- [Kevin] There are two main ways to create parametric dovetail
joints in Fusion 360, but one way is better than the other. We'll also take a look at
the best way to apply Joints to make sure we drive the parameters without breaking the file. If you know an easier or better way, then share them by commenting below as you watch the tutorial. (electronic swoosh) I've gone ahead and
created User Parameters that we can use as we set up the sketches. To save you time, you can grab my demo file with
the parameters already setup. Check out the link below
in the video description. To start, we'll create a new
component for the TailBoard. This will help us manage the assets as we copy the boards. Our initial board will be created with a simple 2-point rectangle. I like to use the shortcuts box, which is activated with the keyboard shortcut
letter "S," as in Sierra. We can then simply search for
the feature we're looking for, or in our case, the 2-point rectangle. Once we select it to activate it, we can select the front origin plane. I'm selecting this plane
as we're going to start with the front board of this box. We'll follow the best practice
of starting the sketch at the origin point. After clicking the origin, we can drag the mouse out and
type out the user parameter of boxHeight for the height, and boxWidth for the width. If you need to toggle between inputs, you can simply hit the tab key. We can then click to place the rectangle. Let's toggle open the Sketches
folder in the Browser. You'll notice the lock icon, which signifies we have
a fully-defined sketch. This is critical in making sure our model is parametric and predictable. We also want to keep our
sketches as simple as possible. If you can, you always want to place
objects in separate sketches. Let's flip to the Solid tab and activate the Extrude command. We'll then extrude this out to the boardThickness parameter. Before we forget, let's also rename the
sketch in the Browser. Click once to select it and a second time to edit the field, and we can type out "Board". We can now sketch on the
front face of this board to make the tail shape of the dovetail. Again, we're separating these sketches so we keep them as simple as possible, making them easier to fully-define. This will also make sure
we can update the design in a predictable way. Right-clicking on the front face, I'll select "CreateSketch". To create the tails, we're going to sketch the negative space where the pins will slide in. We're only going to sketch the center one, and we'll use the modeling
tools to pattern it, again allowing us to
keep our sketch simple. Before we sketch, you'll want to head up to your
profile picture or initials, and select the user preferences. Under the Design tab, you'll want to turn on
"AutoProject Edges on Reference". This setting will ensure we can
snap to the existing 3D edge and will let us sketch in
the middle of the object, while still fully-defining our sketch. Back in our sketch, we can activate the line tool with the shortcut letter "L," as in Lima. Let's also turn the construction option on in the Sketch Palette, since this first line will
serve as our symmetry line. Once we find the midpoint
constraint or triangle icon, we'll click to snap the line in place. The length of this line will be set to the dovetailLength parameter. We also want to snap this in place by clicking when we see
the perpendicular icon in the corner, leaving us with the
perpendicular constraint. Now that we have a center line, we can sketch out the shape on both sides, but we'll only dimension the one side. We'll then use constraints
to fully-define this sketch. We can turn off the construction option and create a line running straight up. I'll set this to the
dovetailHeight parameter, divided by two since
we're only creating half. We also want to place this 90 degrees to the previous line. Next, we need to create our angled line so we get the dovetail shape. We don't know the length of this and always want it to be
driven by the dovetail angle, so we can hit the tab key to switch to the degree field. Plugging in the dovetailAngle
parameter leaves us in the wrong direction. To fix this, we can take 90 degrees for a
line that would be straight out and we'll subtract the dovetailAngle. We can then click on
the edge of the board, where it snaps into place, again because we have
that Auto Project Edges on Reference turned on. Our sketch should be
fully-defined at this point, but we need to create the opposite side. Let's hit the escape key
to clear all commands. I'm first going to click and
drag on these dimensions, to get them out of the way. With the line tool, we'll want to create the same shape on the other side of our center line. However, this time we
won't add dimensions. We'll use the symmetry constraint to force these lines to be the same. Remember, we always want to
minimize the use of dimensions and use constraints when possible. After activating the symmetry
constraint in the toolbar, we're able to select both lines, followed by the center line. Notice how that forces it to be the same. We'll want to do this to
the second line as well. Our sketch should once
again be fully-defined. Let's rename the sketch to keep our file nice and organized. Fusion 360 will automatically
leave the sketch environment if we activate a modeling tool, so we don't need to finish the sketch. Let's instead hit the
keyboard shortcut letter "E," as in Echo, followed by
selecting the sketch profile. We want this profile to
be cut out of the board, so we'll use the boardThickness parameter with the negative sign in front of it. Right now we have two simple
sketches and one 3D body. The key takeaway here is that
you could technically pattern the sketch using the sketch pattern tool. However, when possible, you always want to pattern 3D bodies, features, or components over sketches. That's actually where
