Recipe for Creating V-Carve Inlays in Fusion 360

I was looking at YouTube videos that make v-carve inlays. They look pretty cool so I thought I would try to create one. Most of the time the YouTubers used Aspire. That’s too expensive for me. Since I’ve been using Fusion 360 free for a couple of years now it was my tool of choice. I quickly discovered that v-carve inlays are not so easy in Fusion. After failing to get a simulation that worked after several tries, I switched to Carbide Create, a free tool from Carbide3D. Turns out, with their Advanced V-Carve function the inlays are trivial to set up. I’ve since set up about 50 of them. It only takes me about a minute once I have artwork I like. But it bugged me that I couldn’t do the same in Fusion. So when questions started coming up about Fusion in this forum, I dug my heals in and figured it out. Here then is my recipe for creating v-carve inlays in Fusion 360. It works, at least in simulation. Note that a reasonable familiarity with Fusion 360 is a prerequisite for these instructions to make any sense.

My recipe is based on the 3:2:1 formula found in many examples on YouTube. More on that below.

Base Decisions, Variables and Assumptions

  • These instructions assume the sketch containing inlay geometry (outline artwork) is coplanar with the surface to be cut. That’s not a requirement but if it’s not true then the Top Height values will need to change.
  • Choose the max depth of the inlay pocket (female part) = DEPTH
    • Typically, 0.3" or 3mm Yes, I know these are nowhere near the same. Apparently, Imperials cut deeper inlays and Metrics cut shallower inlays. :stuck_out_tongue:
  • Choose the engraving Bit (e.g., 60-degree V-Bit) based on inlay detail. The finer the details the narrower the v-bit needs to be to cut deep enough for the inlay to stick.
  • Calculate Stock to Leave (StL) value
    • StL, generic formula = tan(V-Bit/2) x DEPTH
    • StL, 15vbit = 0.132 x DEPTH
    • StL, 30vbit = 0.268 x DEPTH
    • StL, 60vbit = 0.577 x DEPTH
    • StL, 90vbit = 1 x DEPTH
    • Example: for a 60d V-Bit and a max depth of 3mm, StL = 0.577 x 3 = 1.731mm

CAM Operations

Setup: Female (pocket)

  • Model = select the body that represents the part the pocket is cut into
  • Stock Mode = “Relative size box”

Op-1: Engrave

  • Tool = V-bit, 30/60/90 depending on inlay detail. Make sure the bit can handle the depth of cut. You can’t cut 0.3" deep with a bit that only has 0.25" flutes.
  • Geometry = selected outline(s) from sketch
  • Top height = “Selected contour”, offset = 0
  • Bottom height = “Top height”, offset = -DEPTH

Op-2: 2D Pocket // cut away the flat bottom areas Op-1 left behind

  • Tool = Flat end mill, 1/8" typical (go smaller to get into tight corners)
  • Geometry = Same as Female Op-1 (flip arrows as needed to cut INSIDE)
  • Stock Contours = none
  • Rest Machining = none
  • Top height = “Selected contour”, offset = 0
  • Bottom height = “Top height”, offset = -DEPTH
  • Radial stock to leave = StL, see definition above
  • Axial stock to leave = 0

Setup: Male (inlay)

  • Model = select the body that represents the part the inlay is cut from
  • Stock Mode = “Relative size box”

Op-3: 2D Pocket // remove the bulk of material around the outside

  • Tool = Flat end mill, 1/4" typical
  • Geometry = Mirror of artwork used in Female Op-1 (flip arrows as needed to cut OUTSIDE)
  • Stock Contours = none
  • Rest Machining = none
  • Top height = “Stock top”, offset = -2/3 x DEPTH
  • Bottom height = “Top height”, offset = -1/3 x DEPTH
  • Radial stock to leave = StL, see definition above
  • Axial stock to leave = 0

[OPTIONAL] Setup: Male Finish //optional setup. If this setup is not used then Op-4 goes under Male (inlay) setup

  • Model = select the Mesh saved from Male Op-3
  • Stock Mode = “From solid”
  • Stock Solid = select the Mesh saved from Male Op-3


Op-4: 2D Pocket // v-bit cut to match engrave wall

  • Tool = Same angle V-bit as used in Female
  • Geometry = Same as Op-3 (flip arrows as needed to cut OUTSIDE)
  • Stock Contours = New geometry needed. See notes below to create it.
  • Rest Machining = none
  • Top height = “Stock top”, offset = -2/3 x DEPTH
  • Bottom height = “Top height”, offset = -1/3 x DEPTH
  • Stock to leave = none

NOTE: Stock Contours requires an additional geometry. This is a boundary that restricts Male (inlay) Op-4 from wasting a lot of time cutting air. You can create this geometry a number of ways.

