Fusion 360 & SolidWorks - EEET2610

Overview

Computer-Aided Design (CAD) software is used in WP2 to design the mecanum robot’s mechanical structure, including the chassis, motor mounts, sensor brackets, and wheel assemblies. This course supports both Autodesk Fusion 360 (cloud-based, beginner-friendly) and SolidWorks (industry-standard, more advanced).

Fusion 360

Free for students, cloud-based, easy to learn, great for parametric design

SolidWorks

Industry-standard, powerful features, extensive simulation tools

Recommendation: Use Fusion 360 if you’re new to CAD. Use SolidWorks if you have prior CAD experience or need advanced simulation features.

Autodesk Fusion 360

Installation

Create Autodesk Account

Visit autodesk.com/educationClick Get started and create account with your RMIT email

Verify Student Status

Complete educational license verification:

Upload proof of enrollment (student ID or enrollment letter)
Or use RMIT institutional email for automatic verification

Download Fusion 360

Once verified, download Fusion 360 for your platform:

Windows 10/11 (x64, 8GB RAM minimum)
macOS 10.15+ (Intel or Apple Silicon, 8GB RAM minimum)

Fusion 360 is not available for Linux. Use Windows/macOS or run Windows VM.

Install Fusion 360

Windows/macOS: Run the installer and follow the wizardLogin with your Autodesk account when prompted

Verify License

Open Fusion 360 → Click your name (top-right) → About Fusion 360Should show “Educational License” with expiration ~1 year

Interface Overview

┌──────────────────────────────────────────────────────────┐
│ File | Design | Render | Animation | Tools   [Profile]   │  Toolbar
├──────────────────────────────────────────────────────────┤
│ CREATE  MODIFY  ASSEMBLE  CONSTRUCT  INSPECT             │  Design Toolbar
├──────┬───────────────────────────────────────────┬───────┤
│      │                                           │       │
│ Data │         Viewport                          │ Canvas│
│ Panel│  (3D model view)                          │ & Mk  │
│      │                                           │       │
│      │                                           │       │
├──────┴───────────────────────────────────────────┴───────┤
│ Timeline: [Sketch1] [Extrude1] [Fillet1] ...            │  History
└──────────────────────────────────────────────────────────┘

Key components:

Data Panel (left): Browse projects, files, and design components
Viewport (center): 3D visualization and modeling workspace
Canvas & Markups (right): Drawings and annotations (collapsed by default)
Toolbar (top): Design, Render, Simulation, Animation workspaces
Timeline (bottom): Design history (parametric, can edit past operations)

Basic Workflow

Create New Design

File → New Design (Ctrl+N / Cmd+N)Save immediately: File → Save (Ctrl+S / Cmd+S)Name: mecanum_chassis_v1

Create Sketch

Click CREATE → SketchSelect plane (XY, XZ, YZ) to draw onCommon sketch tools:

Rectangle (R): Draw rectangular profiles
Circle (C): Draw circular profiles
Line (L): Draw straight lines
Dimension (D): Add measurements and constraints

Add Constraints

Use constraints to define geometric relationships:

Horizontal/Vertical: Lock line orientation
Coincident: Connect points
Tangent: Smooth curve transitions
Dimensions: Specify exact sizes

Fully constrain sketches (all lines turn black) for parametric designs

Create 3D Features

Finish Sketch → Use creation tools:

Extrude (E): Convert 2D sketch to 3D solid
Revolve: Rotate sketch around axis
Sweep: Follow path with profile
Loft: Blend between multiple profiles

Modify Geometry

MODIFY toolbar:

Fillet: Round edges
Chamfer: Bevel edges
Shell: Hollow out solid
Mirror: Create symmetric copies
Pattern: Rectangular or circular arrays

Assemble Components

ASSEMBLE toolbar:

New Component: Create sub-assemblies
Joint: Connect parts with relationships (rigid, revolute, slider)
As-Built Joint: Align components in current positions
Contact Set: Define touching surfaces

Mecanum Chassis Example

Design sequence for robot base plate:

1. SKETCH (top XY plane)
   └─ Rectangle: 200mm × 200mm (chassis size)
   └─ 4× Circle: Ø5mm at corners (mounting holes)
   └─ Dimension constraints: 10mm from edges

2. EXTRUDE
   └─ Distance: 3mm (acrylic sheet thickness)
   └─ Operation: New Body

3. MODIFY → Fillet
   └─ Select 4 outer edges
   └─ Radius: 5mm (rounded corners for safety)

4. PATTERN (motor mount holes)
   └─ Rectangular pattern: 2×2 grid
   └─ Spacing: 150mm × 150mm

Result: Base chassis plate ready for assembly

Export for Manufacturing

3D Printing (STL)
Laser Cutting (DXF)
CNC Machining (STEP)
Drawings (PDF)

