vCarve Inlays with... vCarve Desktop! Details and discoveries

I’ve been using vCarve Desktop for several weeks now and I wanted to put in one place some conclusions I’ve come to after a LOT of test cuts and procedure around doing vcarve’d inlays. When I was starting out wanting to make these, I couldn’t find any good explanation of WHAT each of the various measurements really were and how scaling each affected the others and the fit over all. So I cut a slew of test pockets and plugs using various settings to try and get a handle on it. Here are my findings:

For the Pocket, the Flat Depth is just the depth of the pocket bottom. Easy.

For the inlay;

The Inlay Start Depth:
This number appears to dictate how “deep” into the pocket the inlay goes.
This is the vertical representation of the actual side-cross-section glue surface.
This number should ALWAYS be LESS THAN the Start Depth, otherwise the inlay will bottom out, and the edges wont meet.
Unforunately, because this is a false start depth, the tool will plung to this full depth on first cut. There is no way I’ve found to avoid this. I’ve even spoken to Vectric support and according to them, this is unavoidable

The Inlay Flat Depth:
This appears to only determine the amount of ‘overflow’ ABOVE the surface of the pocket work piece.
Increasing this number ONLY increases the distance between the “bottom” of the inlay and the “top” of the Pocket piece.
Making it bigger allows a bigger blade to pass between the inlay material and the pocket when trimming flush.
This should be a positive number to account for variations in material surface.

Example (Common):
The most common example shown is a Pocket flat depth of .2 inches and an Inlay Start and Pocket depth of .1 and .1
The result of this is a .2" deep inlay pocket. The Inlay plug will “stick” into the pocket .1 inches (this is the side wall contact surface), have a .1" gap between the pocket floor and the inlay “top”, and leave a .1" gap between the two work pieces for sawing.

Example 2 (What I use)
Pocket Flat Depth: .15
Inlay Start Depth: .145
Inlay Flat Depth : .025

This will have a .15" deep pocket vs .2" of the first example, but the inlay will stick deeper into the pocket (.145" deep), giving more wall contact,
and sit a scant .005" from the floor of the pocket.

This example is, in my opinion, superior to the “standard example” used by Vectric and others for several reasons:
First, it leaves a much smaller gap at the bottom between the pocket and inlay flats. Wood glue is NOT gap filling, no matter what youtube says. The idea that you need “glue space” of 1/10th" is just wrong.
A good clamped glue line should be something like .2mm thick. However, the gap serves the second purpose of making sure we “bottom out” on the SIDES and not the FLATS. You always want to bottom out an inlay on the edges, as that is what is seen, vs on the flats (top and bottom)

Second, it provides more thickness to the final remaining inlay wood. This permits a bit more sanding (though proceed with caution), and provides more glue surface where it counts.

Finally, I machine/mill my inlay bulk away, not cut it, so I don’t need the .1" gap between the surfaces (the Inlay’s Flat Depth). That being said, you don’t want it at ZERO because then you’d run the same risk of bottoming out your work flats before the edges made good contact. I’ve found .025 to be a good compromise here.

I’d welcome anybody input or corrections on what I’ve got here. They are not absolute truths, just conclusions based on observation so I’m very open to being wrong. Additionally, I’m planning to do some tests using negative depths on the Pocket cut to see if I can find a way to avoid making the full start-depth+pass-depth plunge in one shot on the inlay cuts.

I hope this helps somebody!



Thanks @Adam_Xett for this post. I’m currently doing my first inlays, and the only examples I have found use the .2" / .1" / .1" setup in your first example. I’m anxious to try your example. Some of the inlays I have in mind are small and delicate, so I worry that without enough side contact, I might break out a piece and ruin it. I will keep you posted how it goes. I’m working on some band logo coasters, and I got this far last night. Lots more work to do.


Thanks Adam, I just pulled the trigger on vCarve desktop a couple of days ago. Been watching tutorials ever since, no cuts yet. Inlays are on my todo list, your advice will be helpful I am sure.

Cheers Griff! I waffled endlessly about buying it, wish I had when I first got the machine. Really capable software.

