How do I save toolpaths in VCarve Pro & Aspire: post-processors, single vs multiple files, and ATC output?

Overview

Saving toolpaths is the final step before cutting. It converts the calculated toolpath data into G-code (or machine-specific code) using a post-processor that matches your CNC controller. The output file is what your machine actually reads and executes. It works the same way in VCarve Pro and Aspire.

The Post-Processor

A post-processor (PP) is a configuration file that tells the software how to format the output code for your specific machine and controller. Different machines use different G-code dialects, file extensions, and motion commands.

How to select: In the Save Toolpaths form:

1. Select your Machine from the pull-down list
2. Select one of the post-processors associated with that machine from the Postprocessor list. The list only shows posts that have been associated with the selected machine
3. Click Save Toolpath(s), enter a name, and click Save

Associating a post-processor with a machine: Use the Machine Configuration dialog (the link in the Save Toolpaths form), or choose <Add Post-Processors> from the Postprocessor list to quickly associate more posts with the current machine. The software ships with many post-processors. For a missing controller, see the online and manual machine configuration documentation, or ask your machine manufacturer.

Examples of what to look for: the Mach3 or Mach4 post for those controllers, a GRBL (inch) or GRBL (mm) post for GRBL machines, the ShopBot post for ShopBot machines, or the specific post for your machine brand.

File extension: Each PP produces a file with a specific extension (.tap, .nc, .gcode, .sbp, etc.). The extension is defined in the PP and should match what your controller expects.

Save Modes

Selected Toolpath

Saves only the selected toolpath.

Visible Toolpaths To One File

Saves all visible toolpaths to a single file. The machine runs through all operations sequentially from one file.

Requirements:

• All toolpaths use the same tool, OR
• The machine has an Automatic Tool Changer (ATC) and the post-processor is set up for ATC commands

ATC workflow: CNC machines with ATC can work with a single file that contains multiple toolpaths, each with a different tool number. The post-processor must be configured to support ATC commands for your machine. The names of the toolpaths written into the file are shown with their tool number in square brackets, for example [1]. Un-tick a toolpath to leave it out.

Error messages: The post-processor checks that it is configured for saving files with ATC commands and that a different tool number is defined for each different cutter. An error message tells you if either is wrong.

Visible Toolpaths To Multiple Files

Saves each visible toolpath to its own file. You are prompted for a file name, which is used as a prefix for each file.

Group where possible: If chosen, consecutive toolpaths that use the same tool are saved to the same file, and the file name includes numbers showing which toolpaths it holds. Example: if you name the files "Toolpaths" and the first 3 toolpaths can go into one file, that file begins "Toolpaths_1-3". A toolpath that uses a different tool is saved separately.

This is the standard workflow for machines without ATC: one file per tool, run in sequence, changing bits manually between files.

Workflow for Manual Tool Change Machines

1. Check the toolpath order in the Toolpath List (use the Up/Down arrows to reorder)
2. Make sure each toolpath you want is visible (checked)
3. Open the Save Toolpaths form (the save icon at the bottom of the Toolpaths tab panels)
4. Select your machine and one of its post-processors
5. Choose Visible Toolpaths To Multiple Files, with Group where possible if you want same-tool toolpaths combined
6. Click Save Toolpath(s). One file is created per tool group
7. Name files clearly, for example "Sign_VBit.tap", "Sign_Profile.tap"

Workflow for ATC Machines

1. Set distinct tool numbers in the Tool Database for each tool (T1, T2, T3 etc.)
2. Use the Up and Down arrows to order the toolpath list in the cutting sequence you need
3. Tick each toolpath so it is visible in the 3D window
4. Open Save Toolpaths and select your machine and an ATC-capable post-processor
5. Select Visible Toolpaths To One File
6. Click Save Toolpath(s). One file is saved with all the operations and automatic tool change commands

Toolpath Order Matters

The order toolpaths appear in the Toolpath List is the order they are saved and run. Always verify:

• Roughing before finishing
• Pockets before profiles (so parts don't fall out)
• V-carve before profile cutout

Use the Up/Down arrows in the Toolpath List to reorder before saving.