It seems that VCarve is a bit heavy handed. If I could halve the step over, I think I would get better results… but that does not appear to be an option.
Ideas?
Switching to a:
different bit
switching to a different program?
How fine a line is realistic? Is anything under 0.1" just to fine?
It looks like your bit is literally tearing chunks out of the wood. Is it dull?
60 degrees is almost certainly too fat for inlay work. I use either a 22 degree v-bit or a 5 degree TBN with a .5mm tip with a .25 or .125 clearing path. I’ve even gone down to .0625 (1/16") at times.
I ALWAYS use a pocket tool path to clear the plug portion down to the V-carve start depth as well.
Finally, if you use endgrain the fibers are running parallel to the cut, which help hold the plug cut in place.
So there’s a few things I’m seeing here, that might just not be the best piece of maple as its chipping out really bad, so in regards to the male piece of inlay I suspect too deep of passes when carving or dull bit.
A 60 Degree bit is absolutely fine depending on the settings you are using. I have gotten my finest details from a 60 bit as it allows to carve closer to the surface with a much larger base below for stability. I suggest you watch this video and pay careful attention to the “Zones” portion.
To also further the topic, I used a 60 degree in an experiment that further goes into the depth of passes when dealing with hardwood and V-Carv Inlays specifically for Wenge but the i utilize the zones as well you can see at the bottom of this thread Duplicating V-Carve toolpath
I have thought about using my: Bits&Bits 1/32″ Tapered Ball Nose – 12 Degree, but was afraid the cut would be to vertical … cutting down on glue area. I take it you have had no issues with the reduced glue surface?
But what is coming through loud and clear from both of you is: clearing path in multiple layers. Multiple layers is not because the machine can’t do it, but rather the material can’t support it. Also, do the clearing paths FIRST, so the VCarves removes as little as possible.
In my case it might make sense to pocket out the larger areas using a simple pocket routine, even before trying to do a vcarve.
tKC, If I understand correctly. you go through machinations to effectively get a “step down” out of your VCarve, i,e. 0.05 DOC first then another 0.05 DOC to get .1 DOC total
Which leads me to the question what are reasonable depths? The guy I was quoting had the female part at a depth of .3 a glue gap of .1. Seems you guys are doing less.
Thanks for your replies, I am obviously doing my best in interpeting your comments
I think the 3-2-1 is a good starting point, but .1" glue gap at the bottom is way more than you need and may eventually lead to the inlay weakening…sort of like a giant sinkhole under Florida.
I use a 5 degree TBN or a 22 degree Vbit. I have a pocket depth of .17.
For the plug I use a clearing pocket path of .1 then a Vcarve path wtih start depth of .1 and a flat depth of .09. That leaves me .02" at the bottom (give or take). It is roughly similar to what the artisan youtubers are using for endgrain boards.
Cool. One thing I’ve learned now that I’m trying to do inlays with multiple different layers is that I need to cut all the plugs first so that the machine zero doesn’t change for the female.
I sometimes carve the plug’s v-bit finish first then perform the clearing steps last. That usually reduces “chip out” thus making the male part cleaner.
I paid for Broinwood’s $140 ‘course’ on setting up the toolpath’s to do his inlay projects. It wasn’t much of a course, but rather just an explanation of his choice of tools and depths of cut. I think it was 100% worth the money to have the information. I, and anyone who buys it, should respect his request to not share the info, but I do recommend it as the canon/gospel of how to set up toolpaths for deep inlays. I don’t think a tiny/shallow inlay makes much difference.
This morning I ran this through a clearing path to remove the excess glue up and then through my drum sander at 80 grit. I didn’t even finish sand it. It was my first project since buying his info. I’ve never had an inlay turn out this perfectly.
I used white oak as the base and mahogany as the inlay. Looking back…the white oak isn’t a good substrate. I think the base needs to be really dark, or really light. This was a goldilocks color, and it doesn’t create enough of a contrast. Going forward I’m going to use maple, padauk or walnut for the board and save the oak/mahogany for the the accents.
Pwpacp, I can make arguments both ways on that one.
