# How to Create an Inlay with a CNC Router

Jan 25, 2018 · 4 min read

I do more inlays than almost anything else with my CNC. I spent a long time doing the math and ‘research’ because they kept not being right. So, here’s how to do an inlay right — not just theoretically but practically.

I use VCarve to do my layouts. So, I’ll refer to it here in images and in cutting tasks. Obviously other apps would work.

## Design

Here’s an actual inlay I’m doing for a friend. I started with a 3d simulation using Rhinoceras 3d in order to get the colors and shapes right.

Then I took the inlay drawing, imported it into VCarve, simplified it down to a small number of curves and saved it.

## Tooling

When it comes time to do the male portion of the inlay you’re going to want a wide engraving bit. A standard 1/4" bit won’t create a male portion right because of the overlap problem — try it.

Anyway, I use a .75" diameter bit. It’s not large.

## Analyze the Inlay

The first step is to create a VCarve engraving path for the inlay. The start depth should be 0.0 and set the Flat Depth to something you like. For smaller inlays (like this one) there is no place at which it becomes flat.

I manually reduced the engraving pass depth (to .07") to make more cuts and have them stress the wood less. This increases the chances of a successful engraving without chipping the wood in fine details (like my first two tries).

Do a sample cut of the engraving path and examine the cut in VCarve.

Rotate the piece and place the cursor in the bottom of the deepest valley. Note this value and call it DEPTH. This is how tall a male inlay we’ll need.

## The Male Inlays

To do the male inlays, flip the entire design vertically (or horizontally) and surround it with a box. I keep the female and male designs in different layers to make life simple.

Then engrave the male (reversed) inlay portion. This is harder than it sounds because there is a lot of flat area and because a default setup will cause major chipping with a typical bit.

The key to engraving a male inlay is offsetting the cutter almost to DEPTH (minus room for glue). In this case I also had to engrave two more paths and lesser offsets to reduce the force generated by the cutting and avoid chipping.

In my case the DEPTH was .22" so I created

Engrave1(offset=0, flat=.1),
Engrave2(offset=.1,flat=.1), and
Engrave3(offset=.19, flat=.15)

Engrave1 and Engrave2 produce toolpaths that clear out some of the area and ease the cutter load before Engrave3 starts at .19". Their flat-clearing toolpaths also ease the flat-load for Engrave3.

Engrave3 is the engraving toolpath that leaves the details. This path, by offsetting nearly the DEPTH leaves .03" for glue (.22-.19) while producing a final flat value of .34 (.19+.15) that’s just below DEPTH (leaving .1" space to clamp down and for glue to be pushed up). In a larger pattern I usually leave .1" for glue area.

Note the two images showing the paths below. One is just Engrave3, the other is all 3.

Here’s a view of the two cuts.

Once the male inlay is machined I run it through a band-saw and trim off the sides so it looks like a thin board with the male inlay attached as in the photo above.

## The Finished Result

I glued them together and clamped the heck out of them for a day. Then I ran it through my planer repeatedly trimming off little bits to get this:

Written by

## Mark Zachmann

#### Entrepreneur, software architect, electrical engineer. Ex-academic.

Welcome to a place where words matter. On Medium, smart voices and original ideas take center stage - with no ads in sight. Watch
Follow all the topics you care about, and we’ll deliver the best stories for you to your homepage and inbox. Explore
Get unlimited access to the best stories on Medium — and support writers while you’re at it. Just \$5/month. Upgrade