Another "inlay won't quite fit" thread - engraving bit

[aarvidsson]

I've got a Shapeoko 3 XL that I'm trying to do inlays with. I've been reasonably successful in the past using v-bits with larger angles (30 degrees and upwards), but I can't get this to work with engraving bits with smaller angles. The included CRV file has three test inlays - the bottom one is cut using the Amana 46280 6.2 degree engraving bit, the middle one using a Kyocera 30 degree v-bit and the top one using a Huhao 15 degree engraving bit (which turned out to be a 7,5 degree bit when I read the docs).

The Kyocera 30 degree bit is entered as a V-bit, the other two as engraving bits, using the information available at Amana and Huhao, respectively. The cut runs fine, but the male inlays cut with the engraving bits are simply too large for the pockets - they go in maybe half a millimeter, and that's pretty much it. The Kyocera V-bit slots in perfectly, leaving 1mm sticking out as expected.

I've used the "classic" v-carve inlay technique (male start depth = depth inside of the pocket, male flat depth = length of male sticking out) and for a 4mm deep pocket, I've gone for 3mm start depth and 1mm flat depth (with a slight twist as I don't want my tool to dive straight in, -> two toolpaths per male inlay: one with start depth 0 and flat depth 3, one with start depth 3 and flat depth 1).

Here are the details for the Amana bit: https://www.amanatool.com/46280-cnc-2d- ... r-bit.html

Here are the details for the Huhao bit (it is called 5487): https://www.aliexpress.com/item/3284489 ... 3222ufb3E1

I'm reasonably sure I'm doing something wrong, but I can't seem to figure out what. Can anyone help out...?

[Adrian]

The 46280 bit is a tapered ball nose bit not a engraving bit. Don't know if that's the problem as I'm pushed for time to investigate further but that's the first thing that struck me reading through your post.

[aarvidsson]

Oh yeah, forgot to mention that. That's quite correct, and trying to do inlays with VCarve set to tapered ball endmill gives an ... interesting result Having said that, I'm thinking that since the radius of the ball is 1/64th of an inch, the difference between an engraving bit and a ball end mill wouldn't be large enough to account for my issues?
I'm starting to think that the classic inlay technique might not work as expected below 30 degrees or so?

[adze_cnc]

trying to do inlays with VCarve set to tapered ball endmill gives an ... interesting result Having said that, I'm thinking that since the radius of the ball is 1/64th of an inch, the difference between an engraving bit and a ball end mill wouldn't be large enough to account for my issues?

It's like déjà vu all over again. Yes it can have an effect. See my reply at this thread: viewtopic.php?p=272222#p272222

and that thread's original poster's reply: viewtopic.php?p=272285#p272285

That "huhao" bit you specified is also a tapered ball end bit.

Remember:

• v-bits come to a sharp point and the angle entered is the entire included angle
• engraving bits have a flat instead of a point and the angle entered is the side angle (i.e. 1/2 the included angle)
• tapered ball end bits have a rounded tip and are not suitable for v-inlay work unless you lie to the software as I mentioned in my link above

Confusing these three and using them interchangeably without adjustment seems to account for many errors of fit.

[aarvidsson]

In that case, the question remains: how on earth does BroinWood manage to do Zank inlays with a tapered ball nose endmill? I thought using the numbers you gave me in the previous thread worked, but, alas, they don't.

[Adrian]

You're using a technique that was never thought of when the software was designed and a bit that isn't what you're telling the software it is so it's little wonder that it isn't a plug and play operation.

If one guy has worked out how to do it with that combination then it's just a matter of breaking down into logical steps and working from there. If the parts won't fit together then to me that would say you should start looking at increasing the size of the female part or decreasing the size of the male part.

Having re-visited the original thread and re-watched the videos I'm not so sure how you know exactly what he is doing. In his pinned post at the top of the "The Warrior" cutting board that you reference he makes no mention of using a tapered ball nose (although it does look like it in the video). You also have no way of knowing what software he's using (he mentions another that can create toolpaths as his main one in the same post) or what toolpath he is actually running at the time the tapered ball nose is loaded. You're making a lot of assumptions that he is doing nothing more than a v-inlay with a ball nose.

