Path Workbench

    From FreeCAD Documentation
    Path workbench icon


    The Workbench Path.svg 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. A general CNC lathe tool path sequence simulation example is presented here.


    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 Workbench PartDesign.svg Part Design, Workbench Part.svg Part or Workbench Draft.svg Draft Workbenches.
    • A Path Job is created in the 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).
    • Path 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. This step is called post processing; there are different post processors available.

    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 Supplemental 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 workbench requirements, passes Check Geometry.


    Some current limitations of which you should be aware are:

    • Most of the Path Tools are not true 3D tools but only 2.5D capable. This means that they take a fixed 2D shape and can cut it down to a given depth. However, there are two tools which produce true 3D paths: Path 3DPocket.svg 3D Pocket and Path Surface.svg 3D Surface (which is still an experimental feature as of November 2020).
    • Most of Path workbench is designed for a simple, standard 3-axis (xyz) CNC mill/router, but lathe tools are under development in 0.19_pre.
    • Most operations in Path workbench will return paths based on a standard endmill tool/bit only, regardless of the tool/bit type assigned in a given tool controller with the exception of the Path Engrave.svg Engrave and Path Surface.svg 3D Surface operations.
    • The operations within the Path workbench are not aware of clamping mechanisms in use to secure the model to your machine. Consequently, please review and simulate the paths you generate prior to sending the code to your machine. If necessary, model your clamping mechanisms in FreeCAD in order to better inspect the paths generated. Look for possible collisions with clamps or other obstacles along the paths.


    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

    Heights and depths

    Many of the commands have various heights and depths:


    Visual reference for Depth properties (settings)


    Some commands are experimental and not available by default. To enable them see Path experimental.

    Project Commands

    • Path Job.svg Job: Creates a new CNC job.

    Tool Commands

    • Path Simulator.svg CAM Simulator: Shows the milling operation like it's done on the machine.

    Basic Operations

    • Path Profile.svg Profile: Creates a profile operation of the entire model, or from one or more selected faces or edges.
    • Path Pocket Shape.svg Pocket Shape: Creates a pocketing operation from one or more selected pocket(s).
    • Path MillFace.svg Face: Creates a surfacing path.
    • Path Helix.svg Helix: Creates a helical path.
    • Path Adaptive.svg Adaptive: Creates an adaptive clearing and profiling operation.
    • Path Slot.svg Slot: Creates a slotting operation from selected features or custom points. Experimental.
    • Path Engrave.svg Engrave: Creates an engraving path.
    • Path Deburr.svg Deburr: Creates a deburr path.
    • Path Vcarve.svg Vcarve: Creates an engraving path using a V tool shape.

    3D Operations

    Path Dressup

    • Path DressupPathBoundary.svg Boundary: Adds a boundary dressup modification to a selected path.
    • Path DressupDogbone.svg Dogbone: Adds a dogbone dressup modification to a selected path.
    • Path DressupDragKnife.svg DragKnife: Adds a dragknife dressup modification to a selected path.
    • Path DressupLeadInOut.svg LeadInOut: Adds a lead-in and/or lead-out point to a selected path.
    • Path DressupRampEntry.svg RampEntry: Adds ramp entry dressup modification to a selected path.
    • Path DressupTag.svg Tag: Adds a holding tag dressup modification to a selected path.

    Supplemental Commands

    • Path Fixture.svg Fixture: Changes the fixture position.
    • Path Comment.svg Comment: Inserts a comment in the G-code of a path.
    • Path Stop.svg Stop: Inserts a full stop of the machine.
    • Path Custom.svg Custom: Inserts custom G-code.
    • Path Probe.svg Probe: Creates a Probing Grid from a job stock.

    Path Modification

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

    Specialty Operations



    • Path ToolLibraryEdit.svg Tool Manager: Edit the Tool Manager. 'Legacy' tool system. version 0.18 and below

    ToolBit architecture

    Manage tools, bits, and the Tool Library. Based on the ToolBit architecture.


    • Path FAQ: The Path Workbench shares many concepts with other CAM software packages but has its own peculiarities. If something seems wrong this is a good place to start.
    • Path SetupSheet: You can use a SetupSheet to customize how various property values for operations are calculated.
    • Path Postprocessor Customization: If you have a special machine which cannot use one of the available post-processors you may need to write your own post-processor.
    • Path fourth axis: Experimental four axis milling.



    See Path scripting.