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Welcome to Day #19 of Learn Fusion 360 in 30 Days. I’m Kevin Kennedy,
and today we’ll look at creating User Parameters, copy and pasting components, and more, as we create a Parametric box.
In Fusion 360, activate the “Change Parameters” dialog from the Modify menu.
Parameters allow you to create equations and relationships to control the size of your Fusion 360 designs. By assigning names to the equations, we can reuse the parameters throughout the design.
Let’s create a new Parameter for our Box’s width. Select the plus symbol to add a new parameter.
We’ll type the name “BoxWidth.” Note that spaces are not allowed in the parameter names. You can utilize camelCase, snake_case, or PascalCase.
The unit of measurement will default to your document units. However, we can also create parameters for other units of measure, including degrees, volume, mass, and so much more.
I’ll set the expression to 50mm, which will be the starting width of the box.
We’re also able to plug in optional comments. Comments are helpful to remind yourself of items later or when collaborating with others.
After selecting OK, you’ll find the BoxWidth parameter in the “User Parameters” list.
Let’s create a second User Parameter called “BoxHeight” with a value set to 40mm.
We can now close the dialog. Our parameters are now ready to be called through any sketch or modeling commands.
Let’s start with a new component called “Box Bottom.”
Once active, we’ll start with a new sketch on the bottom origin plane.
Activate the 2-point rectangle and select the origin point to start the sketch.
For both dimensions, we’ll enter the “BoxWidth” user parameter. Notice the parameter name appears after typing the letter “B”. We can select the correct one without having to type out the full name.
Complete this for both dimensions, which fully defines our sketch.
Let’s also practice good parametric design etiquette by renaming our sketch in the Browser.
We’re now ready to Extrude our sketch. Once selected, we’ll use the BoxHeight user parameter. However, we’re only creating the bottom of the box, so let’s divide this by 2.
Notice the height adjusted to be only 20mm, half of the overall height.
We’ll use the Shell command to hollow out the box. Activate Shell and select the top planar face.
Fusion 360 also allows us to create ‘parameters on the fly’. Start by typing the desired parameter name, such as “WallThickness.” We then have to put the equal sign, followed by the value. Let’s do “WallThickness” equals 2.
Select OK to confirm the Shell operation.
Let’s open the parameters dialog. Notice parameters created on the fly are listed in the Favorites section and not the User Parameters section.
With our parameters dialog still open, we can move it out of the way, and test our user parameters by changing any one of the expressions.
For example, I’ll change the width to 100mm.
Notice the box instantly resizes based on the new expression.
Keep in mind that it’s critical to fully define your sketches, as discussed earlier in this course. Fully defined sketches, combined with User Parameters can provide you with an efficient and convenient way to change your models’ dimensions.
Take a minute to test out some different dimensions. It’s best practice to test your user parameters to ensure everything is working as expected. This makes it easier to fix any issues before your design becomes more complex.
I’ll set the width back to 50mm and the height back to 40mm.
Let’s now create the Box Top by copy and pasting the component.
Remember our Component groups the relevant sketches, bodies, and other assets. This makes it easy to create duplicates of the same part.
Start by right-clicking on the component in the Browser.
Select “Copy” from the right-click menu.
We’ll then right-click on the top-level component, which is also called the “Root” component. This will make sure our pasted component is nested on the same level as our existing one.
Notice we have the option to Paste and Paste New. Paste will create an exact copy that will always remain the same as the original. “Paste New” will create a copy, but will allow us to make changes without affecting the original.
Let’s use “Paste New” In case we want the Box Top to be unique.
Once pasted, we can choose to define the location. However, we’re going to use the Joint command to place this, so let’s click OK.
Before we move the Top Box into position, let’s go ahead and rename the component in the Browser.
Once complete, we can activate the Joint command in the Toolbar. The “Joint” tool lets you position components relative to one another, then define the relative motion between them.
We’ll want to hide the Bottom Box in the Browser so we don’t select that by accident.
To use the Joint command, we need to first set the “Joint origin.” Defining the Joint Origin” for each part is how we position the parts relative to one another.
Generally, it’s best practice to select a corner or an item that will not change.
Let’s select any one of the four corners, making sure to select on the top planar surface.
Once selected, we can turn the other component back on in the Browser.
We’ll now want to select the opposite corner so our lid is flipped to the correct position.
To make it easier to snap to points on a face, place the pointer over a face, then hold the Control key on Windows or the Command key on Mac.
Once the second corner is selected, you’ll see our Box Top moves into place. However, the rotation may not be aligned depending on how the Joint origin was applied. You can fix this by adjusting the rotation slider in the Canvas or the angle in the dialog.
Once again, we should test our user parameters to ensure the Joint was applied correctly.
Everything looks correct!
I’ll see you on Day #20 we’re we’ll add 3D printable hinges to our box.
[End Upbeat Music]