Making G-code for Your FluidNC CNC

Version 1.0 · Updated 21 November 2026 · For BlueCarve machines with a FluidNC controller and TouchBLUE tablet
Back to FluidNC set up

Your machine runs G-code: a text file of moves that the FluidNC controller follows. This guide explains the programs you can use to make it, what they cost, how hard they are to learn, and the settings that make the file run on a BlueCarve FluidNC machine.

1. CAD, CAM and G-code

1. CADDesignYou draw the shape: a sign, a part, a box joint. The result is a drawing (DXF, SVG) or a 3D model (STL, STEP).
2. CAMToolpathsYou tell the program which bit to use, how deep to cut and how fast. It works out the path the bit follows and saves it as G-code (.nc or .gcode).
3. ControlTouchBLUE tabletYou put the G-code file on the controller and run it from the tablet. No computer is needed at the machine.

Some programs do only CAD, some only CAM, and some do both. Any program in this guide works, as long as it can save G-code for a GRBL machine. FluidNC runs the same G-code as GRBL (FluidNC’s GRBL compatibility notes).

2. Which program should I use?

If you want to…Start with
Cut out a shape from a DXF you already have, surface the spoilboard, or try V-carving, laser engraving or a 3D relief, for freeThe tablet’s Tools page (free, built in)
Make signs and simple projects with the least learningEasel (free plan, one export a week)
Do sign-making, V-carving and furniture parts properly, and keep using it for yearsVectric VCarve Desktop (one-off purchase)
A cheaper all-in-one design and toolpath programMillMage (one-off purchase)
Design mechanical parts and 3D modelsFusion (free for personal use, with limits)
Spend nothing and don’t mind learningInkscape to draw, then the tablet’s Tools, Kiri:Moto or FreeCAD for toolpaths

All programs at a glance

Prices are the makers’ own, in US dollars, checked in November 2026. They change, so check before you buy.

ProgramCADCAMCostLearningRuns on
TouchBLUE Tools pageNo (opens DXF and images)YesFreeEasyAny computer browser on the BLUECARVE WiFi
EaselYes (2D)YesFree (1 export a week); Starter US$72 a year; Pro US$216 a yearEasyWeb browser (needs internet)
InkscapeYes (2D)NoFreeMediumWindows, Mac, Linux
Vectric Cut2D DesktopYes (2D)YesUS$149 one-offEasy to mediumWindows (Mac with Parallels)
Vectric VCarve DesktopYes (2D, imports 3D)Yes (incl. V-carve)US$349 one-offMediumWindows (Mac with Parallels)
MillMage Core / ProYes (2D)YesUS$99 / US$199 one-offEasy to mediumWindows, Mac, Linux
EstlcamBasicYesAbout US$59 one-off (free trial)MediumWindows
Kiri:MotoNoYesFreeMediumWeb browser
Fusion (personal use)Yes (3D)YesFree for non-commercial use, with limits; paid licence for businessHardWindows, Mac
FreeCADYes (3D)Yes (CAM workbench)FreeHardWindows, Mac, Linux

3. Settings every program needs

Whatever program you use, set these once and the files will run on your machine:

SettingUseWhy
Post processor (output type)GRBL (mm), or “GRBL” with units set to mmFluidNC runs GRBL G-code. Other posts (Mach3, LinuxCNC, Carbide) can add commands it rejects.
UnitsMillimetresEverything on the tablet is in mm.
File type.nc or .gcodeThe tablet’s Files tab lists these.
Tool number0 (or no tool number) for the router; 1 for the laserThe tablet checks the file’s tool number against Spindle Mode or Laser Mode before it starts. A router file asking for T1 stops with “Tool / mode mismatch”.
One bit per fileSave a separate file for each bitThere is no automatic tool changer. Run file 1, change the bit, set Z zero again, then run file 2.
Work areaYour machine’s X and Y travel (see the size table)So the program warns you before a job is too big.
Zero pointNote where X0 Y0 and Z0 are (usually front-left corner, top of the material)You set the same point on the tablet before you run the job.
Spindle speedStart at about 16000 RPMUse feeds.endmill.com.au for feeds and speeds.

