OPEN SOURCE · CNC WORKSPACE

Read the code.
See the toolpath.

A workspace for multiple turning and milling programs. Switch between documents, follow the tool in 3D, and turn the calculated execution into reports and exports.

New in 2.9.7: GPL-3.0-only licensing and a view cube for face, edge and corner camera views. View supported commands and limits.

Windows & Linux · GPL-3.0-only · All releases

FANUC MillFANUC LatheSINUMERIK 840D HEIDENHAIN iTNC 530
Easy G-Code Plot3D VIEW
Source code and calculated motion, side by side. Watch the demo ↗

01Edit & inspect

02Calculate & play back

03Analyze & export

FROM STOCK TO PART

Milling and turning stock removal

One Stock Removal button and one Stock dialog for milling and turning. Review remaining material using the executed toolpath and configured tool geometry, with settings for the active machining mode.

3D milling stock removal

Automatic or manual X/Y/Z box bounds, machining allowance and five Accuracy levels. Flat, face, ball, corner-radius and tapered-ball cutter profiles determine the cut surface.

Play/Pause, stepping and rewind synchronize the remaining stock with the tool position. Stock and machined-surface colors are configurable. The current machining stage can be exported as STL.

Milling stock settings and limitations →
GPU milling stock simulation with G-code, a 3D box blank and playback controls
Three-axis milling stock simulation

See turning material removal

Review external, internal and face turning, grooves and thread profiles. Material removal follows tool geometry and executed motion. Rewind playback to inspect an earlier state.

See turning material removal
See turning material removal
Turning path and stock examples
Turning cycle paths
Turning cycle paths
Turning stock profile
Turning stock profile

Three-axis milling removal and surface rendering run on the GPU and require OpenGL 4.3. The milling model supports a box blank and vertical cutters. Rotary/TCP removal, undercuts and subtraction from imported STL solids are not supported.

FROM SOURCE TO SCENE

Understand what your program does.

Real screenshots. Calculated toolpaths. Tools for reviewing the details before the next step.

01 / VISUAL REVIEW

Follow every move in 3D

Step through the toolpath and jump to its source line. Bring in STL models, position and rotate them, and inspect sections in the same scene.

STL array creation is limited to a resulting scene of 1,000 objects and 2,000,000 triangles, including existing objects. Excessive requests leave the scene and undo history unchanged.

Start with one empty milling document. Add programs with + or Open, then switch with the document-list arrow. Each document keeps its edits, undo history, machine mode, tools, stock setup, STL scene and playback position. Close with × or Ctrl+W, with a save prompt for unsaved changes.

Options, saved libraries and WCS/Home are shared. Changed CNC settings mark old cached results as stale when selected. Finish or cancel an editing dialog before switching; Tokens follows the active document. The next launch starts a fresh session.

Compare open buffers or disk files side by side, with aligned colored differences and synchronized scrolling. Refresh rereads disk sources; the comparison remains read-only and preserves unsaved editor text.

Follow every move in 3D
Follow every move in 3D
STL placement and milling example
STL models in the scene
STL models in the scene
Milling toolpath review
Milling toolpath review

02 / VISUAL REVIEW

Explore rotary toolpaths

Inspect indexed machining and supported continuous rotary/TCP motion. Choose the machine kinematics for FANUC G68.2/G53.1 or SINUMERIK CYCLE800 and supported AC/BC five-axis programs.

Explore rotary toolpaths
Explore rotary toolpaths

03 / VISUAL REVIEW

Measure directly in the scene

Pick two points on toolpaths or STL geometry in Top, Front, Left or Lathe view. Snap to geometry or the grid, edit point coordinates, and read distances and coordinate differences in millimetres or inches.

Measure tool with editable point coordinates
Distances and coordinates in millimetres or inches

Imported STL models are visual references. Full machine collision simulation is outside the current model.

YOUR EVERYDAY TOOLKIT

Set up once. Keep working.

Keep milling and turning tools in a saved library. Reuse snippets, find tool changes, and tune the editor and calculation settings.

Open saved tools through Settings → Tool Library and the STL object panel through View → STL Objects. Compare, Statistics, Snippets and Tokens/Variables are in CNC Functions.

Right-click a toolbar → Customize Toolbars to choose and reorder buttons. Restore Defaults selects compact groups for files, undo/redo/search, view controls, toolchange navigation, Compare/statistics/measurement and playback. Clipboard, formatting, printing and calculators are optional; saved choices remain until you explicitly restore defaults.

The source chooser offers Text, ISO G-Code and iTNC-code. Set its default in Settings → Options → General → Default file type. iTNC-code highlights Klartext; .h/.H files select native milling execution. Configured kinematics supports PLANE indexed 3+2 and M128/TCPM L motion on AC/BC tables. Hole and pocket calculators can generate native Klartext fragments. Unsupported commands stop execution with a source diagnostic. See the iTNC input coverage and limits.

Milling tool library
Milling tool library
Turning tool library
Turning tool library
Milling tool types — 9 options

On the milling tab, add a tool to the library, then choose its type and dimensions. The names below match the editor list. All types have a diameter, flute length and body length; length to holder is the sum of the two lengths. Enter dimensions in millimetres or inches.

Editor type Shape Specific settings
Flat Mill Flat-ended end mill Diameter and lengths
Bull Mill Corner-radius end mill Corner radius, at most half the diameter
Ball Mill Ball-ended mill Ball radius automatically equals half the diameter
Taper Ball Mill Tapered mill with a spherical tip Ball-tip diameter and taper angle
Face Mill Face mill Shank diameter smaller than head diameter
Slot Mill Mushroom cutter Shank diameter and flute length
Chamfer Mill Chamfer cutter Flat-tip diameter and chamfer angle
Drill Drill Point angle
Tap Tap Diameter and lengths

For face and mushroom cutters, flute length defines the head height. Older records with a single total length retain a separate cutting-height field until the split lengths are edited.

Turning tool types — 9 options

In the turning editor, choose a category, machining direction and available type. OD means external machining, ID means internal machining, and Face means face machining. Available types and P tip orientations depend on the selected direction.

Editor type Shape Settings
Diamond 80 80° diamond insert Nose radius, insert size and P orientation
Diamond 35 35° diamond insert Nose radius, insert size and P orientation
Square Square insert Nose radius, insert size and P orientation
Round Round insert Insert diameter, nose radius and P orientation
Triangle Triangular insert Nose radius, insert size and P orientation
Groove Grooving tool Width, nose radius and P orientation; radial or face groove geometry
Thread Threading tool Insert size, profile angle, tip width EX, corner radius RC and P orientation
Drill Drill Diameter, length and point angle
Tap Tap Diameter, length and point angle

The saved library and current-program tools are separate lists. Assign a library entry to a program tool to use its geometry; save an edited program tool to the library for later work. Use the preview to check shape and orientation before saving.

Editor settings
Editor and calculation options
Editor and calculation options

G-CODE TEMPLATES

Snippets

Editable program fragments and milling or turning cycles for FANUC, SINUMERIK and HEIDENHAIN iTNC 530.

Parameters, formulas and diagrams

Find a template by group and name in the Snippets side panel. Insert asks for its parameters and adds the result to the editor as one undo action.

Edit Snippets opens the manager: change the text, add your own templates and attach diagrams. Each controller has its own library.

Snippet manager with controller selection and editable G-code template
Snippet manager and template editor

LESS REPETITIVE TYPING

From dimensions to G-code.

Preview hole coordinates and pocket paths, adjust the dimensions, and insert the result into the editor.

Hole patterns

Circular bolt patterns or rectangular grids. Set the center, spacing and count before inserting coordinates. Patterns are limited to 20,000 points; for grids, the X and Y counts are multiplied. An excessive pattern disables Insert and explains the limit in its tooltip.

Circular hole pattern
Circular hole pattern
Rectangular hole grid
Rectangular hole grid

Pocket toolpaths

Circular and rectangular pockets with depth steps, stepover and entry options. Review the preview as you change parameters.

Circular pocket
Circular pocket
Rectangular pocket
Rectangular pocket

ONE CALCULATION KERNEL

The same execution, everywhere.

The 3D view, playback, statistics and exports share the resolved motions. The desktop and command line use the same kernel.

01

Evaluate the program

Resolve variables, loops, subprograms, cycles and coordinate systems within the supported dialect.

02

Inspect diagnostics

Distinguish complete execution from warnings, invalid geometry and unsupported commands. Keep each issue tied to its source line.

03

Use actual tool geometry

Saved tools and program overrides supply geometry for supported compensation, turning stock removal and three-axis milling stock removal.

TOKENS AND VARIABLE STATE

Inspect program lines and controller variables

Follow diagnostics and recorded variable values in one inspector for FANUC, SINUMERIK and HEIDENHAIN iTNC.

