cython accelerates contiguous literal position runs, with per-block capability validation before state changes. Controller-specific declarations and G290/G291 switches interrupt the current run, after which eligible positions resume acceleration. Positions inside an active MCALL cycle stay on the Python reference path until cancellation. Metadata or a native cycle elsewhere in the file does not disable acceleration for the whole program.

R assignments, address values and supported cycle parameters accept bounded arithmetic (`+ - * /`), parentheses, comparisons and `SIN/COS/ABS/SQRT`. Trigonometry uses degrees. Siemens R state is independent of FANUC `#` variables and is fresh for each execution. Undefined references, malformed expressions, invalid domains and division by zero fail closed. Native `WHILE/ENDWHILE` supports nesting; `GOTO N...` and `IF condition GOTO N...` use numeric sequence labels. Missing/duplicate targets and unmatched loops produce source-line diagnostics. Shared execution, iteration and cancellation limits apply. Directional `GOTOF/GOTOB/GOTOC`, `RET`, arrays, system variables and arbitrary subprogram calls remain unsupported; SPF recognition does not enable subprogram execution.

Native `M19` emits a spindle-orientation signal without moving the tool or changing spindle state. `G96/G961` enable CSS with revolution/linear feed respectively; `G97/G971` select RPM with revolution/linear feed. CSS retains programmed surface speed without inferring an instantaneous RPM from a milling X coordinate. FULL preserves supported native expressions and flow; EXPANDED exports resolved geometry, but rejects CSS without a reliable reference axis. `ANG`, `SCALE/ASCALE` and `MIRROR/AMIRROR` are recognized but their geometry is unmodeled, so execution stops before motion. Native `M17/M96/M97/M99` flow is unsupported; `M66` and `M98` retain explicit auxiliary warnings, and native M98 never enters FANUC subprogram dispatch.

Native `TURN=n` adds integer 0..999 complete revolutions to the base `G2/G3` arc (IJK or CR, G40, no active MCALL), according to [Siemens](https://support.industry.siemens.com/cs/attachments/104985512/802Dsl_BPF_1006_en.pdf). The trace keeps one analytical arc/helix with the total sweep. Rendering, playback and statistics retain those turns; DXF uses a sampled polyline, and FANUC/ISO exporters split arcs only during serialization. Stock removal supports turning and, since 2.0.0, three-axis milling with vertical cutters. Standalone native `G4 F...` uses seconds and leaves modal feed unchanged; spindle-revolution dwell is not modeled.

The GUI/CLI/kernel also supports a bounded TRAORI/TRAFOOF TCP subset on **5Ax Table AC Angled** and **5Ax Table BC Angled**. Configured numeric A/B/C assignments and direct R references follow G90/G91; rotary TCP arcs retain analytical Cartesian geometry and orientation endpoints. The GUI preserves rotary selection and executes native AC/BC programs through the same kernel. CYCLE800 builds its own Siemens rotation matrix and uses the common TWP solver/rebasing. FR0/1/2 are logical retract requests, with no OEM retract trajectory; FR_I must be zero/blank and DMODE0/1 is supported. DIR chooses the principal first-table-joint branch. IC(numeric/direct R) is incremental independently of G90/G91. ORI*, FGROUP, FL[], FGREF[], SPOS, CUT3DC/CUT3DF/CUT3DFF and path-control extensions are parsed with unverified warnings; their effects are not simulated. Arbitrary Siemens subprogram calls remain fail-closed. Cancel TCP before G290/G291; active TCP transitions are rejected. Native MCALL and G41/G42 cannot be activated under TCP, and active MCALL must be cancelled before rotary positioning. The bundled multiaxis posts reconstruct configured indexed A/B/C, verified **4-axis Table C** continuous motion and the supported AC/BC TCP subset across FANUC and SINUMERIK. Supported G68.2/G53.1 and CYCLE800 indexed AC/BC frames can be converted experimentally through the bundled multiaxis posts; other frame combinations remain rejected.

EXPANDED profiles are tested by re-executing output and comparing geometry, feeds and machine signals. FULL preserves the source dialect.

In `G291`, common integer milling G codes, unit selection, coordinate systems, selected canned cycles and `G50/G51` are accepted. Extended work offsets use `G54 P1..P48`; source `G54.1` and other decimal G codes are rejected, though `G54 Pn` is normalized internally to the milling kernel's `G54.1 Pn` form. Ordinary `G91` incremental positioning is supported. G68 is limited to a standalone 2D form with `G90` active, only the center axes of the active plane and `R`, and no `I/J/K`; incremental-angle and 3D-vector forms are rejected. `G69` is supported. Macro B flow and unsupported ISO functions stop with diagnostics. `G51` uses the modeled `P/1000` scale weighting; machine-specific alternative weighting is not modeled.

`G290` selects the native subset above; `G291` selects ISO-M. Switches must occupy standalone blocks. Cancel native cutter compensation and `MCALL` before `G291`; cancel incompatible ISO cycles, transforms and extended offsets before `G290`.

### How are MPF and SPF files detected?

The GUI Open/Save filters include `.mpf` and `.spf`. The CLI and batch scanner include both extensions by default and select SINUMERIK for every `.mpf`/`.spf` file independently of its contents; execution starts in native mode and processes standalone `G290/G291` switches. Use `--lang fanuc_mill` for milling analysis; the language option selects the milling geometry model and does not turn on full Siemens support. Mixed folders can still use `--extensions` to control discovery.

### Can FANUC milling programs be converted to SINUMERIK?

Yes. Choose **EXPANDED EXECUTION** and the target controller. The postprocessor consumes resolved kernel geometry; `sinumerik_iso` emits ISO-M with G291, and `sinumerik_840d` emits native with G290.

```powershell
.\easy_gcode_plot_cli.exe export fanuc_part.nc --lang fanuc_mill --mode expanded --post-profile app\gcode\export\posts\sinumerik_iso.json -o iso_part.mpf
```

### Can SINUMERIK native milling programs be converted to FANUC?

Yes. Parameters and CYCLE81/82/83/84 have already been executed by the kernel. EXPANDED reconstructs representable drilling/tapping operations through the target post's cycle templates; other supported operations retain resolved motions, feeds, dwell and machine signals. Source MCALL syntax is replaced by the target controller's cycle syntax. The three-axis `fanuc_mill` profile rejects rotary/TCP geometry; `fanuc_mill_multiaxis` can reconstruct configured indexed A/B/C, verified **4-axis Table C** continuous motion and the supported AC/BC TCP subset. Supported G68.2/G53.1 and CYCLE800 indexed AC/BC frames can be converted experimentally through the bundled multiaxis posts; other frame combinations remain rejected. Unverified geometry-changing commands remain rejected.

```powershell
.\easy_gcode_plot_cli.exe export native_part.mpf --lang fanuc_mill --mode expanded --post-profile app\gcode\export\posts\fanuc_mill.json -o fanuc_part.nc
```

### How do Full Program and Expanded Execution differ?

**FULL** answers “keep this controller program, but normalize it safely” for supported FANUC and SINUMERIK milling sources. HEIDENHAIN and SINUMERIK turning FULL normalization are unsupported. It preserves ordinary source structure and the source controller/dialect; FANUC execution-flow constructs that cannot safely survive renumbering are unfolded. Supported native SINUMERIK expressions and WHILE/GOTO/IF remain intact; native jump labels are preserved and sequence renumbering is rejected.