4. CAD programs (design)

Easel (CAD and CAM)

Cost: free Basic plan (design is unlimited, but only one carve or G-code export a week); Starter US$72 a year (20 exports a week); Pro US$216 a year (unlimited, adds V-carving and 3D). Learning: easy. Runs in: a web browser, with internet.

The simplest way to start. Draw shapes and text, import SVG or DXF, and see a preview of the carve. Projects that use Pro features can’t be exported on the free plan.

Inkscape (CAD only)

Cost: free. Learning: medium. Runs on: Windows, Mac, Linux. inkscape.org

A full drawing program for 2D shapes, text and logos (it can trace a picture into outlines). Save as SVG or DXF, then make the toolpaths in the tablet’s Tools page, Easel, Kiri:Moto or another CAM program. Convert text to paths (Path > Object to Path) before you save.

Vectric Cut2D Desktop and VCarve Desktop (CAD and CAM)

Cost: Cut2D Desktop US$149, VCarve Desktop US$349, one-off. The Desktop editions are limited to jobs of about 600 x 600 mm (24 x 24 inches); the Pro editions cost more and have no size limit. Learning: easy to medium. Runs on: Windows. vectric.com

The most popular choice for hobby and small-business routers. Cut2D does profiles, pockets and drilling; VCarve adds V-carving, inlays, textures and importing 3D models. A free trial version lets you try it first.

MillMage (CAD and CAM)

Cost: Core US$99, Pro US$199, one-off. Learning: easy to medium, especially if you already use LightBurn for a laser. Runs on: Windows, Mac, Linux. MillMage

From the makers of LightBurn, launched in 2026. Design and toolpaths in one window; Pro adds V-carving, relief carving and nesting. FluidNC is listed as a supported output.

Fusion (CAD and CAM)

Cost: free for personal, non-commercial use; paid subscription for business use. Learning: hard. Runs on: Windows, Mac.

A professional 3D design program. Best for mechanical parts, joinery and 3D models. The free personal licence has CAM limits: all moves between cuts run at cutting speed instead of rapid speed (jobs take longer), and each file can use only one tool.

FreeCAD (CAD and CAM)

Cost: free and open source. Learning: hard. Runs on: Windows, Mac, Linux. freecad.org

A free 3D design program with a CAM workbench. Powerful, but the least beginner-friendly option here.

A note on Carbide Create

Carbide Create is free, but the free version only saves G-code for Carbide 3D’s own machines. You need the paid Pro version to save G-code for a BlueCarve.

5. CAM programs (toolpaths and G-code)

How to save a G-code file for your FluidNC machine in each program, with a link to the maker’s own instructions.

The tablet’s Tools page (free, built in)

Learning: easy. Nothing to install: it comes with the tablet.

  1. Join a computer to the BLUECARVE WiFi (password bluecarve) and open http://192.168.0.2 in Chrome or Edge.
  2. Open Tools. Choose a tool: Surfacing, DXF to G-code (outside, inside or on-line cuts with holding tabs), V-carve, Nest / array, Laser image, 3D relief, or the G-code checker.
  3. Open your DXF or image, set the bit, depth and speeds (the Feeds & speeds tool suggests values), and check the preview.
  4. Click Save to SD to send it straight to the machine, Save & Run to start it, or Download to keep the file.

Full instructions: section 4 of the TouchBLUE tablet manual.

Easel

  1. Set up a machine profile for FluidNC once: Machine > Set up new machine, manufacturer Blue Carve, model Other, Motion Control Other (not “FluidNC (Beta)”), your work area, Spindle Control Automatic. Easel only lets you download G-code with a profile like this. A full worked example with screenshots, a name plaque from start to finish, is in the FluidNC set-up guide.
  2. Design the job, choose the bit and the cut settings.
  3. Click the green Export… button (or Project > Download > Download g-code). The file downloads straight away. A two-stage carve (roughing and detail) downloads as two .nc files: run them one after the other, changing the bit in between.

Easel’s instructions: Exporting G-code from Easel.

Vectric (Cut2D, VCarve, Aspire)

  1. In Job Setup, set the size of your material, units mm, and the XY datum (usually bottom left) and Z zero (usually top of the material).
  2. Create your toolpaths. In each tool’s settings, set the Tool Number to 0. The Grbl post writes the tool number at the top of the file, and the tablet stops a router job that asks for T1.
  3. Click Save Toolpath(s), choose the post processor Grbl (mm), and save. Save each bit’s toolpaths as a separate file (tick only the toolpaths for one bit).