Tokens table showing SINUMERIK R expressions and line diagnostics
Tokens/Variables: SINUMERIK R expressions

Find the relevant blocks

Open CNC Functions → Tokens/Variables. The Tokens tab shows source lines, parsed words, support status and diagnostics. Select All, Warnings or Errors and search for text such as T1 M6 without recalculating the program. The footer shows the filtered row count; copying and CSV export respect the filters.

Follow values during playback

The Variables tab reads existing execution snapshots at the current playback position. Controller, source line and execution occurrence identify the displayed state, including repeated blocks in loops and subprograms. Inspect values or export them to CSV without running the program again. Stale execution must be updated before viewing its variable state.

FANUC: #

Inspect numbered Macro B variables such as #1 and #100, plus named variables such as #<NAME>. Available for turning and milling execution.

SINUMERIK: R

Inspect native parameters such as R1 and R10, together with recorded named scalar variables. Native identifiers remain distinct from FANUC Macro B identifiers.

HEIDENHAIN iTNC: Q

Inspect Klartext Q, QL and QR parameters captured during execution, using their controller names.

A clean Tokens table does not guarantee complete execution or a valid toolpath. Check the execution status and diagnostics as well.

TAKE THE RESULT WITH YOU

Export the execution.

Choose NC output or DXF geometry. Keep the source dialect in FULL, or serialize the resolved execution for a supported target with EXPANDED. HEIDENHAIN and SINUMERIK turning FULL normalization are unavailable; use Save/Save As to preserve their source text.

Control the output

Choose the target controller, arc representation, precision, numbering and program wrappers. The desktop, CLI and batch export use the same calculation and output rules.

In EXPANDED EXECUTION, select a built-in or saved user post under Target CNC. The + button imports a ready JSON profile for the current machine type, keeping the original file unchanged.

Controller conversion details →
Export settings
Export settings

Postprocessors for your controller

Eight built-in export posts are available:

  • Milling: FANUC, SINUMERIK 840D ISO-M (G291), SINUMERIK 840D native, and Heidenhain iTNC 530.
  • Multi-axis milling: FANUC and SINUMERIK 840D native.
  • Turning: FANUC lathe A and FANUC lathe B.

The Heidenhain post outputs BEGIN/END PGM, TOOL CALL, L/FMAX, CC with C/CP, CR and drilling cycles in EXPANDED.

Customize posts in Settings → Options → Postprocessors. Select a profile on the left and edit it on the right. The buttons below the list add a copy, save, rename and delete user profiles; built-in posts remain read-only.

Save a new copy with Save or OK. The profile is checked before saving; Cancel discards unsaved changes. User profiles appear alongside the built-in posts in Export.

Postprocessor library and embedded editor
Postprocessor library and embedded editor

Five-axis FANUC ↔ SINUMERIK export is experimental. Its compensation, kinematics and verification limitations are listed in the conversion details.

Statistics and HTML reports

See how much of a program was executed, where each tool travels and how cutting and rapid moves contribute to length and estimated time. The desktop Statistics dialog and CLI reports use the same calculations.

Statistics for the program and each tool
Statistics for the program and each tool

A report you can share

Lengths, estimated times and bounds, grouped by tool. Open the standalone HTML report in any browser.

Open sample report ↗

Moves, time and bounds

Grouped tables show motion counts, cutting and rapid lengths, estimated times, average feed and XYZ bounds. Execution status distinguishes complete results, warnings and partial or invalid execution.

Statistics for each tool

Use the tool selector to switch between the whole program and an individual tool. Each tool has its own lengths, times and XYZ bounds. Display measurements in millimetres or inches.

A report you can share

Export HTML from the Statistics dialog or CLI. The standalone report includes all tool sections and a static SVG toolpath projection: XY for milling, XZ for turning. It opens in a browser without installing the application.

Analyze one program

Generate a readable HTML report and detailed JSON in one run. For FANUC milling files, specify --lang fanuc_mill; use fanuc_turn for turning.

.\easy_gcode_plot_cli.exe analyze ".\programs\part.nc" --lang fanuc_mill `
  --html ".\reports\part.html" -o ".\reports\part.json"

In the GUI, open Statistics, choose a tool or units, then select Export HTML. Exported reports always use a light theme; the dialog follows the application theme.

The example was generated from plate_setup_complete.nc: 377 movements and 10 tools. Time is a kinematic estimate; dwell, tool changes and acceleration are not included.

Batch analysis and export

Process a folder in one command instead of opening each program manually. Review diagnostics in a spreadsheet, produce reports for colleagues or export a complete directory tree.

Open in CLI from the GUI

File → Open in CLI (Ctrl+Alt+T) opens an independent terminal for the saved NC file. A colored welcome screen shows help and short examples for folder analysis and batch DXF export. Commands run only when entered. Options → General → CLI terminal selects a terminal or automatic detection.

NC

FULL normalizes source blocks using the execution map and unfolds Macro B, IF/GOTO, subprograms and turning G70–G76 cycles. EXPANDED is one universal serializer of the resolved execution through a configurable JSON controller profile. Every user output option stays available across targets; the profile only supplies syntax and defaults.

DXF

Export resolved toolpath geometry to DXF.

The same kernel without the GUI

Use parse, trace, analyze and export for individual programs. Use batch for directory analysis and batch-export for directory export. Both batch commands reuse the single-file APIs.

CLI commands, controller conversion and export limits

Controller postprocessing

Choose EXPANDED EXECUTION and the target controller. Kernel geometry and states are emitted through JSON profiles fanuc_mill, fanuc_mill_multiaxis, fanuc_lathe_a, fanuc_lathe_b, sinumerik_iso, sinumerik_840d, sinumerik_840d_multiaxis and heidenhain_itnc530. Auto (source controller) picks the profile matching the source; SINUMERIK turning currently falls back to FANUC lathe A/B. Select an external profile with --post-profile path/to/post.json.

Target profiles define syntax, mandatory frames, capabilities and defaults. User formatting options — G90/G91 coordinates, sequence numbers, delimiter, leading zero, modal feed, decimal precision, force decimal, plus sign, arc output and start/end program text — are honored across FANUC and SINUMERIK targets; a profile default is used only when the user does not choose. Cycles and variables are resolved by the kernel; supported drilling and tapping operations use the selected post's cycle templates. Ordinary paths use a zero-offset G54 frame; supported tilted-plane programs retain G54–G59 and require matching target offsets. Three-axis posts reject rotary/TCP geometry; multiaxis posts reconstruct configured indexed A/B/C, verified simultaneous table-C motion and supported angled AC/BC TCP. Experimental indexed AC/BC conversion reconstructs supported G68.2/G53.1 and CYCLE800 frames through the bundled multiaxis posts. Other displaced-WCS indexed cases and unverified geometry-changing commands remain unsupported.

Five-axis FANUC ↔ SINUMERIK conversion is experimental, may contain errors, and is used entirely at your own risk. Successful export or a clean Tokens table does not guarantee safe machining. Before running on a machine, independently verify the controller/post, kinematics, WCS, tool numbers and length offsets, compensation, rotary branches and approach/retract moves; check the output in machine simulation and perform a controlled dry run. OEM CYCLE800 retract paths are not modeled.

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.

Settings → Options → General → 840D Extended cycles selects the native cycle interface: checked uses Siemens 03/2009, unchecked uses classic 01/2008. CLI retains --sinumerik-cycles classic|sl; this selection does not enable unsupported cycle operations.

The profile's format.words controls frame-word order and mandatory output. Each token (motion, X, Y, Z, A, B, C, I, J, K, R) has an order and a required flag with optional decimals/sign. required forces an address to be emitted when it has a resolved value; motion.required=false makes the motion code modal. An axis entry is only valid when the axis is declared in supports.axes, and F is excluded because feed is controlled by Modal Feed.

FULL preserves the source dialect and ordinary blocks, unfolding only flow-dependent FANUC Macro B / IF/GOTO / subprogram constructs and turning G70–G76 when required for safe normalization. Supported native SINUMERIK expressions and WHILE/GOTO/IF flow are preserved; native jumps retain numeric labels and reject sequence renumbering. EXPANDED resolves their executed geometry, but CSS export requires a reliable reference axis. DXF writes motion geometry independently of NC post formatting.

.\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
.\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

Compare generated NC directly with a UTF-8 reference using --compare-with expected.mpf. Exit codes: 0 for a match, 1 for a mismatch with unified diff on stdout, 2 for an error. LF/CRLF differences are ignored; spaces, comments and the final newline are compared. The reference is protected from overwrite.

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

Analyze a folder and collect reports

Scan programs and subdirectories, collect execution errors and warnings, and generate an HTML statistics report for each file. CSV helps identify programs that need attention; JSON retains the detailed diagnostics.

.\easy_gcode_plot_cli.exe batch ".\programs\milling" --lang fanuc_mill `
  --html ".\reports\html" -o ".\reports"
  • reports/batch_report.csv — per-file status, counts and diagnostics, ready for a spreadsheet.
  • reports/batch_report.json — summary and detailed results for further processing.
  • reports/html/…/part.nc.html — one report per program; subdirectories and input suffixes are retained.

