How do I select the right post-processor for my CNC machine in VCarve Pro & Aspire, and what are the most common ones?

Overview

The post-processor is the translator between the software's calculated toolpath data and the specific G-code (or machine code) format your CNC controller understands. Choosing the wrong post-processor means the machine either will not run the file or moves incorrectly. This is one of the most critical first-time setup decisions for any new user. This entry covers picking, defaulting and installing a post-processor in VCarve Pro and Aspire. For machine setup see the machine configuration entry, and for editing a post see the post-processor editing entry.

What a Post-Processor Does

The software calculates toolpaths as abstract move data (XYZ positions, feed rates, tool changes). The post-processor converts this into a specific file format:

• The file extension (.gcode, .nc, .tap, .sbp, .mpf, etc.)
• The exact G-code syntax for your controller
• How tool changes are handled
• How arcs are output (G2/G3 or linearized)
• Whether the file uses inches or millimeters
• Any machine-specific header and footer code

How to Select a Post-Processor

1. Go to the Toolpaths tab and click Save Toolpaths.
2. Pick your Machine in the Save Toolpaths form. The post-processor drop-down then lists the post-processors associated with that machine.
3. Pick the post-processor your machine maker recommends.
4. If yours is not listed, choose <Add Post-Processors> in the list to associate more post-processors with the selected machine.

To make one post-processor the pre-selected choice every time, open Machine > Machine Configuration, right-click the post under Associated Post-Processors and choose Make Default.

To browse every post-processor available, open Machine > Post-Processor Management. There you can view a post's instructions, check its changelog, and customize a copy. Clicking the version column lets you either follow the latest version of a post or pin a fixed version, so later updates do not change your output unexpectedly.

Which Post-Processor Does My Machine Need?

Use the post-processor your machine maker names. Names differ between machines and software versions, so do not guess from a controller brand alone. Two reliable routes:

• Use Machine > Search for Machine Online to find your make, series and model. The machine package comes with its associated post-processors.
• Check your machine manual or the maker's support page for the post-processor name, then find that name in Post-Processor Management.

Common controller families you will see in the list include ShopBot, Mach3 and Mach4, Grbl, LinuxCNC, Centroid and Fanuc style controllers. Many have separate inch and mm versions, and the exact names vary, so match the name your machine maker gives you.

When in doubt: contact your machine manufacturer or search the software maker's user forum for your machine brand. Someone has almost certainly already posted the correct post-processor name.

Installing a Custom Post-Processor

If the software does not include one for your machine:

1. Download the post-processor file (.pp extension) from the software maker's post-processor page or from the user forum.
2. In the software: Machine > Install Post-Processor...
3. Browse to the .pp file and double-click it.
4. The file is copied into your My_PostP folder, and the post appears at the top of the Post-Processor Management list.

Inch vs. Millimeter: Which to Choose?

The post-processor must match the units your controller runs in, not the units of the job. The job can be drawn in either unit, and the software converts automatically when the toolpath is saved.

• Before choosing, jog the machine from X=0 to X=1 in the controller. If it moves 1 inch, use the Inches post-processor. If it moves 1 mm, use the MM post-processor.
• If your controller runs in mm and you output inch G-code, all positions will be wrong by a factor of 25.4.

Arcs vs. Linearized Toolpaths

Many post-processors come in a version that outputs true circular arc commands (G2/G3) and a version that linearizes curves into many short straight segments.

• Arc output: smaller files and smoother cutting on circular paths. Requires that your controller supports G2/G3 (most modern controllers do).
• Linearized: larger files but works with any controller, including older or simpler ones.

If your machine supports arcs, prefer an arc-capable post-processor.

Testing Your Post-Processor

Always test with a simple project first:

1. Create a simple rectangle profile toolpath.
2. Save it with your chosen post-processor.
3. Open the file in a text editor and verify it looks like valid G-code (or whatever format your machine uses).
4. Run it in your machine controller's simulation mode if available.
5. Air-cut first before touching material. The machine should move 1 inch when told to move 1 inch.