RE: Help: What do I need to do to eliminate gaps around inlay using advanced v carve

Continuing the discussion from Help: What do I need to do to eliminate gaps around inlay using advanced v carve:

Have had lots of difficulty achieving precision v-carve inlays that don’t produce gaps at the surface. Since December, have had multiple issues that one by one I’ve eliminated—spindle wobble, loose screws in Z, loose screws in gantry mount, router bits [maybe?] out of conformity. Believe all that is resolved, machine calibration checks out, and have produced some tests with success that makes me think I’m on track, then all of sudden failure again. Only this morning have I stumbled onto what may be at the root, but I still don’t know if it’s pilot error in Carbide Create on my part, or my lack of understanding on how to correctly manipulate CC, or something buggy in the code that is giving me inaccurate tool paths occasionally. I have studied the tutorial on how to vcarve inlay in version 4, but I believe I’m right in understanding the new functionality in advanced vcarve with start and max depth should achieve the same result as cheating the z-zero in the tutorial. Others with better insight than me might have a better notion of that.

So, on to what I stumbled on. Including files for the small test of an intricate lettering for my farm’s logo that I’m trying to inlay on an end grain cutting board. Making several test cuts before I [plunge] into the end grain walnut and ruin a rather expensive bit of wood. The test pocket comes out as expected; I have 0 and .25 max depth. To test that advanced vcarve places the tool path accurately, I created an offset tool path inside = tan of 18 degrees x .25 max depth = .0395. In simulation, I can visually see the tool path and the offset vector are essentially on top of each other. Seems right.
For the inlay, I do have a pocketing pass to clear away material before advanced vcarve as the settings I’m striving for are .22 start and .28 max, which I expect leaves .03 glue gap in the pocket inlay and .06 saw gap above pocket surface. So if I understand advanced vcarve start depth, the idea is to achieve the exact width of the inlay vector at start depth, so when inserted into the inlay everything above that plane sits into the pocket and everything below that plane protrudes above the surface of the pocket. So for 18 degrees and .22 depth, I believe the tool path should be offset .0348. What I find is that the tool path is actually very close to the inlay vector. Through trial an error, made offset tool paths to compare to the tool path in simulation and for .22/.28 it is very close to being offset by .01. Back to trig and believe that implies a depth of .06, which incidentally is the difference between start and max. So I changed settings, did the same checking, and feels like I can confirm the tool path is being calculated offset from the inlay vector by the difference of start and max.

So back to my original question, am I not designing correctly in CC, is CC bugging, or is this just not functionally available in CC [other than the version 4 tutorial on manipulating z-zero / or designing offset tool paths manually using property geometry]?
Has been a tremendous learning experience for me getting to know the Shapeoko Pro better as I approach my 1-year anniversary with the machine and would really like to get this inlay carving figured out. Not an engineer or mathematician by training, so no guarantee my calc’s are right either. Appreciate any other insights.

Test 18 bit-v.1-pocket.c2d (969.5 KB)
Test 18 bit-v.1-inlay.c2d (593.6 KB)

Todd, that is fascinating. How are you compensating for this offset? Does that give you gap-free inlays?

This could explain why I got good results with a 0.11" pocket once I switched to more inlay above the pocket. My early experiments used 0.02" above since I use the cnc to flush the surface, not a bandsaw. After watching too many v carve YouTube videos to remember which one, I switched to 0.08" for a saw kerf gap. For the 0.11" pocket, the kerf offset would be pretty close which is what I started to see. For the 0.2" pocket, the offset of the 0.08 is is still too far away for good alignment which is also what I was seeing. Of course this is on a run of only two at each depth.


A correction in my typing before, the math is tangent function of 1/2 the included angle of the v-bit tool I specified. So when I described 18 based on the tool I selected for recent tests, the formula is tan(18/2).

Moving on, my theory is that we are using advanced vcarve in CC as a perfect substitute for shortcut into inlay carving tool paths, and that it wasn’t necessarily created to serve that purpose. It just so happens to work for certain combinations: .2 pocket and .1 start with .2 max for example produces good fit between the pieces if you’re willing to accept .1 glue gap. But stray from that, especially with narrow angle tools for thin design elements where there less room for error and you quickly develop poor fit and gaps.