Without --lang, native turning signatures select turning for MPF/SPF; other MPF/SPF and H files select milling. Other extensions default to turning. For a folder of FANUC milling programs, explicitly use --lang fanuc_mill.

Export a folder while keeping its structure

Apply one export configuration to every program: expanded NC, FULL source normalization or DXF. Results go to a separate directory with the same relative subdirectories.

.\easy_gcode_plot_cli.exe batch-export ".\programs\milling" --lang fanuc_mill `
  --mode expanded -o ".\exported"

For DXF toolpaths, add --format dxf. Use --mode full for source-preserving normalization, or --mode expanded --post-profile ... for controller postprocessing.

  • Exported NC or DXF files follow the input directory structure.
  • batch_export_report.csv and batch_export_report.json record output paths, status, diagnostics and effective export settings.
  • A failed file is reported while processing continues with the remaining files.

The output directory must be outside the input tree. Choose the machine type and supported target for the folder; unsupported conversion is recorded as an error rather than silently changing the program. The four shipped conversion scripts are covered by a semantic regression gate that re-executes successfully exported programs and compares their trajectory signature with the source.

Scanning, encodings and rotary profiles

--extensions .nc,.mpf,.spf limits the files processed; --top-level-only disables recursive scanning. Use --encoding cp1251 for legacy Cyrillic NC files.

Use --kinematics for a shared rotary profile or --kinematics-map profiles.json to assign profiles by input-relative filename. Export uses the same controller and geometry limits as single-file processing.

The examples use the Windows CLI executable. On Linux, use ./easy_gcode_plot_cli with the same arguments.

CLI commands and examples →

Supported commands and cycles

Inspect command coverage by controller. The FAQ contains exact parameter limits and diagnostics.

Open the controller reference

FANUC Turning — Type A / Type B

FANUC Turning Type A / 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
Turning cycles
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 behavior
Cycle Description
G70

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.

G71

The common two-line FANUC form is modeled:

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. After the final contour pass, retract by R, return along Z, then return X to the cycle start. Curved contour sections remain analytical arcs through allowance calculation and Type I pass generation. A configured turning tool's nose radius and tip orientation are used in roughing; without a tool table, geometry is nominal.

G72

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

Typical two-line form:

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.

G73

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.

G74

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.

G75

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.

G76

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

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.
G83

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.
G84

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

G90

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.

G92

Example:

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.

G94

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

G71 Type II supports pocketed profiles conservatively. G72 Type II rejects multiple disjoint spans in one facing plane (UNSUPPORTED_G72_TYPE_II_SPANS). G76 supports tool angles 0°, 29°, 30°, 55°, 60° and 80°; other angles produce UNSUPPORTED_G76_TOOL_ANGLE.

Parameters and limitations in the FAQ →

FANUC Mill

Milling G functions
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 on the angled AC/BC table profiles, including Cartesian arcs with rotary interpolation; combination with G68.2 remains 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; expressions support bitwise AND/OR/XOR and LN/EXP
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
G74 / G84 Q Left tapping and synchronized peck tapping. Kernel options milling_tapping_retract_distance and milling_tapping_full_retract model parameters 5213/5200.
G76 / G87 Fine/back boring with Q shift and oriented spindle stops. milling_boring_shift_direction supplies parameter 5101 direction; the logical default is -X.
G89 / G92.1 Feed-return boring with dwell / coordinate preset without physical motion.
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: 1/F minutes per cutting block. Reprogram positive F on G93/G94/G95 changes; 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
Milling M functions
M code Function in the kernel
M00 / M01 Stop / optional-stop signal; trace execution continues
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 Non-blocking warnings; motion and known commands in mixed blocks still execute.
Milling cycle behavior
Command Description
G73 / G83

G73 is high-speed peck drilling with short intermediate retract behavior. G83 returns to R and rapidly re-enters at clearance d above the previous depth, bounded by R, before continuing at feed. The kernel option milling_g83_clearance sets d in millimetres; the default 1.0 mm is a modeling assumption, not a value read from the controller. This affects feed distance and cycle-time statistics. Turning and native CYCLE83 are unchanged.

G82

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

G84

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

G86

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

G98 / G99

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

Parameters and limitations in the FAQ →

SINUMERIK 840D ISO-M — G291

SINUMERIK ISO-M
ISO-M function Support and limitations
G290 / G291 Standalone blocks select native / ISO-M mode. MPF/SPF execution starts in native mode.
XYZ / G90 / G91 Three-axis positioning, including incremental positioning. Rotary axes and TCP are unsupported.
G2 / G3 / IJK ISO-M and native use incremental IJK centers. Native I=AC(...), J=AC(...), K=AC(...) explicitly select absolute centers; G90/G91 controls endpoints.
G54 P1–P48 Extended work offsets. Source G54.1 and other decimal G codes are rejected.
G50 / G51 Coordinate scaling; G51 uses P/1000 weighting.
G68 / G69 Standalone 2D rotation with G90, center axes of the active plane and R. I/J/K, incremental-angle and 3D-vector forms are rejected.
Cycles and units Common integer milling G codes, unit selection, coordinate systems and selected canned cycles are accepted within the ISO-M subset.
Unknown auxiliary M codes Non-blocking warnings, including mixed motion blocks. M98 is not a FANUC subprogram call here; M99 remains unsupported. M2/M30 end the program.
Macro B / ISO-T Macro B program flow is unsupported. Turning mode supports a bounded ISO-T motion/threading subset; ISO turning cycles remain unsupported. Unsupported ISO functions produce diagnostics.

Parameters and limitations in the FAQ →

SINUMERIK 840D native — G290

Native XZ turning is also supported in MPF/SPF: DIAMON/DIAMOF/DIAM90, G33, spindle/CSS with LIMS, WCS, and bounded CYCLE93/95/97 and centerline drilling subsets. Standalone G290/G291 switches select native/ISO-T in turning mode. See the turning coverage and limits. Native turning FULL normalization and a Siemens turning output post are not implemented.

CYCLE95 uses the nominal contour; automatic tool-nose correction is unverified for configured nonzero nose radii. Completion does not establish controller equivalence. Allowance and pass-planning differences need independent validation with known tool data; another backplotter is not a normative Siemens reference. The table below describes native milling, whose command policy differs from turning.

