Kevin Kennedy: Hey there, It’s Kevin Kennedy and welcome to 3D Sketching 101. In this video, we’ll look at the key differences between 2D and 3D Sketching. We’ll then build this “C” shaped side-table using the latest 3D Sketch enhancements in Fusion 360. [Logo Chiming] The March 2020 update brought significant changes to Fusion 360’s 3D Sketch feature. Beforehand, it was cumbersome and very unintuitive. You had to use the move command to manipulate sketch objects. For most users, it was hard to figure out how 3D sketching should fit in the typical workflow. Before we take a look at how to 3D sketch with the new update, let’s look at the key differences between 2D and 3D sketching. With a 2D Sketch, we constrain sketch geometry to the plane used to create the sketch. We’re able to create a new 2D sketch on any of the origin planes, construction planes, or any planar faces of a model. 2D Sketches can originate anywhere in 3D space. However, they’re considered 2D sketches because we’re constrained to the 2 coordinates of our sketch plane. With a 3D sketch, Fusion 360 removes the planar restriction, allowing us to create the sketch geometry anywhere in 3D space. This means we can start with a typical 2D sketch and we can continue the geometry onto other 2D planes, keeping the sketch geometry one continuous piece. Knowing when to use a 3D sketch instead of a 2D sketch can make all the difference. In short, you’ll want to use a 3D sketch to create a path for tubing, sweeps, lofts, or surface edges, when the design continues to multiple planes. Contrary, 2D sketches should be used for common features like extrude and revolve. Looking at this image, these are four great examples of items that would benefit from a 3D Sketch. The shape of an axe is very unique because it tapers in multiple directions. Using a 3D sketch we can minimize the number of sketches and other features needed to recreate the shape. The second object, the C-shaped table, is what we’ll build in the remainder of this video. If you look at the frame of the table you’ll see that it’s one continuous path of square tubing that’s welded together. Because the shape is one continuous path, we can use the 3D sketch feature to sketch out that path, followed by using the pipe command. Bike handlebars are another common use case, as they’re often bent in multiple directions, which is something that we can’t easily recreate with a flat 2D sketch. The fourth object is a shower caddy. Similar to the furniture example, we can use 3D sketching to our advantage to recreate the outer contour as well as the continuous shape of the baskets. We could then use the pipe command or even the sweep command to create the 3D bodies. Ultimately, saving us time, while having to use fewer features. Let’s now get started with the example, which should make the concept of 3D sketching easier to understand. To start, you’ll want to make sure you’re in the Design workspace and under the Solid tab. We’ll first “Create Sketch” and select the XY origin plane. I’m choosing this bottom plane as I’m going to start with the bottom of the table frame. At this point, we need to turn on the 3D sketch feature. The easiest way to turn it on is to simply check the 3D Sketch option in the Sketch Palette. Before starting with a line, I’ll also hit the home icon next to the ViewCube. You’ll almost always need to look at the sketch from a perspective to understand what’s going on with the 3D sketch. Pay close attention to what happens in the middle of the screen, as I activate the line command in the toolbar. You’ll see that additional sketch planes appeared, along with some rotation manipulators and some extra axis lines. These all represent the new enhancements to the 3D sketch feature. With the latest update, we’re now able to continue sketching directly onto another sketch plane. We can rotate the plane in real-time, or we can extend the axis out, to help us better manage the geometry. To start, I’ll select the center origin and drag my mouse over to the right. At this point, we’re just creating a 2D Sketch, while viewing it in 3D. For the dimension, I’ll type out 45cm. I’ll then make sure it snaps into the green “y” axis, at 90 degrees. Now that we have this first section of the base, we can head straight up to create the vertical part of the frame, resulting in a 3D sketch. To do this, we’ll move our mouse to the “Z” axis, where it snaps to the axis. You’ll see that we’re now able to continue with this line in the third dimension. I’ll type out 60cm for the height. This time, we’ll need to select the Z-axis, again making sure it snaps in at 90 degrees. If we rotate the model, we’ll see that we now have the start of a 3D sketch. Take note of how the sketch plane and 3D sketch features move. They’ll always move to the last sketch entity. We now need to head back to the left, to create the first piece of the top of the frame and to finish off the first “C” shape. One challenge with 3D sketches is the fact that we still want to make sure we fully-constrain our sketches when possible. We also want to make sure that we use the least amount of dimensions as possible, so it’s easier for us to have design intent, keeping the model predictable. With that in mind, we don’t want to add a dimension for this line, as we want it to match the first line, which includes the length. Instead, we’ll simply click on the green “y” axis to place the line. We’ll then use a constraint to force the line lengths to be the same. Hitting the escape key will not only clear out the line command, but it will remove the 3D sketch options, making it easier to add constraints. We can then select the “Horizontal/Vertical” constraint in the toolbar. Selecting the endpoint of our last line and the starting point of our first line will force this vertical relation. This will ensure this top line will remain the same length as our first, without having to use a dimension. To continue, we can reactivate the line