Path Workbench

From FreeCAD Documentation
Jump to: navigation, search


The Path workbench is used to produce machine instructions for CNC machines from a FreeCAD 3D model. These produce real-world 3D objects on CNC machines such as mills, lathes, lasercutters, or similar. Typically, instructions are a G-Code dialect.


The FreeCAD Path Workbench workflow creates these machine instructions as follows:

  • A 3D model is the base object, typically created using one or more of the Part Design, Part or Draft Workbenches.
  • A Job is created in Path Workbench. This contains all the information required to generate the necessary G-Code to process the Job on a CNC mill: there is Stock material, the mill has a certain set of tools and it follows certain commands controlling speed and movements (usually G-Code).
  • Tools are selected as required by the Job Operations.
  • Milling paths are created using e.g. Contour and Pocket Operations. These Path objects use internal FreeCAD G-Code dialect, independent of the CNC machine.
  • Export the job with a g-code, matching to your machine.

Links for the impatient

Depending on your interest in the Path workbench there are different topics for further reading:

  • If you are a new new user trying to get familiar with Path, you might be interested in a fast walk-through tutorial.
  • If you have a special machine which cannot use one of the available postprocessors you may want to learn about post-processor customization
  • As an experienced user you may want to write a macro or automate a process might need to learn about scripting
  • Power users who want to streamline their workflow can learn about customization.
  • New developers who want to contribute to path might want to understand core concepts.

General concepts

The Path Workbench generates G-Code defining the paths required to mill the Project represented by the 3D model on the target mill—in [the Path Job Operations FreeCAD G-Code dialect ], which is later translated to the appropriate dialect for the target CNC controller by selecting the appropriate Postprocessor.

The G-Code is generated from directives and Operations contained in a Path Job. The Job Workflow lists these in the order they will be executed. The list is populated by adding Path Operations, Path Dressups, Path Partial Commands, and Path Modifications—from the Path Menu, or GUI buttons.

The Path Workbench provides a Tool Manager (Library, Tool-Table), and G-Code Inspection, and Simulation tools. It links the Postprocessor, and allows importing and exporting Job Templates.

The Path Workbench has external dependencies including:

  1. The FreeCAD 3D model units are defined in the Edit → Preference... → General → Units tab's Units settings. The Postprocessor configuration defines the final G-Code units.
  2. The Macro file path, and Geometric tolerances, are defined in the Edit → Preferences... → Path → Job Preferences tab.
  3. Colors are defined in the Edit → Preferences... → Path → Path colors tab.
  4. Holding tag parameters are defined in the Edit → Preferences... → Path → Dressups tab.
  5. That the Base 3D model quality supports the Path WB requirements—passes Check Geometry.


Unit handling in Path can be confusing. There are several points to understand:

  1. FreeCAD base units for length and time are 'mm' and 's' respectively. Velocity is thus 'mm/s'. This is what FreeCAD stores internally regardless of anything else
  2. The default unit schema uses the default units. If you're using the default schema and you enter a feed rate without a unit string, it will get entered as 'mm/s'
  3. Most CNC machines expect feed rate in the form of either 'mm/min' or 'in/min'. Most post-processors will automatically convert the unit when generating gcode.


  1. Changing schema in preferences changes default unit string for the input fields. If you're a Path user and prefer to design in metric, it's highly recommended that you use the "Metric Small Parts & CNC" schema. If you design in US units, either the Imperial Decimal and Building US will work
  2. Changing your preferred unit schema will have no effect on output but will help avoid input errors


  1. Generating the correct unit in output is the responsibility of the post-processor and is done only at that time
  2. Machine output unit is completely unrelated to your selected unit schema
  3. Post-processors produce either metric (G21) output, Imperial (G20) output or are configurable.
  4. Configurable post-processors default to metric (G21)
  5. If you want your configurable post-processor to output imperial gcode (G20), Set the correct argument in your job output configation (ie --inches for linuxcnc). This can be stored in a job template and set as your default template to make it automatic for all future jobs

Path Inspection:

  1. If you use the Path Inspect tool to look at g-code, you will see it in 'mm/s' because it is not being post-processed

Path Commands

These commands are used for seting up a CNC project and manage your templates.

  • Path-Job.png Job: Creates a new CNC job
  • Path Simulator.png Simulator: Shows the milling operation like it's done on the machine
  • Path Contour.png Contour: Creates a path of the contour of the base object
  • Path Pocket.png Pocket: Creates a pocketing operation from one ore more selected pocket(s)
  • Path-Helix.png Helix: Creates a helical path

Path Dressup

  • Path Dressup.png Tag Dressup: Adds a holding tag dressup modification to a selected path

Partial Commands

  • Path Fixture.png Fixture: Changes the fixture position
  • Path Comment.png Comment: Inserts a comment in the G-code of a path
  • Path Stop.png Stop: Inserts a full stop of the machine
  • Path Custom.png Custom: Inserts custom G-code

Path Modification

  • Path Copy.png Copy: Creates a parametric Copie of a selected path object
  • Path Array.png Array: Creates an array by duplicating a selected path
  • Path SimpleCopy.png Simple Copy: Creates a non-parametric copy of a selected path object


  • Path Sanity.png Path Errors: Checks the selected Job for missing values



The Path workbench offers a broad python scripting API. With it, you can create and modify paths from python scripts, or extend the available functionality of the workbench.



The Path Workbench shares many concepts with other CAM software packages but has its own peculiarities. If something seems wrong, this might be a good place to start.

Other languages:
Deutsch • ‎English • ‎español • ‎français • ‎hrvatski • ‎italiano • ‎português • ‎română • ‎русский • ‎中文(中国大陆)‎