A simple way to make inlays

[tmerrill]

Two other issues that can create gaps on one side or area only can be if your machine isn't cutting accurately in both X and Y directions OR your router/spindle isn't exactly perpendicular to the table top.

To check X and Y accuracy you can cut some simple shapes in hardwood, or better yet, corian and measure them with a quality dial indicator. For example, your circles should be perfectly round and not oval. Squares should have the same dimensions across the sides and on the diagonals. I use scrap corian for this because you don't have any issues with grain deflection on the bit.

If your router/spindle isn't exactly perpendicular to the table top, it will be cutting with a smaller angle in one direction and a larger angle in the other.

Tim

[Paul Z]

Taylor,

Sorry it took so long for me to look at this.

You have a start depth of 0.05" for the inlay. That's how much of the inlay will actually fit into the pocket. The inlay may fit but it will be difficult to get it lined up just right. There will be no tactile feedback until the rotational alignment is almost perfect and horizontal alignment is within 50 thousandths. That is pretty difficult. With larger start depths, it is much easier to line things up and get tactile feedback when they fall in place. If you want to make thin inlays using this method, I'd recommend cutting some registration holes along the edge as part of the inlay process.

I'd suggest that you cut out one of the wavy pieces leaving a significant amount of the inlay backing all around the piece. Try fitting just that into the pocket. If you are careful when you cut out the wavy piece, it can serve as a guide for placing the rest of the inlay. Straight pencil lines put on the inlay before cutting out one of the "wavies" would also help in registration of the pieces.

It is diffucult to a visual check because the mating part of the pocket and inlay are part way down the side of the inlay piece. I have had some inlays that I was sure that they would not fit, only to have them slide in place and come out extremely well.

By the way, cutting the inlay into multiple pieces can be very helpful. Suppose that one cuts two pockets and two inlays out of two different materials. If the inlays are cut into pieces, the mix and match possibilities are almost endless.

Paul Z

[SparksStudios]

Paul,
I went back and tried again, this time using the numbers in the doc. just as they were. Got the two halfs to go together enough to glue. I'm using a 60 deg. bit, which to me just doesn't seem to give very much overlap between the top and bottom halfs for the depth that you have to cut the paths. I wonder if a 90 deg. would give greater overlap without stressing the machine to go for those deep single-pass paths?

Anyway, here's my results after two tries. It's Walnut on Cherry, finished off with some Teak Oil I had laying around.

Taylor

[rodon]

Thanks so much for this thread. Just found it a couple days ago. Man does it work awesome! These are my first two inlays ever! These signs will be donated and auctioned off for St. Jude this weekend. Maple in walnut. Thanks again for the info!

[Paul Z]

Very nicely done. Someone will be very happy with them.

[danr]

here is a way to avoid deep single pass cuts when using the v inlay method. Also useful for making thin inlays with very small tools. When V cutting the female pocket there is no issue, simply make the top surface the start depth and choose your flat depth as desired for the engagement you want with the inlay. It is v cutting the inlay side that is problematic because the start depth is below the material surface by an amount that you may be reluctant to cut.
In my case I must use very small tools. I have a high speed spindle that I use with 1/8" tools.

Here is the procedure that I use to avoid having to make deep cuts. If you visualize the vbit placed at the start depth
it will clear all the material above it that lies within the cone of the cutter. The problem is that the physical extent of the cutter may not reach from the start depth up to the material surface. In this case, by visualizing the cutter moving through the material it is clear that offsetting the inlay vector by an easily computable amount makes the vector "slide" up the cone of the cutter to the top surface (or any other depth you desire.) The amount to offset is related to the geometry of the vbit. When using a 90 deg bit raising the shape a tenth of an inch you would offset the curve inward by a tenth of an inch. In general the amount to offset is equal to the amount raised * tan(vbit angle).
Here, the vbit angle is the angle between the cone axis and the cone surface. A 90 deg vbit has a 45 deg angle, etc.

This procedure is used in V-Carve pro to cut the inlay in several steps.
I typically make a new layer, offset the original geometry and then cut this using a vcarve path that goes from the top surface to the actual desired start depth. I also use a flat area clearance tool at this step. In effect, I have created a roughing tool path that removes the material above the start depth that would be removed if the cutter was much taller.

After this toolpath I genertae a normal toolpath using the correct start depth and flat depth.

At the end I reorder all the flat area clearance paths as these will be cut by the same end mill. This leaves the material with a scalloped look to it that the vbit bevels with no problem.


One interesting aspect of this method is that when "projecting" small features up to the top surface they may disappear. This is correct, as small features don't have much height with usual vbit angles. On the other hand, if you create geometry on the top surface and cut too deeply below the surface (a "greedy" flat depth) you may remove material with the clearance tool that should be there. It is as if you are cutting off the tops of the peaks.
As the intended contact between the inlay and pocket is along the beveled sides this shouldn't be a big problem. I have used this technique even for geometry whose offset curves bears little or no resemblence to the original shape.
Again, the geometry gets thinner as you project upward and a lot of it can disappear.

