Path Walkthrough for the Impatient
|Time to complete|
Here is a demonstration showing the creation of a Path WB Job from a 3D Model, generating dialect-correct G-Code for a target CNC mill.
The 3D Model
The Project begins with a simple FreeCAD model: 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.
With the 3D Model completed, the Path Workbench is selected.
The Job is created.
In the Job creation dialog click OK to accept the Body as the Base Model, with no Template.
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.
The Output tab defines the output file path, name, and extension, and the Postprocessor. For advanced users, Post Processor Arguments can be defined—the mouse over hints show common arguments.
We modify the Default tool by selecting it and clicking the Edit button. This opens the Tool Controller edit window.
The name given to the tool and the tool number correspond with the tool number of the machine. Here it is tool Nr. 4. The tool controller is configured for horizontal and vertical feed rates of 2mm/s and a spindle speed of 2000 rpm.
Select the Tool subpanel of the tool controller. Set the diameter and - if you wish to use the simulation tool later - add a cutting edge angle and cutting edge height.
The values are confirmed with OK.
For easy access all the tools can be predefined and selected from the Tool manager.
The Workplan tab begins empty, and is 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
For now we will keep it simple. The Contour button opens the Contour panel. After confirming with OK using the default values, see the green path around the object is visible.
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.
The pattern is changed to "Offset" and the Job Operation is confirmed for the pocket configuration with OK.
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 start the simulation use the Path Simulator tool.
Adjust speed and accuracy and start the simulation with the play button.
If you want to end the simulation click the Cancel button, it will remove the stock created for the simulation. If you click Ok 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
- 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.