I spent most of today re-writing the shapeoko post-processor for vcarve. Adding tool change support and some better code commenting mainly. I’ll get it tested out and hopefully post it tomorrow night.

Okay @Adam_Xett, need help with the above picture. I did the standard Vcarve recommendation of .2" depth for the pocket, and .1" / .1" for the male side of the inlay. Unfortunately, they are too close in size to fit properly. Can I re-run the V-carve toolpath for the female portion with a depth of .25" or .3" and salvage this without wasting the Male portions I have milled? I don’t want to try to cut the male portions smaller, as I will lose detail I think. Suggestions?

@EvanDay, can’t see a picture, but based on what you said… maybe.

Don’t adjust the female flat depth, this will just make it deeper, not affect the fit of the sides. I believe that if you re-run your female pass using an increased start depth (say .005 to start with) and the same .2 flat depth, it should widen out the pocket.

God speed! Let me know if you rescue it…

Thanks for the quick reply. May try that tonight. The picture I was referring to is earlier in this thread.

1 Like

Looking forward to trying your post processor. Managed a few cuts last evening following my normal routine and got bitten immediately when I hit Run and the cutter dove right in before I could start the router! No harm though it was scrap wood and a 1/4” bit, just had to re-zero z.
I do like the fact that the vCarve post doesn’t return to home on an abort. I broke my SuckIt, twice, crashing in to clamps on the way back home. My preference on an abort is to retract z 100% and stop.
I like the software, much simpler and better for engraving etc then F360. Double sided looks simpler too, can’t wait to try it.
Thanks again Adam.

Just posted the pp here: vCarve Desktop Shapeoko3 Post Processor

1 Like

@Adam_Xett, Haven’t tried the new post processor yet, however one question: I prefer to saw apart the two pieces after glueing. Will I have enough space for this using your values of .15" / .145 / .025? I use a really thin bladed hand saw that I normally use for cutting dovetails. On a happy note, after many long hours at work, I was finally able to get back to my inlay coaster project and I was able to save the ones I had messed up on. They are glueing up this evening so I think they will turn out well using the standard values of .2 / .1 / .1

@EvanDay - Nope, my values will not allow room for a saw blade to pass between, but you don’t have to split them, you can always just saw through the inlay backer material. Adjusting the inlay’s Flat Depth will give you the gap you’re looking for to pass the blade. Glad you got your coasters squared!

I use VCarve and love it. For this type of inlay I also discovered the F-Engrave. See it here:
VCarve will handle it too but no experience as yet.

1 Like

Considering the price (free), F-Engrave is really great. I worked with it a bit and got decent results, again, knowing the price. That being said, I wish I’d bought vCarve out of the gate, such a great application (especially for vCarve’d inlays)

Long follow up since I can’t edit the OP:

The values above work best with a 60 degree vBit that’s got AT LEAST 3/8" cutting surface. The Whiteside 1550 is what I used in my testing.


Do you still recommend this post processor or is there a newer version?

The non-carbidemotion one should still be fine (I used it yesterday), if you need to send with carbide motion I updated that one recently here:

Thanks for the response, I only got started with my Shapeoko and CNC in general about a month ago. I’ve cut a few things but just invested in Vectric carve desktop and was surprised, or at least dismayed, that there was no tool change prompts for my bitrunner. That’s why I asked if this was the newest version of your modified post processor since I apparently revived a 4 year old post. Any suggestions are welcome!

So is Carbide motion good for Vcarve desktop? I’ve been debating purchasing it since the start/flat depths make so much more sense for inlays compared to carbide create.

This video is great at explaining how to correct the bit from plummeting the entire start depth for your plug. It pretty much tells you to break it down into multiple jobs to avoid going so deep in one shot.

Design wise, it’s amazing. I exported my G code and ran the job for each tool independently, I was just disappointed by the fact that it doesn’t support tool changes natively. I’ll have to rewatch that video though because I am having an issue with the depth of my V bits. My test inlays so far have these ugly gouges in them.