I find the inlays that can be created by the v inlay technique are astonishing. Anyway, I wanted to share my tweak on this method.

[Paul Z]

Danr

Thanks for posting your procedure. I think I understand it but diagrams or pictures would help a lot (and might get others to use it).

I'd love to see some of your results if possible.

Paul Z

[danr]

Hi Paul Z

I'll post some pictures and more documentation to try to clarify my procedure.

Dan R

[danr]

I will try to explain how I cut inlays using multiple passes to cut the male inlay. Attached are three picture of inlays I cut using this method: a tulip, a seahorse, and a geometric design. The file inlayexp1.pdf contains a picture of how the inlay would be cut in one pass using Paul Z's method. In my case my tools are too small to do this in one pass so I cut these inlays in two passes. The female pocket side is not an issue since Vcarve Pro will cut the pocket in multiple passes already by setting up the tool properties.

For these inlays I am using a 1/8 engraving vbit. It has an included angle of 30 degrees and a 0.005" flat. I use 40000
and 60 ipm when cutting, plunge is at 10 ipm. I restrict the tool to 0.075 per pass, which is still pushing the tool pretty hard. I'm inlaying colored Corian into white Corian. The final inlays are really breathtaking, they don't look inlayed at all,in fact some people don't believe they are inlays. They think I chemically etched the Corian somehow.

Now, when cutting the female side there is no problem because the geometry lives on the top surface. Vcarve Pro can correctly cut below the surface in multiple passes. The top surface is what I called the waterline in the file. For these inlays I cut the pocket 0.15 inches, and I want a gap of 0.05 inches at the bottom of the pocket and at the top also. This leaves 0.1 inches of beveled contact area which is plenty strong enough for Corian. When I cut the male inlay the picture becomes flipped: the waterline is now 0.1 inches below the surface of the male pieces. If I simply tell Vcarve a start depth of 0.1 inches and a flat depth of 0.05 inches it will cut the male piece in one pass. The problem is that there is no geometry layer at the top surface which would let me start there and cut down. I use the vector offset function to create a new geometry layer using these steps. Please look at the file inlayexp2 to see a picture . Since my total depth is 0.15 inches I decided to do this in two passes. I will create a geometry layer 0.05 inches below the surface and cut this to a depth of 0.075. I do this by using start depth = 0.05 and flat depth = 0.025 In VcarePro I selct the actual geometry and then clcik on vector offset. I offset the curves 0.0134 inches inward.
This number is calculated from the fact that I am moving the realo waterline up by 0.05 inches and the vbit has a 15 angle. 0.05 * tan(15) gives 0.0134. I make sure that I have a new layer created (I call it offset layer) to gather all the offset curves together. Otherwise things become a mess to look at.

After creating the geometry I cut the inlay in two passes.

First pass (using the fake waterline) has start depth 0.05 and flat depth 0.025. Here I use an end mill as a flat area clearance tool. After this pass I have effectively removed the top of the material but all the bevels have been retained. They are finsihed by the second pass

Second pass uses the real waterline. Start depth = 0.1 flat depth is 0.05

Notice that each pass removes half the material.

The choice of where to place the fake waterline has a lot of freedom as long as it is done correctly. For this pass you can trade off start depth vs flat depth but I have achieved good results by creating two very balanced passes.

Note that when you offset the curves from the real waterline a lot of geometry can disappear, so the fake waterline may not look much like the real waterline. This would also be true if you could cut the whole thing with a taller tool. The real issue is not to make the flat depth too much below the start depth for the first pass because you don't want to remove materail that should be left. For my inlays I have obtained "perfect" contact between my pieces so the issue may not be too fussy.

Please let me know if this explanation is helpful.

dan R

[Paul Z]

Thanks for the explanation with diagrams. I can see how this dramatically reduces the forces while cutting and will result in a better fit.

The results are superb!!!

[danr]

I'm getting addicted to making these inlays! Thanks for sharing the method.
Even when I look at the inlays with a magnifying glass there is no visible gap or glue line.
I'm going to try some inlays with several colors to see how the method holds up. I'm predicting great results.
Corian seems to machine superbly with these engraving bits.

Dan R

[danr]

here's an example that was inlaid with three different colors: black, red and blue inlaid into white. Material is Corian. The piece is 3.5" x 3.5". The small features are amazing. This is a Grateful Dead logo for all Dead Heads out there.
(Like my wife!)


Danr

[Greolt]

Great corian inlays.

May I ask what glue you use?

Greg

[danr]

I use Zap-A-Gap. It's medium gap filling CA. It gives a little bit of time to mate the inlay before it sets. Available at all model and hobby shops.

[Greolt]

Thanks for that Danr.

I have been using epoxy and find that because it is quite viscous I end up using a lot of it to make sure all areas of contact are covered. Miss a tiny bit and it will chip out when machining the top off.

I will get some Zap and give it a try.

Greg