SINUMERIK native
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, G70/G71/G700/G710 Absolute/incremental coordinates and work offsets. G70/G71 select inch/metric lengths; G700/G710 also select feed units.
G60 / G64 Exact-stop / continuous-path metadata; acceleration, stop time and blending are not simulated.
G93 / G94 / G95 Inverse-time / per-minute / per-revolution feed. G93 uses 1/F minutes per cutting motion; reprogram positive F on mode changes. G93 cycles and cutter compensation are unsupported.
G500 Modal deactivation of the settable work offset until the next G54–G59 call. Coordinates are rebased without motion. Default: zero G500 and base frame; API wcs_offsets[500] can supply a translation. OEM base-frame rotations, mirroring and scaling are not modeled.
DIAMON / DIAMOF / DIAM90 Parsed with warnings; execution continues using DIAMOF semantics for all coordinates. Diameter programming is not simulated.
CHR / RND Nonmodal chamfers and rounding between continuous planar G1 elements, before cutter compensation. Fixed rotary and tilted working planes use local coordinates. A selected profile alone does not alter a three-axis contour.
CHF / RNDM / FRC / FRCM Parsed with warnings without changing geometry or feed. Modal rounding and corner feed are not simulated; RNDM=0 is recognized but has no geometric effect. Reports retain these warnings; resolved NC export is rejected.
G40/G41/G42 Modeled cutter-radius compensation using the configured tool with TCP off. G41/G42 under active TRAORI is not modeled and stops execution with UNSUPPORTED_TCP_CUTTER_COMPENSATION.
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
G0 SUPA ... D0 Nonmodal machine-coordinate positioning; zero XYZ addresses use the configured G28/SUPA return coordinates in the application's reference-coordinate model, as FANUC G53 does. WCS and the rotary frame determine the displayed position
Configured A/B/C axes are also supported, including rotary-only blocks. SUPA targets remain absolute under G91.
G64, MSG(...), WORKPIECE(...), ; comments Path-control/display metadata and comments; no blending or stock geometry is generated from these declarations
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
CYCLE83 Modeled first depth, amount degression, minimum peck depth, chip-breaking/full-retract options and reentry clearance
CYCLE84 Metric right/left rigid tapping in G94, including VARI=1/2 deep tapping with DAM/VRT and balanced final steps. PIT is explicit; SST matches S and SST1 is equal or omitted. SDAC=3/4/5 is retained. Synchronized withdrawal reaches RFP+SDIS, followed by rapid return to RTP.
CYCLE85/86/87/89 CYCLE85 uses separate cutting/return feeds FFR/RFF; CYCLE89 feeds in and out with dwell. CYCLE87 records spindle stop and operator stop, then rapid withdrawal. CYCLE86 includes oriented stop POSS and the signed RPA/RPO/RPAP clearance move.
G2/G3 Two endpoint axes select a block-local circle plane; the modal G17/G18/G19 plane is retained for subsequent blocks.
TRAORI / TRAFOOF GUI/CLI/kernel TCP via the common angled AC/BC table profiles; G0/G1/G2/G3 with configured numeric rotary axes
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, legacy R_DATA setup and active-frame reset supported
TRANS / ATRANS / ROT / AROT / RPL= Programmable rigid frames: replacement/reset or composition in local axes, preserving physical tool position. XYZ rotation uses RPY (MD10600=1); RPL rotates in the active plane. FULL preserves commands; EXPANDED resolves their geometry. Active TWP/TCP, polar mode, cycles and compensation cannot be combined with these frames.
G505–G599 / G601 / G641 / G642 / G645 Unverified warnings; controller-specific effects are not simulated.
Unknown auxiliary M codes Non-blocking warnings; motion and known commands in mixed blocks still execute. M2/M30 end programs. Native M17/M96/M97/M99 stop with unsupported-flow diagnostics; M66/M98 warn without subprogram dispatch.
CIP / I1= / J1= / K1= Spatial circular interpolation through three points, including G90/G91 and AC/IC intermediate coordinates. Plot/Playback preserve the circle; EXPANDED uses G1 chords within the configured linearization tolerance. Requires a fixed frame, G40 and no active cycle.
DEF REAL / named-scalar assignments Underscore-named scalar variables default to zero; direct numeric, R and scalar assignments are supported. Arrays and compound named-scalar assignments are rejected; R expressions use the separate subset below.
I/J/K / AC(...) Plain IJK offsets are relative to arc start. AC explicitly selects absolute centers, including mixed center addresses. Source Arc Type and autodetection do not override SINUMERIK syntax.
T="name" / M6 / T0 Case-sensitive named tool selection; M6 activates the selected tool and T0 with M6 unloads it. G41/G42 remains unverified without configured cutter geometry.
D0..D12 under TRAORI Cutting-edge selection preserves the active TCP transform.
FNORM / COMPOF / SETMS(1) Normal feed and compressor-off metadata; only main-spindle selection SETMS(1) is accepted.
CYCLE832(...) Ignored without geometry or display events; zero to three direct arguments are accepted.
CYCLE81(RTP,RFP,SDIS,DP) The four mandatory arguments are accepted; DPR is optional.
CYCLE800: 14/15/16 arguments Classic calls may omit FR_I/DMODE; new/additive frames use the common swivel model. OEM machine configuration and retract paths are not inferred.
DC(...) Shortest-path absolute approach for configured rotary axes; exactly 180-degree ambiguity is rejected. Signed or unwrapped Fusion DC targets are reduced modulo 360 for backplotting with a source warning; this does not certify controller acceptance.
R assignments / address and cycle expressions Bounded + - * /, parentheses, comparisons and SIN/COS/ABS/SQRT; trigonometry in degrees. Siemens R state is separate from FANUC variables.
WHILE / ENDWHILE / GOTO / IF GOTO Nested loops and numeric N-label jumps. Shared execution/iteration limits and cancellation apply; invalid flow stops with source-line diagnostics.
M19 Spindle-orientation signal without motion or a spindle-state change.
G96 / G961 / G97 / G971 CSS / CSS / RPM / RPM with per-revolution / per-minute / per-revolution / per-minute feed. CSS retains surface speed; instantaneous milling RPM is not inferred.
ANG / SCALE / ASCALE / MIRROR / AMIRROR Recognized but geometry is unmodeled; execution stops before motion.
POCKET3 / POCKET4 / CYCLE90 Classic 01/2008 pocket roughing/finishing and internal/external thread milling. Configured cutter, G17/G40/G80, feed per minute, no active MCALL or TCP. Extended signatures and preformed-blank variants are unsupported; internal passes are not independently controller-verified.
HOLES1 / HOLES2 Six-argument row/circle patterns invoke the active supported MCALL drilling cycle in G17 without TCP. HOLES1 starts from the nearer row end; omitted/zero HOLES2 INDA gives equal spacing.

GUI/CLI/kernel TRAORI/TRAFOOF supports TCP on the angled AC/BC table profiles, including rotary arcs. Numeric A/B/C and direct R references, incremental IC and shortest-path absolute DC require a matching profile. Exact DC half turns remain rejected. CYCLE800 uses Siemens matrices and the common TWP core; OEM retract paths are not simulated. G70/G71 select inch/metric lengths without changing feed units; G700/G710 also select feed units and retain the modal numeric F. G93 uses 1/F minutes per cutting motion, including rotary TCP motion; F must be positive. Reprogram F on G93/G94/G95 changes. G93 cycles and cutter compensation are unsupported. ORI*, FGROUP, FL[], FGREF[], SPOS and CUT3D* are warning-only and unverified. SCALE/ASCALE and MIRROR/AMIRROR and ANG are recognized with unmodeled geometry and stop execution. R parameters support bounded arithmetic, comparisons, parentheses and SIN/COS/ABS/SQRT; trigonometry uses degrees. WHILE/ENDWHILE supports nesting, and GOTO/IF GOTO use numeric N labels. Missing targets, malformed flow and invalid expressions fail closed; execution and iteration limits and cancellation remain active. GOTOF/GOTOB/GOTOC, RET and arbitrary subprogram calls are unsupported. M19 emits spindle orientation without motion or a spindle-state change. G96/G961 select CSS with revolution/linear feed; G97/G971 select RPM with revolution/linear feed. CSS stores surface speed without inferring instantaneous RPM from milling X. FULL preserves supported native flow; EXPANDED exports resolved geometry but rejects CSS without a reliable reference axis. CYCLE84 supports right/left metric tapping and chip-breaking/full-retract pecks; unequal entry/withdrawal speeds and thread-table/technology options remain outside the modeled subset.

Parameters and limitations in the FAQ →

HEIDENHAIN iTNC 530 — native Klartext

Native three-axis, indexed 3+2 and AC/BC table TCP input in version 2.9.7. Opening .h/.H selects Klartext automatically; iTNC-code selects it manually. Unsupported execution stops at the source block with a diagnostic.

HEIDENHAIN iTNC 530 commands and cycles
Native function Support and limitations
BEGIN/END PGM, MM/INCH, BLK FORM 0.1/0.2 Program metadata, units and stock bounds.
L, IX/IY/IZ, F/FMAX/FAUTO, R0/RL/RR XYZ straight motion, incremental coordinates, feeds and planar cutter compensation.
CC, C, CR, CT, DR+/DR− Circle centers, full/partial circles, radius and tangent arcs.
LP, CP, PR/IPR/PA/IPA Polar positioning and polar/helical circular motion.
APPR/DEP LT/LN/CT/LCT Approach/departure lines and tangent arcs to planar contours.
TOOL CALL, TOOL DEF, S/F Numeric, named and Q tools; spindle and feed state. DL/DR/DR2 tool offsets are not executed.
M0/M1/M2/M3/M4/M5/M6/M8/M9/M13/M14/M30 Logical stops, spindle/coolant signals and program end.
M91 Nonmodal absolute machine XYZ with configured WCS.
Q/QL/QR, FN 0–4/6/7, expressions Bounded arithmetic and trigonometry; FN 6/7 use degrees.
LBL, CALL LBL, REP, FN 9–12 Numeric/named labels, calls, repeats and conditional GOTO.
CYCL DEF, CYCL CALL, M99 Drilling/boring/tapping cycles 1/2, 200–209, 240/241 within supported parameter subsets; cycle 9 dwell. Cycle 32 stores metadata without smoothing simulation.
CYCL DEF 220/221 DEF-active circular/grid patterns execute the previous supported machining cycle at each position. Explicit Q parameters and R0 are required; no extra CYCL CALL triggers the pattern.
CYCL DEF 251/252/262 Rectangular/circular pocket roughing and finishing; internal thread milling with analytic helices. XY/Z, R0, M3/M4 and cutter geometry are required. Helical/reciprocating pocket roughing needs an explicit tool ANGLE. Unsupported variants are diagnosed; internal passes are not independently controller-verified.
Q cycle continuations, Q208=MAX Cycle parameters are consumed in execution order; symbolic rapid retraction feed is supported for cycles 202/203. Q253 MAX/FMAX selects rapid pre-positioning in cycles 204/205/241/262.
Cycles 7/10 Axis-address datum shifts and XY planar rotation (ROT); zero resets. Datum-table and tilted-plane variants are unsupported.
Cycle 247, Q339=1..6 Selects the application's configured G54–G59 offsets while preserving machine position. Other preset numbers are unsupported.
M140 MB distance / MAX Retraction follows physical machine +Z, mapped through configured table orientation. MAX uses Z from Home (G28) in WCS with Home emulation enabled, in the positive direction only. The approximation emits a warning and blocks NC trace export; physical travel limits are not modeled.
F0, optional / blocks F0 retains geometry with a warning. Optional blocks follow Block Skip settings.
RND / CHF Planar tangent rounding and straight-line chamfers before RL/RR compensation, with block-local feeds.
A/B/C, IA/IB/IC Rotary indexing requires a matching configured profile, including zero angles. Continuous rotary L motion requires active TCP.
PLANE SPATIAL SPA/SPB/SPC, PLANE RESET STAY changes the coordinate frame; TURN solves orientation with two rotary joints. SEQ+/SEQ− select the swivel branch. MOVE and TABLE COORD are unsupported.
M128/M129, FUNCTION TCPM / RESET TCPM Logical tool-tip control on AC/BC tables with PLANE reset. The supported FUNCTION form is F TCP AXIS POS PATHCTRL AXIS. Traces retain start/end tool orientations.
M126/M127, M94 Enable/cancel shortest-path rotary positioning and reduce displayed rotary angles.
M120, U/V/W, tool offsets DL/DR/DR2 Not executed; unsupported operations stop with a source diagnostic. OEM pivot lengths and full machine collision simulation are outside the model.
Save Source / EXPANDED / FULL Save retains source. EXPANDED exports a supported resolved three-axis trace via the selected post. Klartext FULL formatting is unavailable.