**EXPANDED** answers “emit this resolved execution for this controller.” It serializes resolved geometry/state through one of the JSON post profiles. Three-axis profiles remain XYZ-only; bundled multiaxis profiles additionally reconstruct the verified rotary/TCP subsets. Ordinary paths use a zero-offset G54 frame; supported tilted-plane programs retain G54–G59 with matching target offsets; supported milling drilling/tapping operations are emitted through the post cycle templates when representable. Other operations retain their resolved motions; macro variables and subprogram calls are not recreated.

```powershell
.\easy_gcode_plot_cli.exe batch-export C:\Fanuc --lang fanuc_mill --mode expanded --post-profile app\gcode\export\posts\sinumerik_iso.json -o C:\SiemensISO
.\easy_gcode_plot_cli.exe export native_part.mpf --lang fanuc_mill --mode full -o normalized.mpf
```

GUI and CLI use the same FULL / EXPANDED / DXF split. Target-controller selection belongs to EXPANDED. Three-axis posts reject rotary/TCP geometry, while the bundled multiaxis posts reconstruct configured indexed A/B/C, verified **4-axis Table C** continuous motion and supported AC/BC TCP. Supported G68.2/G53.1 and CYCLE800 indexed AC/BC frames can be converted experimentally through the bundled multiaxis posts; other frame combinations remain rejected. A selected kinematics profile by itself does not make an XYZ-only program multi-axis. DXF is an independent geometry output and has no NC post profile.

### Is SINUMERIK lathe supported?

**Yes, within the native XZ turning subset.** `.mpf/.spf` select the SINUMERIK container and start in G290. Turning signatures (`DIAMON/DIAMOF/DIAM90`, `CYCLE93/95/97`) select turning automatically; otherwise choose turning in the GUI or `--lang fanuc_turn` in the CLI. Standalone G290/G291 switches preserve the tool, position and WCS. G291 uses the selected A/B turning code system; native syntax is rejected until G290 resumes.

Native coverage includes G0/G1/G2/G3, G18, G33 with I/K lead, CR arcs, IC/AC coordinates, DIAMON/DIAMOF/DIAM90, G70/G71 and G700/G710, G90/G91, G94/G95, G96/G97 with LIMS, numeric T and logical D selection, G40/G41/G42, G53/G153/SUPA, G54–G59/G500, TRANS/ATRANS XZ, scalar expressions and supported WHILE/IF/GOTO flow. Public X coordinates remain diameters; arc I and TRANS X are physical radii. G71 is metric geometry, not a FANUC roughing cycle.

- CYCLE95: local quoted `START:END` contours, including labels after M30, external/internal longitudinal/facing variants, balanced paraxial roughing, X/Z finishing allowances and finishing contour replay. Overhangs, contour-normal allowance, chip breaking and extended G/diameter modes are rejected. Roughing uses the nominal contour and does not model controller-specific automatic nose compensation or exact controller pass optimization.
- CYCLE93: rectangular axis-aligned grooves, variants 1–8/11–18, with a configured square groove tool, width, active D and zero corner radius. Flank angles, corner radii and chamfers are rejected. D selects a logical edge; controller tool-table offsets are not imported.
- CYCLE97: longitudinal straight/taper threads with explicit pitch, constant-depth/constant-area infeed, finishing allowance and idle passes. Requires fixed running RPM, IANG=NSP=0 and NUMTH=1. Other infeed/multistart variants are rejected.
- Centerline drilling: CYCLE81/82/83/84/85/89, using the supported shared axial cycle interfaces. MCALL turning cycles and arbitrary subprogram calls are not implemented.
- ISO-T: linear/circular motion, feed/spindle modes, WCS and G32/G33 threading in the selected A/B code system. ISO canned turning cycles and G28 reference return remain unsupported.

Both supplied CAM files in `tests/fixtures/turning/sinumerik` execute through M30. Both contain CYCLE95 and CYCLE97; the second expands drilling, so it is not an independent fully expanded turning reference. Numerical cycle tests cover dimensions and infeed separately. FULL turning normalization and a native Siemens turning output post are not implemented; EXPANDED conversion retains its existing preflight restrictions, including native CSS rejection. Save the source document to retain a native program.

Reference interfaces: [Siemens 840D programming guide](https://cache.industry.siemens.com/dl/files/510/28713510/att_53953/v1/PGK_1000_en.pdf) and [Siemens compatibility turning cycles](https://cache.industry.siemens.com/dl/files/300/109751300/att_931853/v1/808D_808D_ADV_turning_op_man_0917_en-US.pdf).

**CYCLE95 verification boundary:** with an active D edge and a configured nonzero tool nose radius, `UNVERIFIED_SINUMERIK_CYCLE95_NOSE_COMPENSATION` marks nominal-contour execution without the controller's automatic correction. Reaching M30 is not a verified controller-equivalent result. The current model scales FALX through the active diameter mode (DIAMON FALX=0.2 adds 0.1 mm to the radius) and distributes paraxial infeed evenly; matching controller allowance and pass-planning behavior still requires independent validation with known tool data. A DXF from another backplotter is comparison evidence, not a normative Siemens reference. It cannot by itself identify which model is correct.

The CYCLE95 nose-compensation warning does not by itself block EXPANDED export. Native CSS and other modeled preflight restrictions can independently reject export; a successful export is not further validation of cycle geometry.

Native/ISO-T turning accepts only the modeled M-function subset; unknown M codes stop execution rather than following the milling auxiliary-warning policy. G0 toolpath contact and turning stock removal consume this same trace; they do not independently certify cycle semantics.

---

## HEIDENHAIN iTNC 530 input

HEIDENHAIN is a separate input dialect, not a FANUC/SINUMERIK variant. `.h`/`.H` files — or unnamed text whose block structure contains `BEGIN PGM ... MM/INCH` — select native milling execution (`fanuc_mill` with `source_dialect=heidenhain`). The **iTNC-code** source type selects it manually and enables Klartext highlighting. The parser builds an immutable native AST with unevaluated Q/QL/QR expressions, separate numeric/named label maps and physical source locations; the runtime consumes that AST directly and never lowers commands to ISO.

The scope includes **three-axis CAM contours, bounded parametric programs, indexed 3+2 and table TCP with configured AC/BC kinematics**. Unsupported semantics are not silently skipped: execution stops at the source block with a diagnostic and keeps the valid prefix of the trajectory. Structured results and CLI/batch reports expose `source_dialect=heidenhain` independently of the shared `fanuc_mill` geometry language.

Select the rotary profile before executing A/B/C or PLANE blocks; zero rotary angles also require a profile. `PLANE SPATIAL SPA/SPB/SPC` uses fixed-axis `Rz(SPC) Ry(SPB) Rx(SPA)` rotations. STAY changes coordinates without indexing; TURN solves the tool axis using the configured two-joint profile, with optional SEQ+/SEQ− branch selection. PLANE RESET cancels the tilted frame. MOVE and TABLE COORD are unsupported. `M128/M129` enable/disable logical tool-tip control on AC/BC tables with PLANE reset; the supported FUNCTION form is `FUNCTION TCPM F TCP AXIS POS PATHCTRL AXIS` and `FUNCTION RESET TCPM`. Continuous rotary interpolation requires L blocks and active TCP. `M126/M127` select/cancel shortest-path rotary positioning; `M94` reduces displayed angles. OEM pivot lengths and physical machine travel are not modeled.