command, and select the endpoint where we left off. We now need to create the width of the table frame. For the width, I’ll follow the red “x” axis. I’ll type out a dimension of 25cm. Once again, we’ll make sure to click where this snaps in at 90 degrees, or in this case, along the x-axis. For the next line, we’ll head back to the right. Once again, we’ll want to place the line without a dimension value, so we can force the length with a constraint. However, I do want to point out that the 3D sketch feature also has a lot of great reference lines that help us place geometry. Notice all the lines that appear as I reference other points of the sketch. I’ll select the “Equal” constraint in the toolbar. Select the last line and the opposite line. This will force the lines to remain equal in size. We could’ve used an equal constraint for the previous line. However, I wanted to show you that there are often several ways to achieve the same result. We can now reactivate the line command and continue the frame by drawing a line straight down. This time, I’ll use the reference geometry to make sure the line snaps in at 60cm while remaining vertical. We can then finish off the frame by creating the last two lines, making sure they snap in at 90 degrees. Once they’re both complete, hit the escape key to clear the line command. You’ll see the last two lines are blue, which means they’re not fully-constrained. To fix this, we have to think a little bit different, since we’re working with a 3D sketch. Our shape is also somewhat of a unique case because we’re essentially mirroring the “C” shape while connecting it together. By constraining this back line, we’re freezing these last two lines in place - since everything else is already constrained. I’ll apply the equal constraint to the back two lines. Notice how the front two lines turned black as well, and our 3D sketch is now fully-constrained. We can double-check that it’s
fully-constrained by looking for the lock icon next to the sketch name. This means we can now update the length, width, or height, without skewing our desired shape of the 3D sketch. We’re now ready to turn this 3D sketch into a 3D body. First, however, I want to point out one more thing with 3D sketches. That is the fact that 3D sketches result in only one sketch feature in the parametric timeline. Contrary, if we were to create this same table shape with 3 different 2-dimensional sketches, then we would have 3 separate sketch features in the timeline. At this point, we can switch over to the Solid tab, where we’ll find the Pipe command in the create dropdown. If you’re not familiar, the pipe command lets us create a solid that follows a selected path. As you’ll see, the difference from the Pipe command and the Sweep command is the fact that we can define several details of the pipe. Once activated, we simply need to select the path. I should also point out that with 3D sketches, you can apply sketch Fillets to any of the corners, giving you more control over the shape. You’ll also find on this tutorials resource page, I’ve listed all of the sketch tools that work with this 3D sketch feature. Within the pipe dialog, we can first change the “section” shape to a square, to represent our square tubing. The distance options let you define how far along the pipe should follow the path. We can leave that set to 1 and 0, which makes it follow 100% of the path. For the section size, I’ll type out 2.5cm, which represents the width of the square tubing. One advantage of the Pipe command over the sweep command is that we can easily make pipes hollow. If we check the “hollow” option, we’re presented with the “Section Thickness,” which means you’re defining the thickness of the material, not the width of the hole. For this, I’ll type out 2mm. I’ll then click OK to confirm the Pipe command. Using the Section analysis tool, we can check to confirm that the pipe is hollow on the inside. At this point, we’re done with the frame of the table. Hopefully, this beginner 3D sketching tutorial helps you understand a few of the advantages to using 3D sketching. If you’d like me to cover more advanced 3D sketching concepts then let me know by dropping a comment down below this video. To finish off the tutorial, we can create a new component for the top surface. Watch what happens when I select “create sketch” and click on the top surface of the frame. Many of you will expect Fusion 360 to automatically reorient the model, so we’re looking directly at it. However, when the 3D sketch feature is enabled, this will override the “Auto Look at Sketch” feature. I’ll disable the 3D Sketch feature and I’ll finish the sketch and delete it. Watch what happens as I now create a new sketch. As expected, the model reorients, so we can create a 2D sketch while looking directly at it. I’ll simply use the 2-point rectangle command to create the top surface. I’ll then use the extrude command to create a thickness of 2cm. Of course, you can take the model even further by adding fillets, appearances, and other details. To summarize, I want to remind you that the advantage of 3D sketching is the ability to be more efficient with certain shapes and paths. 3D sketching is also really powerful when used in conjunction with surface modeling. Again, I’ve listed that and several other use cases on this tutorials resource page. Last but not least, I want to give a quick shoutout to those who supported my content over the last two weeks. Special thanks to my new Patrons... Laszlo B, Ryan S, Neil T, Thomas L, Louie L, Brodie S, Sebastian S, David K, and David V. And thanks to those who supported the channel via my Buy Me a Coffee page. Tomas D, Ben, Olly, Steven D, and of course the anonymous contributors. [Upbeat Music] If you’ve learned something new in this video then hit that thumbs up icon for me and click that subscribe button if you haven’t already. I’ve got a lot of exciting videos lined up that you won’t want to miss! [End Upbeat Music]
