Inlay Pass Depth Problem

[CAGreen]

In trying to learn how to do inlays I have run across a problem cutting the plug that I can't seem to solve. I have tried using .1 start and .1 flat settings and I am finding that the deeper I set the start depth the deeper the first pass ends up being. The depth is so deep that I am getting tear out that ruins the plug. (for example parts of the inlay are missing). I have also tried using .18 start and .08 flat. The tool dives even deeper and not only overloads the tool but nearly destroys the plug. I have been using a 60-degree carbide v bit at many different speeds and feeds and I have not been able to make this work. My question is does the vcarve toolpath have a setting someplace that will create multiple passes at lesser depths? I have noticed that the toolpath seems to have a .40 cleanup pass at the end which may help if I limit the start and flat depths. The problem is if I do that the plug will not fit properly.
Material is Box store Maple.

[adze_cnc]

From the balance of your post I intuit that you are asking about tapered inlays (a.k.a. v-carve inlays, v-inlays, Zank inlays) rather than the straight-sided inlays made with the built-in Inlay toolpath. Tapered inlays are a technique developed by Paul Zank at this thread: viewtopic.php?f=3&t=564 and detailed in the PDF file in the first post.

A recent similar question to yours has spawned a currently 4 page thread elsewhere that I'll refrain from linking to.

Your observations are indeed correct. Because the tapered inlay process is using the "V-Carve / Engraving" toolpath in a manner that it was not developed for certain side effects are inevitable. By setting the starting depth to other than zero VCarve can only presume, and rightly so, that you have made provision to eliminate all the material above the starting depth.

My question is does the vcarve toolpath have a setting someplace that will create multiple passes at lesser depths?

There are two ways to solve this:

1. manually create "V-Carve / Engraving" toolpaths to eliminate the material above your starting depth (see this link for more info: viewtopic.php?p=264755#p264755 )
2. use the "Easy Zank Toolpath Maker" by jimandi5000 found here: viewtopic.php?f=51&t=38177

Looking at the manual option for your initial example of start depth = 0.1 and flat depth = 0.1 you could create two "V-Carve / Engrave" toolpaths with the following parameters:

1. start depth = 0.0; flat depth = 0.1
2. start depth = 0.1; flat depth = 0.1

The first toolpath eliminates the material for VCarve so that the second toolpath (your desired inlay toolpath) can cut with less stress on the machine/cutter.

At my suggestion, Jim created his gadget to automate the manual method. This is especially userful if you are doing very thick inlays that need multiple toolpaths to clear material above the final toolpath.

A discussion of the settings involved in the inlay and pocket pieces that tend to confuse people might be of use to you. The settings really aren't that complex (inches presumed substitute millimetres as desired). In the examples for the inlay and pocket I'll use your start depth = 0.18; flat depth = 0.08 that you mentioned as one of your attempts:

Pocket (a.k.a. base, female)

• start depth: almost always zero (0)
• flat depth: the amount of inlay material you want in the pocket plus the amount of glue squeeze-out space you want

For your example we need a minimum of 0.18 as the flat depth although that would have no space for excess glue. So, we might instead choose a flat depth = 0.20 (0.18 for the inlay material and 0.02 for the glue).

Inlay (a.k.a. plug, male)

• start depth: amount of inlay material you want in the pocket (see pocket flat depth above)
• flat depth: amount of space you want between the plug piece and the pocket piece so that you can, perhaps, slip a bandsaw blade to cut things apart (or so that the two pieces don't jam together)

For your example: start depth = 0.18; flat depth = 0.08.

FixitMike has a good image explaining things here: viewtopic.php?p=202721#p202721

Three other things about tapered inlays that are useful to keep in mind:

1. use the same angle v-bit for both the pocket and inlay pieces, For some reason people think they can use, say, a 90 degree for one and a 60 degree for another but I think it's obvious the two cut pieces can't possible mate flat
2. when specifying a v-bit in the tool database we use the included (full angle) of the bit. When specifying an engraving bit (v shape with a flat bottom) we specify the side angle (i.e. the angle from the vertical).
3. the vectors for the pocket and the plug should not be altered in any way except to mirror the pocket vectors so that they can be used with the plug toolpaths.

I hope this is of some use,
Steven

[laflippin]

Steven,

It was a pleasure to read that very lucid summary.

I think you nailed it from A(ngle) to Z(ank).

[rink]

Good afternoon everyone.
Steven has provided an excellent outline of the process with links to more detailed info, like the gadget, the FixitMike diagram, etc. It should be a permanent post, like the ones pinned at the top of each forum.

And…there are so many questions and discussions specific to the “v-carve” or “Zank” inlay process, seems like it could warrant it’s own sub-forum.

Thx, rink.

[adze_cnc]

CAGreen:

While enjoying a coffee at my most favourite coffee shop this morning I decided that I don't like the term "pocket" for the material that a tapered inlay will be placed into. I think that "base" is a better term. Pocket carries an implication that a "Pocket" toolpath is somehow used in its creation but the entirety of the tapered inlay method is accomplished using the "V-Carve / Inlay" toolpath.

I also reject "male" and "female" as being archaic terms leading to the kind of sniggers you get when referring to certain plumbing fixtures as nipples.

Attached is a sample tapered inlay using some crab vectors found on one of the pages of this original Paul Zank post: viewtopic.php?f=3&t=564

The "crab inlay.crv" file demonstrates the manual creation of toolpaths (I call pre-score) to elminate material above the final (true) tapered inlay toolpath. Pre-score 1" cuts from 0 to 0,0625; pre-score 2 cuts from 0.0625 to 0.125. The true toolpath cuts from 0.125 to 0.250.

The "crab base.crv" file is your basic "base" file. The original material was 12mm Baltic birch plywood hence the "material fibre scoring" toolpath using a down-cut bit to prevent splintering.

For each file the toolpaths will need to be recalculated. By not having the toolpaths calculated mean the files are 2.6 megabytes smaller.

Steven

[laflippin]

Re: “ I also reject "male" and "female" as being archaic terms leading to the kind of sniggers you get when referring to certain plumbing fixtures as nipples.”

I’m not trying to divert the conversation from other more important issues but I will say this about the “male” and “female” jargon—sniggering and giggling aside, everyone intuitively knows what these words mean in the current context. Since it is pretty nearly impossible to misunderstand them, I’d vote to keep them.

However, I can’t offer a coherent opinion about plumbing nipples.