The unmodified three-post project is stored in `tests/fixtures/milling/test_5ax/1001.nc`, `1001.mpf` and `1001.h`. All three programs reach M30 using `5ax_table_ac` and Home Z=100. Regression tests compare all 1182 normalized cutting segments, arc centers and intermediate points, feeds, tools and start/end tool axes. The positional tolerance is 0.002 mm to account for postprocessor rounding. Controller-specific rapid/home transitions are tested separately rather than equated to cutting geometry. GPU stock removal remains three-axis.

### What HEIDENHAIN support is included?

| Native function | Current behavior |
| --- | --- |
| `BEGIN/END PGM`, `MM/INCH`, `BLK FORM 0.1/0.2` | Program/unit metadata and stock bounds; coordinates and feeds are converted to millimetres |
| `L` and coordinate-only straight blocks | XYZ motion with `IX/IY/IZ` incremental addresses and `F`/`FMAX`/`FAUTO`, `R0/RL/RR` |
| `CC`, `C`, `CR`, `CT` | Circle center and full/partial arcs with `DR+`/`DR-`, radius arcs and tangent arcs; circular motions require an explicit direction |
| `LP`, `CP` | Polar positioning and polar/helical circular motion with `PR/IPR/PA/IPA` |
| `APPR/DEP LT/LN/CT/LCT` | Approach/departure lines and tangent arcs to a planar contour |
| `TOOL CALL`, `TOOL DEF` | Numeric, named and Q tools, spindle axis X/Y/Z, `S`/`F`; tool offsets `DL/DR/DR2` are parsed but stop execution |
| `M0/M1/M2/M3/M4/M5/M6/M8/M9/M13/M14/M30` | Logical signals/spindle state and program end; `M99` calls the active cycle. Other M words stop execution |
| `M91` | Nonmodal absolute machine XYZ using the configured WCS |
| `Q/QL/QR`, `FN 0–4/6/7`, expressions | Bounded arithmetic, comparisons, trigonometry and function trees evaluated without `eval`; QL locals are saved across label calls |
| `LBL`, `CALL LBL`, `REP`, `FN 9–12` | Numeric and named labels, call stack, repeats and conditional `GOTO`; unmatched labels, duplicate definitions and LBL 0 misuse are diagnosed |
| `CYCL DEF`/`CYCL CALL` | Cycle 32 is metadata only; drilling/boring/tapping cycles 1/2, 200–209 and 240/241 expand to physical geometry; cycles 251/252 execute pocket milling and 262 thread milling; 220/221 execute position patterns at definition time; cycle 9 is dwell; unsupported cycle codes stop execution |
| Q cycle parameters | Physical `Q...=` continuation blocks remain in the AST and are consumed by `CYCL CALL` in execution order. `MAX`/`FMAX` is a symbolic feed for Q208 and Q253, not a numeric expression: Q208 rapid retraction in cycles 202/203; Q253 rapid pre-positioning in cycles 204/205/241/262. The required Q parameters of cycles 220/221/251/252/262 must be explicitly defined |
| Cycle 247 datum selection | Application mapping: `Q339=1..6` selects the configured G54..G59 offsets in millimetres. The tool's machine position is preserved; other preset numbers are unsupported. This is not an import of a controller's preset table |
| Cycles 7/10 | Axis-address datum shifts and XY planar rotation (`ROT`) apply immediately without moving the tool; reset with zero values. Coordinate and circle-center transforms are retained in the machine-space trace; datum-table and tilted-plane variants remain unsupported |
| `M140 MB distance`, `M140 MB MAX` | Retraction follows physical machine +Z before positioning, with a separately scoped feed. Configured table kinematics maps this retraction through the table orientation even with a tilted program frame. MAX requires enabled Home emulation and uses Z from Home (G28) in WCS, only in the positive direction, with a warning. Physical travel limits are not modeled; the MAX approximation blocks NC trace export |
| `F0`, repeated feed addresses | Geometry is retained; F0 is disclosed as a warning instead of inventing a feed; repeated feeds use the last value |
| Optional `/` blocks and source numbers | Physical source lines and optional skip markers are retained; block numbers are not treated as `LBL` subprogram labels |
| `RND R… [F…]`, `CHF … [F…]` | Tangent rounding arcs/chamfers trim adjacent elements before existing RL/RR compensation; feed applies only to the inserted segment. Planar local corners and explicit geometric diagnostics; see the limits below |
| Rotary `A/B/C`, PLANE SPATIAL/RESET, M128/M129 | Configured rotary indexing, tilted frames and AC/BC table TCP as described above; unsupported combinations stop at the source block |
| `M120`, auxiliary `U/V/W`, tool offsets DL/DR/DR2 | Not executed; execution stops at the block |
| FULL formatting | Rejected for Klartext; EXPANDED and Save Source remain available |

### Which pocket and thread-milling cycles are supported?

The input interpreter executes documented subsets of **251 RECTANGULAR POCKET**, **252 CIRCULAR POCKET** and **262 THREAD MILLING**. Their geometry is expanded during execution; this does not imply that the export post preserves these cycle definitions.

| Cycle | Supported geometry and parameters |
| --- | --- |
| 251 | Rectangular pocket with Q218/Q219 dimensions, Q220 corner radius, Q224 rotation and Q367 reference position |
| 252 | Circular pocket with Q223 diameter |
| 262 | Internal thread with Q335 nominal diameter, signed Q239 pitch, Q201 depth, Q355 cutting strategy and Q351 milling direction |

Cycles 251/252 implement Q215=0 roughing and finishing, Q215=1 roughing only and Q215=2 finishing only. Q202 controls roughing depth increments; Q338 controls wall-finishing depth increments. Q368/Q369 are side/floor allowances; Q370 sets the lateral stepover as a multiple of the cutter radius. Q206, Q207 and Q385 specify plunge, milling and finishing feeds. Q351 selects climb/up-cut milling relative to M3/M4.

Q366=0 selects vertical entry, Q366=1 helical entry; Cycle 251 also accepts Q366=2 reciprocating entry when there is sufficient room. Helical/reciprocating roughing requires an explicit cutter `ANGLE` (or `plunge_angle`), in degrees between 0 and 90. No default angle is guessed. Vertical entry and finishing-only execution do not require this angle.

For Cycle 262, Q355=0 produces one full helical revolution for a multirow cutter; Q355=1 produces a continuous helix over the depth; larger integer values produce separate full revolutions with axial offsets of Q355 times the pitch. The sign of Q239 selects right/left-hand thread. Circular entry/exit and multi-turn helices retain analytic arc geometry. The supported cutter diameter is at least one quarter of the nominal diameter and smaller than it; the lateral repositioning strategy for smaller cutters is unsupported. Q253 accepts a positive numeric pre-positioning feed or `MAX`/`FMAX`; Q207 requires a positive numeric cutting feed.

These three cycles require the XY working plane with Z spindle axis, R0, known M3/M4 spindle direction and configured cutter geometry. Use the existing `milling_tools` or `tool_resolver` execution API to supply the tool type and diameter in millimetres; `TOOL CALL` alone does not supply a diameter or entry angle. The controller's external tool table is not imported automatically. NC dimensions follow MM/INCH program units.

All required Q parameters must be explicitly defined. PREDEF, OEM-dependent defaults and symbolic automatic cutting feeds are unsupported here. Q201=0 skips machining; positive depths are diagnosed because their interpretation depends on OEM MP7441 policy. Unsupported parameters, entry strategies and insufficient cutter clearance stop execution with diagnostics. This is a bounded geometric implementation, not a claim of identical internal controller passes.