The three-post CAM project in milling/test_5ax reaches M30 for FANUC, SINUMERIK and HEIDENHAIN with 5ax_table_ac and Home Z=100. Tests compare 1182 normalized cutting segments, arcs and tool axes with a 0.002 mm positional tolerance. GPU stock removal remains three-axis. See the iTNC coverage and parameter limits.

A CLOSER LOOK

CIMCO Edit 8 & Easy G-Code Plot

Compare MDI, text comparison, FANUC, SINUMERIK and HEIDENHAIN support. Updated for 2.9.7, with sources, tested scope and explicit unknowns.

Read the full comparisonFANUC Mill · FANUC Lathe · 840D · iTNC 530

Comparison of document editing, text comparison, FANUC milling, FANUC turning, native SINUMERIK 840D milling/limited XZ turning and native HEIDENHAIN iTNC 530 Klartext. Русская версия.

Scope: CIMCO Edit 8 editor and Backplot, not CIMCO Edit 2022–2026 or the separate CIMCO Machine Simulation product. Easy G-Code Plot describes the 2.9.0 working tree and its regression fixtures. The MDI/Compare update concerns the editor; controller-command rows retain their previously stated evidence. This is a capability comparison, not a measured accuracy or performance ranking.

Legend: ✅ supported within the stated scope; ⚠️ partial or restricted; ❌ explicitly unsupported; ? not established for CIMCO Edit 8. Unknown does not mean unsupported. ≈ means comparable only within the stated scope. A command in a filter is not evidence of correct geometry. Statements marked [N] are historical comparison notes, not vendor certification.

What's new in 2.9.0: external CLI integration

File → Open in CLI opens a separate persistent Windows/Linux terminal for the saved NC file, forwarding supported CLI document parameters. File toolbar customization and hotkeys reuse the same action. Options provides a terminal path or automatic detection; the terminal shows DXF, conversion and batch commands. This is a launcher for the existing CLI, without an embedded console or a second CNC implementation.

The editor also has separate controller snippet spaces with validated input fields, context literals, arithmetic and degree-based trigonometry. Insert shows parameters and an optional zoomable SQLite illustration, without a text preview. Built-in entries cover program/cycle fragments, tool-description comments, spindle speed, drill-point height and separate MM to INCHES / INCHES to MM conversions. Picture manages attachments; Update Defaults restores the selected controller's standard texts and missing bundled pictures while retaining custom-named entries and existing attachments. This describes the Easy G-Code Plot implementation; it does not change the stated CIMCO ratings.

Features introduced in 2.8.0: native milling cycles

HEIDENHAIN input now executes bounded 220/221 patterns, 251/252 pockets and 262 thread milling. SINUMERIK input executes classic 01/2008 POCKET3/4, HOLES1/2 with supported MCALL drilling, and CYCLE90. Required tool data and unsupported variants are described in the FAQ. These are implementation capabilities; their internal passes have not been independently confirmed against controller trajectories. No new paired CIMCO measurements or export-cycle capabilities are implied.

What's new in 2.7.0: native iTNC rotary execution
  • Bounded native SINUMERIK XZ turning and ISO-T input, including the implemented CYCLE93/95/97 subsets. CYCLE95 nominal-contour execution and its unverified nose-compensation warning do not establish controller-equivalent geometry. DXF observations from another backplotter are comparison evidence, not a normative Siemens reference. See turning coverage and limits; no new CIMCO support or accuracy rating is inferred here.
  • Native PLANE SPATIAL/RESET with STAY/TURN, SEQ branch selection, A/B/C indexing and AC/BC table M128/M129 or the supported FUNCTION TCPM form. Continuous rotary motion requires L blocks and active TCP.
  • The supplied three-post CAM project reaches M30 on all three dialects with 5ax_table_ac and Home Z=100. Tests compare 1182 normalized cutting segments, arcs, feeds, tools and start/end tool axes within 0.002 mm positional tolerance. This verifies the reference project, not arbitrary posts or full machine simulation.
What's new in 2.6.0: view rotation
  • Rotate view rotates Top/Front/Left around model X/Y/Z without CNC recalculation, retaining scale and per-document camera state. Available in View, plot context menus, toolbar customization and Hotkeys; disabled in ISO/3D and turning. Grid and ruler follow coordinate planes and are disabled at oblique angles.
Document and controller features retained from earlier releases
  • MDI and Compare were introduced in 2.4.0; native HEIDENHAIN input and three-axis execution in 2.5.0; RND/CHF contour geometry in 2.6.0.
  • MDI keeps multiple NC programs in one workspace. The application starts with one empty milling document. Use + / File → New, the document-list arrow and × / Ctrl+W to create, select and close documents. Opening an already open file selects its existing buffer; opening a different file preserves nonempty documents and their unsaved edits. Close All and application exit check each modified document for Save, Discard or Cancel.
  • Each document retains its text and undo history, cursor/selection, encoding, machine mode, source overrides, current-program tools, cached execution, view direction and playback position. Stock settings, STL objects and STL edit history also belong to the document. Shared Options, saved libraries, WCS/Home and rotary selection remain application preferences; changed shared CNC inputs make an inactive cached trace stale on selection. Finish or cancel pending editing dialogs before switching documents.
  • CNC Functions → Compare opens two read-only text panes with file selectors, a resizable splitter and synchronized vertical/horizontal scrolling. Sources can be open MDI buffers, including unsaved text, or independently selected disk files decoded through the existing UTF-8/legacy mechanism. Yellow marks changed lines, green added lines and red removed lines; display padding aligns corresponding rows. Refresh reloads selected disk files and rereads MDI buffers without replacing unsaved documents. Copying and both application themes are supported. The command participates in Hotkeys and Customize Toolbars.
  • Easy Compare is an ordinary line diff: spacing, block numbers and comments remain significant; CRLF/LF line endings are normalized. It does not merge/edit sources, save/print diff reports or compare CNC semantics, geometry or toolpaths. These limits distinguish it from CIMCO's configurable File Compare; they do not change the execution kernel or export capabilities.
  • Menu groups follow the document workflow. View → STL Objects opens the scene panel; CNC Functions → Tokens/Variables opens the inspector. Settings → Options contains editor, plot, hotkey, postprocessor and rotary-profile preferences. Customize Toolbars restores compact default groups while leaving saved button selections intact until an explicit reset; printing, clipboard/formatting buttons and calculators are optional.
  • iTNC-code provides highlighting for native Klartext input. .h/.H opens with a native immutable AST and three-axis execution for L/CC/C/CR/CT/LP/CP, APPR/DEP, tools, feeds, spindle, M91, Q parameters, label flow and drilling/boring/tapping cycles; Cycle 32 retains smoothing metadata. RND/CHF construct programmed-contour geometry before existing RL/RR/R0 compensation. Configured rotary indexing, PLANE SPATIAL/RESET and AC/BC table M128/TCPM execution are available in 2.7.0. Tool offsets DL/DR/DR2, auxiliary axes and M120 remain unsupported. See the iTNC input coverage in the FAQ and section 4 below. The existing Heidenhain export post has separate coverage.
Editor and document workflow
FeatureCIMCO Edit 8Easy G-Code Plot 2.9.0Assessment
Multiple open programs / MDI✅ multiple file windows [C7]✅ independent buffers and document scenes; compact controls without visible tabs [E]Both support multiple programs; window organization differs
Side-by-side text comparison✅ two-pane comparison with colored differences [C7]✅ read-only aligned line diff; changed/added/removed colors and synchronized scrolling [E]≈ feature present; comparison options differ
Compare unsaved open buffers and disk files? exact unsaved-buffer contract not established here✅ current MDI text or independent disk snapshots; no document replacement [E]Easy behavior is covered by regression tests
Ignore formatting or selected text categories✅ optional ignoring of block numbers, spaces, comments, case and numeric formatting [C9]❌ no such filters; ordinary text diff with normalized line endings [E]CIMCO offers additional comparison filters
Editing / synchronizing differences✅ editing modes and difference synchronization documented [C9]❌ read-only; no merge or synchronization of source text [E]Different scope; synchronized scrolling is not merging
Print a comparison report✅ side-by-side/differences printing [C8, C9]❌ no diff-report printing or saving [E]Separate from Easy's existing CNC export and plot printing
Token/diagnostic filters? equivalent V8 workflow not established here✅ All/Warnings/Errors, shown/total count and case-insensitive text search; copying and CSV respect filters. Opening/refreshing reuses the current execution result [E]Tokens workflow; filtering does not recalculate; missing/stale results require analysis
Missing/incompatible rotary profile? equivalent notification not established here✅ persistent plot notice with detected axes and source line; direct profile selection and editor navigation, including zero-angle addresses [E]Rotary workflow; machine geometry is not inferred from axis letters
Controller variable inspector? equivalent snapshot coverage not established here✅ Variables: FANUC numbered/named, SINUMERIK R/named and HEIDENHAIN Q/QL/QR snapshots; dialect, source line and occurrence context, numeric ordering and CSV [E]Recorded variable state; playback reads existing execution snapshots