If I make a shape, create an advanced vcarve first with start =0 and max=desired start depth value, I can go back to design and create an offset identical to the tool path as a marker. If I then edit the vcarve to the actual desired start and max depth, I believe the tool path would be expected to move outward for the male inlay. By using the offset as a marker, you can see the tool path in fact moves inward not outward.

Have to assume that the AVC function in CC is working exactly as it was intended, just wasn’t intended to manage vcarve inlays. I think one work around is creating your own offset vector for the male inlay and design tool paths from that. I have a somewhat intricate logo im wanting to inlay and expect it would become too easy to lose track of the original vectors and the offset, mirror images. I’ve been exclusive to CC so far, but I’m developing a notion that others that have achieved success have perhaps used different software which I maybe need to explore. Will be a few days before I can jump back into this.

1 Like

@CoalWaterFarms I think you may be overcomplicating things. No trig needed. I’m all for math, but it’s all taken care of for you by using the same V-bit for the male and female parts.

Why? The parts will be wider the farther you go down, so at Z0 (using CC), it should be narrower.

A problem that is fairly common with steep angled bits is that not enough room is left for clamping pressure. With a “glue gap” of 0.03", you’re leaving yourself less than 1mm before you bottom out. That’s not leaving much room for error (deflection, bit tolerance, machine tram, toolpath tolerances, temperature changes, humidity, etc.)

I doubt that’ll make a difference in concept. I don’t use Create much, but I’ve done V inlays in Create, F-engrave, Easel, Vcarve, and Fusion 360. The principal is the same in all of them.


@CoalWaterFarms, I agree with your math, and have had similar frustrations in trying to do VCarve inlay. For the male piece, it is correct that the cutter offset is based on 0.06tan(angle/2) rather than the 0.22tan(angle/2) - using your numbers.

What I FINALLY concluded was that the error was in the bit I was using. Ironically, my very first attempt at an inlay worked great! The inlay was from 1/8th inch material and I was using a 60 degree bit. I made a nice little coaster with dolphins on it.

So, I decided to go bigger and used a narrower bit (Amana 46282K bit with 10.8 degree angle). Results were depressing as, although cuts were definitely cleaner, I had that annoying gap that you are dealing with. I messed around with changing glue gap size, inlay depth, and cutoff overhang. Still, the issue persisted!

What I finally (duh?) realized is that my bit did NOT come to a sharp point. So what? I was using the same bit for both parts. Well, in looking closely at the math, I realized that the software doesn’t consider the “tip” diameter of the bit. It expects a sharp point. So, when you zero your bit (z axis), the bit actually sits LOWER than it should. This works against you on both pieces! On the female carve, it makes it slightly larger, and the male piece becomes slightly smaller. (In both cases the bit is too low and so it cuts too close to the image boundary.) You get a gap! Making the glue gap deeper, and the cutoff larger as well, can help A BIT because you then just force the inlay in deeper than it SHOULD go, but it really doesn’t help for those “corners” where the carve depth doesn’t reach the bottom.

I thought about trying to create an offset path for both parts to compensate, but that really doesn’t fix the issue (and offsets can mess with the actual shape of the image).

None of my small angled (tapered) bits came to a sharp point, so I concluded that I just need to use bits that do.

SIDE NOTE (aka: the geometry). If you bit has a tip radius R, and an angle (included angle) of A, then the “missing part” of your bit is R/tan(A/2). This is how much lower your bit sits. In my case, the bit had a 1/32” radius ball, so it made the female part 0.0283” too big and the male part 0.0283” too small. Seems almost negligible, but that adds up to almost 1/16” on EACH side of the inlay - very noticeable!

PS: This may or may not be your issue, but from the bit angle you mentioned, it seems likely.

