VCarve Inlay - A simple way to make inlays

The all time great topics from elsewhere on the forum
Paul Z
Vectric Wizard
Posts: 517
Joined: Sun Apr 30, 2006 10:04 pm
Model of CNC Machine: shopbot PRT Alpha 96x48
Location: New Hampshire, USA

VCarve Inlay - A simple way to make inlays

Post by Paul Z »

For full details on how to design and machine V-Inlays read the attached PDF document.
This has been updated for the latest procedures.

The steps listed below were Paul's original thoughts on a generic procedure for cutting
inlays, but he later found they are not always correct and the PDF method has been updated

The original topic can be found here ->


I have wanted to make some inlays with my shopbot but there were two issues:
1. the artwork has to be revised to accommodate the bit size and that would require a fair amount of CAD work for each inlay
2. the resulting inlay would have rounded edges.

I remembered that people who do intarsia will often angle their blade and rotate the piece as they cut to make up for the thickness of the blade. The resulting pieces fit perfectly even though they fit on a bevel. Could one achieve a similar effect using v bits?

It came to me that I might already have the necessary tools, both hardware and software (V Carve). Here is the process that I used:

1. This test was done with a 90 degree bit (‘cuz that’s what was in the router and I was too lazy to change it. A 60 degree bit might have produced better results.)
2. Pick a graphic. I used inkscape (free on the web) to generate an outline of the graphic. (One could also start from a DXF file or even make the design in V Carve.)
3. Start V Carve and import the path file.
4. Check for open or duplicate vectors and correct them if necessary.
5. Copy the path; paste it; and, using the mirror function, flip it horizontally.
6. Move it to the right to get it away from the original path.

(Top figure)

7. Now decide how deep you want the inlay to be. Keep it relatively deep to make the inlay piece less fragile. For this example, let’s use 0.2 inches.
8. Create a V Carve tool path with the original path (the one on the left) using a flat depth of 0.2 inches. This will be used to create the pocket for the inlay.
9. Now create profile tool path 0.2 inch deep on the flipped path (the one on the right) using the Machine Vectors “ON” option and no tabs. This will be used to create the inlay itself.

(Middle Figure)

10. Cut the pocket into your base material.
11. Cut the inlay into material that is thicker than the cut depth.
12. Sand the back of the inlay until the inlay falls away from the rest of the material.
13. Glue inlay into the pocket.

Here are the pocket and the inlay and below that is the inlay in the pocket.

(Bottom Figure)

The inlay rides a little high because I haven’t cleaned off some “fuzzies” from the cutting. When I press the inlay down, it fits almost perfectly.

I am working on a slight modification to the process of cutting the inlay to make it thicker than the pocket. This would allow cutting the inlay with tabs and eliminate the process of sanding until the part becomes free. The inlay will be higher than the pocket when installed but it can then be sanded flush.

The result of this method is that graphics (many? most?) can be used without alteration and that the inlay can have sharp points. I hope some of you find this useful and please let us see anything you might create.

Paul Z
two paths.JPG
two paths formatted.JPG
pocket and inlay.jpg
inlay layout.jpg
PDF document describing the V-Inlay process
(1.09 MiB) Downloaded 7484 times