most people go wrong. They want to pattern the sketch, making it complex and
more likely to break. Using the modeling pattern
feature helps us keep the sketches super simple
and lowers our chances of breaking something when we plug in different parameters. Before we pattern this cutout, we're going to mirror it over to the other side of our board. This will make our mirror feature simpler, putting the 'heavy lifting'
on the pattern command, which generally performs better. Let's first create a
midplane construction plane to serve as the mirror plane. We can select each end of
the board and click OK. With the modeling mirror command, we'll change the mirror type to Features, which allows us to
select the Extrude object in the timeline.. Our mirror plane will be the midplane that we just created. Once that is complete, we can also right-click on the plane and find the option to hide it. Now that we have a cutout on each side, we can activate the
Rectangular Pattern feature in the toolbar. The pattern type should
also be set to Features, which lets us select the last Extrude, as well as our Mirror feature. For the direction, I'll select the edge of the board. Before we fill out the quantity, we'll need to set the
Direction Type to Symmetric. That way our pattern
runs in both directions. We can then plug in
our pinNumber parameter into the quantity option. This will dictate how many dovetail pins the adjoining board has. If you look at standard dovetails, you'll find there are usually
half-pins on the outside. With this in mind, we'll want to set our distance
so the pattern ends up with the last cutout
being only half the shape. Our boxHeight parameter is
currently set to five inches, so I'm going to set the distance to boxHeight divided by two, which should correctly
space out the five pins. The good news is, is that we've now done the hard part. Making the board with the
pins will be even easier, as we can quickly reference
the existing geometry. Let's first create a new
component for the Pin Board. Again, we'll start with
a 2-point rectangle from the origin point of
the front origin plane. We'll need the BoxHeight parameter and the boxThickness parameter. With the Extrude command, we can make this run back the distance of the boxLength parameter. Before we use a feature to cut
out the shapes on this board, we'll want to copy the two boards to make the rest of the box. That way we can maximize
how the cutout is computed. Let's first ground one
of these existing boards by right-clicking on it in the Browser, followed by the Ground option. This will freeze or
lock the board in place so we can apply joints
to the remaining boards. We can then apply a rigid As-built Joint since the other board is
already in the correct place. To create the other two boards, we'll want to copy them in the Browser. I'll copy the Pin Board first, making sure that we use
the Paste New function, which will keep it
independent from the original. This is crucial as we don't want them to inherit the pin cutout. We'll also want to click OK to place it, and we can hide the original
component in the Browser. That will let us use the Joint command to position the board. To join this first board, we'll select the middle area since our middle cutout will never change. We can also use the CMD key
on Mac or Alt key on Windows, to lock in to the face, making it easier to
select the joint origin. Selecting the Joint
origin on the other side will place this board
close to the position. Again, the goal is to make
sure our board is joined here no matter what our parameters change to. We'll have to follow this same process for the Tailboard. This time I'll use the top inside edge. You'll see that we may
have to once again flip the joint origin by
hitting the flip button. With all of our components turned back on, we should now have four boards
that are joined together, and can only be altered by our parameters. We need to cut out the
negative space for the tails. With the use of the Combine
command from the toolbar, we can select the left
sideboard as the Target Body and the front and back
boards as the Tool Bodies. Of course, we also want
to cut this object out, so be sure to change the operation to cut. Check the Keep Tools option as well, as that will ensure that
our front and back boards still exist after the operation. Notice how clear the dovetail
on the left is compared to the one on the right. We can also check that
things are cut out properly by hiding the other components. Repeating the Combine command, we can do the same process
for the right side. Remember, we want to use both Tail Boards as our cutting tools. Our dovetail joints are now complete, and we can test the User Parameters. Perhaps we want our pins to be smaller. We can simply change the
dovetailHeight to a half-inch instead of three quarters. We could also change our
degree from 14 to 17 degrees. We can also change the
width or length of our box, and the boards should
remain joined together. Utilizing these parameters can help us explore dovetail
styles or dimensions before trying them in real-life. To summarize this video, make sure you keep sketches
as simple as possible, and when possible, use the modeling commands over sketches. Thanks to all the new Patrons who joined in the last two weeks: Corinne, Phil, Josh, Tom,
both Michael's, Gary, Hannes, Jo, Chamberlain,
Chris, Antoine, and Bill. And thank those who supported the channel via my Buy Me a Coffee page: Clem, Joseph, and the
anonymous contributor. I appreciate all of your support as this helps me continue
to invest in my equipment to make all the tutorials even better. Be sure to hit the like button if you learned something in this video. Then click on that playlist
in the lower right-hand corner to watch more woodworking tutorials. (upbeat music)
