Fusion 360 Basics

Class outline and student handout.

Fusion 360 Basics Class Outline

Fusion 360 Basics: From Sketch to Solid

Class flow at a glance

Time Section Length
0:00 Welcome and UI orientation 10 min
0:10 Sketching fundamentals 25 min
0:35 Extrude and fillet 15 min
0:50 Sketching on faces and cutting 20 min
1:10 Guided project: phone stand 15 min
1:25 Wrap-up and next steps 5 min

Before class: setup email

Send this to registered students one week before class and again the day before:

Subject: Fusion 360 Class Prep: Please Do This Before Class

Hi! Looking forward to seeing you at the Fusion 360 Basics class. To make the most of our 90 minutes together, please complete these two steps before you arrive:

  1. Create a free Autodesk account at https://www.autodesk.com/products/fusion-360/personal. Choose the "Personal Use" license (free for hobbyists and non-commercial use). You'll need a valid email address.
  2. Download and install Fusion 360. After creating your account, download the installer, run it and sign in with your new account. Open Fusion 360 once to make sure it loads (it may take a minute the first time).

If you get stuck, no worries: arrive 15 minutes early and we'll help you get set up.

Bring: a laptop with a mouse. Fusion 360 works with a trackpad, but a mouse makes 3D navigation much easier.

Section 1: Welcome and UI orientation (10 min)

Opening (2 min)

Start with a finished model on screen: something simple but impressive, like a custom bracket or enclosure that was 3D printed.

Key point: "This was made entirely in Fusion 360, starting from a blank canvas. By the end of today, you'll understand every technique that went into making it."

Set expectations

UI tour (8 min)

Walk through these with everyone's Fusion 360 open.

The toolbar (top)

The browser panel (left)

The timeline (bottom)

Navigation (critical)

Practice moment: "Everyone orbit around. Zoom in and out. Pan left and right. If you ever get lost and your model disappears, click the house icon to reset your view."

Section 2: Sketching fundamentals (25 min)

Why sketching matters (2 min)

Key concept: "Everything in Fusion 360 starts as a 2D sketch. You draw a flat shape, then you pull it into 3D. The quality of your 3D model depends on the quality of your sketch. This is the most important section of the class."

Analogy: "Think of a cookie cutter. The sketch is the cutter shape. Extruding is pressing it into the dough. If your cutter shape is sloppy, your cookie is sloppy."

Starting a sketch (3 min)

  1. Click Create Sketch in the toolbar.
  2. Fusion asks you to pick a plane; three planes appear (XY, XZ, YZ).
  3. "For now, always pick the bottom plane (XZ). It's the one that looks like a floor."
  4. Click the XZ plane.

What just happened: "You're now in sketch mode. The toolbar changed: you have sketch tools like Line, Rectangle and Circle, and a grid appeared. That's your sketching surface."

Common mistake to head off: "You'll know you're in sketch mode because you see 'Finish Sketch' in the toolbar. If you try to draw and nothing happens, check whether you're actually in a sketch."

Drawing basic shapes (8 min)

Rectangle

  1. Click Rectangle, then 2-Point Rectangle.
  2. Click once near the origin to place the first corner.
  3. Move the mouse and click again to place the opposite corner.
  4. "Don't worry about exact size yet. Just get a rectangle on screen."

Add dimensions:

  1. Click Sketch Dimension (or press D).
  2. Click one side of the rectangle, then click to place the dimension.
  3. Type 60 and press Enter. That side is now 60 mm.
  4. Repeat for the other side: 40.

Key concept: constrained vs unconstrained

Show what unconstrained looks like:

Circle

  1. Click Circle, then Center Diameter Circle.
  2. Click to place the center.
  3. Move outward and click, or type a diameter.
  4. Add a dimension: 20.

Practice moment (2 min): "Delete everything in your sketch (Ctrl+A to select all, then Delete). Now draw an 80 mm x 50 mm rectangle on your own. When you're done, your lines should be black. Raise your hand if they're still blue."

Constraints: the big three (5 min)

"Dimensions control size. Constraints control relationships between things."

Coincident: "These two points are the same point."

Horizontal/Vertical: "This line must be perfectly flat or perfectly upright."

Equal: "These two things must be the same size."

