In this video we will demonstrate practical CNC wood joinery (practical meaning that there will be no need for special jigs).

The material will be 3/4" sheet stock and the parts will be milled using a 3 axis CNC machine (Our greenBull).

We will start with a simple joint, a finger joint. This joint - as it's name implies - is a joint that exhibits protrusions that measure the thickness of the wood, so that when put together, the corner is flush.

Both pieces of wood will have these protrusions offset from each other so they both marry correctly. The aim is to make the fingers sized so that they are snug, but may allow some wood glue to be added to secure it permanently.

The finger joint will not lock together unless the joint is very tight, but even with a tight fit, the joint (without glue) is not permanent. AutoCAD was used to design the pieces. The pieces are small to demonstrate the joint specifically. The joint is four inches wide with fingers one inch each.

The sheet stock that we used actually measured .755 so we wanted to go a bit farther than .755 so it could compensate for the corner. We used .757 for all of these fingers. We then had four inches of width and the fingers protruding out .757 and each finger one inch wide. We took that same piece and rotated it 180 degrees. First we joined all the lines to create a polygon. Then we copied it and rotated it. Normally we would put a bit of a tolerance between the finger and make it a little bit thinner, but for the time we kept it at zero to see if the wood was forgiving enough to do this, if not we would need to add a thousandths of an inch displacement.

The inside corners are not going to be perfectly square because we used a bit that is round. The bit had to do an overcut to be able to marry flat to the adjacent corner. This is also a good place for some glue to sit to provide added strength. The rounded corner also provides a relief for any stress at the corner, or stress cracks that could arise.

Now we want to input the file in our CAM program to establish the machining operations. Save it as a DXF file. We'll be using CAMBAM for this. Once you have the two selected, create a roughing and finishing profile. We use styles to do this so we don't have to keep adjusting the parameters. Our roughing pass will have a clearance of .01 so when it comes to the finishing it will just shave off that little bit of material. We only want two holding tabs on these so we select both of them and change our holding tabs to minimum of two. The roughing pass actually does two passes and then the finishing pass does a single pass, just shaving off a little bit of material at the end. It will also do the overcut, and you can see inside the profile under the parameters that corner overcut is true, so this is an automatic machining operation that CAMBAM provides.

Next we move to the CNC machine to cut it out. We have our stock setup, and we're going to zero the X, Y, and Z axes. It is not imperative that the Z axis is perfectly zeroed on the surface, we went as close as we could, but because this is not a locking joint and the joints are based mainly on the X and Y depths, it is really just going to be dependant on the X axis to get the thickness right so the Z axis doesn't really need to be perfect. After zeroing we are ready to start the machine.

We cut out the two pieces and kept the holding tabs intact, because we wanted to test the mirroring of the two pieces. You can see in the video that there is a slight overcut, this is really a way for the short edge to meet and not conflict with the curve that could have happened because of the end mill. This is also a stress reliever. If you had a perfect inside corner, there is a stress point for cracks to happen so this actually works out really well. Our shop guy tells us this is a good place for glue to sit to make the piece even better.

Remember we didn't put any tolerance between the pieces so they're right on. We want them to fit very snugly. You can put them together with a vice and they'll never come out. You may need to do a little bit more of an adjustment in the depths of these ends to make it a little deeper. These parts of the fingers don't protrude above the end-grain parts because it would be more difficult to make the surface smooth. If you're using a laminated product you wouldn't want to take any sanding off the laminated portion of it.

The finger joint is now complete, and there is zero tolerance, so you may want to add a little bit of tolerance to make it easier and to have glue sit in between. Another aspect of this finger joint is that these ends are perfectly flush. There is no difference between them so this worked out very well. We also put this in a vice to tighten it up a little bit more. It was able to move a little bit but not enough to make it perfectly flush, so you want to move it back about .005 of an inch.

That is how we make a finger joint with a CNC machine.

In this video we’ll be showing you how to make a complex jigsaw miter flat joint. We aimed to make it a little fancier than the standard joint, but that presented some challenges. The amount of material matters because of the vibrations, and there was a bit of a sawtooth issue. Getting the depth perfectly right is also an issue, so on this particular joint you want to make sure the half depth perfect, with a spoilboard that is perfectly flat and surfaced.

We start out with four inch pieces of wood, just like last time, but in a flat arrangement. First we make the design a bit longer (offset by four) so it looks like a frame, and mirrored at a right angle. For a more complex type of joint, we just want to take a line and move it around and meet back at the other corner. You want to make sure there are enough corners around that allowed it to be locked in place. This is further illustrated in the video. With the regular type of joint, you’d be able to lock it in place, but not tear it apart. From here you’d need to consider the size of bit you will be using. In the video we’re using ¼” so you’d need to make the radius of all the corners 1/8th of an inch. Now you have a general joint.

However, there are a couple problems with this joint. If you draw the lines you will see that the joint crosses a boundary you don’t want it to. You want it to work within the square. There are a lot of designs that can be created to add attractive features to the corner of the wood. We place the lines inside to make sure we know where our boundaries are. Once the design has been prepped, the corners need to be rounded for the size of the bit (1/8th inch). Once completed, we can see there is a little bit of a room, and the end mill would have to get through the area, cut out, and then leave material behind. The piece also looks brittle like it could break easily, so we need to increase the radius of the curves. Now the joint looks like it will be useable and does not go outside of the boundary.

From here we create two pieces from the first one. After both are generated, we’re going to only pocket the first piece halfway through the wood, the other will be halfway through the other side. This way all material can be removed halfway through the wood, so everything will be able to marry itself very easily into the other portion. In the last video (part one), we used a zero tolerance between the fingers. In this case, we want to create more space between the puzzles pieces because of the nature of the geometry. Tolerances are put in to make sure the pieces will fit snugly. We will use .01” of an inch. After looking at the tolerances, we realized we needed to readjust some of the lines. Once mirrored, we can see the small amount of difference between the two pieces when put on top of each other.

Next we used the BO command to put a polygon to make sure there is a nice corner around the edge. This creates a polygon boundary. We then rounded off the corners using circles. We needed to make sure it will pocket the pieces correctly we polygon boundaries. For this we used an offset of .25. After pocketing, we will cut out the square and replace it with a rectangle. From here we are now able to save the file and open it in CAMBAM.

Inside CAMBAM, after loading the file, we create the pocket for the first piece. We select the polygon and use the pocket machining operation. Next we need to figure out the target depth. At this point you need to measure the actual thickness of the wood you’ll be using. Our piece is .76 so our target depth is .38. After setting the target depth we did an inside profile (a finishing profile) to do a roughing pass in order to make it nice and precise. Also make sure the profile is .38. There should be 2 outside profiles. One for finishing and one for roughing. Again, you’ll want to watch the video for more precise instructions on everything that is being done.

After completing the design, we are ready to produce g-code and run the machine! You will notice that we’re using the greenLean vertical for this particular cut. After the pieces finished, we discovered we didn’t quite make enough of a tolerance between the two, so we had to adjust the tolerance a little bit to make sure they locked into place perfectly. After the adjustment you will see the two pieces were able to fit after an adjustment of .02.