In this lesson, we will begin exploring the concept of applied sketching.

If you still have an open file, you can close it now.

From the file drop-down,

select new design from file.

Now, navigate to find the FSAE Steering Wheel2 file, and click to open it.

This will load its geometry and its history into the new file.

Now, save the file into the tier two folder and call it FSAE Steering Wheel2.

In this file, there is already a component named steering wheel base-plate,

hovering over the name,

a radio button will appear on the right.

Select this to activate the component,

so now that any edits made will be

captured in the timeline associated with that component.

Next, we will expand the component and expand

the sketches folder to see that we have a single sketch called Main Plate.

Now in the browser, expand the origin folder and select

the XZ plain which is aligned to the component's top,

right click and select create new sketch.

I use the marking menu to start the circle diameter tool,

and I'll place the center point at the origin of the sketch.

As the circle is dragged,

the diameter will appear displayed in blue,

I will press one on the keyboard,

and notice now that there's a lock icon to the right of the value.

I'll press the enter key and fusion will place the dimension for me.

I could still move the dimensions at any point in time but

this saves us a step from having to manually apply the dimension.

Next, we'll create another circle but this time,

use the C key on the keyboard,

and place the circle directly below

the one-inch circle and set its diameter to point two five inches,

and press enter twice to create the dimensions circle.

The way the circle is sketched,

it also creates a cleanse in relationship with the vertical reference line.

This constraint was created with

the vertical line that is located in the main plate sketch.

If you want to avoid placing constraints to other sketches,

it's a good idea to turn them off.

But one thing that happens is that

reference geometry is projected into the current sketch,

this vertical line was brought in as a reference from the main plate sketch.

Whether this is acceptable depends greatly on what you're trying to accomplish.

For this design, I want to make sure that these holes stay in line with the name plate,

so the reference is a good fit.

I used the look at tool to select the sketch

which will return us to a view normal to the sketch.

Now, use the D key to start

the sketch dimension to place a vertical dimension between the two holes.

I pick the sketch origin and then select the center point of the smaller hole,

then place the dimension to the right,

enter one for the value,

and press enter to place the dimension.

Now, we need to create a pattern of the smaller hole.

In the sketch drop-down,

we'll select circular pattern.

This will open the circular pattern dialog box above the sketch palette.

This dialog can also be undocked and depending on your default location,

yours could be floating.

Just make sure that you're able to find it.

The first thing we need to do is select the object that we want to be patterned.

In this case, it will be the smaller circle.

Then, we'll select the center point which will be the origin of the sketch.

There are some on-screen options for the pattern,

check boxes that allow us to omit instances of the pattern.

We can also increase or decrease the number of instances by

using the manipulator or by entering the value on the dialog.

We can also use a drop-down option,

whether or not we want to do a full 360 revolution,

or a specific angle,

or make the pattern symmetric.

All of these options are also properties of the circular pattern dialog.

For this design, we'll create a quantity of three,

we'll set the values, and click okay to create the new fully defined circles.

Now, I'll click on sketch three twice slowly,

and be able to rename it,

shaft pattern, by pressing enter after typing the new name.

Now, let's save a new version of the file.

Sketching basics: Applied Sketching

Autodesk Fusion 360 Integrated CAD/CAM/CAE

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