Bancada de trabalho Path
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. This step is called post processing; there are different post processors available.
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 and read the Development Roadmap.
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:
- 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.
- The Macro file path, and Geometric tolerances, are defined in the Edit → Preferences → Path → Job Preferences tab.
- Colors are defined in the Edit → Preferences → Path → Path colors tab.
- Holding tag parameters are defined in the Edit → Preferences → Path → Dressups tab.
- 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: experimental feature as of November 2020). and (which is still an
- 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 and 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:
- 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
- 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'
- 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.
- 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
- Changing your preferred unit schema will have no effect on output but will help avoid input errors
- Generating the correct unit in output is the responsibility of the post-processor and is done only at that time
- Machine output unit is completely unrelated to your selected unit schema
- Post-processors produce either metric (G21) output, Imperial (G20) output or are configurable.
- Configurable post-processors default to metric (G21)
- 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
- 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
Many of the commands have various heights and depths:
Visual reference for Depth properties (settings)
Jobs, Tools, and Generating G-Code
These commands are used for seting up a CNC project (a Job object), managing your Job templates, creating a tool(cutter) with its tool controller, and post processing the Job.
- Job: Creates a new CNC job
- Export Template: Export the current job as a template
- Tool Manager: Edit the Tool Manager
- Post Process: Exports a project to G-code
- Path Tools (0.19_pre): Manage tools, bits, and the Tool Library
Basic Path Operations
- Profile (New in 0.19): Creates a profile operation of the entire model, or from one or more selected faces or edges. This operation combined the pre-existing Contour, Profile Faces, and Profile Edges operations.
- Pocket: Creates a pocketing operation from one ore more selected pocket(s)
- Slot (New in 0.19): Creates a slotting operation from selected features or custom points
- Drilling: Performs a drilling cycle
- Adaptive: Creates an adaptive clearing and profiling operation
- Engrave: Creates a engraving path
- Mill Face: Creates a surfacing path
- Helix: Creates a helical path
- 3D Pocket: Creates a path for a 3D pocket
- Vcarve: Creates a path for a 3D pocket
- Boundary Dressup: Adds a boundary dressup modification to a selected path
- Dogbone Dressup: Adds a dogbone dressup modification to a selected path
- Dragknife Dressup: Adds a dragknife dressup modification to a selected path
- Lead In Dressup: Adds a lead-in and/or lead-out point to a selected path
- Ramp Entry Dressup: Adds ramp entry dressup modification to a selected path
- Tag Dressup: Adds a holding tag dressup modification to a selected path
- Fixture: Changes the fixture position
- Comment: Inserts a comment in the G-code of a path
- Stop: Inserts a full stop of the machine
- Custom: Inserts custom G-code
- Gcode from a Shape: Creates a path object from a selected Part object
- Op Active: Used to activate or de-activate a path operation
- Copy: Creates a parametric Copy of a selected path object
- Array: Creates an array by duplicating a selected path
- Simple Copy: Creates a non-parametric copy of a selected path object
- G-Code Inspector: Shows the G-code for checking
- Simulator: Shows the milling operation like it's done on the machine
- 3D Surface: Creates a path for a 3D surface ( experimental , December 2019 )
- Waterline: Creates a waterline path for a 3D surface ( experimental , 0.19_pre )
- Feature area: Creates a feature area from selected objects
- Feature area workplane: Creates a feature area workplane
- Path Errors: Checks the selected Job for missing values
- Complete Loop: Completes a loop from two selected edges
- Fourth Axis: Developmental four axis milling
- Preferences...: Preferences available in Path Tools.
See the Path scripting page.
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.
See the Path FAQ
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.