Path Post/it

Descrizione
Questo comanda esporta una Lavorazione selezionata in un file di codice-G

Ogni controller CNC parla un dialetto G-Code specifico, che richiede un postprocessore dialettale corretto per tradurre l'output finale dal dialetto G-Code di FreeCAD agnostico interno.

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 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
 * 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 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
 * 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 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.

Utilizzo

 * 1) Selezionare la Lavorazione che si desidera esportare
 * 2) Premere il pulsante
 * 3) Confermare il nome e la directory del file di output

Opzioni

 * Se le proprietà del file di output e del post-processore non sono impostate nel Progetto, il contenuto del progetto viene invece mostrato in una finestra di dialogo per la verifica
 * È anche possibile esportare un progetto o qualsiasi altro percorso direttamente in Codice G utilizzando il menu File-> Esporta

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 FreeCAD/Mod/Path/Path/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 →  menu for export to G-code, it will produce damaged G-code!