Key point: "You won't often apply constraints by hand. Fusion applies them automatically as you draw: a line that looks horizontal is made horizontal. Knowing they exist helps you understand why things snap, and how to fix a sketch that misbehaves."

Finish the sketch (2 min)

  1. Click Finish Sketch (green checkmark in the toolbar, or right-click and choose Finish Sketch).
  2. "You're back in 3D space. Your sketch still exists; see it in the browser panel."

Common mistake to head off: "Always finish your sketch before you extrude. If Extrude is grayed out, you're probably still in a sketch."

Section 3: Extrude and fillet (15 min)

Extrude: pulling 2D into 3D (10 min)

Key concept: "Extrude takes a closed 2D shape and stretches it into the third dimension. It's the most-used tool in Fusion 360."

Basic extrude

  1. Click Extrude (or press E).
  2. Click your rectangle sketch; it highlights in blue.
  3. Drag the arrow upward, or type 20 in the distance field.
  4. Click OK.

Pause and celebrate: "You just made your first 3D solid. Orbit around it. It's a real object now."

Symmetric extrude

  1. Undo the extrude.
  2. Click Extrude again and select the rectangle.
  3. Change Direction from "One Side" to Symmetric.
  4. Type 20 (10 mm each way, 20 mm total).
  5. Click OK.

Why it matters: "Symmetric extrude builds equally above and below the sketch plane. It keeps your model centered, which makes later steps easier. Get in the habit."

What about that circle?

If the sketch has both a rectangle and a circle: "When you hover over the sketch during Extrude, Fusion highlights individual regions, not the whole sketch. You can pick the rectangle without the circle, or both."

Fillet: rounding edges (5 min)

Key concept: "Fillet rounds off sharp edges. It takes five seconds and makes everything look far more professional."

  1. Click Fillet (in the Modify menu, or press F).
  2. Click an edge of the box.
  3. Type 3 for a 3 mm radius.
  4. Click OK.

The "wow" moment: "One rounded edge and it already looks like a real product instead of a blocky box."

Let them experiment (2 min): "Try different edges, a bigger radius, or several edges at once (keep clicking edges before you hit OK). What happens if the radius is too big?"

Common mistake to head off: "If Fusion gives you an error when filleting, the radius is probably too large for the shape. Make it smaller."

Section 4: Sketching on faces and cutting (20 min)

The key concept (2 min)

"So far you've sketched on a flat plane in empty space. You can also sketch directly on the face of a 3D object. That's how you add holes, pockets, slots and engravings."

Sketch on a face (8 min)

  1. Click Create Sketch.
  2. Instead of a plane, click the top face of your box.
  3. "You're sketching on the surface of your object now."

Draw a circle on the top face:

  1. Select Circle.
  2. Click on the top face to place the center.
  3. Type 10 for a 10 mm diameter.
  4. Optionally add dimensions to position it from the edges.
  5. Finish Sketch.

Extrude as cut (8 min)

  1. Click Extrude.
  2. Click the circle on the top face.
  3. Drag the arrow down into the box (or type a negative value such as -10).
  4. Check that Operation says Cut. "Fusion usually suggests Cut when you extrude into a body, but always double-check."
  5. Click OK.

Pause and orbit: "You just made a pocket in your box. Orbit underneath: it's a real pocket, not a mark on the surface."

The concept landing: "This is the core Fusion workflow: sketch, extrude, sketch on a face, cut. Repeat that cycle to add detail. Holes, pockets, slots and channels are all extrude-as-cut from a sketch on a face."

Try a second cut (5 min)

  1. Create Sketch on a side face of the box.
  2. Draw a rectangle, about 30 mm x 5 mm, near the bottom.
  3. Finish Sketch.
  4. Extrude as a cut going through the box: in the Extent menu choose All instead of typing a distance. "This cuts all the way through, however thick the box is."
  5. Click OK.

Result: "A box with a pocket on top and a slot through the side. That's already a useful part: a cable organizer, a bracket, a pen holder."

Section 5: Guided project: phone stand (15 min)

Build a simple angled phone stand that ties together sketch, extrude, sketch on face, cut and fillet. Show a picture or a printed example of the finished stand first so students know where they're heading.