Option: // use any one of these

  • Draw a rough outline around your artwork at least StL outside the artwork. This can be crude, but the better (tighter) you make it the less wasted time.
  • If the artwork is simple enough use the offset tool in the sketch palette to generate the geometry. Offset >= StL.
  • Save the result from Male (inlay) Op-3 simulation. Import the saved result into the model. Use the mesh outline tools to trace the outline of the remaining material.
  • Disable Stock Contours. Inefficient, but does not affect the viability of the inlay.

NOTE: You don’t really need Op-3. Alternatively, omit Op-3 and just cut around the inlay with a jigsaw.

NOTE: OPTIONAL Setup Male Finish - You can save the simulation produced from Male (inlay) Op-3 as an .stl file and re-import it as stock for Male Op-4. This makes the simulation look prettier but does not change the g-code.

The attached .f3d file is a v-carve inlay example using these instructions. The images above were captured from the Fusion’s CAM display for each operation. Normally you wouldn’t put the pocket and the inlay in the same design file. They are going to be from two different, presumably contrasting, pieces of stock and there might be other features in the pocket file that prevent putting the inlay anywhere convenient. I just put them in one file to make it easier to distribute.

The 3:2:1 formula comes from the depth of the inlay pocket (3) and how far the inlay inserts into the pocket (2) and the additional depth of the male inlay cut (1). To make the parts fit, the sum of the insertion depth and the additional depth must match the depth of the pocket (3=2+1). The inlay does not insert fully into the pocket to leave room for glue and ensure a tight fit between pocket and inlay edges. With the 3:2:1 formula the inlay goes in 2/3 of the total depth. This formula seems to be the most common, but other folks have posted some variations. In his YouTube video, Dave Van Antwerp talks about the formula they use as being 2:1:1. That is, the total pocket depth is 2 and the inlay inserts 1 or half way into the pocket. Dave talks about these as dimensions, but it is really the ratio that is important. In her YouTube video, Beki from Vectric LTD starts using a 3:1:2 formula but then switches to an extreme 3:2.8:0.2 formula when she has issues with subsequent operations tearing out the inlay. Chet Weatherl says in his video that he has done a comparison and the best formula is 2:1.8:0.2.

I believe that it depends on your artwork. If Op-2 can’t clear out everything because the artwork has tight corners then the uncut remainder will keep the more extreme formulas from seating fully therefore leaving a gap at the edge. The 3:2:1 formula is a reasonable compromise between leaving room for the junk underneath and maximizing support and glue surface area. By understanding this compromise, you can push the formula either way. Remember simulation is your friend. You can clearly see the uncut areas in both the Fusion and Carbide Create simulations.

I said this at the beginning and I’ll say it again here: Setting up to make v-carve inlays is much easier in Carbide Create than it is in Fusion 360. Both are free. Both work. The only reason I created the Fusion solution is because I’m a stubborn sob and was determined to figure it out. BTW, this doesn’t mean I like Carbide Create better than Fusion. Fusion is still my go-to tool for most CAD/CAM. Fusion is far more flexible and capable. But in this case, Carbide Create has this particular function preprogrammed in a simple to use package. For this task Carbide Create is specialized and better.

  • Chip

Horus (1.2 MB)


Thank you for this. I feel like fusion is an awesome and likely most powerful suite available but that doesn’t mean easiest or canned as far as a solution is concerned. With great control… Comes great responsibility :slight_smile:

Thank you very much for such an informative post. That’s a heck of a lot of information to absorb and you obviously put a ton of time into it. Thank you!


Hey Chip - that’s really great work. Agree about Fusion’s lack of advanced v-carving capabilities. I feel like there is a way, but I’ve not been able to find it. I generally use Easel for inlays, but it’s not v-carving - just profile outlining, which can accomplish the same outcome with a little less precision in the corners.


Eric, hopefully this gives some hints for doing your sign in Fusion as well. Or if not, let me know and I’ll see if I can figure something out for you.

1 Like

Thanks for the comments, folks. Are there other recipes for Fusion that would be of interest to the group? Another one I struggled with is relief carving in Fusion. Would anyone be interested in a recipe for that?