Vectric’s tutorials are in the Help menu and on vectric.com. Sienci Labs’ post processor list confirms Grbl (mm) for Vectric.

MillMage

  1. In the device settings, add your machine as a FluidNC device (or GRBL), with your work area in mm.
  2. Draw or import your design and add the operations (profile, pocket and so on).
  3. Use the option to save G-code to a file. Don’t connect MillMage to the controller’s USB port: the tablet runs the machine.

MillMage’s documentation: MillMage (links to guides and the support forum).

Fusion

  1. In the Manufacture workspace, create a Setup: choose the stock and set the work coordinate origin (usually top of the stock, front-left corner).
  2. Add your toolpaths (2D Contour, 2D Pocket and so on).
  3. Right-click the setup and choose Post Process. Search for and choose the GRBL post (Autodesk), output units mm.
  4. In the post properties, set Safe Retracts to Clearance Height (not G28), and untick Output tool number. Fusion numbers tools from 1, and a T1 in the file makes the tablet stop with “Tool / mode mismatch”. Leave Output M6 off.
  5. Click Post and save the .nc file. With the personal licence, post one tool per file.

Autodesk’s instructions: the Fusion GRBL post. Sienci Labs’ post processor list also covers the Safe Retracts setting.

Estlcam

  1. In Setup > CNC Programs, choose GRBL as the program the G-code is for.
  2. Open your DXF, SVG or STL, choose the bit and draw the toolpaths (part, hole, engraving).
  3. Click Save CNC program.

Estlcam’s own tutorials: estlcam.de.

Kiri:Moto

  1. Open grid.space/kiri and switch to CNC mode.
  2. Choose a GRBL machine profile and set its work area to your machine’s size.
  3. Import an STL or SVG, set the stock and the bit, then add roughing, outline or contour operations.
  4. Click Export to save the G-code.

Kiri:Moto’s documentation: docs.grid.space.

FreeCAD

Use the CAM workbench (called Path in older versions): create a Job, add operations, then Post Process with the grbl post processor. Instructions: FreeCAD CAM workbench.

6. Getting the file to the machine

  1. microSD card: copy the file to the card with the card reader, then put the card back in the controller. Or WiFi: join the computer to the BLUECARVE network, open http://192.168.0.2 and drop the file on the page.
  2. On the tablet, open Files and tap Refresh. Tap the blue eye to preview the file and check its size and shape.
  3. Not sure a file is right? Open it in Tools > Viewer & checker on the tablet’s web page. It shows the toolpath in 3D and warns about common problems (rapid moves below the material, cutting with the spindle off, a job bigger than the machine).
  4. Run the job as described in the FluidNC set-up guide.

7. Troubleshooting

ProblemWhat to do
“Tool / mode mismatch” on the tabletThe file asks for a different tool from the selected mode. For router jobs set the tool number to 0 in your CAM program and save again, or switch to the right mode on the Status tab. (Easel files have no tool number, so they always pass.)
Error 20 (unsupported command)The file was saved with the wrong post processor. Save it again with GRBL (mm).
The job is much bigger or smaller than expectedUnits mismatch. Save the file again with a millimetre post processor.
Jobs from Fusion are slow between cutsThe free personal licence runs moves between cuts at cutting speed. Raise the cutting feed where safe, or use a paid licence or another CAM program.
Easel won’t let me download G-codeCheck your machine profile uses Motion Control Other, that you haven’t used your free weekly export, and that the project doesn’t use Pro-only features.
The file doesn’t show in the Files tabTap Refresh. Check the file ends in .nc or .gcode and the card is fully inserted.
The machine plunges into the material or cuts in the airThe Z zero on the tablet doesn’t match the CAM program’s Z zero (top of material vs bottom). Set them the same.
Need help?
Email adam@bluecarve.com.au with your machine model, size, the program you used and the G-code file. Owners also help each other in the BlueCarve owners group on Facebook.
0
0
Quote Request
Your cart is emptyReturn to Shop