Making inlays using geometry

Since Carbide Create doesn’t have explicit support for doing inlays (software which does includes Vectric Vcarve and possibly F-Engrave) one has to calculate out the toolpaths for this manually. Considerations include:

  • endmill geometry
  • glue line / thickness — suggestion here is to glue together a stack of 6 popsicle sticks, then after it dries, measure the difference between the glued stack and 6 which are not so fastened — that thickness difference divided by 5 is a typical glue line for the glue / clamping technique used
  • inlay thickness
  • part geometry

Some cases can be quite simple: — a flat inlay of a part which doesn’t have any corners which the endmill won’t fit into is simply a matter of cutting out the part, then cutting a matching (possibly mirrored) pocket which is deeper and larger around the perimeter by the glue line (if using hide glue, this may be negligible).

A more complex situation is a V inlay of a material of one thickness into a material of greater thickness — this will require that one:

  • measure the material (plus anticipated glue line)
  • calculate the offset necessary to cut the part to the desired size
  • calculate the inset needed to cut the perimeter of the pocket as a V carve
  • calculate the inset needed to cut the bottom of the pocket

Let us consider the following case:

  • 60 degree V bit (Carbide 3D #302)
  • 0.316" thick material
  • 0.004" thick glue line
  • 0.5" thick stock material to inlay into

For simplicity, we’ll use a 1" circle.


One can either draw up the geometry, or calculate it. To calculate some useful references include:

To draw, one begins by making a 1" circle:

Draw a triangle to represent the angle of the endmill, and a rectangle to represent the width to which we will wish to cut (which is also the depth since a 60 degree endmill is an equilateral triangle):

Then do a Boolean intersect of the two shapes.

To cut the pocket you will need to inset by the desired thickness to cut a V carve to that depth along the perimeter, and by half that so that you can clear the bottom of the pocket:

Select the inner and outer circles and assign a V carve toolpath:

Select the middle circle and assign a pocket toolpath at the desired depth to clear the pocket:

The two pockets will preview as:

Inlay-vcarve-pocket.c2d (85.3 KB)

Cutting the inlay is a slight variation — we instead need to:

  • set the stock thickness to match the piece we will be using for the inlay
  • inset and outset by half the desired cutting width/depth
  • assign a V carve to the inner and outer paths — this will result in the V carve cutting along the original path

Again, select the inner and outer geometry to cut out:

Inlay-vcarve-part.c2d (96.5 KB)

1 Like