### How do position-pattern cycles 220 and 221 execute?

**220 CIRCULAR PATTERN** and **221 CARTESIAN PATTERN** are DEF-active: they execute when the last Q-parameter continuation of their definition is reached. First define the machining cycle (supported drilling/boring/tapping, 251, 252 or 262), then define the pattern. No extra `CYCL CALL` is needed to trigger the pattern. The previous machining cycle remains active afterward.

- Cycle 220 uses Q216/Q217 for the center, Q244 for the diameter, Q245/Q246 for the start/end angles, Q247 for the angular step and Q241 for the number of positions. Q247=0 distributes positions over the full circle or partial arc. Q365 selects straight or circular transfer.
- Cycle 221 uses Q225/Q226 for the start, Q237/Q238 for spacing, Q242/Q243 for column/row counts and Q224 for rotation. Rows are traversed in alternating directions.
- Q200/Q203/Q204 set the shared clearance and surface coordinates. Q301=0 transfers between operations at setup clearance; Q301=1 uses second clearance. Pattern parameters must be explicit, and R0 is required. The nested machining cycle retains its own plane and tool restrictions.

### How are Klartext source, parameters and diagnostics represented?

The public parser is [`parse_heidenhain_program(source)`](app/gcode/kernel/frontend/heidenhain.py). Each physical line, including comments, empty lines, optional `/` skip and numeric block prefixes, remains a source `Block` with original text and locations. `Block.native_syntax` and the immutable AST share typed Klartext commands, expressions, M-function parameters (including typed `M120 LA`/`M140 MB` parameters and a separately scoped `M140` retraction feed) and cycle-parameter continuation records; no synthetic FANUC G words, ISO motions or Macro B nodes are introduced. The portable and Cython AST builders agree on these native nodes.

Q expressions are parsed into trees **without evaluating them**; the dedicated runtime subsequently evaluates supported arithmetic, functions and assignments without Python `eval`. The accepted ranges are `Q0–Q1999` and `QL/QR0–499`. Program block numbers and numeric/named `LBL` definitions have separate maps; `LBL 0` returns, duplicate or unresolved static labels are diagnosed, and active cycle definitions are resolved in execution order rather than assumed from the lexical `CYCL CALL` reference. The parser does not invent missing cycle parameters; supported runtime defaults are applied only during execution. Unsupported PLANE variants and `FN 18` instructions stop execution instead of generating motion.

Parse errors include a physical line, column, source text and diagnostic code. During execution, emitted motions and steps keep source-block provenance; unsupported operations stop on the offending line with the valid prefix preserved. Execution limits and cooperative cancellation also apply to native Klartext. The shared `fanuc_mill` machine contract provides geometry, while `source_dialect=heidenhain` selects the independent interpreter.

### Which iTNC editor tools and exports are available?

**Open Document** includes `.h`/`.H`; the **iTNC-code** selection enables Klartext syntax highlighting with the configured editor font, colors and theme. Hole and pocket calculators generate native signed `L`/`CR` blocks and, where applicable, `CC`/`CP` helical entries instead of an ISO postprocessed fragment. **Renumber** writes numeric prefixes without `N`, allows a start at zero, retains optional `/` markers and supports selected lines; removing numbers also respects Klartext prefixes.

**Save** retains the original source. Klartext **FULL** formatting is rejected; **EXPANDED** uses the distinct `heidenhain_itnc530` output post and resolved trace. It can emit `BEGIN/END PGM`, `TOOL CALL`, `L/FMAX`, `CC` with `C/CP`, `CR` and `CYCL DEF 200/201/202/203/207`. This output support is **not** evidence that every emitted native construct can be consumed by the separate input interpreter. The iTNC output post remains restricted to its supported three-axis geometry; native rotary input does not imply five-axis Klartext output support.

### How is the iTNC implementation verified?

RND/CHF follows iTNC 530 manual 737759-23, sections 5.3, 6.3–6.4, pages 237–238 and 244. Corners are constructed on the programmed contour before the existing RL/RR cutter compensation; APPR/DEP approach and departure construction remains in place.

- `RND R… [F…]` trims the two neighboring contour elements and inserts a tangent rounding arc. Supported combinations are line–line, line–arc, arc–line and arc–arc, provided the local solution is unique.
- `CHF … [F…]` trims two straight lines and connects them with a chamfer. Its value is the setback along each neighboring line, not the diagonal length. At a right-angle corner, `CHF 10` produces a diagonal of approximately 14.142 mm in an MM program.
- `F` on RND/CHF applies only to the inserted arc/chamfer; the surrounding contour retains its own feed.
- R0/RL/RR, XY/XZ/YZ working planes and program units are supported. RND without compensation requires both working-plane coordinates in the preceding contour block.

For example, with compensation off, the following contour rounds the corner at X20 Y0 with a 5 mm radius in an MM program:

```text
L X0 Y0 R0 F100
L X20 Y0
RND R5 F50
L X20 Y20 F100
```

The rounding starts at X15 Y0 and ends at X20 Y5; its center is X15 Y5. Only the rounding uses F50. Replacing `RND R5 F50` with `CHF 5 F50` connects X15 Y0 to X20 Y5 with a straight chamfer.

Spatial/helical, full-circle/multi-turn, ambiguous corners and corners consuming an entire neighboring element produce explicit diagnostics. During cutter compensation, an inward rounding/transition radius below the configured cutter radius stops execution; equality collapses the compensated arc to a point. The cutter geometry must therefore be configured correctly.

Numeric regressions check tangent coordinates, radii, continuity, compensation, units, source-block ownership and local feeds. The six-rounding reference `6bas154.h` uses explicitly configured T4 diameter 6 mm; APPR/DEP R3 does not declare cutter geometry. `manual_chf.h` follows the manual's LINEAR example. These checks cover the stated subset, not full controller conformance.

Cycles 252 and 262 now have the bounded implementations described above. Their presence in `fusion_benchmark.h` does not guarantee completion of the full CAM program: each parameter set, tool configuration and remaining command must satisfy the supported contract. A stopped execution retains only the valid prefix.

Short cycle examples are collected in [`heidenhain/cycles/`](tests/fixtures/milling/heidenhain/cycles/), extracted from machine programs and the cycle manual. These examples are not independently confirmed controller trajectory references.

The 13 contour/drilling programs in `tests/fixtures/milling/heidenhain/` are registered in execution and Qt open/plot regressions with Home emulation enabled. The `6bas154.h` setup explicitly assigns T4 diameter 6 mm; APPR/DEP R3 does not declare tool geometry. Its six RND corners and the official `manual_chf.h` chamfers have independent numeric expectations. The unchanged `cycles_itnc530.h` reaches M30 and executes eight holes; `itnc530_cycl200macro.h` executes ten holes using FN 6/7 trigonometric assignments; `ellipse.h` completes its 40-step loop using Cycle 7 datum shift and Cycle 10 planar rotation. MAX retraction uses Z from Home (G28) in WCS, emits `HEIDENHAIN_M140_HOME_EMULATION`, and blocks NC trace export. With Home emulation disabled, MAX stops with a source diagnostic. Cycle 247 maps entries 1–6 to G54–G59. Native motions, arc centers and drilling operations use machine coordinates.

