How to use the auto inlay toolpath in Vectric software | 2D Toolpaths

Overview

This video demonstrates the Auto Inlay toolpath in Vectric software, which automatically compensates for tool radius so that male parts fit cleanly into female pockets or holes. It explains why standard Profile and Pocket toolpaths fail for inlays, then covers straight male/female inlays, adding an overcut allowance for fit, and a stepped inlay example using two different materials.

Steps

Demonstrate the problem with standard toolpaths

1. Open the example file and switch to the Toolpath tab, then the 3D view.
2. Notice two identical letter “E” vectors: one assigned a Profile toolpath (male), one assigned a Pocket toolpath (female).
3. Preview both toolpaths.
4. Observe that the male part will not fit into the female pocket:
   • Profile toolpaths leave sharp external corners but radius internal corners.
   • Pocket toolpaths radius external corners but leave sharp internal corners.
5. Reset the preview, select the existing toolpaths, and delete them.

Create a straight male inlay

1. Select the vector for the male part.
2. Click Inlay Toolpath under the toolpath operations.
3. Choose Male Inlay → Straight.
4. Set Start Depth to 0.
5. Set Cut Depth to cut through the material. Use the Z= button to automatically input the material thickness.
6. Click Select and choose a tool, e.g. a 1/4" End Mill.
7. Name the toolpath, e.g. Male Inlay.
8. Click Calculate, then preview the toolpath.
9. Note that all corners are now rounded, matching the tool radius.

Create a straight female inlay / pocket

1. Select the matching vector for the female part.
2. Open Inlay Toolpath again.
3. Choose Female Inlay → Pocket.
4. Set Start Depth to 0 (or the depth already pocketed if starting below the surface).
5. Set Cut Depth, e.g. 0.25".
6. Select the exact same tool used for the male inlay.
7. Choose an offset or raster strategy; this example uses Offset.
8. Name the toolpath, e.g. Pocket Inlay.
9. Click Calculate and preview.
10. Confirm the corners are rounded so the male part can slot into the female pocket.

Add an overcut allowance for fitting

1. Open the female pocket toolpath settings.
2. Set Overcut Distance to a small value, e.g. 0.02".
3. Recalculate and preview.
4. In the 2D view, toggle on the toolpath drawing and switch to solid view to see the overcut extending slightly past the vector boundary.
5. Cut the male part first, then the female part. Use the male part to test-fit while the female part is still on the machine bed.
6. Increase the overcut distance if a larger allowance is needed.

Create a stepped male inlay

1. Open the provided stepped inlay example file.
2. Note the two sheets: acrylic (0.5" thick) and aluminium (0.125" thick).
3. Switch to the Toolpath tab and open the Inlay Toolpath form.
4. Choose Male Inlay → Stepped.
5. Set Cut Depth through the acrylic material (Z=).
6. Select the same 1/4" end mill.
7. Set Step Depth to 0.375", leaving a 0.125" backing.
8. Set Step Width to 0.2".
9. Click Calculate and preview.
10. Adjust the material appearance to acrylic, if desired, and use the preview to inspect the step.
11. Switch to the aluminium sheet to create the corresponding female hole in the next step.

Key Points / Warnings

• Standard Profile/Pocket toolpaths do not work for inlays because the tool radius creates mismatched corner geometry.
• The Auto Inlay toolpath automatically rounds all corners based on the selected tool geometry, allowing male/female parts to match.
• Always use the exact same tool for the male and female inlays. Different tool radii