[aarvidsson]

Absolutely, I might be having the wrong assumptions. But looking at Stephan Forseilles ( ) he is using VCarve, the Zank method (with the normal calculations) and a ball-nose. From the videos it would seem he's entered the ball nose as a v-bit (the icon for the tool in the toolpath properties page to the right seem to indicate it is a V-bit as opposed to an engraving bit). This leads me to conclude it IS possible, I just can't seem to figure out how.

Decreasing the size of the male part would mean a start depth that is deeper than the "classic" calculations, and while I'm more than happy to try it, I can't see Stephan doing it that way.

[martin54]

15 degree engraving bit (which turned out to be a 7,5 degree bit when I read the docs)

Engraving bits are entered by side angle & v bits entered by included angle so an engraving bit with a 7.5 degree side angle would give a 15 degree included angle

Just a quick thought, how much does your machine affect your results? The steeper the angle the more things like bit deflection & how ridged the machine is come into play when fitting two parts together. Have you tried reducing your speed & feed settings or maybe running the finish bit toolpath a couple of times? Might not make any difference but it is definately something I would try. With things like this there is often a lot of experimenting to be done, as Adrian has said the whole process is something that was thought up by a user & not something the software was designed to do, over time others have refined changed or modified that process to fit better with what they are doing.

[aarvidsson]

I was juuust waiting for someone to point the 15 degree thing out Quite right; if it is entered as an engraving bit then it is 7,5 degrees, if it's entered as a V-bit, then it's 15 degrees. I'll be adding deflection/rigidity to the equation down the line for sure, but I'm thinking the machine will have to be pretty darn flexible to give me the results I'm seeing - especially as all the pocket cuts are correct.

[aarvidsson]

As I can't edit, I'll add another post: strike my previous comments. Stephan Forseilles IS using the ball nose as an engraving bit as per 11:33 in the video above. The ball nose in question he is using is this: https://www.aliexpress.com/item/33015343567.html (called the H18010602).

8mm deep pocket, 7mm (and 3mm flat depth) for the largest part of the inlay. This is both exciting and frustrating

[Adrian]

So then your issue is probably going to be your combination of start depths, cut depths and flat depths. I'd also look at the way you're using a clearing toolpath rather than a single male toolpath.

It's just a matter of stepping through the process and understanding what the software is doing at each stage and relating that back to the examples you have.

[adze_cnc]

Decreasing the size of the male part would mean a start depth that is deeper than the "classic" calculations, and while I'm more than happy to try it, I can't see Stephan doing it that way.

Perhaps you should contact him directly to find out what exactly he does?

Also, in the comments to the video he does specify the cutter he's using and why (it's more prosaic than you might expect).

[adze_cnc]

https://www.vectric.com/vectric-communi ... vingInlays

[aarvidsson]

I have, and I'm hoping he'll answer.

Are you referring to the comment about anything under 30 degrees has (or will have) a flat tip? If so, does it change the equation in some way I'm missing?

I've fiddled with it some more, and with a pocket depth of 8mm and a male part of 7mm/2mm flat depth, it does indeed go into the pocket. I would expect it to stick out 2mm but instead I'm looking at 3.5, so either the Zank math doesn't quite hold up at this angle, or something is off with my machine and I can't figure out what. I did a 4mm deep pocket and a 3/2 male piece that only barely entered the pocket.

[martin54]

I have, and I'm hoping he'll answer.

Are you referring to the comment about anything under 30 degrees has (or will have) a flat tip? If so, does it change the equation in some way I'm missing?

I've fiddled with it some more, and with a pocket depth of 8mm and a male part of 7mm/2mm flat depth, it does indeed go into the pocket. I would expect it to stick out 2mm but instead I'm looking at 3.5, so either the Zank math doesn't quite hold up at this angle, or something is off with my machine and I can't figure out what. I did a 4mm deep pocket and a 3/2 male piece that only barely entered the pocket.

Inlays are not something I really do & for the sort of work I do the inlay toolpath is all I need so can't really help with how best to set up & what sort of settings to use

However I would say you need to look at things like bit deflection & machine flex now rather than at some point down the line, as I said in the previous post the steeper the angle then the more noticable it will become. There is more than likely more flex in your machine than you realise, it's a hobby machine after all. Still capable of producing decent work but has obvious disadvantages over an industrial production machine