Inlays using Carbide Create (and other software)

(William Adams) #1

There are a number of ways to do inlays, and a number of alternatives. Some of the simpler options can be done using just Carbide Create, while others require additional software, possibly just Inkscape, or specialized commercial software such as Vectric Vcarve or Amazon Canvas.

First, the work-arounds:

Carbide Create’s native facility with inlay is necessarily limited by the round endmills and their diameter for normal techniques, and its inability to flip designs. Symmetrical work can be done as shown in: Let’s make a coaster — basically one draws a symmetrical shape which will allow the endmill to get into all corners as discussed at: Inlay Work (Woodworking) — if the inlay and the stock material are the same thickness, then one doesn’t need to be able to flip one or the other, just cut both from the same side and then assemble.

One work-around for the inability to flip is to use the center of the stock for the origin (and place that at or near to the center of the machine), home / move the machine to that point, then reconfigure Grbl to reverse the X-axis, cut the part, then undo the reversal.

7 Likes
Pre-purchase help for bits from Drillman1 Ebay Store
(William Adams) #2

One technique for getting around the limitation of a round endmill and attendant detailing limits is to use a V endmill to cut both the inlay piece, and the pocket — the pocket needs to be cut from behind, and the inlay portion from the front, so as to get them to nest properly and to take advantage of the added detail the V endmill affords.

As noted above, it is possible to cheat the flipping in Carbide Create by instead using the center of the machine and reversing an axis, but for this discussion, we will flip the graphic and put both copies in a single file:

and attached: dachshund-black-silhouette.c2d (966.6 KB)

0 Likes
Let's make a coaster
(William Adams) #3

Next we need to know how thick the inlay material will be, and how wide we should expand the path — a 90 degree V endmill makes this simple, since to cut to a given depth, one needs the width of the V to be twice that:

So we offset each version of the dog to the outside twice, once to 0.25", and once to 0.5":

0 Likes
(William Adams) #4

It should now be possible to select the inner and outermost paths for the part which will be the inlay and assign a V carve to them:

Note that the V carve path to a great degree follows the middle path — this is important below.

0 Likes
(William Adams) #5

Then select the middle path and the surrounding rectangle and assign a pocket toolpath — this should probably be adjusted to be at least deeper than the inlay thickness by the expected glue line (calculating that is left as an exercise for the reader):

This may then be previewed to see:

(Note that the material which the inlay is cut from should actually be thicker than the 0.25" dimension — this way, if there are multiple small portions showing, they may all be manipulated as a single part which will be glued on from the back)

0 Likes
(William Adams) #6

Next it turns out that the two additional offsettings weren’t needed — select the path which describes the desired inlay pocket and assign a no offset contour to it using a V endmill:

When that path is cut, it is important that one zero so as to cut all the way through (cheat the Z zero by at least the thickness of the glue line) — unfortunately, V endmills assigned to a follow path / contour toolpath do not preview properly, so one has to take it on faith that the resultant pocket will match up.

1 Like