How to use the VCarve inlay toolpath in Vectric software | 2.5D Toolpaths

Overview

This video demonstrates how to create a V-carve inlay toolpath in Vectric software. It covers setting up separate plug and pocket sheets, generating the plug and pocket toolpaths, adding a clearance tool, and preparing a profile cutout for the plug.

Steps

1. Set up two sheets in the job: a larger pocket material (e.g., Walnut) and a smaller plug material (e.g., Maple). Different thicknesses are allowed.
2. Assign material names/appearances in the material settings for each sheet to distinguish them in 3D previews.
3. Ensure all vectors selected for the inlay are closed vectors. Open vectors are not allowed.
4. Go to the Toolpaths tab and confirm the material setup: thickness, XY datum, model position, rapid Z gaps, and home start position.
5. Select the vectors to include in the V-carve inlay toolpath (e.g., text and rectangle).
6. Choose the V-carve inlay toolpath strategy and configure:
   • Pocket depth – how deep the pocket is cut into the pocket material.
   • Glue gap – space between the bottom of the pocket and the plug surface for glue.
   • Surface gap – space between the pocket material surface and the deepest part of the plug.
7. Select a V-bit for both plug and pocket. For this example: 60° quarter-inch V-bit.
8. Select a clearance tool (e.g., ⅛-inch end mill) to remove excess plug material. This may also be used for the pocket depending on the vectors.
9. Choose the destination sheet for the generated plug vectors and toolpaths (Plug Maple sheet).
10. Choose how to handle the outer boundary of the plug:
    • Cut to sheet limits, or
    • Use a vector offset with a boundary offset (e.g., 0.25 inch) for an organic boundary.
11. Calculate the toolpath. The software:
    • Keeps original vectors intact.
    • Copies plug vectors to the specified sheet.
    • Flips the plug geometry left-to-right.
    • Creates a boundary vector for the plug.
12. Review the pocket toolpaths:
    • Clearance toolpath with the end mill.
    • V-carve toolpath for final pocket finish.
13. Review the plug toolpaths:
    • Clearance toolpath removes bulk material around raised plug areas.
    • V-carve toolpath cleans up the plug.
14. Create a profile toolpath to cut the plug out:
    • Select the boundary vector created by the V-carve inlay toolpath.
    • Set start depth to 0.
    • Cut through the full material thickness.
    • Use the same end mill or another suitable tool.
    • Cut on the line to remove any bevel remnants and leave a flat plug base.
15. Preview the cutout and inspect the final plug.

Key Points / Warnings

• The V-carve inlay toolpath creates both plug and pocket toolpaths, mirrors the geometry, and places toolpaths on the correct sheets.
• Closed vectors are required; open vectors will cause issues.
• If you change the XY datum later, you must recalculate the generated toolpaths.
• The plug stock value in the plug clearance toolpath indicates how much material will stand proud above the pocket after gluing. This is useful if you plan to surface the plug on the CNC machine.
• Consider cutting the plug first, test fitting it into the pocket, then gluing and surfacing if desired.
• Some users cut the V-carve pocket toolpath before the clearance toolpath to reduce chipping on raised plug parts or small pocket features.
• A typical warning can occur if the clearance tool is too large or otherwise unsuitable for the selected geometry.
• You may add tabs to the profile cutout depending on your machine setup.