Right-click component in Browser
Save As STL
Settings:
- Format: Binary (smaller file size)
- Refinement: High
- Structure: One File Per Body
Upload to PrusaSlicer / Cura for slicing

Collaboration

# Share design with team members
1. Click Share icon (top-right)
2. Enter teammate's email
3. Set permissions:
   - View only (read-only)
   - Edit (full access)
4. Click Send invitation

# Version control (automatic in cloud)
File → Version History
- Fusion auto-saves every ~5 minutes
- Can restore previous versions
- See who made changes and when

SolidWorks

Installation (RMIT Students)

Access RMIT Software Portal

Visit RMIT Software DownloadLogin with RMIT credentials

Download SolidWorks

Select SolidWorks 2023 or laterDownload the full installation package (~15GB)

SolidWorks is Windows-only. macOS users must use Boot Camp or Parallels Desktop.

Install SolidWorks

Extract downloaded archive
Run setup.exe as Administrator
Choose installation type: Individual (on this computer)
Select products:
- ✓ SolidWorks (required)
- ✓ SolidWorks Simulation (recommended)
- ✓ PhotoView 360 (for rendering)
- ⬜ eDrawings (optional)

Activate License

Use RMIT network license server (on-campus or VPN required)Or request standalone educational license from RMIT IT

Interface Overview

┌──────────────────────────────────────────────────────────┐
│ File Edit View Insert Tools Window Help        [?] [×]   │  Menu Bar
├──────────────────────────────────────────────────────────┤
│ [≡] Sketch | Features | Assembly | ... [Search]          │  CommandManager
├─────────┬──────────────────────────────────────┬─────────┤
│         │                                      │         │
│ Feature │        Graphics Area                 │ Property│
│  Tree   │     (3D viewport)                    │ Manager │
│         │                                      │         │
│ ├─Base  │                                      │         │
│ ├─Hole  │                                      │         │
│ └─Fillet│                                      │         │
├─────────┴──────────────────────────────────────┴─────────┤
│ ◀ Ready                            [View tools]          │  Status Bar
└──────────────────────────────────────────────────────────┘

Key components:

Feature Tree (left): Shows design history and components
Graphics Area (center): 3D modeling viewport
PropertyManager (right): Context-sensitive tool settings
CommandManager (top): Tabbed toolbar (Sketch, Features, Assembly, etc.)

Basic Workflow

Create Part

File → New → Part (Ctrl+N)Select units: MMGS (millimeter, gram, second)Save as: chassis_plate.SLDPRT

Create Sketch

Select plane (Front, Top, Right)
Click Sketch tab → Sketch tool
Draw profile using:
- Rectangle: Corner/Center rectangle
- Circle: Center/Perimeter circle
- Line: Straight line segments
- Arc: 3-point or tangent arcs

Add Dimensions

Smart Dimension (D):

Click two points for distance
Click line for length
Click circle for diameter
Enter exact value in dialog

Fully define sketch (all entities turn black)

Create Features

Features tab:

Extruded Boss/Base: Create solid from sketch
Extruded Cut: Remove material
Revolved Boss/Base: Rotate sketch 360°
Fillet: Round edges
Chamfer: Bevel edges
Hole Wizard: Standard holes (M3, M4, etc.)

Create Assembly

File → New → Assembly (Ctrl+Shift+N)

Insert components: Insert Components → Browse to parts
Add mates:
- Coincident: Align faces/edges
- Concentric: Align cylindrical features
- Distance: Set spacing between components
- Angle: Set rotation between components

Design Best Practices

Design Intent

Start with sketches on standard planes (Front/Top/Right)
Use symmetry whenever possible
Build features in logical order (base → details)
Name features descriptively (not “Extrude1”, use “Motor Mount”)

Parametric Modeling

Use equations for related dimensions (e.g., "wheel_diameter"/2)
Create design tables for variants (different sizes)
Link dimensions to global variables
Avoid over-constraining sketches

Assembly Efficiency

Use sub-assemblies for repeated structures (e.g., wheel assembly)
Leverage patterns (circular, linear) for repeated components
Apply lightweight mode for large assemblies
Use configurations for multiple variants

File Management

Keep all files in single project folder
Use consistent naming: projectname_partname_v1.SLDPRT
Pack and go before sharing (includes references)
Back up regularly (SolidWorks doesn’t auto-save to cloud)

Simulation (Optional)

SolidWorks Simulation allows stress testing of mechanical designs:

Example: Motor mount bracket stress analysis

1. SIMULATION → Study Advisor → New Study
   └─ Type: Static (constant forces)

2. Apply fixtures (Fixed constraints)
   └─ Select mounting holes → Fixed Geometry

3. Apply external loads
   └─ Select motor mounting surface
   └─ Force: 10N downward (motor weight)

4. Mesh the model
   └─ Right-click Mesh → Create Mesh
   └─ Mesh density: Fine (smaller elements = more accurate)

5. Run simulation
   └─ Right-click study → Run

6. View results
   └─ Stress plot (von Mises)
   └─ Displacement plot
   └─ Factor of Safety (FOS)

Accept design if:
- Max stress < Material yield strength
- Factor of Safety > 2.0 (for student projects)

