Inlays with Estlcam?

Hello, I’m experimenting with inlays. I’m able to cut a good looking pocket and parts, but they don’t quite fit together.
I’m using a 1/8" flat mill, 5mm deep for both the pocket and parts.
It seems like the inlay “part” would be better if it were beveled slightly such that it’s a tiny bit narrower on the portion that goes into the pocket and wider near its base. Is it possible to make a cut beveled like this or could I maybe change my bit radius in the configuration to be just a bit smaller for the pocket cut so that the pocket comes out just a bit larger - allowing the part to fit better?

In general, is Estlcam a good tool for doing inlays?

Thank you.

I don’t think EstlCAM is bad or good at inlays. Do other CAM software packages have special inlay features?

EstlCAM couldn’t cut the bottom smaller, unless you cut it upside down. Then it could cut the top smaller. To do that, you’d need an STL of the inlay.

To increase the tolerances, you can change the bit size. If you make the size in EstlCAM smaller, then it will cut closer, which will increase the tolerances.

Is it just not fitting because the pieces are too big? Are both cuts square?

Also, is the inlay complicated? Can you just use some sandpaper or a sharp chisel to get it to fit? Somewhere I heard that the difference between good and great woodworkers is their ability to fix their mistakes. If you’re just making one, I would do that. If you have a lot to make, then I’d change the bit size in EstlCAM to be smaller, and fill the gap with epoxy and sawdust.

Can you share some pictures? I am going to be doing some inlays as soon as I get some shop time.

What tolerances are you using and how deep are your inlays?

Inlays are typically very shallow because getting a good fit is hard enough but the deeper it is the issue is multiplied. Some Old Guy Coding has an inlay vid and the veneer is very thin and flexible, that is what you should be using. The more complicated the thinner is needs to be. Some hand sanding is probably always going to be needed for a really nice fit.

Also I am assuming you are using the same path for the pocket and the inlay. It is best to give yourself an offset path, you need room for glue, and for machining variances.

I can’t wait to see how it comes out.

I want to use the deep inlays, not the veneer type. There are other folks using other CNC equipment doing it this way on youtube. Even when SOGC uses the laser cut veneer, it looks like there is a slight line/gap around the finished product.

I’ve tried a few things and this is what I have so far (see pics). I used the same E10 file for pocket and inlay with the following exceptions: the inlay is reversed w.r.t the pocket, the inlay uses a -0.17mm finishing allowance on the outside parts of the letters and a +0.17mm tolerance on the inside of the letters (I mean the holes in the A and D). The negative allowance cuts the piece just a bit smaller. For the holes, I used a positive value because I wanted them just a bit bigger. The depth of cut was 5mm for both pieces.

The experiment used white wood for the inlay and MDF for the pocket. I wouldn’t ordinarily use MDF for this, but it was handy and flat. All four letters were glued in at the same time and clamped overnight. Next I ran a 3/4" flat bit over the letters to cut away the top layer revealing the inlay. There are some gaps.

If I could find a way to make only the top of the inlay (the portion that contacts the bottom of the pocket) smaller, then I might get a tighter fit at the expense of the inlay not reaching all the way to the bottom of the cut.
It would be shaped sort of like this:
\ ----
/ ----
The inlay would be like a wedge shape.

I’ll continue experimenting.

Those are actually pretty close, nice work.

To put a draft on your parts the easy way would be to only draft one side and do one flat but you can get 1-3 degree draft bits. These are very common it is how they make molds.

You say you are leaving a tolerance but are you actually doing a finish pass? If you are using the finish pass tolerance to leave your tolerance you are still just rough cutting the shape. It really would be best to use an offset path and use a proper finishing pass and I think you could easily get this real tight. At least I hope so I have 9.5mm “inlay” type joint I am itching to finish.

The good news is once you figure out what offset works best you should be able to use it for most projects and materials, or it will always at least give you a great ballpark starting number.

Thanks for the tips, but you speak as if I know what I’m doing :slight_smile:

What is a draft/draft bit?