The repository retains the real CAM and parametric programs under [`tests/fixtures/milling/heidenhain/`](tests/fixtures/milling/heidenhain/). Regression checks cover AST structure, exact source positions, cycle continuations, portable/native AST equivalence, diagnostics, cancellation and source-to-motion links in [`test_heidenhain_frontend.py`](tests/dialects/test_heidenhain_frontend.py) and [`test_heidenhain_execution.py`](tests/dialects/test_heidenhain_execution.py). Small AST cases are inline test inputs. The full `sample.h` fixture reaches `M30`; Cycle 32 smoothing and `F0` generate explicit warnings. The corpus includes decimal-comma coordinates and `STOP M30` in `sample_cr.h`, plus `arcs.h` cases with repeated feeds and circle planes derived from `CC`. GUI highlighting, calculators, renumbering and the export post have separate tests. These checks are not a claim of full iTNC 530 controller or machine simulation coverage.

Cycle reference: [iTNC 530 34049x-06, Cycles, 670388-21](https://content.heidenhain.de/doku/tnc_guide/pdf_files/iTNC530/34049x-06/zyklen/670_388-21.pdf), covering cycles 220/221, 251/252 and 262.

Syntax references: HEIDENHAIN's [Klartext programming manual](https://content.heidenhain.de/doku/tnc_guide/pdf_files/iTNC530/34049x-neu/en/bhb.pdf) and [iTNC 530 60642x-03 manual](https://content.heidenhain.de/doku/tnc_guide/pdf_files/iTNC530/60642x-03/bhb/737759-22.pdf).

---

## CLI

**Open the current document in a terminal:** choose **File → Open in CLI** or press **Ctrl+Alt+T**. The same command is available on the File toolbar, in Customize Toolbars and in the hotkey editor. Unsaved documents must be saved first; Cancel leaves the document untouched. A separate terminal opens in the NC file's folder and waits for input; no CLI command runs automatically. The `egp` shell shortcut forwards arguments directly to the existing CLI. A colored logo and compact help show `egp --help`, folder analysis with `egp batch` and batch DXF export with `egp batch-export`. The examples use the current folder (`.`) and supported document settings; type or copy a command to run it.

**Settings → Options → General → CLI terminal** accepts a terminal executable path. Leave it empty for automatic detection. Windows supports Windows Terminal, PowerShell and cmd (the session uses PowerShell); Linux supports common terminals such as GNOME Terminal, Konsole, XFCE Terminal and xterm, with Bash for the session. In packaged installations, put `easy_gcode_plot_cli.exe` (Windows) or `easy_gcode_plot_cli` (Linux) beside the GUI, or make it available on PATH. Source installations use their console Python and `cli_main.py`.

The launch forwards the current machine language, encoding, FANUC lathe G-code system, SINUMERIK cycle interface and milling kinematics profile. It passes only options supported by the existing CLI: GUI-only WCS/Home, tool libraries, correction and rendering settings are not copied. CLI file dialect detection and export limitations still apply. Batch commands process the displayed directory, not the list of MDI buffers. The terminal and running commands remain independent when the GUI closes.

### Does the CLI use the same kernel as the GUI?

Yes.

The standalone CLI is an interface over the same parser, Macro B runtime, machine execution, cycles, compensation and export modules.

### Which commands exist?

Current commands are:

```text
parse
trace
analyze
batch
export
batch-export
```

### What does `parse` do?

`parse` executes one program through the normal kernel and prints a readable summary of instructions, motions and diagnostics.

Example:

```powershell
.\easy_gcode_plot_cli.exe parse program.nc --lang fanuc_turn
```

### What does `trace` do?

`trace` executes one program and can write detailed JSON including resolved motions.

JSON and HTML destinations must differ from the source program and from each other, including aliases of the same file. Collisions are rejected before writing. Input decoding and read/write failures return exit code 2 with an error message. JSON output is committed atomically. GUI program and Tool List export also reject the open source as a destination; use Save/Save As to save source edits.

```powershell
.\easy_gcode_plot_cli.exe trace program.nc --lang fanuc_turn -o trace.json
```

### What does `analyze` do?

The exported HTML report always uses a light theme. The Statistics dialog follows the application theme. GUI report and program exports display success or failure notifications after writing. Playback tail highlighting follows the current logical motion, including all its sampled arc segments, using the current-move color from Options; it also works while stepping backwards and during Stock Removal playback.

`analyze` executes one program and prints trace statistics plus diagnostics. With `-o`, it writes analysis JSON.

```powershell
.\easy_gcode_plot_cli.exe analyze program.nc --lang fanuc_mill -o analysis.json
```

### What does `batch` do?

`batch` analyzes every discovered NC file under a directory and writes JSON/CSV reports.

Add `--html C:\Reports\html` to save a separate statistics report with a tool selector and static XY/XZ SVG for each input, using the same API as single-file `analyze`. Subdirectories and full filenames are preserved; `--inches` changes report units. Without `--lang`, `.mpf/.spf` select SINUMERIK turning when native turning signatures are present, otherwise milling; other files keep the turning default. Explicit `--lang` overrides this for the whole batch.

```powershell
.\easy_gcode_plot_cli.exe batch C:\Programs --lang fanuc_mill -o C:\Reports
```

### What does `export` do?

`export` executes one file and sends it through the shared NC/DXF export service.

```powershell
.\easy_gcode_plot_cli.exe export program.nc --lang fanuc_turn -o expanded.nc
```

### What does `batch-export` do?

`batch-export` discovers a directory tree and calls the same single-file export service for every input program.

For indexed A/B programs, choose a profile with `--kinematics PROFILE_ID` when all files use one machine, or pass `--kinematics-map profiles.json` for different machines. Both `batch` and `batch-export` accept the map. It is a JSON object from input-relative paths to profile IDs, for example `{"a.nc":"PROFILE_ID_A","sub/b.nc":"PROFILE_ID_B"}`. Without a profile, affected files fail with `ROTARY_KINEMATICS_REQUIRED`. EXPANDED requires a multiaxis target post for rotary output and rejects geometry it cannot reconstruct. FULL preserves the source rotary commands while applying supported text normalization. DXF uses resolved geometry and the selected profile.

```powershell
.\easy_gcode_plot_cli.exe batch-export C:\Programs --lang fanuc_mill -o C:\Normalized
```

### Are single export and batch export different exporters?

No. They use the same `ExportRequest`, validation and `export_file()` pipeline.

Directory export is orchestration around the single-file service.

### Which dialect names are used?

```text
fanuc_turn
fanuc_mill
```

There is no separate `sinumerik` `--lang` value. SINUMERIK MPF/SPF input is detected from its extension independently of its contents. Select geometry with `--lang fanuc_mill` or `--lang fanuc_turn`; without an explicit language, unambiguous native turning signatures select turning and other MPF/SPF files default to milling.

### What are the exit codes?

Normal successful/acceptable CLI execution returns zero. Failed/incomplete single execution, batch `ERRORS`, batch `NO_FILES` and export failures return a nonzero code (currently 2 for the command-level error states).

### How do I see every option and default?

Use:

```powershell
.\easy_gcode_plot_cli.exe --help
```

or command-specific help, for example:

```powershell
.\easy_gcode_plot_cli.exe batch-export --help
```

Top-level help also prints the subcommand help sections.

---

## Batch analysis

### What does batch analysis validate?

Each discovered file is executed through the same authoritative analysis setup as single `analyze`.

