|Time to complete|
Demonstrating the creation of a Path Workbench Job derived from a 3D Model. Then generating dialect-correct G-Code for a target CNC mill.
The 3D Model
1. The Project begins with a simple FreeCAD model designed in the Part Design a cube with a rectangular pocket,
Above: Created in the Part Design including a Body, a Box with a Pocket, based on a Sketch oriented in the XY plane.
3. Now we create a Path Job by either of the following methods:
- Press the button from the toolbar.
- Using the then keyboard shortcut.
- Using the Path → Job entry from the top menu.
Above: Path Job creation dialog
4. This opens a Job creation dialog. Within this dialog, clickto accept the Body as the Base Model, with no Template.
5. The Job Edit window opens in the Task window, and the model view Window shows the Stock as a wire frame cube surrounding the Base Body. The Setup Tab is selected.
6. The Output tab defines the output file path, name, extension, and the Postprocessor. For advanced users, Post Processor Arguments can be customized (mouse over to show tooltips of common arguments).
Above: Path Job Edit dialog with the Output tab selected
Above: Path Job Edit dialog with the Tools tab selected
7. Modify the Default tool by selecting it and clicking thebutton. This opens the Tool Controller edit window.
Above: Path Job Tool Controller subpanel Edit dialog
8. The name given to the tool and the tool number correspond with the tool number of the machine. In the dialog (see above) it's Tool Nr. 4. The tool controller is configured for horizontal and vertical feed rates of
2mm/s and a spindle speed of
9. Select the Tool subpanel of the Tool controller. Set the diameter (and if you wish to use the Path Simulation tool later: add a cutting edge angle and cutting edge height).
Above: Path Job Tool controller 'Tool' subpanel dialog
10. The values are confirmed with
Note: For easy access, all the tools can be predefined and selected from the Tool manager.
The Workplan tab initially is shown as empty. It is then populated by the sequence of Job Operations, Partial Path Commands, and Path Dressups. The sequence of these items is ordered here.
This tree is shown after the Job's configuration once the Path Job is unfolded:
The Path Operations
12. For now we will keep it simple. The Profile button opens the Contour panel. After confirming with using the default values, see the green path around the object is visible.
13. Selecting the bottom of the pocket and then the Pocket button opens the Pocket Shape window. The default values for Base Geometry, Depths, and Heights are used, and the Operation subpanel is selected, and the Step Over Percent is set at 50.
14. The pattern is changed to "Offset" and the Job Operation is confirmed for the pocket configuration with
The result is a model with two paths:
There are two ways to verify the created paths. The G-Code can be inspected, including highlighting the corresponding path segments. The milling process of the Path Job can also be simulated to demonstrate the idealized tool paths, required for the Tool geometries to mill the Stock.
To inspect the G-Code use the Path Inspect tool. Selecting the corresponding G-Code lines within the G-Code Inspection window highlights individual path segments.
Above: Path Inspection tool opens the G-Code Inspection dialog
To start the simulation use the Path Simulator tool.
Above: Path Simulation in progress
If you want to end the simulation click thebutton, it will remove the stock created for the simulation. If you click this object will be kept in your Job.
Postprocess the Job
The final step to generate G-Code for the target mill is to postprocess the Job. This outputs the G-Codes to a file that can be uploaded to the target CNC machine controller. To invoke the Postprocessor:
- Select the Job object in the tree view
- Select the Path Postprocessing tool to postprocess the file. This opens a G-Code window allowing inspection of the final output file before it is saved.