Step 1: Base (3 min)

  1. Create Sketch on the XZ plane (the floor).
  2. Draw a rectangle: 70 mm x 80 mm.
  3. Finish Sketch.
  4. Extrude symmetrically: 10 mm (5 mm each way).

Result: a flat base, 70 x 80 x 10 mm.

Step 2: Back support (3 min)

  1. Create Sketch on the back face of the base (the 70 mm x 10 mm face).
  2. Draw a rectangle from the top-left corner of the face: 70 mm wide x 60 mm tall. Use a coincident constraint or simply start at the corner.
  3. Finish Sketch.
  4. Extrude 10 mm away from the base.

Result: an L shape, the base with a tall back wall.

Step 3: Phone slot (3 min)

  1. Create Sketch on the top face of the base.
  2. Draw a rectangle near the back wall: 50 mm x 4 mm, about 5 mm from the back face.
  3. Finish Sketch.
  4. Extrude as Cut: -8 mm. That leaves a 2 mm floor, so it's a slot and not a hole.

Result: a slot for the bottom edge of the phone.

Step 4: Fillet the edges (2 min)

  1. Click Fillet.
  2. Select the top edges of the back support, radius 5 mm.
  3. Click OK.
  4. Optionally fillet the outer bottom edges of the base: 3 mm.

Result: a finished-looking phone stand.

Step 5: Make it yours (4 min, if time allows)

If you're running behind, skip Step 5. The stand is complete at Step 4.

Section 6: Wrap-up and next steps (5 min)

Celebrate what they built

"Look at the timeline. Count the steps. You went from an empty canvas to a working object with four core tools: sketch, extrude, cut and fillet."

The workflow

Write this on the board or show it on screen:

1. SKETCH a 2D shape
2. EXTRUDE it into 3D
3. SKETCH on a face
4. CUT to add detail
5. FILLET to finish
6. Repeat 3 to 5 until done

"This workflow handles most of what you'll ever want to model."

Show the timeline superpower

"Every step remembers how it relates to the steps before it. Change one dimension and the model adapts. That's parametric modeling, and it's a topic for next time."

What to learn next

  1. Components: organizing multi-part models (essential for assemblies)
  2. User parameters: named variables that drive your dimensions
  3. Patterns: circular and rectangular repeats
  4. Joints: connecting components so they move realistically
  5. Export for 3D printing: File, Export, STL

Resources

Tease the next class

"If there's interest, the next class would cover components, user parameters and multi-part assemblies: designing things that fit together."

Instructor notes

Before-class checklist

Pacing tips

Common student problems

Problem Cause Fix
"I can't see my sketch" The view is edge-on to the sketch plane Click Home on the view cube, or "Look At" on the sketch in the browser
"Extrude is grayed out" Still inside a sketch Click Finish Sketch first
"My extrude didn't cut" Operation was New Body or Join Undo, redo the extrude, set Operation to Cut
"My sketch lines are still blue" Sketch not fully constrained Add dimensions or constraints. For this class it still extrudes
"I can't select the face" Clicking an edge instead of a face Zoom in and hover until the face highlights
"My model disappeared" A body got hidden, or the view zoomed too far Check the eye icons in the browser panel, or click Home
"I made two bodies by accident" Extrude created a new body instead of joining or cutting Undo and redo with the right Operation

If you're short on time

  1. Skip the second cut in Section 4 (saves 5 minutes).
  2. Build only the base, back wall and fillets for the phone stand (saves 5 minutes).
  3. Show just one fillet example (saves 2 minutes).

If you have extra time

  1. Let students customize their stand (charging hole, rounded back, wider base).
  2. Show how to export an STL and send it to one of the makerspace's 3D printers (students need a check-off before printing on their own).
  3. Demo the Revolve tool: sketch a profile and spin it around an axis to make a bowl or vase.
  4. Let students start a second object of their choice with your help.

Appendix A: Pre-class setup

System requirements

Installation

  1. Go to https://www.autodesk.com/products/fusion-360/personal.
  2. Click "Get Started" or "Download Free".
  3. Create an Autodesk account, or sign in.
  4. Choose "Personal Use" as the license type.
  5. Download the installer for your operating system.
  6. Run it. It downloads more components, which can take 5 to 10 minutes.
  7. Launch Fusion 360 and sign in.