Per-file reports include:

- status;
- `ok` / `complete`;
- file size and line count;
- motion count;
- executed-block count;
- diagnostic counts;
- unsupported G-codes;
- unsupported M-codes;
- full diagnostic records;
- elapsed time.

For rotary milling, JSON reports also include `kinematics_definition` and `kinematics_fingerprint` (SHA-256). They capture the effective profile used by that execution, including normalized table/head axis vectors and their order. CSV reports store the same definition as JSON text. A profile ID alone is not enough to reproduce a calculation when user overrides differ. Reporting does not reload the current catalog after execution.

### Which batch statuses exist?

```text
CLEAN
WARNINGS
ERRORS
NO_FILES
```

`CLEAN` means no diagnostics were emitted.

`WARNINGS` means execution is valid/complete but diagnostics remain.

`ERRORS` means at least one file is invalid/incomplete or contains an error-level diagnostic.

`NO_FILES` means discovery found no matching programs.

### Which extensions are scanned by default?

```text
.nc
.cnc
.ptp
.mpf
.spf
.tap
.txt
```

Scanning is recursive unless `--top-level-only` is supplied.

### Can files without a normal NC extension be discovered?

Yes, when the default extension set is used. The scanner also recognizes likely text CNC programs whose first data contains an O-program header or multiple G/M blocks.

Binary-looking files are not treated as NC text.

### Is discovery deterministic?

Yes. Paths are sorted by normalized relative path so the report order does not depend on filesystem enumeration order.

### Can I restrict extensions?

Yes:

```powershell
--extensions .nc,.tap
```

When a custom extension set is supplied, content-based discovery of arbitrary filenames is intentionally not used.

### What is aggregated in the batch summary?

The report aggregates:

- file status counts;
- total diagnostics;
- error and warning totals;
- diagnostic-code frequencies;
- unsupported G-code occurrence/file counts;
- unsupported M-code occurrence/file counts;
- total elapsed time.

### What files are written?

The default report names are:

```text
batch_report.json
batch_report.csv
```

CSV is UTF-8 with BOM for convenient spreadsheet opening.

### Does a bad input file stop the whole batch?

A read/decode failure becomes a per-file `FILE_PROCESSING_ERROR`, and processing continues.

Unexpected internal analyzer failures are not intentionally swallowed as fake user diagnostics. Programming regressions should remain visible.

### Are there preset batch scripts?

There are no separate preset scripts for ordinary `batch` analysis. Run the CLI command directly so the input directory and report destination are explicit.

---

## Batch export

### What problem does batch export solve?

`batch-export` applies one validated export contract to a complete directory tree.

Typical uses include:

- expanding execution;
- normalizing sequence numbers;
- adding/removing spaces;
- removing comments;
- converting supported resolved programs between mm and inch;
- changing milling arc representation;
- generating a directory of DXF trajectories.

### Does batch export modify the input files?

No. Output must be a separate directory.

The output directory may not be the input directory or a child of it, preventing recursive self-processing.

### Is the source directory hierarchy preserved?

Yes.

Example:

```text
input/
  part1.nc
  machine_a/
    part2.tap
```

NC output becomes:

```text
output/
  part1.nc
  machine_a/
    part2.nc
```

DXF output uses `.dxf`.

### What happens if two source names map to one output name?

The batch is rejected before writing ambiguous outputs. For example, two sibling inputs whose different source extensions would both become the same `.nc` destination are detected as a collision.

### Does one export error stop every file?

Normal per-file read/export/value failures become an `ERRORS` file entry and processing continues.

A successfully executed file with diagnostics is exported and marked `WARNINGS` under the current policy.

An execution that is not `ok` or not `complete` does not produce an output file.

### What files describe the batch export?

The output root contains:

```text
batch_export_report.json
batch_export_report.csv
```

The manifest includes source/output relative paths, status, motion counts, execution counts, diagnostics, effective output units, effective milling arc type and elapsed time.

### What are batch-export statuses?

Per file:

```text
EXPORTED
WARNINGS
UNSUPPORTED
ERRORS
```

Overall:

```text
CLEAN
WARNINGS
UNSUPPORTED
ERRORS
NO_FILES
```

### Which export modes are available from the CLI?

NC has two modes:

```text
expanded
full
```

DXF is selected with `--format dxf`; NC-only mode/formatting controls are rejected when explicitly supplied.

### Which options are intentionally rejected in Full Program mode?

Full Program does not accept explicit:

- unit conversion other than `auto`;
- arc-type selection;
- coordinate-mode conversion;
- modal-feed control.

The goal is to avoid pretending those transformations are semantically equivalent to Expanded Execution. Safety-line, start/end program text, sequence numbering, delimiter and leading-zero options are applied by FULL because they change text framing, not geometry.

### Can sequence start/increment be supplied without sequence numbers?

No. Explicit sequence start, increment or spacing requires `--sequence-numbers`.

### Are there preset batch-export scripts?

Yes. The development tree contains four concrete EXPANDED conversion checks for Windows and Linux:

```text
fanuc_mill_to_sinumerik_native
fanuc_mill_to_sinumerik_iso
fanuc_lathe_a_to_b
sinumerik_native_to_fanuc_mill
```

They run the built CLI with an explicit JSON post profile and write below `tmp/test_export`. They do not rebuild the application.

Run the named scripts as `.\scripts\ps1\batch\<name>.ps1` on Windows or `bash scripts/sh/batch/<name>.sh` on Linux. Their semantic regression gate, `tests/export/test_batch_export_semantics.py`, re-executes successfully exported programs and compares trajectory signatures with the source.

---

## Configuration

### Where is application configuration stored on Windows?

```text
%LOCALAPPDATA%\easy-gcode-plot\config.ini
%LOCALAPPDATA%\easy-gcode-plot\tools.db
```

Snippets use their own SQLite store under Local AppData.

### What is stored in `config.ini`?

Application/UI preferences include items such as:

- language;
- theme;
- document encoding;
- editor settings;
- Auto Update;
- maximum generated motions;
- compensation options;
- arc tolerance and milling arc autodetection;
- Block Skip behavior;
- plot colors and geometry display;
- stock settings;
- playback speed;
- hotkeys;
- comment style.

### Is `tools.db` replaceable by old JSON values in config.ini?

No. `tools.db` is authoritative. Legacy tool JSON in configuration is not used as a fallback write target for a current database.

### Where is the log file?

When logging is enabled:

Enable **Logging** in Options; it is off by default. The log records NC file opening/saving, CNC export (format, post, encoding, completion, cancellation and errors), tool-list and Current Program JSON operations. Milling Stock Removal records startup bounds, Accuracy, OpenGL initialization, texture allocation, frame timings and STL export results. File contents are not recorded.

```text
%LOCALAPPDATA%\easy-gcode-plot\main.log
```

### What does DEBUG logging add?

DEBUG logging includes additional execution, rendering, camera, option and Stock Removal timing information. Slow stock frames are rate-limited so logging does not create an even larger performance problem.

---

## Troubleshooting

### The plot is empty

Check:

- selected machine mode;
- execution diagnostics;
- WCS/home configuration;
- whether the program contains supported motion;
- whether a previous unsupported position-changing block left position unknown.

### Macro B motion is missing

Inspect the first diagnostic. Common causes include:

- undefined variable;
- missing GOTO label;
- missing O-program target;
- unmatched WHILE/END;
- G65 argument error;
- call-depth/resource limit.

Use Tokens/Variables to inspect the execution state at the relevant logical occurrence.

