|Path → Post Process|
|Introduced in version|
Each CNC Controller speaks a specific G-code dialect, requiring a Dialect-correct Postprocessor to translate the final output from the agnostic internal FreeCAD G-code dialect.
Typical functions of the Postprocessor include
- Using a correct Job output G-code file extension.
- Selecting the G-code commands. CNC controllers typically support a subset of available G-code commands. The super-set of G-code commands contains powerful and specialized commands that otherwise must be processed using multiple simpler commands. Postprocessors are written to select the best G-code for an Operation, available on the target.
- Formatting the G-code syntax by reordering the Feed, X, Y, Z, A, and B inputs, and the precision.
- Inserting a Pre-amble to set units, units format, Work plane, coordinate system, etc...
- Inserting a Post-amble to park the machine, stop it, process any arguments.
- Inserting Tool changes, or suppressing them between subsequent operations using the same tool.
- Formatting the Feed and Speed rate information to revolutions per minute, or per second.
- Formatting Function Call Naming and Calling.
If you want to write your own postprocessor, have a look at the Path Postprocessor Customization page.
Note: Several provided Postprocessors generate suitable code for many CNC controllers, or can be used as templates for modification
Postprocessors contain configuration flags and are designed to be tuned by adding G-codes and M-codes to provided definitions for:
- Machine initialization
- Job finalization
- Cooling on /off
Postprocessors use FreeCAD's internal G-code dialect in conjunction with the Postprocessor configuration definitions, to generate Dialect-Correct G-code for target machines. This allows the Path workbench to generate correct G-code to target various CNC machine controllers by invoking different Postprocessors.
CNC Machine Controller types include:
- CNC mills
- CNC lathes
- 3D Printers
- DragKnife Cutters
- Laser Cutters
- Plasma Torch Cutters
- Wire Benders
- EDM Cutters
If only one CNC machine is used, or if all CNC machines share a common Postprocesor, the Path workbench would need to include only a single Postprocessor. If a single Postprocessor is inadequate to output G-code for all target CNC controllers, then multiple Postprocessors must be installed.
- Select a Path Job in the Tree view.
- There are several ways to invoke the command:
- Confirm the Output File name and directory
Output file and Postprocessor properties can be set in the Job, at any time, prior to invoking the Postprocessor.
The provided Postprocessors are written with comments indicating areas containing Flags, Configuration Variables, and Sections of G-Codes and M-Codes that are to be used by the Postprocessor to configure the output.
Typical Configuration True/False Flags include:
- OUTPUT_COMMENTS (True = Allow, False = Suppress): Used to insert Text Comments in the output G-code file.
- OUTPUT_HEADER (True = Allow, False = Suppress): Used to insert Text Headers in the output G-code file.
- OUTPUT_LINE_NUMBERS (True = Allow, False = Suppress): Used to insert Line Numbers in the output G-code file.
- SHOW_EDITOR (True = Allow, False = Suppress): Used to show the output G-code in a Pop-up window when invoking the Postprocessor.
- MODAL (True = Allow, False = Suppress): Used to reduce the number of output G-code lines by stripping Mode information when the Mode is not changing.
Typical Configuration Variables include:
- LINENR (Line Number): Used to Set the Line Number index.
- UNITS (G20 or G21): Used to explicitly communicate to the target CNC controller what Units to use to interpret the final output file.
- MACHINE_NAME (Name of Target CNC Mill): Used to Insert a machine name label in the final output file.
- PRECISION: Used to Set the number of digits to include after the decimal place in final output file
Typical Configuration Sections include:
- PREAMBLE: Code configuration inserted at beginning of the Job.
- POSTAMBLE: Code configuration appended to the Job, providing for parking the machine, etc...
- TOOL_CHANGE: Code inserted with each tool change in the Job.
The→ → → → → is used to set the default Postprocessor selected on Job creation. This allows Path workbench to be configured to only display desired Postprocessors, and to set a default.
Included Postprocessors are saved in the FreeCAD/Mod/Path/Pathscripts/Post by default:
- grbl, including support for bCNC header blocks using Job output argument --bcnc
- jtech (laser)
- Do not use the → menu for export to G-code, it will produce damaged G-code!