So proposing V bit first:
Pro:
you have the most supporting material … hopefully reducing top layer chip out
Con:
You are almost always taking a full bit width cut …the worst-case scenario for a bit, highest deflections, possibly bogging the machine down, highest heat load/tool wear
Now proposing clear cut first:
Pro:
The bit could see as little as half a tool bit width if the clearing path could get close enough
Con:
you may have no supporting material … going to a knife’s edge
My guess is in any given part both of these situations exist.
I really wish there was a “stepover” option on the V Carve. As in “kiss” off 0.005" off the profile in each pass. Sure I have just 2-10x the run time so my V Carve now takes 5 min instead of 1. But I don’t toss the work piece. tKC I believe is kinda suggesting this technique, but he comes at it from a vertical dimension approach.
I’ve learned a lot about inlays over the last year, and the ‘aha’ moment for was when I finally started working with endgrain boards. I suppose this should be obvious as the artisans all use endgrain. End grain boards hold details so much better than face or side grain boards. If you’re going to do an inlay that is more than a few inches or includes highly detailed then you should really consider using endgrain for the plug at least and you’ll probably get the best results with a pocket cut into endgrain as well.
I am not ignoring this thread; the actual project is for a cutting board for a nieces wedding in 3 days.
Taking the hints from this conversation, I actually made decent looking female/male pieces. Using the taper bit VCarve actually seemed to have a Z step down… I am guessing 2 or 3 in my case. This meant a LOT of finer detail was left behind. What also surprised me was the amount of residual material was left befind … slivers really, but they had to be removed. Removing those slivers meant I was at risk of slipping and removing detail I wanted.
I think in the future when it comes to the male pieces, I will try to make those is smaller chucks, instead of one big piece. That way if I mess up one, I make a small piece that takes less time than a big one.
Speaking of messing up, I did. Somehow, I had a male piece that was slightly oversize, and they did not mesh. I did a model rescale at one point and it appears I did not regen the toolpaths …yup assuming that one is on me.
So on to plan B, ordered the crushed turquoise and superglue from Amazon. A cherry board with a turquoise inlay should look nice. Finish will be clear shellac on inlay and board butter on the working face.
I have heard it said the difference between a master and a journeyman is how they fix mistakes.
growth rings: “They affect the density of the wood” … and hence the machining. Standing the material on end (like a bunch of straws) likely gives a more uniform material property. Think smaller gaps between changes in strength regions.
This also means that if you are machining inside a fast growth region between rings you are likely to see the material cleave off into strings or “tear out” rather produce a regular chip.
Just think about how poorly fast growth pine machines vs old growth.
This has provided insights more than just inlays, thank you
I think the reason endgrain holds details is simply because what’s left are long fibers anchored deep inside the workpiece. By working in end grain you are working with the growth of the wood rather than in opposition to it.
I use Easel & the way I cut my plugs is to rough cut them with Z zero start depth then cut them again with Z -2 or -3 or even -4 mm. & get good results, if I go too deep it is a simple matter to touch the faying surface to the belt sander with fine paper.
tKC, If I understand correctly. you go through machinations to effectively get a “step down” out of your VCarve, i,e. 0.05 DOC first then another 0.05 DOC to get .1 DOC total
For that particular project with Wenge yes I did, as if you haven’t had the pleasure of working with that wood yet it can be a real pain to work with and will break your bits without hesitation.
For other types of woods I just run the regular numbers you see in the Video I posted. I primarily do boxes that are of only 3/8 thick on face grain though (Similar to what you are doing on face grain) I saw @quesohusker using a .22 degree bit, I have one of those long fancy amana spektra bits and I agree they work really well for deeper inlays, and when i saw him mention the cutting boards that made perfect sense. As for the more shallow things I do I had too many problems with it leaving too thin of walls on the male plugs that were to brittle and would break easily.
I have found with V-Carve inlays there is no single right way to do it, it all depends on your particular application and you just need to play around with the settings and bits and find what works best for your usecase. When I’m in wood stores I always search the hobby/scrap bins for small scraps of walnut, sapele, cherry or maple for less than $5 so I always have small scraps around to test my inlays with before i commit to it on an expensive piece of stock.
