Just getting into Carbide Create, and I’ve got some funky lettering I’m trying to get correct in a piece of wood. The bit I’m using is a 3.175mm 60* vee bit, so I’ve entered 3.175mm and 30* (half) into the ‘edit library’ tools section.
Now, for some very small lettering, everything looks correct, with very sharp edges.
With this large, funky lettering (maybe 1/4" to 3/8" across at its thickest), Carbide Create does not cut all the way down and out. It goes down a few millimeters, and then etches the spidercracks out to the edges…and then never cuts further down. So now I’ve got skinny letters with some cuts out to the corners of each letter, and it looks goofy.
Stock thickness was at 25.4mm, I changed to 50.8mm and the ‘show simulation’ still made it look goofy.
If I use one of the stock tools (#301 or #302), it looks PERFECT in the simulation. If I swap back to my 1/8" bit, it looks goofy again (and doesn’t cut right).
Is this a configuration issue on my end (hopefully), or some sort of weird bug?
If the bit is narrow, it just can’t plunge deep enough to make it all the way to the edges. a v-carve is special in that it acheives width of cut with more plunge - there’s no way to acheive the “v” effect with multiple side-by-side cuts and the way it calculates paths. Just he way it is. So if the bit is more narrow than the width of the area that needs to be cut, there’s no way to make a cut that’s wider than that (if it plunges further than the width, it won’t get a wider cut than the width of the bit). It’ll try, and fail. This is part of the reason for why there are different angles of v-bits available - a shallow angle bit carves less deep for the same width, so you can use it on thin material.
You’re assuming its only making one pass, which it shouldn’t. It should make multiple passes. If the maximum diameter of the letter is greater than the diameter of the vbit, the vbit will have to make multiple passes on each side of the letter, then plunge further into the material.
Vectric Vcarve properly generates a toolpath (quite a few paths, given the small bit size), but it still works, and goes to the correct depth to generate a correct vcarve. Carbide Create doesn’t do this. Looks like a bug to me, as if it has a limit of not going any further than the diameter of the bit.
No. That’s not how v-carving works in carbide create. It’s not a bug, that’s the way it works in almost every app that can do this. F-engrave, fusion 360, mastercam all work this way.
Fiddling with the tools in CC, the 1/2" 60* vbit should work correctly (according to the simulation anyways). For $22 it’ll be easier to buy that vbit rather than find a workaround, or deal with the longer milling time.
Math.
I don’t use CC, but I’ve done similar in Fusion 360.
Knowing your desired depth, you could create a path offset the radius of your end mill at that depth. Create a contour on that path with your v-bit. Use a pocket to create the flat in between.
(Doesn’t keep me from complaining about it…my computer is better at math than me, so why isn’t it doing this for me?)
In Vectric VCarve you can set a flat depth, in Carbide Create you can not. The work around is as @neilferreri described. It’s not a bug, Carbide Create just doesn’t have a flat depth feature.
Edit: another way would be to use a wider tool. Depending on stock thickness and lettering size you might use a larger v bit with a shallower angle. @WillAdams used to have, and probably still does have a webpage that described best v bit angle versus lettering size.
Thanks for the links, as well as the work-around, I appreciate it!
I was hung up on getting it to work with the bit I have, when in reality, a larger diameter (but same angle) bit would work just the same on all the other features, AND work correctly on the larger lettering. Buying the larger bit is an easy fix, I should’ve thought about it more.