I have created a V Carve inlay, run it in MDF as a test, and all looks good. The female finish side has already been run in maple and came out beautifully. The male finish side was done in black walnut and did not turn out so good.
I uploaded a “simulation” picture showing “some” of the areas I am having problems with. By the way my design work is done in Vectric V Carve Pro. I could upload the actual file if anyone wanted to look at it.
The problem I’m running into is chip or tear out. I don’t know if that due to the tool settings (bladed 60 Degree V bit), the spindle speed (18,000 RPM) or size of the letters.
I’m wondering if anyone has any experience with this and can help.
@Trying_to_learn I don’t use vectric to v carve and I settled on an Amana 30° V bit. That’s said, hopefully some of this will still help. The things I changed for the inlay/male are to do the v bit first, change the feeds n speeds, and re-run the v pass again at the end.
Doing the V first leaves more support material to reduce tear out. The higher rpm (20k) and lower (40) IPM reduces it too.
Using a final V pass cleanup at depth is more about getting rid of the fuzzies to make cleanup easier.
It could be the specific piece of walnut you’re using. Sometimes the fibers are a little wispy to cut so I contour everything lightly first with the v bit to sever the grain at the surface while it has some support. Then I rough cut and finish pass, this helps with tearout. (Have to do a bit of trig here too find the right path for the bit for a male inlay).
The spindle speed looks a little low, but that could be my perception, I only make .060 passes or lower when doing an inlay when roughing - keep in mind on the v bit the diameter is changing smaller toward the tip so more rpm will keep the chip load in a more ideal spot.
I also have a replaceable carbide v-bit I found on Amazon, currently showing out of stock. I use this because I can change carbides when they wear out and keep the tool ultra sharp.
My guess here is that the 60 degree bit is still too wide, and as it goes deeper into the material, your Start and Flat depth settings are causing the sides of the bit to start knocking off the tops (or bottom however you look at it) of real small detailed tool paths.
I found for detailed carvings, a 15 degree bit having a 0.127mm sized tip works great as long as I don’t go deeper (start + flat depth) than 4.0mm total, and the minimum width of line is at least 1.0mm. If I do go over this depth, the sides of my 15d bit start knocking down the tops and sides of the wood.
Some suggestions:
Going down from your current 60d bit, start using smaller angles until you find one that works
For male inlays, I found carving the V-Bit path first, then do the clearing path, can help prevent blowouts as there is more material on either side of the bit as it’s cutting.
Go into node editing mode of Vectric and start adjusting those small points into something your 60d bit can handle
I’m currently trying to figure this out as well. I’ve ran two pieces so far and with mixed results. I’ve use the same bit as well. I bought a couple other bits I need to try, one being solid carbide 60 degree and another being a 3.6 degree spiral ball nose. I can’t seem to get the spiral ball nose to even get me a descent looking model in Aspire Vectric so far. I’m still fairly new to the software, so hopefully it will get easier as I progress. Cheers.
Forrest: I know nothing about the node editing mode you mention. I will have to look into that. I do have a 30 and 15 degree V bit. I could try cutting it with one of those, however, I have already carved the female side with the 60 degree. I suppose I could cut that again as well, but I’d have to make sure that my axis points were exactly the same as the first time I ran the cut and that makes me a bit nervous.
