CAM Post/it

Descrizione

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.

Postprocessor Customization

If you want to write your own postprocessor, have a look at the CAM 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
• Tool-Changes
• Cooling on /off
• Etc...

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 CAM 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
• Engravers
• Plasma Torch Cutters
• Wire Benders
• EDM Cutters
• Etc...

If only one CNC machine is used, or if all CNC machines share a common Postprocesor, the CAM 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.

Utilizzo

Opzioni

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 Edit → Preferences... → CAM → Job Preferences tab → Defaults → CAM is used to set the default Postprocessor selected on Job creation. This allows CAM workbench to be configured to only display desired Postprocessors, and to set a default.

Included Postprocessors are saved in FreeCAD/Mod/CAM/CAM/Post/scripts by default:

• centroid
• comparams
• dxf
• dynapath
• grbl, including support for bCNC header blocks using Job output argument --bcnc
• jtech (laser)
• linuxcnc
• mach3_mach4
• nccad
• opensbp
• phillips
• refactored* (These postprocessors are works-in-progress and will be changing a lot)
• rml
• smoothie
• uccnc

Limitations

• Do not use the File → Export menu for export to G-code, it will produce damaged G-code!