Deep v-carving and start depth problem

[sfo2406]

Hello. I've been trying for a long time to make deeper inlays (around 10mm) in end-grain cutting boards. I know the "documented technique": pocket = start depth 0, flat depth 10; plug = start depth 10 (or less if glue space), flat depth = clearance for the bandsaw.

That works well for shallop inlays (a couple mm), but for dapper ones, the problem is the start depth of the plug: the bit will directly plunge at start depth + pass depth (for me that's a total of around 12mm). For my X-Carve-like CNC, that's way too much. The cringe!

I've started trying 'foolingl' VCarve by creating 'pre-passes' but the fit isn't super good. So I've reverted to trigonometry and I made a calculation model for an offset to give to each closed vector based on contact and clearance depths (see below). This seems to work relatively well as long as carved areas aren't too thin.

I was wondering if anyone else was struggling with that "Start Depth" problem and found an elegant solution to it.

[sfo2406]

A test with that technique, carving 10mm (around 1/3rd IN, is that a thing? )

[TReischl]

You cannot control that by setting a shallower depth of cut?

[sfo2406]

Nope, unfortunately it will directly plunge to the Start Depth + depth of cut.

[Adrian]

Will your design only work with that technique or could you use the built-in inlay toolpaths instead?

There's no way around the start depth issue as it's not really being used in the way that it was designed for. There's not supposed to be any material present when a start depth is used.

[FixitMike]

You can reduce the depth of tool cut by starting with a toolpath with no start depth, then repeat with a start depth.

[laflippin]

Hi Mike, I have experienced exactly the same problem with various of my Zank Inlay projects. Eventually, I settled on a female V-carve depth of 0.2" and for the corresponding male carving, start depth = 0.15" and flat depth = 0.1". That may leave a slightly larger glue-gap (0.05") than necessary, but it generally gives me good results so I've kept that without thinking too much more about it. The real problem, of course, is V-carving the male piece: 0.15" + 0.1" = 0.25" single-pass depth with a 60 deg V-bit. Some woods, like walnut and maple, seem to tolerate it better than others but chipping is a really serious problem for finely detailed, fragile male carvings. The only solution that I've found to make any difference in the outcome is to slow the feed rate. Whereas the default value on my machine is 100 ipm for everything, I now use a feed rate of 40 or 50 ipm for Zank Inlay male V-carvings and that gives much cleaner results with all the woods I have tried in my limited experience.

[sfo2406]

@Adrian: as far as I know the built-in inlay toolpaths are meant to work with straight bits and an offset so you don't need all that maths but you'll never get such a good fit. That's why so many people try to make V-carved inlays.

In terms of feeds and speed, I use a (very good) 6mm shank 7,6° V-Bit (ball-nosed but I'm waiting for a really pointy 15° to be delivered) with 3mm passes at 800 to 1200mm/min (around 50ipm). I think anything above 15° is probably too shallow to make anything solid. As I do everything at Start Depth 0, I don't have the problem of the "adding depths" for the first pass.

@FixitMike: I've tried making those 'pre-real-carve' toolpaths to trick Vcarve into not plunging directly to the start depth but I've never managed to get a really good fit that way.

Here's one I'v made this weekend:



Full video (2min): https://www.youtube.com/watch?v=sZJmFp3j__c

[Adrian]

Personally I use the built-in inlay toolpath all the time and get great results. Some of the inlay projects I've seen with really sharp detail can't be done that way as the size of the tool precludes it. For lettering and shapes I have no issues with it.