1 Like

Since the first posting in this topic, I have continued to apply this recipe for different projects and geometries. In particular I wanted to solve the sign problem posted by AdamsLeatherWorks and if possible, create a generalized solution. What I found was that this recipe does not work in all cases. The Advanced V-Carve operation in Carbide Create and Aspire is actually three machining operations. I was trying to get it done in two. Also, within those three operations is an optimized “Rest Machining” that I had improvised with an additional geometry. In short, there is a better solution, so this one should be discarded.

Forum managers, if you would turn editing back on for the original posting, I will edit the above paragraph into that.

There is a new solution. Almost. It turns out that the math is a little more complicated than what I have here, so a simple recipe would not be so simple. Too many calculations and opportunities to get things wrong. Instead, I was hoping to publish an add-on script for Fusion which would implement Advanced V-Carve. I figured out the more general three operation solution. I figured out Rest Machining. I even started coding up the script. That’s where I ran into a roadblock. The APIs to give script access to choosing a tool and geometry have not been released yet by the Fusion team. I have it from Fusion on their forum that the APIs are coming, hopefully soon. When the APIs are available, I will complete the script. Rather than continue with this thread I will create a new topic and post the finished script there.

In the meantime, here’s just a teaser to show it off. In its current state the script does the math and creates the three ops, then you have to go back and manually edit each op to pick the tool and select the geometry. It’s a pain to select the same geometry three times. In the finished version you’ll just select the geometry once from within the script.


Hey Chip, really great work!

I’d be happy to beta test your Fusion script / add-in if that’s helpful. Particularly is there is a reasonable amount of custom UI, since they often seem to fail in this area.

Is is easy to alter the 3:2:1 ratio with the scripted approach?


Looking forward to it Chip - I’ve been wanting this capability for a long time. Great work!


Thanks for the interest.

As far as the UI goes, here it is.

You change the ratio by changing the Start Depth and the Flat Depth. These are similar to Aspire. Carbide Create uses Start Depth and Max Depth, but Max Depth is just Start Depth plus Flat Depth.

The tool selection drop downs will be replaced by tool select buttons in the final version. The buttons will take you to the tool selection dialog just like any other Fusion operation. At least, that’s the plan. Again, it is dependent on what the Fusion team exposes in the API.

The UI needs some other improvements as well. The button and drop downs are too far to the left. This cuts off the labels unless you manually expand the dialog. Also, the graphic showing how Start Depth and Flat depth are measured needs improvement. I’ll be tinkering with these while I wait on the APIs.

I am open to feedback on the UI. I want to keep it consistent with the rest of Fusion but if there is something that is confusing, let me know.

I will definitely be looking for beta testers once the script is complete and I’ve written some instructions. Right now it is too fragile and the instructions too cumbersome to really be useful. But I may get bored and write something up. We’ll see.



Hey Chip - I’m totally in when you are ready.


Ditto… I prefer fusion…

Hey Chip,

Were you able to get your script working? This is a big gap in Fusion’s workflow for hobbyists. I’d be happy to help with testing if you need it…or be a paying customer if you get your add-in published.


The script is working as far as it goes but AutoDesk has yet to release the APIs in Fusion to select tools and geometry from a script. Until they do that the script doesn’t really do what you want. They said that they are working on it, but that could mean weeks, months or years. If they publish the APIs I will certainly try to finish the script.

Thanks for your interest.

1 Like

Wow- Fantastic work, chips. The beginning of this thread was a great lesson in manually setting up a v-carve inlay, and I was all excited reading through. But then you went on to develop a script to implement it as an automated process and I am beyond impressed. Hopefully the APIs will be released and we can put your work to use.
Well done.

Thank you for figuring this out. I am wiling to work through a few extra steps if I can create a working inlay using F360. I am not smart enough to learn multiple programs and F360 is hard enough, so being able to use F360 for in lays is fabulous.

1 Like

Now that you’ve put the work into V-Carve inlays with Fusion. What about doing stacked word carvings in Fusion. I have to play around with it and I’m thinking maybe using a separate construction plane on top of the bottom word to add the stacked word. Then moving it downwards towards the bottom word and trying to combine them together. Any thoughts?

I’m also interested in this. I spent an hour or two trying to find a machining strategy for stacked words in Fusion 360 and got frustrated and haven’t went back to try again. I’m sure it’s something simple, but I’m still new to the CAM side of things and it wasn’t immediately obvious.

I figured out how to do it. It’s actually very simple.


Of course it’s simple after you’ve figured it out :stuck_out_tongue_winking_eye:

Do you mind helping us slower folks out?