Implementation and regressions: MDI, MDI tests, Compare, Designer dialog, Compare tests, Hotkeys, toolbar customization.

Backplot capabilities in the current version
  • G0 stock contact is visualized in both machining modes. Milling GPU removal retains a rapid-damage marker in the height field; turning marks the intersection with remaining material without removing it on G0, restores marks on rewind and clips them as later cuts remove the affected material. Neither model checks holders, fixtures or machine components.
  • Settings → Options → Rotary Kinematics contains 24 read-only built-in configurations, named user copies, table/head ownership, signed direction vectors, joint order and visibility. Optional paired Min/Max angular limits on user copies produce nonblocking source-line warnings; they do not alter geometry, wrap angles or select another inverse solution.
  • Milling 3D picking selects sampled lines and arcs by camera depth and synchronizes the editor and playback occurrence. Shift+left-click remains the default. Settings → Options → General → Cimco Like Picking enables left-click selection and right-button panning, with a context menu on a right-click without dragging.
  • Measure provides two-point coordinates and distances in fixed XY/XZ/YZ and turning views. It has priority over trajectory picking while active; turning displays diameter coordinates separately from physical distances. Measure in a free 3D view remains outside its scope.
  • The 2.0 release adds 3D Stock Removal for three-axis FANUC and native SINUMERIK milling, alongside existing 2D turning stock removal; 2.5.0 extends it to native HEIDENHAIN iTNC three-axis Klartext. The current comparison includes the 2.7.0 native rotary execution updates.
  • Milling removal runs on the GPU using configured cutter geometry and a sampled height field. It supports box stock, vertical cutters, playback/rewind, five Accuracy levels and STL export of the current machining stage. OpenGL 4.3 is required; rotary/TCP removal, undercuts and subtraction from imported STL solids are outside this model.
  • Milling and turning use the same Stock Removal button and Stock dialog, with settings for the active machining mode. Imported STL models remain visual references.
  • Previously checked FANUC/SINUMERIK comparison rows retain their recorded evidence; they have not undergone a new paired CIMCO review. This does not imply unchanged language support: native HEIDENHAIN execution was added in 2.5.0 and RND/CHF geometry in 2.6.0. Stock removal is distinct from full machine collision simulation.
Language updates retained from 1.9.8
  • FANUC milling adds G74 left tapping, G76 fine boring, G87 back boring and G89 dwell/feed-return boring. G74/G84 Q now produces synchronized tapping pecks. Q shift direction and tapping retract behavior are configurable machine assumptions.
  • Native SINUMERIK adds CYCLE85/86/87/89 and extends CYCLE84 to metric right/left and deep tapping, including VARI=1/2, DAM/VRT and balanced final pecks. CYCLE88 remains unsupported.
  • Siemens circles can select a block-local plane from two endpoint axes; helical TURN moves retain the modal plane. Pure rapid rotary indexing can retain an active CYCLE800 frame.
  • Both Fusion 1001 regression programs reach M30 on 5Ax Table AC. Tests cover home Z=0 and 500. This verifies those fixtures, not arbitrary CAM output. Missing tool geometry leaves compensation unverified. Out-of-range DC angles are normalized with warnings for backplot compatibility; that does not validate them for a real controller.
  • G92.1 zero-valued axis selectors are treated as coordinate preset without physical motion. The model has no manual/G92 shift to cancel. FANUC G53 machine coordinates and configured G28 reference returns were already supported.
  • An invalid arc produces a diagnostic and execution can continue to later blocks. Completion and validity are separate result fields; reaching M30 alone does not establish a valid result.
Visualization and configuration
FeatureCIMCO Edit 8Easy G-Code Plot 2.9.0Assessment
Stock contact on G0? exact remaining-stock/damage contract✅ milling rapid-damage markers and turning remaining-stock intersectionsPresent in both Easy modes; no paired accuracy test
Rotary profile editor and limits✅ 4/5-axis setup [C2]; exact limit contract unconfirmed✅ Options tab, named copies, optional angular warning limitsSettings do not establish physical machine equivalence
Milling 3D toolpath picking? exact selection/control contract✅ depth-aware line/arc selection; source and playback synchronizationNo new CIMCO binary comparison
Optional mouse controls? exact binding contract✅ default Shift+left-click or Cimco Like Picking; click/drag separationEasy offers two control modes
Two-point measurement? V8 contract not established here✅ fixed milling views and turning; editable coordinates and mm/inchFree 3D Measure is not supported

Implementation and regressions: navigation, 3D picking, Measure, rotary limits, turning collisions, milling rapid damage.

