Fusion 360 Tutorial – Reverse Engineering IKEA Mirror – Part 2

This is Part 2 of the IKEA Mirror tutorial.

In this part we’ll add the mirror’s handle into the same sketch.

Q: Wait, why are we still sketching? When do we create something solid?
A: It is often better to use one sketch for several features.
It keeps the timeline short and easy to understand.

Big Tip:
The line tool has a secret – you can draw straight lines AND curves with it!

Sketching: Handle

  1. If you don’t still have the sketch open, right-click or two-finger-click on it and select ‘Edit Sketch’.
    • Select the line tool by pressing L, click once to start a new line, move the mouse to draw a straight line, and click again to set the end point.
    • Now, hover the mouse pointer back on top of the end point. This time, hold the mouse button down while moving to draw a curved arc.
    • Continue clicking or clicking and dragging until you have finished the shape.
  2. Now, we will use this trick to draw the handle. It does not have to look xactly right, we will fix it later with dimensions and constraints.
    Tip: When you have finished drawing lines you can stop by clicking on the tick mark, or by pressing Esc.
  3. Right now, one end of the curved arcs is smooth, but the other end is not. This can be fixed by adding some tangent constraints:
    Click on the line on the not-smooth side, hold down Shift and click on the arc, then in the Sketch Palette menu click on the Tangent constraint.
    Repeat until the whole line is smooth.
    Tip: You must select the line and the arc, not the point that joins them. If you select the wrong thing, just press Esc and try again.
  4. Next, we want these lines to wrap evenly around the mirror frame.
    Click on one arc, hold down Shift and click on the rounded corner of the frame, then in the Sketch Palette menu click on the Concentric constraint.
    Repeat for the other side.

    If you then try to move one part of the line, it all moves together!
  5. Lastly, the left side and the right side of this handle need to be at the same height. Select both ends (Click on one, then hold Shift and click on the other) and apply the Horizontal/Vertical constraint. (Click on the icon in the Sketch Palette menu)
  6. With these constraints, we only need two dimensions:
    The handle sides come up 250 mm from the bottom of the frame.
    The gap between the frame and the handle is 2 mm.
    Tip: Remember just press D for dimension – it will save you a lot of time.
  7. Now we can use the offset tool to form the other side of the handle.
    The thickness of the handle is 10 mm.
    (If you need to, refer back to the previous step)
    Then, use the line tool to join the ends of the handle shape.
    Tip: If you use a mouse with a scroll wheel, you can zoom in and out at any time, even while drawing or selecting geometry.
    At this stage the sketch should be fully defined, (all lines are black) and you’re ready to start making components.
    Press the ‘Stop Sketch’ button to get out of the sketch.
    Now is a good time to save your design, so hit the ‘Save’ icon and give your design a name.

← Part 1 | Part 3 →

Leave a Reply

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