Fusion 360 Tutorial – Reverse Engineering IKEA Mirror – Part 3

This is Part 3 of the IKEA Mirror tutorial.

Each of the pieces in this design will be a component.
This follows Fusion 360’s RULE #1: “When in doubt, before doing anything, create a component and make sure it’s activated.”

Components are the best way to organise, connect, isolate and view the different parts of your design.

First Component: Frame

  1. Right-click (or two-finger click on a Mac?) the top part of the tree and select Create Component.
    Notice the new component ‘Component1’ that’s just appeared in the tree.
    Click on the component, then click again and rename it to “Frame”.
  2. Notice the little filled in circle to the right of the ‘Frame’ component. This means that ‘Frame’ is the currently active component; anything you create now will go inside this component.
    Tip: If you hover over the parent component you will see an empty circle. Clicking these circles lets you change the active component. (Make sure to activate the ‘Frame’ component before continuing)
  3. Click on the Extrude tool (or press E), and extrude the outer part of the frame.
    The outer mirror frame is 35 mm thick, but don’t click Ok just yet!
    It will be easier later if the extrusion is symmetric.
    Set ‘Direction’ to ‘Symmetric’.
    Set ‘Measurement’ to ‘Whole Length’.
    Now click Ok and you’ve got the outer frame.
    Tip: If you grab and drag the view cube or use the Orbit tool to change your view while the Extrude tool is active, you can see what happens when these settings are changed.

    Important: Once the outer frame is extruded, you should see a body appear in the browser tree inside the ‘Frame’ component. If it is not there, then undo the action, make sure the ‘Frame’ is the active component, and try again.
  4. The next part to build is the mirror glass, but our sketch has disappeared.
    Find the sketch in the tree, and click on the light bulb to show it again.
  5. Make sure the ‘Frame’ component is still active.
    Use the Extrude tool again, and highlight the glass profile.
    The glass is recessed from the front by 8 mm, and is 3 mm thick.
    This time, the extrusion starts from somewhere new:

    • ‘Start’ should be’From Object’.
    • ‘Object’ should be the front face of the frame.
    • ‘Offset’ should be -8 mm.
    • ‘Distance’ should be 3 mm.
    • ‘Operation’ should be ‘New Body’ not ‘Join’. (Because the glass is a separate piece to the frame)
    • Click Ok to create the glass.

    Now, there should be two bodies in the browser tree.
    Selecting one of the other will highlight that body in the window.

Second Component – Handle

The handle starts in much the same way as the Frame.

  1. Create another new component, and name it ‘Handle’.
  2. Confirm that the Handle component is active.
    (The circle next to the component is filled in)
    Using the Extrude tool, click on the handle profile, and symmetrically extrude the shape by 35 mm, creating a ‘New Body’.
    Confirm that the shape looks correct and click Ok.
  3. The handle looks pretty good now, but the real mirror’s handle has rounded ends. We can add them with the Fillet tool.
    First though, the Frame component will get in the way – hide it by clicking on the light bulb next to ‘Frame’. The sketch can be hidden now, too.
    Press F to open the Fillet tool, then select the four narrow edges of the ends.
    Tip: If you select an edge by mistake, you can hold down Ctrl and click it again to deselect it.
    The radius should be half of the handle thickness. Fusion 360 lets us write an equation in any field, so for radius enter 35 mm / 2 and it will make the ends perfect half-circles.
    Click Ok and our handles are complete!

    Re-show the Frame component by clicking on its light bulb again.
  4. Complete?

    The design is starting to look a lot like the IKEA mirror! A bit drab though…

← Part 2 | Part 4 →

Leave a Reply

Your email address will not be published. Required fields are marked *