How to cut dovetails joints on your CNC

[BillK]

I’ve made a lot of boxes for people and myself. Some with box joints, most with dovetails, and some with special CNC designed joints. My go to have most recently been the dovetail joint, and I love cutting those by hand, but have done many with my CNC. I see a lot of the paradise design, which is a good box, but I see very little to none with dovetails on the CNC, so I thought it might be good to pass on some of my knowledge to you so when you’re tired of cutting signs and plaques (which make great box tops), you’ll be able to knock out a dovetail box quickly.
The biggest difference in hand cutting vs. CNC cutting is the aesthetics of the design. With hand cutting you can make small pins, much smaller than with CNC because the cutter size limits you. This is how you can usually tell if a dovetail was machine cut or hand cut.
I have not used the dovetail gadgets that you can find on the Vectric website or user produced gadgets, but some of the advice below will also be very useful with them. I like to layout my own. As a rule of thumb, I like to follow the old woodworker’s standards for building a box with dovetails. Board width of 2” or less gets one dovetail. 2” to 4” gets 2 dovetails, and 4-5 gets 3 dovetails. For box sides this gives you plenty of surface area for glue up, the dovetails look like a more prominent feature (vs. many small dovetails spread far apart) and are more than strong enough.

[BillK]

Design tails
In designing dovetail cuts in the software, the design must make its concessions to the tool used. In this case I’m using a dovetail bit with a 0.5” major diameter (biggest dia. at the bottom) and an 8-degree side angle (from the center of the tool to the side is 8 degrees) you can pick one up in HD or Lowes.
For a medium sized box, say 6” to 15” across the front, I like to use ½” thick material. It just looks less clunky than ¾” for this size. So those parameters are all you need to complete the design.
First thing to find out is what is the diameter of the dovetail bit at 0.5”(depth of cut) from the bottom? You can use trig, or you can just draw it in vectors to find out it is 0.359” and that is as close as you can get for your dovetail to dovetail spacing. I round up to 0.5” for my spacing.
First I layout three rectangles about 0.5” wide. The length needs to be the thickness of the wood (0.5”) plus a little more. This is so the dovetail bit can plunge to full depth when doing a pocket cut without cutting the sides of your workpiece where you don’t want it to.
That’s the layout and considerations. For cutting sequence first I will use the rectangles and a ¼” bit to clear out the waste material to full depth. Then I will use the dovetail bit, defined as an endmill with a 0.359” diameter, to make a full depth cut that will create the angled sides of the tails. Use a small stepover (0.06”) and an offset cutting strategy.
The other part of the design is board height. The best approach, if you can do it in your machine, is to cut both tail boards (I prefer they be the front and back board for a box) at the same time. So the height of my design board becomes one inch.

Design pins
You know from your tails how thick your pins will be from the narrow end. Using that geometry and the 8-degree angle, you can layout pockets to remove the waste for the pins. Nothing fancy here, you can use a ¼” endmill and you need to extend more than 0.25” past each face of the board to keep sharp edges. These must be cut one at a time. When you cut, you will flip the board top to bottom, keeping the left and right sides where they are. This necessitates you making another tool path where you flip the design from the first side over by mirroring it around the center of the ½” board. Make sure to add 0.005 offset to both tool paths so the dovetails fit together nicely, that would be a -0.005 entry to make sure you cut just outside the lines.

[BillK]

Fixturing
Take the variables out of your cut and make a solid fixture. Here is a picture of mine. Two pieces of aluminum extrusion with T-tracks, and one piece of aluminum angle. I attach the top part to the edge of my CNC table, indicate the front face parallel to the X-axis of my machine. Then I add the bottom extrusion leaving it loose for now, then add the aluminum angle. I use a square from the top extrusion to the angle and bolt that in place, it puts the bottom extrusion in the right place which I then tighten. So now I have a fixture parallel to my X axis and square to my CNC table. Don’t scrimp here.

Cutting


I cut the tails boards first. Two boards at a time. My design zeros in the lower left corner. For my most recent project, we wanted to go with the new antique look. I had some cherry that had a great patina on it, and I wanted to preserve that look. In this case I arranged the boards show face to show face. I try to avoid tear out at all costs, especially on the show faces, this is a great way to do it. Make sure you align the faces of the two boards that must be exactly equal in length. Snug the boards to your vertical surface. Raise the boards high enough so that you will clear the angle when cutting (more than 0.5” in this example). Now we are establishing the permanent sides of these board, mark the sides to the vertical angle as the bottom. That is an extremely important step. Clear out the waste with the ¼” endmill and your first TAP file , finish off with the dovetail bit and your second TAP file. Flip the two boards bottom to top, leaving left and right as is, and the two show faces touching, bottoms against the vertical. Cutting is done and you have the front and rear box boards.
Keeping the Zero point for X and Z, load one pin board. I designed this to use the same Y zero so the cuts are all in one file. If you have decided which is the front and back of the board, select the correct tap file so the pins will face the correct position for mating with the tails. I like to move my bit to 0,0,0 and slide my board up to it for zeroing Z. Again, mark the side touching the angle as bottom.
Flip the board, bottom to top again, and use the other pin tap file. Your pins on either end of the board must be angled the same way. Run the tool path. Load the last board and repeat.

Assembly

All your bottom marked board must be on the same side. You can interchange the front and back, and either side. Assemble with light soft-mallet taps. If everything was done correctly, all board tops and bottom will line up perfectly, if not, you switched top and bottom on one board, it may stick out proud of the other sides.
Unless your boards were perfectly milled, slight thickness variations will cause the pin or tail end to stick out slightly. You can sand that off to make a perfect looking joint, or do what I do and use a hand plane smoother to level them up. Of course, this is after glue up. I only apply glue to the pockets sides and bottoms on the pin boards.
At some point you will have to give thought to the box bottom. If you want it under the box, it can be glued on, with or without pin nailing. If you want to put it inside the box, you will need to mill slots for it in all four sides before assembly. Not through slots, they will show on the outside, slots that are about 0.5” shorter than the side length.
Add hinges to it with your top and you’re done.
Hope that helps someone, some day.

[IslaWW]

Nice job Bill...
Back in the day we had to hand code if we wanted to cut dovetails. This one copies the half blind version that you get off numerous commercial jigs:

[BillK]

Thanks! I have one of those jigs, it was just limited to the half blind style. I probably only used it once.

[4DThinker]

Nice post Bill. As a furniture design instructor I occasionally get a request for dovetails to be CNC cut. In this blog post there are half blind mitered dovetails that I figure out how to cut after a student showed me a non-CNC example he found on the web. You can also see pseudo dovetails done with a small endmill and the tail board laying flat. Lastly an open sample on some 2x4 material I did as a test for framing a tiny house with CNC joinery rather than nails or screws. Not much is impossible if you can clamp boards vertically or at an angle under the spindle.
https://4dfurniture.blogspot.com/2016/0 ... c-cut.html
4D

[scottp55]

Nice Bill!!

Interested in watching 4D's link, as I can't cut vertically like Desktops can do now
(even a Shopbot factory jig for it) .

(Thank goodness for Tailmaker and Fingermaker when I get back into it.)
scott

[BillK]

Thanks 4D and Scott. Its really important to share the how to’s with people on the forum. A lot of people buy these hobby CNC’s and get frustrated trying to figure out other tasks they can use them for. Hopefully Vectric might realize people are using machines and their software like this and start to include dovetail bits and a machining preview for this type of cut.