Learn Fusion 360: Model a USB Charger

In this Fusion 360 tutorial, you’ll see step-by-step how to model a simple USB charger. You can follow the same sketch and make this exact device.
If you have a USB charger nearby, try sketching, measuring and modelling that one too.

NOTE: IF at any point something goes wrong, the easiest way to recover is just to press Ctrl+Z (Apple+Z) to undo.

Preparation: Paper Sketching

Here’s a scanned paper sketch of the DELL-brand USB charger we’ll be modelling: Note that dimensions were drawn in a different colour to the charger; colours make the sketch clearer.

  • Sketching helps clarify the mind’s view of what to make, and how to proceed.
  • Measuring and writing down distances beforehand makes modelling much faster – no need to stop and measure multiple times during the process.
  • Consider the purpose of the sketch when you draw it, and draw just enough to meet that purpose:
    • Does it need dimensions?
    • Does it need colour?
    • Does it need to be to scale?
    • How many angles are needed to capture the critical information?

Part A: Modelling the Plug End

Step 1: Sketch Plug Profile

  1. Create a sketch on the Front plane.
  2. Draw a circle on the canvas.
    (Press C  or go to Sketch > Circle > Centre Diameter Circle in the toolbar, click on the centre point, move the mouse away, click again to create)
    Set circle diameter to 40.6 mm.
    (Press D or go to Sketch > Dimension in the toolbar, click on the edge of the circle, move the mouse away, click again, type in the dimension)
  3. The circle is still blue, meaning it hasn’t been defined completely.
    We should lock it to the origin with a constraint.
    (Lines in a sketch turn from blue to black when they are completely defined/constrained/locked in place)
    Click on the centre of the circle. Then, hold Shift and click on the origin point.
    We’re now going to add a ‘Coincident’ constraint by clicking on the ‘Coincident’ icon in the Sketch Palette.
    (You could also right-click (mac: two-finger-click) in the canvas and choose ‘Coincident’ from the popup menu)
    Now that the round plug profile is fully defined, click on ‘Exit Sketch’ to leave sketch mode.

Step 2: Plug Extrusion

  1. Extrude the profile away from the front plane by 8.75 mm.
    (Press E or click on Extrude in the toolbar, then enter the dimension in the distance field)
    Confirm that the operation is ‘New Body’ and click Ok.

Step 3: Prong

  1. Create a new sketch on the front circular face.
    (Click on ‘Create Sketch’ in the toolbar, then click on the face)
  2. Draw a 3-point rectangle as shown.
    (Click on Sketch > Rectangle > 3-Point Rectangle, then draw three corners of a slanted rectangle)
  3. Give it dimensions of 6.5 mm x 1.5 mm.
    (Press D for dimension tool, click one line then click somewhere else, then type the value)

Step 4: Prongs

  1. The second prong will be added with a mirror operation.
  2. First we  project the face – this lets us refer to that existing shape inside this sketch. Press P for project tool (or find in Sketch > Project / Include > Project) to bring up the Project dialog.
  3. Click on the face to project it into the sketch, then click ‘Ok’.
  4. The sketch does not seem to have changed much, so let’s hide the plug body away. Click on the ‘lightbulb’ visibility button next to the Bodies to hide them.
    Now you will only see the sketch, and can see that a purple circle has been created.
    (Purple lines mean projected from outside the sketch. You can delete them, but can’t modify them)
  5. Next, we draw a vertical “centre” line from the origin up to the top of the circle.
    (Press L for the line tool or find in Sketch > Line in the toolbar)
    Notice the small icon that appears next to the line when it is near vertical. This is a Vertical constraint.
    Fusion 360 will automatically add constraints when it thinks appropriate.
    (If a constraint is added incorrectly, click on the bad constraint and press the Del key)
  6. Now the prong can be mirrored. Open the Sketch > Mirror tool in the toolbar.
    Select the four sides of the rectangle, either by clicking on each or by double-clicking one side.
    In the Mirror tool dialog select ‘Mirror Line’, then click on the centre line we drew earlier.
    A preview will appear. Make sure the mirrored prong looks right and complete, then click ‘Ok’.
  7. The prong lines are all blue, showing that they’re not fully defined yet.
    In the sketch the measurements were; 13 mm from the top of the plug, and 9.5 mm apart.
    (If you measured differently that is no problem, there are many ways to measure)
    Using the dimension tool (press D) click on the top of the plug and click on one prong.
    Notice that as you move the mouse around, the measurement applies in a different direction.
    Align the dimension to measure vertically, click again and enter the value.
    Do the same for the horizontal measurement.
    Finally, we need to specify the angle. Click on a line on one prong, then the other, then click between and type 60 degrees.
    The lines should all be fully-defined and black now. Exit the sketch.