1. FANUC milling
Area / commandCIMCO Edit 8Easy G-Code Plot 2.9.0Assessment
G0/G1, modal XYZ✅ Backplot [C1]✅ execution and motion trace≈
G2/G3, IJK, R✅ configurable arcs [C1, C2]✅ absolute/incremental IJK and R≈; variants not compared
Full circles✅ zero-arc setting [C2]✅≈
Helical G2/G3? exact geometry✅ analytic arcs and helicesNot established
G4✅ [C1]✅ dwell signal≈
G17/G18/G19✅ [C1]✅≈
G20/G21✅ [C1]✅ units and mm/inch export≈ for input
G90/G91✅ [C1]✅≈
G28✅ [C1]✅ configured home and intermediate point≈ in basic use
G53? exact nonmodal contract✅ machine-coordinate G0/G1Not established
G30?❌ second reference return not modeledNot established
G54–G59✅ [C1]✅ WCS offsets≈
G54.1 P1–P99?⚠️ selection; zero offset without G10 L20Not established
G10 L2/L20? runtime WCS programming✅ runtime WCS updatesNot established
G52?✅ local shiftNot established
G68/G69✅ filter and fixes [C3]✅ plane rotation/cancellationPresence comparable; accuracy untested
G50/G51 scaling?⚠️ restricted scaling modelNot established
G15/G16 polar?⚠️ polar coordinates with arc restrictionsNot established
G40/G41/G42✅ compensation settings [C1, C2]✅ supported 2D geometry with known tool radiusNo paired accuracy test
G43 H / G49⚠️ recognized; author observed no H path shift [C3, U]⚠️ state retained; H does not shift plotted path [E]≈ observed geometry
G68.2/G53.1⚠️ G68.2 filter support; G53.1 contract unconfirmed [C3]✅ supported indexed AC/BC and two-axis profilesNot ranked
G43.4 TCP? V8 interpretation contract✅ restricted AC/BC TCP, G0/G1/G2/G3Not established
G68.2 with G43.4?❌ composition unsupportedNot established
Indexed 3+1 A/B/C✅ configurable 4/5-axis Backplot [C2]✅ selected A/B/C table profiles≈ supported profiles
Indexed 3+2✅ 4/5-axis setup; frame coverage unconfirmed [C2, C3]✅ supported G68.2/G53.1 subsetNot ranked
Continuous 4-axis X/C✅ 4/5-axis class [C2]; X/C semantics unknown✅ tested 4Ax Table C subsetNot established
Continuous 5-axis AC/BC✅ 5-axis Backplot [C2]; TCP scope unknown✅ AC/BC TCP and tool orientationNot ranked
Full machine simulation? not established for this Backplot❌No verified equivalence
Finished-part STL overlay? V8 overlay scope✅ visual STL overlay; removal uses separate box stockNot established
3D milling stock removal✅ Solid Animation [C2]✅ GPU three-axis box stock; height-field model, OpenGL 4.3 [E]≈ feature present; scope and accuracy not compared
G73 high-speed peck? exact semantics✅ restricted peck cycleNot established
G74 left tapping?✅ feed withdrawal; Q pecksNot established
G76 fine boring?✅ oriented Q clearance shift; configurable XY directionNot established
G80✅ [C1]✅ cycle cancellation≈
G81✅ [C1]✅≈
G82? exact form✅ bottom dwellNot established
G83✅ historical fixes [C4]✅ pecks with R-plane returns≈ cycle class; details unknown
G84 + M29✅ G84 [C1]; M29 unverified✅ rigid-tapping preparation, feed withdrawal, Q pecks≈ for G84 presence
G85✅ historical fixes [C4]✅ feed-return boring≈ cycle class
G86?✅ spindle-stop boring signalNot established
G87?✅ back boring with Q shift; always initial-plane returnNot established
G88?❌Not established
G89?✅ dwell and feed withdrawalNot established
G98/G99 cycles? exact geometry✅ initial/R-plane return; G87 always initialNot established
G92.1?⚠️ zero-selector preset, no physical motion or modeled manual shiftNot established
G93 inverse-time?✅ restricted rotary/TCP inverse-time feedNot established
G94/G95✅ basic programming; details unverified✅ feed/min and feed/rev≈ presence
M3/M4/M5, M6, M8/M9✅ example [C1]✅ states/signals, no machine physics≈
Variables and nested #[...]✅ nested variables in V8 FANUC/Haas filter [C3]✅ Macro B read/write and indirect variables≈ presence; depth unknown
Macro B IF/GOTO, WHILE/DO⚠️ V8 fixes; exact forms unconfirmed [C3]✅ executable expressions and flowNot ranked
G65 and local variables? runtime behavior✅ O macros, local stack, L repeatsNot established
M98/M99? exact runtime✅ subprograms and L; no M99 PNot established
EXPANDED / FANUC↔SINUMERIK? equivalent replay contract not found✅ semantic export; experimental AC/BCDifferent documented contracts
2. FANUC turning
Area / commandCIMCO Edit 8Easy G-Code Plot 2.9.0Assessment
G0/G1✅ turning Backplot [C5]✅ X/Z trace≈
G2/G3 I/K, R✅ turning examples [C5]✅ G18, absolute/incremental I/K and R≈ basic arcs
Diameter/radius programming✅ diameter setting [C2]✅ physical radius and diameter input mode≈
U/W incremental✅ relative-axis setup [C2, C5]✅ independent of X/Z mode≈
FANUC Type A / B? filter dialect distinctions✅ selectable A/B; no Type CNot established
G20/G21✅ [C5]✅ mm/inch≈
G53?✅ nonmodal G0/G1; arcs rejectedNot established
G28/G30? complete semantics✅ configured G28; no G30Not established
G54–G59✅ G54 example [C5]✅ WCS≈
G54.1 P / G10 L2/L20?✅ runtime offsetsNot established
G40/G41/G42 nose compensation✅ tool setup [C2, C5]; accuracy untested✅ supported 2D compensation with tool geometryNot ranked
T0101 tool/offset✅ [C5]✅ tool/offset state≈
G96/G97 CSS/RPM✅ [C5]✅≈
G50 S spindle clamp✅ [C5]✅≈
G98/G99 Type A feed✅ G99 example [C5]✅ feed/min and feed/rev≈
G94/G95 Type B feed? for Type B✅Not established
G32/G33 single threading? geometric execution✅ synchronized threading motionsNot established
G70 P/Q finishing✅ example and Backplot [C5]✅ P/Q profile expansion≈
G71 longitudinal roughing✅ OD/ID example and V8 fixes [C3, C5]✅ OD/ID passes; Type II restrictions≈ basic function
G72 face roughing✅ historical V7 fixes [C4]✅ restricted complex Type II≈ cycle class
G73 pattern repetition? in V8✅ repeated profile displacementNot established
G74 face peck/grooving✅ historical V7 fixes [C4]✅ Z direction≈ cycle class
G75 grooving✅ historical V7 fixes [C4]✅ X direction≈ cycle class
G76 multipass threading✅ two-line example and V8 fixes [C3, C6]✅ two-line passes, supported flank infeed and thread geometry; chamfer interval is axial≈ main cycle; not every variant
G83 axial peck drilling✅ historical mention [C4]✅≈ cycle class
G84 axial tapping✅ historical mention [C4]✅≈ cycle class
G90/G92/G94 Type A cycles? exact V8 geometry✅ modal turning/threading/facingNot established
G77/G78/G79 Type B cycles?✅ modal turning/threading/facingNot established
A contour angle?✅ restricted endpoint calculationNot established
C chamfer / R fillet?✅ G1 contour chamfer/filletNot established
Macro B, IF/WHILE, G65⚠️ V8 fixes; runtime not fully specified [C3]✅ shared milling/turning runtimeNot ranked
M98/M99?✅ O subprograms, LNot established
2D turning stock removal✅ Solid Animation [C2, C5]✅ calculated stock and thread profile≈ presence; different algorithms
C/Y mill-turn? for V8; later demos are not V8 evidence❌ in fanuc_turnNot established
Full machine simulation? not established for this Backplot❌No verified equivalence
Turning → EXPANDED? comparable mode not found⚠️ geometric export with turning-cycle restrictionsNot established
3. Native SINUMERIK 840D milling

SINUMERIK ISO mode is excluded from this comparison. Native-cycle support applies to documented parameter subsets, not every technology option on a Siemens controller.

Area / commandCIMCO Edit 8Easy G-Code Plot 2.9.0Assessment
G0/G1, modal XYZ✅ [N]✅≈
ANG=✅ [N]❌ unmodeled geometry stops executionCIMCO in historical comparison notes
CHF/CHR/RND✅ geometry [N]⚠️ CHR/RND geometry between planar G1 elements, including fixed tilted frames; CHF remains warning-onlyCIMCO in historical comparison notes
G2/G3, CR=, TURN=✅ G2/G3 [N]; extensions unconfirmed✅ arcs, CR/TURN, block-local circle planeExtended-form equivalence untested
CIP✅ [N]✅ spatial arcs through an intermediate point≈
G4 F/S✅ [N]⚠️ G4 F; G4 S warnsCIMCO for G4 S in observations
G17/G18/G19✅ [N]✅≈
G40/G41/G42✅ [N]✅ supported 2D milling compensation≈ subset
G500✅ [N]✅ WCS rebasing≈
G54–G59✅ [N]✅≈
G70/G71, G700/G710 units✅ [N]✅≈
G90/G91✅ [N]✅≈
G93/G94/G95✅ [N]✅ inverse-time with rotary/TCP restrictions≈ presence
G96/G97, G961/G971✅ [N]✅ restricted CSS/RPM model≈ subset
G937✅ [N]❌CIMCO in observations
TRANS/ATRANS✅ [N]✅ executable programmed frames≈
ROT/AROT/RPL✅ [N]; V8 fixes [C3]✅ supported spatial rotations and RPL≈ supported forms
SCALE/ASCALE✅ [N]❌ unmodeled geometry stops executionCIMCO in observations
MIRROR/AMIRROR✅ [N]❌ unmodeled geometry stops executionCIMCO in observations
GOTO / IF GOTO✅ [U, C3]✅ numeric N labelsMore CIMCO forms observed
WHILE/ENDWHILE? exact native V8 flow✅ bounded nested loopsNot established
RET/GOTOC/GOTOB/GOTOF✅ [N]❌ native flow stops with diagnosticCIMCO in observations
AC() / IC()✅ AC; ⚠️ IC arcs in author test [N]✅ IJK AC and XYZABC ICNo general ranking
DC() rotary endpoints? exact V8 semantics⚠️ shortest-path angles; out-of-range values normalized with warning; half-turn ties rejectedNot established
R parameters and arithmetic✅ [N]✅ arithmetic, comparisons, SIN/COS/ABS/SQRT≈ subset
Named production variables✅ [N]⚠️ R and restricted _NAME; arbitrary names unsupportedCIMCO in observations
Symbolic labels / SPF calls✅ [N]❌ arbitrary named calls/labelsCIMCO in observations
M17, M96/M97/M99✅ [N]❌ native flow stopsCIMCO in observations
M66/M98✅ [N]⚠️ warning; no native subprogram callCIMCO for calls in observations
M3/M4/M5/M6/M8/M9, M19✅ [N]✅ logical signals, no machine physics≈ signals
Named T / D0/D1/D2✅ [U, C3]✅ name and D state; no inferred offset tables≈ subset
SUPA / G0 SUPA✅ [N]✅ configured reference-return model≈ subset
CYCLE800 3+2 / reset❌ in author's tested setup [N]; other V8 builds untested✅ static AC/BC, 14–16 arguments; pure rapid rotary indexing retains frameEasy in that test only
TRAORI / TRAFOOF? exact V8 TCP contract✅ supported AC/BC TCP subsetNot established
4/5-axis Backplot / rotary✅ setup [C2]✅ AC/BC profiles and tool orientation≈ class; geometry untested
3D milling stock removal✅ Solid Animation [C2]; native SINUMERIK scope unverified✅ three-axis native milling, GPU box stock and STL export [E]≈ feature present; dialect scope not compared
Full machine simulation? not established for Backplot❌No verified equivalence
CYCLE81✅ [N]✅ supported drilling parameters≈ subset
CYCLE801✅ [N]❌CIMCO in observations
CYCLE82✅ [N]✅ dwell drilling≈ subset
CYCLE83✅ [N]✅ peck/chip-breaking subset≈ subset
CYCLE84✅ [N]✅ metric right/left and deep tapping; equal SST/SST1 matching S, G94, explicit PIT≈ supported subset
CYCLE840✅ [N]❌CIMCO in observations
CYCLE85✅ [N]✅ reaming with distinct FFR/RFF feeds≈ supported subset
CYCLE86✅ [N]✅ fine boring, orientation and RPA/RPO/RPAP clearance≈ supported subset
CYCLE87✅ [N]✅ boring with spindle-stop/manual-stop signals and rapid return≈ supported subset; no operator simulation
CYCLE88✅ [N]❌CIMCO in observations
CYCLE89✅ [N]✅ bottom dwell and feed withdrawal≈ supported subset
CYCLE90✅ [N]⚠️ classic 13-argument internal/external thread milling; configured cutter, G17/G40/G80, no TCP/MCALLDocumented subset; no matched trajectory comparison
POCKET1/2/3/4✅ [N]⚠️ POCKET3/4 classic 01/2008 roughing/finishing and supported entry strategies; POCKET1/2 and preformed blanks unsupportedPartial scope; no matched trajectory comparison
HOLES1/HOLES2✅ [N]⚠️ six-argument row/circle patterns with active supported MCALL drilling in G17 without TCPSupported subset; no matched trajectory comparison
LONGHOLE, SLOT1/SLOT2❌ comparison notes [N]❌Unsupported in this comparison
CYCLE71/72❌ comparison notes [N]❌Unsupported in this comparison
CYCLE73/74/75/76/77❌ comparison notes [N]❌Unsupported in this comparison
CYCLE60 engraving❌ comparison notes [N]❌Unsupported in this comparison
CYCLE899❌ comparison notes [N]❌Unsupported in this comparison
CYCLE832❌ comparison notes [N]⚠️ recognized, ignored settingRecognition only
MCALL CYCLE81/82/83/84/85/86/87/89✅ [N]✅ supported modal drilling/tapping/boring≈ subset
MCALL custom SPF✅ [N]❌CIMCO in observations
HOLES2 with MCALL✅ [N]⚠️ positions invoke the active supported modal drilling cycleSupported subset; no matched trajectory comparison
STOPRE✅ [N]❌ unsupported native commandCIMCO in observations
EXPANDED / native↔FANUC? equivalent replay contract not found✅ three axes, experimental AC/BC; unsupported cases rejectedDifferent documented contracts
4. Native HEIDENHAIN iTNC 530 milling

