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### Transcript

Welcome to Day #16 of Learn Fusion 360 in 30 Days. I’m Kevin Kennedy,

and today we’ll discuss “Design Intent” and why it’s important to fully define your sketches.

2D Sketches are the foundation of parametric modeling. When done correctly, they drive our 3-dimensional bodies and allow us to change dimensions ‘on the fly,’ making design changes a breeze.

For this demo, we’ll recreate this square washer plate that is a square with a hole cut out of the middle.

While looking at this shape, we can ask ourselves, “What do we know about this without knowing the dimensions?”

We can see that all four sides appear to be equal. The lines are perpendicular at the corners. The lines opposite from each other appear to be parallel. It appears that our hole is directly in the middle.

These important design elements are all things we can drive using sketch constraints before we apply any dimensions.

I recommend sketching out your designs on pencil and paper – or at least thinking about them before you start sketching in Fusion 360. Doing so will help you consider how the sketch should be constrained based on your ‘Design Intent.’

How you constrain your sketches will differ per each individual design file. That’s why it’s important to come up with a strategy for how entities relate to each other. This strategy is often referred to as ‘design intent.’

Let’s start by creating a New Component for our first square washer. The design intent of this first one is to make the circle always remain half the size of the outer square.

We can start with the center rectangle command and we’ll start the sketch at our origin point. Remember that starting at our origin point is best practice so we can fully define the sketch.

Let’s click to place the rectangle, without defining any sketch dimensions.

Keep in mind that Fusion 360’s sketch tools will automatically apply sketch constraints for us. We can always delete these by selecting them, followed by the Delete key.

We already have parallel sides, which is one of our known items. You’ll see we also have a perpendicular constraint in this corner. This will work together with the parallel sides to keep each corner set to 90 degrees.

We’ll want to use the equal constraint to make sure all four sides remain the same length.

Select the equal constraint in the toolbar to activate it.

We’ll then select any two adjacent sides.

If we were to try applying the equal constraint to additional lines, you’ll see that we receive a warning that this would overconstrain the geometry.

The four sides will remain equal with our existing sketch constraints and our newly added equal constraint.

If a constraint is automatically applied and you can’t remember what it stands for, then select the glyph and you’ll see the name in the lower-right-hand corner.

As you’re defining sketch geometry, you’ll want to select and drag on the geometry to see what degrees of freedom are remaining. In this case, we can only increase or decrease the size. That means we’re now ready to apply a sketch dimension.

With the Sketch Dimensions tool, I’ll select one side of the rectangle. Let’s dimension this as 100mm.

Notice our sketch is now fully defined, as confirmed by the red lock icon in the Browser.

This means our sketch will never change in size unless we choose to update this dimension.

Let’s now add our circle in the middle. Use the shortcut letter C and start the circle from our center origin point.

Remember that our ‘design intent’ for this first washer is for the circle to be half the rectangle. Let’s define this as 50mm, and we’ll discuss why this approach is problematic.

Let’s first Extrude this to a distance of 5mm, so we have a 3D body to test.

We’ll start testing our design intent by editing the sketch and changing our rectangle dimension to 200mm.

Notice our sketch does not adapt to our ‘design intent,’ as the circle is no longer half the size of the rectangle.

We can fix this by making the circle’s dimension update any time our rectangle dimension updates.

Double-click to edit the circle’s dimension.

We’ll start by selecting the first dimension. Notice this places ‘d1’ in the input field. Calling the number of the dimensions will allow us to reference any other dimensions dynamically.

Note that dimensions are simply numbered in the order you create them. Hover over a dimension to see the number.

Because we want it to be half of this dimension, we can divide this by 2. Press the Enter key when you’re done. This will calculate the dimension based on our new formula, making sure the circle always equals 50% of the rectangle.

Let’s double-check that everything is working by changing the flange length back to 100mm. Notice how the circle updated automatically, resulting in 50mm. This is the power of leveraging sketch constraints and dimensions in parametric design.

Let’s right-click on our component and select Copy. We’re going to use the Paste New feature when right-clicking on the top-level assembly. This will create a second instance that is no longer tied to the original.

I’ll rename this as “Washer #2,” followed by activating the component.

This second washer has a different design intent. Instead of the circle remaining in the center, it should always remain 40mm from the bottom edge, while remaining centered in the horizontal direction.

In this case, we’ll need to select our circle so we can find the coincident constraint that is attaching it to the center origin. You’ll see that we have four coincident constraints. If we carefully hover over each one, it will highlight what they are related to. These will also appear in the order they’re created. We know that our center circle is the one furthest away from the selected point.

Let’s go ahead and delete this. We can now move our circle around freely.

Let’s add a new sketch dimension that is 40mm from the center of the circle to the bottom edge.

We can then add a vertical constraint to the center of the circle and the center origin to ensure this remains centered.

Before we test this, we’ll need to update the dimension of our circle to 50mm, no longer relying on the equation.

Let’s test this new design intent by changing the rectangle size. Notice the circle now remains 40mm from the bottom edge, regardless of the rectangle size.

Comparing these two examples, you can see how leveraging different constraints and types of dimensions gives us different results while allowing us to have predictable and manageable designs.

Last but not least, here are some Fusion 360 sketching tips.

The goal should always be to keep sketches as simple as possible. Remember that a sketch’s history is not captured. The more you use modeling tools, the easier it will be to change or edit features.

Complex sketches are often the root cause of latency in Fusion 360.

To help keep your sketches simple, avoid adding fillets to your sketches, when possible. Sketch fillets remove constraints and they can cause problems if you want to go back and edit your original sketch. Use the modeling fillets instead.

Avoid mirroring the sketch, when possible. Mirroring the 3D body or component will perform better and make it easier to keep your sketch simple, especially if you need to make updates.

That goes hand-in-hand with the sketch pattern tools. You’ll run into many problems if you need to edit the sketch later. In addition, the 3D pattern features perform a lot better.

You now have a solid understanding of *how* and *why* to fully define your sketches.

[Upbeat Music]

I’ll see you on Day #17 where we’ll look at how to use all the types of sketch constraints.

[End Upbeat Music]