### My G65 M/S/T words did not start spindle/coolant/change tool

That is intentional. On a G65 block those words are macro arguments, not machine side effects.

### Cutter compensation is not visible

Confirm that:

- G41/G42 is active;
- the selected tool was discovered or configured;
- its geometry is valid;
- the contour type is supported.

Inspect diagnostics for an `UNVERIFIED` compensation state.

### G43 appears in the source but the plotted Z does not include tool length

G43/G49 and H are tracked, but tool-length offset geometry is not currently applied to the trace.

### G71 leaves material on the wrong side

Check the sign of the second-line U allowance and whether the contour is OD or ID. The project intentionally preserves signed U semantics.

### G72 Type II reports an error

A facing plane can contain multiple disjoint profile spans whose exact selection is controller-dependent. Such a case is rejected as `UNSUPPORTED_G72_TYPE_II_SPANS` rather than guessed.

### G76 reports `UNSUPPORTED_G76_TOOL_ANGLE`

The packed P angle must currently be one of:

```text
0, 29, 30, 55, 60, 80
```

### Batch shows `UNSUPPORTED_M_CODE` but the geometry looks correct

The M-code is not modeled as a machine effect. Batch keeps the geometric trace while warning that the complete real-machine behavior is not verified.

### Export unit conversion is refused

EXPANDED unit conversion operates on resolved geometry/state rather than scaling source text. If conversion is refused, inspect the reported execution/postprocessor diagnostic (for example unsupported TWP/CYCLE800 or other unverified geometry, or incomplete execution). FULL intentionally supports only `--units auto`.

### Batch-export says the output directory is invalid

The output root must be outside the input directory tree. This prevents exported files from being discovered and exported again during the same run.

### A large program does not update while typing

Use Refresh. Auto Update intentionally avoids continuously rebuilding a trace above the configured automatic sampled-segment threshold.

### The GUI says the current execution is stale

The editor text changed after the displayed `ExecutionResult` was created. Refresh before using execution-dependent information such as Variables or export.

---

## Development and architecture

### How is the CNC kernel organized?

Since 2.2.1, the public API coordinates request setup (`api/execution_request.py`), arc-source policy and geometry postprocessing (`api/trace_geometry.py`). Milling block contracts, controller policy and result publication are separate modules. Historical entry points remain available. Trace geometry, sampling and statistics live in `app/gcode/trace/`; HTML/SVG/text reports and templates live in `app/gcode/reports/`. Execution setup, generators and batch workflows have their own packages. Milling stock replay is separate from snapshot contracts and mesh/STL serialization. These changes do not alter supported CNC semantics or GUI/CLI workflows.

The important packages are:

```text
app/gcode/kernel/api/
app/gcode/kernel/frontend/
app/gcode/kernel/geometry/
app/gcode/kernel/runtime/
app/gcode/kernel/turning/cycles/
app/gcode/kernel/milling/
app/gcode/kernel/milling/cycles/
app/gcode/kernel/compensation/
```

### What belongs in `frontend/`?

The frontend owns:

- comment stripping;
- word lexing;
- Macro B-aware expressions;
- flow-node parsing;
- source blocks;
- AST/model construction;
- native parser acceleration.

The lexer is bracket-aware so Macro B function names and `GOTO` are not misread as CNC address words.

### What belongs in `runtime/`?

Runtime owns shared execution mechanics such as:

- Macro flow;
- G65 local scope;
- M98/M99 dispatch;
- modal-group validation;
- signals and structural events;
- cycle contracts;
- resource limits;
- turning trace construction;
- cycle expansion orchestration.

### Why are turning cycles separate files?

Each major cycle has a focused implementation under `turning/cycles/`, while common dispatch/expansion machinery lives under runtime. This keeps G70-G76 geometry testable without building one monolithic interpreter function.

### What belongs in `milling/`?

Milling state, motion execution, polar programming and canned-cycle execution live under the milling package. Native milling execution accelerates selected motion paths without creating different semantics.

### What belongs in `compensation/`?

Turning tool-nose and milling cutter-radius compensation are deterministic geometry layers applied to resolved source motions.

They do not belong to the OpenGL renderer.

### What belongs in `app/gcode/export/`?

The public export families remain FULL, EXPANDED and DXF:

- `common.py` — shared export options, motion formatting and unit scaling;
- `full.py` — source-preserving FULL normalization using source + execution map;
- `expanded.py` — the single JSON-profile postprocessor for resolved geometry/state;
- `dxf.py` — DXF geometry output;
- `posts/*.json` — the seven bundled controller profiles.

Single-file CLI orchestration lives in `app/gcode/export/service.py`; `batch/export.py` only applies that contract to a directory tree. No export path contains a second G-code interpreter.

### What does `execution/program.py` do?

It is the shared application setup path used to execute a program with the same tool-discovery and kernel configuration used by GUI/CLI workflows.

### What does `batch/analysis.py` do?

It performs deterministic file discovery and repeatedly invokes authoritative execution to construct analysis reports. It does not contain a second G-code analyzer.

### What does `batch/export.py` do?

It is directory orchestration around the same `export_file()` service used by single-file CLI export.

### Which native components exist?

The project builds native extensions for:

- frontend parsing;
- selected milling execution paths;
- tool discovery;
- turning stock polygon clipping and swept-profile intersections.

The Python contract remains authoritative. Native and Python paths are regression-tested for parity where applicable. `app.native` caches parser, discovery, executor and turning-collision availability and import reasons. Source checkouts support fallback; frozen releases require all four extensions and fail explicitly if one is absent or its DLL cannot load. No runtime build or dependency installation is performed.

Turning G0 collision detection clips only newly swept geometry; existing marks are clipped again when the affected material changes. Derived stock sections are cached by material intervals and profile boundaries. Cython accelerates convex clipping and the existing horizontal-span algorithm without changing removal semantics. The real `basic_turning_cycles.NC` fixture covers Python/native parity, rewind and a relative performance guard.

`parser_statistics()` exposes total/native/fallback blocks for the most recent successful parse in the current context, counting actual fallback callbacks. Uncommon source line separators and oversized literal words use the Python reference parser to preserve parity; ordinary LF/CRLF numeric programs keep the native scanner.

CLI parse/trace/analyze/batch do not load ezdxf. The DXF backend is imported only when DXF export is executed; a missing backend produces a controlled export error.

### How are execution results represented publicly?

The kernel imports no Qt bindings: per-user profile paths come from `app.paths`, while GUI settings remain in `app.settings`. Execution and parsing do not change process-global garbage-collection settings; execution budgets remain local to their context.

Parsed `Block` objects are authoritative. A compiled Block-to-AST builder accelerates the same contract as the portable Python builder: AST nodes and first-occurrence N/O label maps are built in one pass. Repeated immutable words share a bounded construction-local cache. The native parser installs its freshly derived canonical AST through a private constructor without rebuilding it; public `Program(blocks, ast)` construction still rejects disagreement. AST nodes and words remain frozen, and label maps remain immutable defensive copies. Parsing never changes process-global GC settings. Relative synthetic performance guards compare compiled and portable AST construction and their complete parsing pipelines; run them with `pytest tests/core/test_ast_acceleration.py -m performance` after building the native extension. Application code imports canonical frontend/API/runtime modules; historical aliases remain available for external compatibility.

The core immutable public types include:

- `Diagnostic`;
- `SemanticInstruction`;
- `TraceMotion`;
- `ArcGeometry`;
- `MachineSignal`;
- `ExecutionEvent`;
- `ExecutionStep`;
- `ExecutionResult`.

