Dovetail joints are a bit of a holy grail in the world of traditional woodworking. They look amazing, are super strong but can be a pain to figure out. I walk through two different way you can model them inside of Fusion 360 to use as template for you next project!
We are going to create the dovetails in two different ways. First an easy process if you know the number of dovetails that you would like. Second a great way to automatically change the number of dovetails using parameters so they can be adjusted on the fly.
Even though we won't make the number of dovetails a parameter we will be setting everything else us as adjustable. These are the parameters to define and can be changed at any time during the modeling process.
Next create a simple box using the "boardHeight" and "boardWidth" as the dimensions.
I actually created the sketch in reverse to start out (I always forget which way a dovetail actually goes ;). I first created a construction line that split the drawing in half horizontally. Then using the line tool create the basic dovetail shape.
Depending on where you click you will need to set up several constraints. But the main one is symmetry between the two slanted lines and the center construction line. Then to fully constrain the sketch the dovetailHeight and dovetailWidth parameter are added.
Inside the sketch we set up a rectangular pattern. This is only repeated in vertical direction with a quantity of 5. I set the distance type to extent so that it would be adjustable with our parameters. Then with a symmetric distance type the distance is defined as: (boardHeight-2*dovetailWidth)/2.
With the rectangular pattern created it is mirrored to the other side with the mirror command. You'll need to create another construction line that splits the board to be able to mirror.
With our sketch complete we can create an actual component by using the extrude command and selecting the sketch. I set a thickness of 0.75 in but this could also be defined as a paramter if you wanted to adjust this in the future.
After the dovetail board is created I went back into the timeline and edited the initial sketch to add a line that's used to extrude the pin board which is perpendicular to our first board.
With the sketch updated a new component is made by extruding the edge profile of the board
Using the combine tool the two boards are selected and the dovetail features is cut out of the pin board leaving just the pins.
Now you might want to model the dovetails so that you can not only adjus their shape but also their number. Since we defined that in the sketch it won't create new dovetails if the number is increased. Instead we need to go back to our initial dovetail sketch and model it a little different.
After extruding one dovetail the rectangular pattern tool is used (not the sketch version). This allows you to create a pattern out of components, bodies as well as features. The previous extrude created a feature in the timeline and that can be set as the pattern object.
The number of dovetails is set as a parameter so then any time that number is updated the rectangular feature pattern is updated as well.
There are only dovetails on on side of the board. Similar to how we did it with the sketch we use the mirror command. Instead of line you'll need a construction plane. This is made with the Mid-Plane command. Then the initial dovetail extruded and rectangular pattern can be selected to mirror to the other side.
Just like before the board with pins is extruding from the intial sketch. Then the combine command is used to cut the dovetail feature from the pin board.
Now the model is set up to adjust the number of pins by just changed the number in the parameters setting. We have a fully adjustable model!
Having model is great but how can you use it on an actual piece of wood? You can either create plans from this within Fusion at a 1:1 scale OR create a DXF drawing of the boards.
I typically going the DXF route. To create it make a new sketch and select the dovetail board as the surface. This automatically pulls in the profile of that component.
To export the sketch right click on it and select "Save as DXF". This file can then be using in most vector editing software or printed directly.
The printout can then be used as a template directly on the board to be cut with the ability to fine tune everything to your specific situation!