Your explanation makes perfect sense to me and I expect was a part of my troubles. Same experience/growth path. Started with a larger inlay piece at 60 degrees, worked great, move on to smaller and more detailed pieces that require a steeper angle and the wheels came off! In the process, tried a variety of different cutters and still couldn’t generate good results. I think your words described very well what I thought I saw–overcut on both the female and the male. So extending your ideas on how to potentially address plus a few more changes the last couple days and I think I’m pretty close to having a working solution.

I elected to give Vcarve Desktop a try in the middle of this too, and with the insight provided in your reply about the flat tip, feel like I’m nearly there and just a few more micro adjustments to depth will get me where I would like to be. Most recent test used the Amana 45611 15 degree, entered and selected as an engraving bit for the v-carve, and assuming there’s been some incremental wear to the tip made that parameter .008 instead of the .005 specified. Experimented with different tool paths selected from v-bits first, then as engraving and substantiated there is an incremental offset to the tool path when selecting a engraving bit with a specified flat tip. Tested a cut with female .25, start .22 plus .125 flat and achieved great fit along the sides. Didn’t end up with much of an actual glue gap, which could be too much clamping pressure [small piece, put it in the bench vise for expediency] along with small but acceptable errors in the cut. I’d frankly prefer not having much of a glue gap [I tend to believe that gap is for addressing minor cut/fit issues, not a space for glue], but would be concerned that if no actual gap remains there might be too much force from the inlay pushing against the sides and what that might do to a end grain cutting board in time. Thinking I’ll do another test at .30/.25+.125 and be more disciplined in the clamping. Attracted to the notion of a deep inlay for the cutting board.

Many thanks to you, Mitch and really all the posts I’ve read from so many people willing to share and help, as well as Will at C3D for patiently helping a relative newbie like me wearing him out with near daily questions!

Todd, what you said got me thinking that has lead to a recipe that works…I am not sure it is repeatable yet, but I got at least four predictable results. Rushing to work so will need to wait to post pictures.

The two things you said that unlocked it for me were maybe we are using it in ways that are unintended an that your experiments creep away from the offset. Add that my pockets and inlays (if you ignore tear out of the wood!) look good by themselves but just don’t fit together well. Also, I noticed from the sim (I did not cut) that not using “Enable Area Pocket Tool” lead to very different V bit cuts. I thought to myself, “Self, what if it was the interaction between the flat end mill and the V bit causing the issue? If I am already using the advanced VCarve in a way that was not intended, maybe there is another way to use it that was not intended to get the results I wanted?”

Short version: Create two offsets around the inlay design. One using your StL formula at flat depth (StL = Tan (1/2 included angle) * Flat Depth and one halt way between start depth and flat depth. Do advanced V carve between design and first offset. There is no room for the flat end mill so the V bit clears the entire space. Then pocket between perimeter (box around whole design) and second offset. The catch is sometimes my 1/8" does not get in all the corners. So sim, check for uncleared areas, delete enough points in first offset to clear but not so much the 1/8" gets used.

More to follow and some pictures…hopefully tonight.

Feels good when it starts to work, yes?! I had another good test over the weekend on the logo in plywood, 0.30 flat on the female and 0.25 start on the male with .375 on the male flat [having switched to Vcarve it’s spec’d 0.125 in that software]. Hydraulic press is a great way to get even pressure over the full inlay–my male piece was 10’x13’ minus just a little trim of excess around the perimeter. Still think ‘overcut’ is the best description of the problems I had before and Scott’s input regarding the flat portion when a v-bit doesn’t come to a sharp point explains a good deal of the issue. Vcarve software allowing an engraving bit that includes the flat spec gave me an easy solution. Pretty certain you can manipulate CC to get there as well either by creating offsets [which you’re doing] or doing the math to figure out how much your Z is off when measuring a bit with a small flat vs sharp point and making a manual adjustment after zeroing off.

I feel confident enough that I made the walnut end grain board which is now ready to carve, just waiting until I can get the hard maple glue up done for the male inlay, but office first now and won’t get back to that until the weekend.

This topic was automatically closed after 30 days. New replies are no longer allowed.