### What is an `ExecutionStep`?

It records one executed occurrence of a source block and includes information such as:

- source block index;
- number of emitted motions;
- unit scale;
- diameter/radius mode;
- absolute/incremental state;
- evaluated words;
- signals;
- position;
- active WCS;
- feed/spindle state;
- Macro B variable snapshot;
- execution events.

This occurrence-level model is essential for loops and subprograms where one source line executes multiple times.

### What is an `ExecutionEvent`?

Events describe structural facts that are not ordinary geometry, including program/subprogram boundaries, tool changes and reference returns.

Export can therefore preserve structural execution order without reconstructing it from motion geometry.

### How are tests organized?

Tests are grouped by domain, including:

```text
tests/core/
tests/dialects/
tests/stock/
tests/tooling/
tests/export/
tests/gui/
tests/render/
tests/meta/
```

The fixture corpus contains representative turning, milling, Macro B, cycle, compensation, WCS and export programs.

### How do I run the main checks?

```bash
uv sync --group dev
uv run pytest
uv run ruff check .
uv run ruff format --check .
```

Project scripts add resource/generated-file and complexity checks around the standard lint commands.

On Windows, run the full test suite and project lint checks from the repository root:

```powershell
.\scripts\ps1\test.ps1
.\scripts\ps1\lint.ps1
```

| Task | Windows PowerShell | Linux shell |
| --- | --- | --- |
| Tests | `.\scripts\ps1\test.ps1` | `bash scripts/sh/test.sh` |
| Lint | `.\scripts\ps1\lint.ps1` | `bash scripts/sh/lint.sh` |
| Native extensions | `.\scripts\ps1\build-native.ps1` | `bash scripts/sh/build-native.sh` |
| PyInstaller package | `.\scripts\ps1\build.ps1` | `bash scripts/sh/build.sh` |

Repository working-tree text uses CRLF; Bash scripts use LF. Git attributes and VS Code workspace settings enforce these defaults. Run `.\scripts\ps1\lint.ps1 -Fix -CheckResources` to normalize text and regenerated Qt modules. Without `-Fix`, the linter reports incorrect or mixed endings. Normalization preserves encoding and skips binary assets and ignored build/temporary outputs. Git stores normalized text with LF.

New CNC semantics belong in `app/gcode/kernel/` and require deterministic regression coverage. Exporters consume the authoritative execution result. See [website publishing](docs/PUBLISHING.md) for landing-page development.

### How do I run the daily GUI smoke test with a visible window?

The launchers configure the environment automatically: `scripts\ps1\start-sandbox.ps1` on Windows, or `bash scripts/sh/start-sandbox.sh` on Linux/macOS. They run the visible demo by default. Use `-Automated` / `--automated` for offscreen mode and `-DelayMs 1500` / `--delay-ms 1500` to adjust demo pacing. The PowerShell launcher restores previous environment values; the Bash launcher sets overrides only for its child process.

Run the automated sandbox from the repository root in PowerShell:

```powershell
.\scripts\ps1\test.ps1 tests/gui/test_daily_workflow_smoke.py -q -s
```

For a visible, paced demo, enable both the Windows Qt platform and demo mode:

```powershell
$env:QT_QPA_PLATFORM = "windows"
$env:EASY_GCODE_SMOKE_DEMO = "1"
try {
    .\scripts\ps1\test.ps1 tests/gui/test_daily_workflow_smoke.py -q -s
}
finally {
    Remove-Item Env:QT_QPA_PLATFORM -ErrorAction SilentlyContinue
    Remove-Item Env:EASY_GCODE_SMOKE_DEMO -ErrorAction SilentlyContinue
}
```

Setting only `QT_QPA_PLATFORM=windows` shows the window but does not enable presentation pauses or the final demo summary dialog. The default `EASY_GCODE_SMOKE_DELAY_MS` is 1000 ms: actions pause for 1 second, major stages/dialogs for 2 seconds, and the final summary for 4 seconds. You can adjust the pacing:

```powershell
$env:EASY_GCODE_SMOKE_DELAY_MS = "1500"
```

Both modes execute the same assertions. The scenario opens these existing inputs without moving or changing them:

- FANUC milling: `tests/fixtures/milling/fanuc/flange_plate_benchmark.nc`, without STL; dark theme, grid/colors and settings persistence, Statistics with a per-tool selector and SVG HTML export, expanded FANUC export and kernel replay. Line width stays unchanged.
- FANUC turning: `tests/fixtures/turning/lathe_cycles_example.nc`; G71/G76 and real Stock Removal with deterministic rewind/replay. Saved-library geometry takes priority over automatic discovery.
- SINUMERIK 3+2: `tests/fixtures/milling/test_5ax/5ax_test.mpf` with `stl/test6.stl` and the AC profile. STL Objects: Base Point Origin, Position Z=-100, Move Here.
- SINUMERIK impeller: `tests/fixtures/milling/test_5ax/impeller.mpf` with `stl/test7.stl` and **5Ax Table BC Angled**. STL Objects: Transform rotates Z by +90 degrees, then Section Y at zero, Apply, Undo, and STL edges only. The sandbox editor uses saved T60 taper-ball-mill geometry with D1. Play briefly, then seek in 10% slider steps through completion. Turning Stock Removal and the flange benchmark retain complete continuous playback.

Pytest isolates settings, the tool library and all output files in temporary directories. The sandbox's fixed T0303 P2 record is in that temporary library, not the user's configured SQLite. File pickers receive predetermined paths; application dialogs and actions remain real. Unexpected message boxes fail the stage instead of hanging. Assertions inspect widget/model/scene state, not OpenGL pixels. Both modes print stage results; demo mode also displays a timed final summary and identifies the failed stage if an assertion fails.

See [GUI sandbox](docs/GUI_SANDBOX.md) for the complete stage contracts and platform notes.

### Are generated Qt Python files edited manually?

No. `.ui` and `.qrc` sources are authoritative. Regenerate through the project scripts.

Windows:

```powershell
.\scripts\ps1\generate-qt.ps1
```

Generated modules are build artifacts.

---

## Build and release

### How do I build on Windows?

```powershell
.\scripts\ps1\build.ps1
```

The build produces separate GUI and CLI executables plus SHA-256 checksum files.

### How do I build on Linux?

```bash
bash scripts/sh/build.sh
```

For console-only packaging after tests have already passed:

```bash
bash scripts/sh/build.sh --console --skip-tests
./dist/easy_gcode_plot_cli --help
(cd dist && sha256sum -c easy_gcode_plot_cli.sha256)
```

### Does the project use a separate build environment?

Yes. Native/release tooling uses a persistent `.venv-build` rather than replacing or pruning the developer `.venv`.

The native build checks tracked `.pyx` and dependency state and can reuse the build environment when nothing relevant changed.

### How are releases validated in CI?

The release workflow runs the full tests and static checks on Linux and Windows before packaging. Both packaged CLIs are smoke-tested with `--help`; Linux is archived with a SHA-256 sidecar, Windows publishes GUI/CLI hashes, and the release job downloads both artifacts before creating or updating the tagged GitHub Release.

### Does a Linux executable run as a Windows `.exe`?

No. Windows and Linux artifacts are platform-specific builds even though they share the same Python/kernel implementation and CLI contract.

---

## License

Easy G-Code Plot is distributed under the MIT License. See `LICENSE.md` for the full text.