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.
- Typically, 0.3" or 3mm Yes, I know these are nowhere near the same. Apparently, Imperials cut deeper inlays and Metrics cut shallower inlays.
- 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
[END OPTIONAL]
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 v7.zip (1.2 MB)