Step 5: Prongs Extrusion and Fillet

  1. Extrude both profiles by 17.1 mm.
    (Press E or click on Extrude in the toolbar, then enter the dimension in the distance field)
  2. By default Fusion will Join features together, but the prongs should be separate bodies.
    Ensure that the extrusion operation is set to ‘New Body’ then press ok.
  3. Lastly, let’s round the ends of the prongs off slightly.
    Press F or click on Fillet in the toolbar.
    Select the four short edges of the prongs, then drag the arrow until they look right.
    (Or type in a value of 1.75 mm)

Part B: Charger Body

Step 6: Body Profile

  1. Swivel the view around and create a sketch on the back.
    (Click and drag on the View Cube until the back is visible, click on ‘Create Sketch’, then click on the face)
  2. Draw a centre rectangle of 43 x 27.5 mm at the origin.
    (Click on Sketch > Rectangle > Center Rectangle in the toolbar, click on the origin, expand the rectangle and click again)
    (Press D for dimension, enter the height and width as above)
  3. UH OH: When you hover over the rectangle, the wrong profile appears! The circle is interfering with the profile.
    We need to change it to a construction line.
    Click on the circle, then press X or click on the ‘Construction’ icon in the Sketch Palette.
    Now hover over the rectangle and the rectangular profile should appear.
  4. Extrude the rectangle 43.1 mm.
    (Press E or click on Extrude in the toolbar, then enter the dimension in the distance field)
  5. This time we do want it to join to the plug body, so select the ‘Join’ operation and press Ok.

Step 7: Body fillets

  1. The charger body is not a hard rectangle; it has rounded edges.
    Open the ‘Fillet’ tool with F or in the Modify menu.
  2. Select the four edges of the body, and fillet to a radius of 5.5 mm.
    Note: Once you add a radius value you are blocked from changing the edges. Hold down the Ctrl (Apple) key to temporary disable preview and let you add/remove edges.
  3. Press ‘Ok’ to apple the fillets.

Part C: USB Socket

Step 8: Sketch

  1. Create a sketch on the back surface of the charger.
    (Drag the ViewCube around until it is visible, then click ‘Create Sketch’ and select the face)
  2. Draw a centre rectangle on the sketch origin, 5.5 x 12.5 mm.
    Hint: You can dimension a shape as you draw it! Click once to begin it, then type the values with the keyboard and the Tab key before you click a second time.
  3. Draw a second 2-point rectangle inside the first.
    (If it’s in the wrong place initially, click and drag the rectangle to move it)
  4. Create a Midpoint constraint between the origin and the bottom line of the second rectangle.
    (Click on the line, Shift+Click on the origin, then click on the ‘Midpoint’ icon in the Sketch Palette)
  5. Add a 0.5mm dimension between the side and top of the first and second rectangles.
    The lines should all turn black.
  6. Exit the Sketch

Step 9: USB Socket

  1. Extrude both the profiles back 12 mm, using the Cut operation.
    (Press E or click on the Extrude tool, select both profiles, set distance to 12 mm, ensure operation is set to ‘Cut’, click Ok)
  2. Sketches automatically hide when they are used. Expand the ‘Sketches’ tree in the browser, and click on the lightbulb icon to show the last sketch.
  3. Extrude just the second rectangle by 12 mm, using the New Body operation.
    (Press E or click on the Extrude tool, select the smaller rectangle profile, set distance to 12 mm, ensure operation is set to ‘New Body’, click Ok)
  4. Hide the sketch again – click on the lightbulb a second time.

Part D: Finishing

Step 10: Labelling

It is important to think about how you might need to revisit a design.
Good practice is to label each part of the design – that way you or another collaborator know their purpose.

    1. Expand the ‘Bodies’ and ‘Sketches’ trees.
    2. Click on an element, then click again to bring up a text field.
    3. Give each element a sensible name.
    4. Hint:If you If you select multiple elements then rename one, all will be renamed.
  1. Now is a good time to save your document.

Step 11: Appearance

Let’s make it look good!
Fusion 360 has a number of built-in materials and finishes available.

  1. Open the Appearance dialog by pressing A or going to Modify > Appearance in the toolbar.
    The Appearance dialog has a section showing a list of materials currently in use, a search function, and a library of available materials.
  2. We’ll be using four materials – find each and drag them up into the ‘In This Design’ box:
    Plastic -> Opaque -> Plastic – Glossy (Black)
    Plastic -> Opaque -> Plastic – Rough (Black)
    Plastic -> Translucent -> ABS (White)
    Metal -> Steel -> Steel – Brushed Linear Long
  3. Click and drag the rough plastic material on to the main body.
  4. Drag the ABS and Steel onto the USB insides and the prongs.
  5. Lastly, the rear face of this USB charger is a glossy material.
    Change ‘Apply To’ mode to ‘Face’, then drag the glossy plastic material on to only the rear face of the charger.
  6. When you are happy with how the charger looks, click ‘Close’.


Tutorial complete! Good job.
Be sure to save your design.

If you prefer to see the modelling process in one video, it can be viewed below.

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