Selfie Ring Light Tutorial #2: Layout Sketch

This is Tutorial #2 in the Selfie Ring Light Tutorial series.
If you have not yet completed the previous tutorials, you can find Tutorial #1 here.

In the previous tutorial, you uploaded and organised the electronic components into your Fusion 360 account.
All these components need to fit into the Selfie Ring Light design.

How can we bring them into our design?
How can we position them in a sensible way?

In this tutorial, we’ll start a new design and create a Layout Sketch inside it.

What’s a Layout Sketch?
A Layout Sketch is a sketch that defines rough outlines and placement for components in the design.
Components and later sketches can all reference and be aligned to the Layout sketch – it’s kind of like the foundation of our design.
(There are other ways to design using Fusion 360. The Layout Sketch approach is a good way to design the Selfie Ring Light)
Really complicated designs might need more than one Layout Sketch!

So the Layout Sketch is pretty important.
That is why it’s the first thing to create in the Selfie Ring Light design, and why you should follow these instructions carefully… 🙂

Step 1: Create And Save A New Design

Gotta start somewhere…

  1. Open Fusion 360.
  2. Navigate to the Selfie Ring Light folder you created in Tutorial #1.
  3. Ensure that you’ve got a blank design by clicking on ‘New Design‘ in the top drop-down menu.

  4. Save the design,
    Set Location to be inside the ‘Selfie Ring Light’ folder,
    Name it “SRL Test mk1“,
    Click ‘Save’.


It’s empty now, but not for long…

Step 2: Create and Name the Layout Sketch

  1. Create a new sketch on the front plane.
    (Click on “Create Sketch”, click on the plane to start the sketch)
  2. Rename the sketch you’ve just created to Layout.
    (Expand the ‘Sketches’ browser tree so the sketch is visible, click twice on the sketch, then type in the new name)

Remember – naming parts of your design is always a good idea!
You’ll be coming back to the Layout Sketch again later…

All the tools are somewhere in the Toolbar menu… but it can take a while to find them.
Fusion 360 has a really helpful search box:
1. Press ‘s’ on your keyboard at any time to open it,
2. Start typing for the tool you want, (like r e c t … for Centre Rectangle) and just click on it when you see it.

You can also click on the ‘‘ icon to pin frequently-used tools to the top.

Step 3: Sketching Component Outlines

In this step, we’ll draw outlines with centre points for each electronic component.
We will accurately dimension these outlines to match our components.
This is so that we know where the components will be placed relative to one another.
(And whether they’ll fit together in the design and real life, or block each other!)

In the Layout sketch created in Step 2:

  1. Draw the LED Ring Outline
    Sketch a circle that is centred on the origin,
        (Press c to select the Circle tool, click on the origin, move the mouse away and click again)
    Dimension it to be 92.25 mm.
        (Press d to select the Dimension tool, click on the edge of the circle, click somewhere else, type in the dimension)

  2. Draw the Battery Box Outline
    Use the Centre Rectangle tool to draw a rectangle inside the circle…
        (In the toolbar at Sketch > Rectangle > Centre Rectangle, or just press s and search for it)
    Click somewhere above the origin, move the mouse out, click again.
    (Do not start on the origin, do not click on the edge of the circle)
    Dimension it to be 63 mm wide and 37 mm high.
        (Press d, click on a line, click somewhere else, type in the dimension)
  3. Draw the Digispark and Tact Switch Outlines
    Select the Centre Rectangle tool again.
    Draw a medium-sized rectangle and a small square as shown in the video below.
    Dimension them to be 18 x 24.5 mm and 6 x 6 mm.

Step 4: Tweaking

Now that all the component outlines are defined, you can arrange them in an initial layout.
(Click and drag, or use the Move command)

When you’re happy with how it looks;

  1. Click “Stop Sketch“, and
  2. Save your design by clicking on the  icon.

All done!
Remember, you can go back and edit this sketch at any time.

Did you have any trouble? Check out this next PITSTOP|TOP TIPS.

PITSTOP|TOP TIPS: Auto Constraints
Did part of your sketch get ‘stuck‘ to another shape?

Or you couldn’t drag something where you wanted?
Fusion 360 automatically adds some sketch constraints based on what it thinks you’re doing.

For example;

  • If you drag a corner over a line, it will be locked onto the line with a coincident constraint. (see picture)
  • If you draw a line that’s vertical, it will be locked at a vertical angle with a vertical constraint.
  • If you draw a line that’s parallel to a nearby line, it will be locked at that angle with a parallel constraint.

You can remove them:

  1. Click on the ‘stuck’ part of the sketch, and the constraint should appear.
    (In the picture above, clicking on the circle has shown the coincident constraint:  )
  2. Click on the constraint to select it.
  3. Delete the constraint by pressing the Delete key, or right-click (two finger click) and select Delete
  4. Done! It should move now.

You can prevent automatic constraints from happening;
By holding down the Ctrl key as you drag or draw. OR

By using the Move command when moving sketch geometry.


Now that the layout sketch is finished, we can start adding components into the design!

Next: Selfie Ring Light Tutorial #3 – Adding Electronics

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