HEIDENHAIN is a separate input dialect, not a FANUC/SINUMERIK variant. Easy G-Code Plot parses and executes a documented Klartext subset with three-axis, indexed 3+2 and AC/BC table TCP execution and stops at unsupported semantics; the comparison below does not rank Klartext backplot accuracy.

Area / commandCIMCO Edit 8Easy G-Code Plot 2.9.0Assessment
Source detection and highlighting? Klartext support in V8 not established here✅ .h/.H, BEGIN PGM detection and iTNC-code highlighting [E]Not established
BEGIN/END PGM, MM/INCH, BLK FORM?✅ program/unit metadata and stock bounds; metric conversionNot established
Native source/AST fidelity? no equivalent internal contract assessed✅ immutable Klartext AST; original lines, / skip, numeric prefixes, source line/column and cycle Q continuations preservedEasy implementation guarantee, not a backplot ranking
L, omitted-L, IX/IY/IZ?✅ three-axis straight motion with incremental addressesNot established
CC/C/CR/CT?✅ center, direction, radius and tangent arcsNot established
LP/CP polar and helix?✅ polar positioning and polar/helical arcsNot established
APPR/DEP LT/LN/CT/LCT?✅ approach/departure lines and tangent arcsNot established
TOOL CALL/TOOL DEF, S/F?✅ numeric/named/Q tools and spindle axis; DL/DR/DR2 stop executionNot established
R0/RL/RR?✅ modal compensation state passed to the shared geometry resolverNot established
M0/M1/M3/M4/M5/M6/M8/M9/M13/M14/M30, M99?✅ logical signals, spindle state, program end and cycle callNot established
M91 machine coordinates?✅ nonmodal absolute XYZ using the configured WCSNot established
Cycle 247 datum selection?✅ application mapping Q339=1..6 to configured G54..G59; machine position preservedController preset tables are not imported
Cycles 7/10?✅ axis-address datum shifts and XY planar rotation, including circle-center transforms and cancellationNo tilted-plane or datum-table variant
M140 MB distance / MB MAX?✅ physical machine +Z retraction mapped through table orientation; MAX uses enabled Home Z with a warning and NC trace export guardPhysical travel limits are not modeled
LBL, CALL LBL, REP, FN 9–12?✅ label flow with call stack, repeats and conditional GOTONot established
Q/QL/QR, FN 0–4/6/7, expressions?✅ bounded arithmetic, comparisons and function trees without evalNot established
Q ranges and parse diagnostics?✅ Q0–Q1999, QL/QR0–499; errors keep source line, column and diagnostic codeNo matched CIMCO test
F0 and repeated feeds?⚠️ geometry retained, zero-feed timing warned; final repeated feed appliesNo matched CIMCO test
CYCL DEF/CYCL CALL 1/2, 200–209, 240/241?✅ expanded drilling/boring/tapping geometryNot established
Cycles 220/221?⚠️ DEF-active circle/grid patterns; invoke the previous supported machining cycle, explicit Q parameters and R0No matched CIMCO trajectory comparison
Cycles 251/252?⚠️ rectangular/circular pocket roughing/finishing, supported Q366 entries; XY/Z, R0, cutter geometry and explicit ANGLE for helical/reciprocating roughingInternal passes not independently confirmed
Cycle 262?⚠️ internal thread milling, signed pitch, Q355 strategies, analytic multi-turn helices; XY/Z, R0 and supported cutter diameterInternal passes not independently confirmed
Cycle 32 smoothing?⚠️ metadata only; controller smoothing not simulatedNot established
Optional / block skip and LBL 0?✅ skip and source block numbers preserved; separate named/numeric label maps and return handlingNot established
Klartext editor calculators and renumber?✅ native L/CR, CC/CP fragments; numeric prefixes without N, optional / retainedEditor tools, not CNC execution equivalence
RND R… [F…] / CHF … [F…]?✅ tangent line/arc rounding and straight-line chamfers; neighbor trimming, block-local feed and existing RL/RR/R0 compensation. ⚠️ unique planar local corners with residual neighboring lengthsReferences and limits; no matched CIMCO run
A/B/C indexing, IA/IB/IC?✅ matching configured kinematics required, including zero anglesNo matched CIMCO run
PLANE SPATIAL/RESET?✅ STAY/TURN and SEQ branch selection with two rotary joints; MOVE and TABLE COORD unsupportedNo matched CIMCO run
M128/M129, FUNCTION TCPM?✅ logical tool-tip control on AC/BC tables with PLANE reset; continuous L motion and start/end tool orientationsOEM pivot lengths are not modeled
M126/M127, M94?✅ shortest-path rotary positioning and displayed-angle reductionNo matched CIMCO run
M120, U/V/W, DL/DR/DR2?❌ unsupported execution stops at the source blockNot established
3D milling stock removal✅ Solid Animation [C2]; Klartext scope unverified✅ three-axis native Klartext, GPU box stock and STL export [E]≈ feature present; dialect scope not compared
EXPANDED iTNC output?✅ heidenhain_itnc530 resolved post (L/FMAX, CC+C/CP, CR, CYCL DEF 200/201/202/203/207); FULL rejectedDifferent documented contracts
Full machine simulation? not established for this Backplot❌No verified equivalence

Input implementation and regression evidence: HEIDENHAIN FAQ, native parser, AST tests, execution tests, rotary and three-post geometry tests, GUI lexer tests and export tests. The real sample.h fixture reaches M30, but neither that test nor output-post support proves complete controller coverage.

Sources and verification limits

Support means the stated documented or tested behavior. It does not establish equal trajectory accuracy, complete controller emulation, machine collision detection or interchangeability of NC output. Configure tools, WCS and kinematics for the program being reviewed. Experimental five-axis export retains its documented limitations.

Download the Markdown comparison ↗ · CIMCO Edit 8 editor and Backplot. Unknown support is not marked as absent.

Documentation

Supported commands, settings, limitations and usage examples.