Troubleshooting

Appendix B: Keyboard shortcuts

Print and hand out, or show on a second screen.

Shortcut Action
S Search (find any tool by name)
L Line
C Circle
R Rectangle
D Sketch Dimension
E Extrude
F Fillet
Q Push/Pull
M Move/Copy
Cmd+Z / Ctrl+Z Undo
Cmd+Shift+Z / Ctrl+Y Redo
Middle mouse Orbit
Shift + middle mouse Pan
Scroll wheel Zoom

Tip: press S and type a tool's name. It's the fastest way to find anything when you forget where a button lives.

Appendix C: Phone stand dimensions

For students who need to catch up or rebuild at home.

BASE
  Width:   70 mm
  Depth:   80 mm
  Height:  10 mm (symmetric extrude)

BACK SUPPORT
  Width:   70 mm (same as base)
  Height:  60 mm
  Depth:   10 mm (extruded from the back face)

PHONE SLOT
  Width:   50 mm (centered on the base)
  Depth:    4 mm
  Cut:      8 mm deep (leaves a 2 mm floor)
  Position: 5 mm from the back wall

FILLETS
  Back support top edges: 5 mm
  Base bottom edges:      3 mm (optional)

Student Handout

The take-home cheat sheet for the Fusion 360 Basics class. The same sheet is in the Digital Fabrication book as the Fusion 360 Cheat Sheet.

The core workflow

You will repeat this for almost everything you build in Fusion 360:

1. SKETCH a 2D shape on a plane or face
2. EXTRUDE it into 3D (add material)
3. SKETCH on a face of your 3D object
4. CUT to remove material (extrude inward)
5. FILLET to round edges and finish
6. Repeat steps 3 to 5 to add detail

Keyboard shortcuts

Shortcut Action
S Search (find any tool by name)
L Line
C Circle
R Rectangle
D Sketch Dimension
E Extrude
F Fillet
Q Push/Pull
M Move/Copy
Ctrl+Z / Cmd+Z Undo

Tip: press S and type a tool's name. It's the fastest way to find anything.

Mouse navigation

Action Control
Orbit Middle mouse button
Pan Shift + middle mouse button
Zoom Scroll wheel
Reset view Click the house icon on the view cube (top right)

The class project: phone stand

Dimensions are included so you can rebuild it at home.

Step 1: Base

  1. Create Sketch on the XZ plane (the floor).
  2. Draw a rectangle: 70 mm x 80 mm.
  3. Finish Sketch.
  4. Extrude (Symmetric): 10 mm.

Step 2: Back support

  1. Create Sketch on the back face (the 70 mm x 10 mm face).
  2. Draw a rectangle from the top-left corner: 70 mm wide x 60 mm tall.
  3. Finish Sketch.
  4. Extrude: 10 mm, away from the base.

Step 3: Phone slot

  1. Create Sketch on the top face of the base.
  2. Draw a rectangle: 50 mm x 4 mm, 5 mm from the back wall.
  3. Finish Sketch.
  4. Extrude as Cut: -8 mm (leaves a 2 mm floor).

Step 4: Fillet

  1. Select Fillet (or press F).
  2. Click the top edges of the back support, radius 5 mm.
  3. Optionally fillet the bottom edges of the base: 3 mm.

Dimensions

BASE:           70 x 80 x 10 mm
BACK SUPPORT:   70 x 60 x 10 mm
PHONE SLOT:     50 x 4 mm, 8 mm deep cut
FILLETS:        5 mm (top), 3 mm (bottom)

Stuck? Check here first

Problem Fix
Can't see my sketch Click the Home icon on the view cube
Extrude is grayed out Click Finish Sketch first
Extrude didn't cut Undo, redo the extrude, set Operation to Cut
Sketch lines are still blue Add dimensions to fully constrain it (it still works if you don't)
Can't select a face Zoom in and hover until the face highlights, not an edge
Model disappeared Check the eye icons in the browser panel (left side)

What to learn next

  1. Components: organizing multi-part models
  2. User parameters: named variables for dimensions
  3. Patterns: repeat features in circles or grids
  4. STL export: File, Export, STL to 3D print your designs

Resources