I’m using the “finishing allowance” box with no finishing tool selected. Does that mean it’s not doing a finishing pass? The context help isn’t exactly clear - it says if you choose a finishing tool, it will do a roughing and finishing pass. If you don’t choose a finishing tool, what then?

Is there a video explaining more about the finishing pass? I assume its a more accurate pass, but what does the “finishing allowance” do if a finishing tool is selected? The context menu is clear that if you don’t select a finishing tool, then “finishing allowance” will make the cut smaller or bigger. Otherwise it defines the machining allowance for the roughing pass. But what does that mean?

This video shows what I am trying to achieve. Not as elaborate, but the same technique except using Estlcam and mpcnc.

It has a 2 degree (or whatever) taper too it to cut slightly tapered walls. I still don reccomend doing it this way but you asked so this is how it is done.

Correct, you need to select a tool. I just use the same tool I am already using so you don’t have to figure out how to do a tool change. If you don’t select a finishing tool then you do it the way my intermediate walk through shows it an make a second tool path. It is much easier now.

A finishing pass is one where the tool is cutting a much lighter load giving a drastically improved tolerance. so if you pocket with a 45% stepover 45% of the tool is under load and the tool flexes, the spindle runnout, mount flexes, gantry flexes, legs flex, etc. Then you come to do your finishing pass and it only loads the bit with a 2-5% load, at this point the entire system is under a much lighter load and flexes much less resulting in higher accuracy cuts. When I say flex it sounds drastic, but it is tenths of a mm, but you can see in your inlay cuts it matters.

I still stick to my original suggestion, an offset path Determined by trial and error on a small inlay test piece, using .4mm or less (depending on wood density) finishing passes.

Just to keep this clear for anyone reading this. Finish passes are always recommended. Not just for inlays.

Ryan, this has been very helpful. Just one more thing …
[blockquote]I still stick to my original suggestion, an offset path Determined by trial and error on a small inlay test piece, using .4mm or less (depending on wood density) finishing passes.[/blockquote]

How do I make an offset path? That is what I thought I was doing by setting finishing allowance but no finishing tool. You are suggesting using a finishing pass, so that would seem to eliminate my method of creating an offset path.

Let’s say I wanted a square inlay. I think you are suggesting creating a hole (part) 1" x 1" and an inlay piece that is .99" x .99". For the inlay, I create a stl that has a 1"x1" square, bring it into Estlcam, then what? how do I shrink it down or rather make the cutting path shrink?

No, using whatever program you created the 1"x1" square, also great a square with a slight offset. This is extremely common in all CAD programs even illustrator, vector programs.

Estlcam should just be used to create your toolpaths, repetier or an LCD to deliver than code and a separate program to create your object. It is best to keep them separate for now. They all have some crossover but seem to work so much better when they only do one function.

Fusion is a bit of a standout but it is many times more difficult to do CAM with than ESTLCAM. Had to put this line in before someone felt the need to correct me.

Sorry, I somehow didn’t subscribe to this. But it looks like Ryan has it under control. Just to explain more about what he’s saying, if you made the original “SAND” word in some CAD or drawing program, you would add an offset to the letters, so that they would be wider and the holes would be smaller. In the 1"x1" square example, the original was 25.4mmx25.4mm and the offset version would be 26.2x26.2mm (25.4 + 0.4mm per side) and the corners would end up with a 0.4mm roundover. It’s annoying to do by hand, but like Ryan said, most programs have some function where you can select the letters, and just hit “offset”. Make sure you actually do the offset, and you don’t just scale the text. Scaling it will make the inside of the hole tighter, instead of looser.

Those taper bits are neat.

You might also want to break up the inlay before inserting it. That way each letter can distribute it’s own gaps as evenly as possible.

You also need to make sure your machine is very square. Otherwise, it’s like fitting a parallelogram into a square hole.

1 Like

Jeff, thanks for the tips. Are you suggesting that the inlay should be larger than the hole? I was doing the exact opposite.
I’ve found an offset function in inkscape. I will try it out.

You’d make the inlay smaller, so it fits easier.

It’s my understanding that if you use a V-Bit for deeper work, that will help compensate for some of the problems you have talked about as well on deeper inlay work.