SolidWorks Simulation requires significant RAM (16GB+ recommended) and is optional for this course

CAD Comparison

Feature	Fusion 360	SolidWorks
Cost	Free (students)	Free (RMIT license)
Platform	Win, Mac	Windows only
Learning Curve	Beginner-friendly	Steeper (more powerful)
Cloud Storage	Built-in (auto-save)	Local files only
Collaboration	Easy (cloud sharing)	Manual (file exchange)
Rendering	Good (built-in)	Excellent (PhotoView)
Simulation	Basic (FEA add-on)	Advanced (built-in)
CAM (Manufacturing)	Integrated	Separate (SolidWorks CAM)
File Format	.f3d (proprietary)	.SLDPRT (industry std)
Industry Use	Startups, hobbyists	Automotive, aerospace

Bottom line:

New to CAD? → Use Fusion 360
Want industry skills? → Use SolidWorks
Need portability? → Use Fusion 360 (cloud)
Advanced simulation? → Use SolidWorks

Common CAD Tasks

Creating Motor Mount

Fusion 360
SolidWorks

1. Sketch on XY plane
   ├─ Rectangle: 40mm × 30mm (mount base)
   ├─ 4× Circle: Ø3mm (M3 mounting holes)
   └─ Dimension: 25mm × 20mm spacing

2. Extrude: 5mm (base plate thickness)

3. Sketch on top face
   └─ 2× Circle: Ø2mm (motor shaft holes)

4. Extrude Cut: -10mm (through motor mount)

5. Fillet: 2mm radius (all outer edges)

6. Export → STL for 3D printing

Creating Wheel Assembly

Assembly structure:

mecanum_robot_assembly.asm
├─ chassis_v1.prt
├─ wheel_assembly (sub-assembly) ×4
│  ├─ mecanum_wheel_v1.prt
│  ├─ motor_shaft_v1.prt
│  ├─ shaft_coupler_v1.prt
│  └─ M3_bolt.prt ×4
├─ motor_mount_v1.prt ×4
├─ raspberry_pi_mount_v1.prt
└─ lidar_bracket_v1.prt

Mates:
- Chassis (fixed reference)
- 4× Wheel assemblies (concentric to motor shafts)
- Motor mounts (coincident to chassis holes)
- Electronics mounts (distance offset from chassis)

Bill of Materials (BOM)

Generate parts list automatically: Fusion 360:

1. Open assembly
2. Tools → BOM
3. Select:
   - Structure: Parts Only (no sub-assemblies)
   - Columns: Part Name, Quantity, Material
4. Export → Excel/CSV

SolidWorks:

Open assembly
Insert → Tables → Bill of Materials
Place on drawing
Right-click table → Save As → Excel

Troubleshooting

Fusion 360: 'Login failed' or license issues

SolidWorks: 'Unable to obtain license' error

Solutions:

Connect to RMIT network (on-campus or VPN)
Check firewall allows SolidWorks license manager
Contact RMIT IT Support (ithelp@rmit.edu.au)
Verify correct license server in SolidWorks License Manager

Sketch won't fully define / turns blue

Symptoms: Can’t extrude sketch, dimensions don’t lock geometrySolutions:

Add missing dimensions (click Smart Dimension, select entities)
Add geometric constraints (horizontal, vertical, tangent, etc.)
Fix over-defined sketches (delete conflicting dimensions)
Check for duplicate/overlapping lines

Assembly mates fail or components move unexpectedly

Solutions:

Check mate types (Coincident ≠ Concentric)
Verify mate references (faces vs. edges vs. points)
Delete and recreate problematic mates
Use As-Built Mate (Fusion) or In Place Mate (SolidWorks) for pre-positioned parts
Suppress other mates temporarily to isolate issue

Model turns black / rendering issues

Symptoms: Viewport shows solid black or missing surfacesSolutions:

Reset graphics: View → Display → Reset Standard Views
Update graphics drivers (NVIDIA/AMD)
Disable hardware acceleration (if crashing)
- Fusion: Preferences → General → Graphics
- SolidWorks: Tools → Options → Performance
Check for corrupted geometry (use Check Entity tool)

Exported STL has gaps or errors

Symptoms: 3D printer slicer reports non-manifold edgesSolutions:

Fusion 360:
- Check mesh refinement: High (before export)
- Tools → Inspect → Interference Detection
- Repair: Modify → Mesh → Repair
SolidWorks:
- Tools → Evaluate → Check
- File → Print3D → Preview to validate
- Increase export resolution in STL options
Use external repair tool: Meshmixer or Microsoft 3D Builder

Learning Resources

Fusion 360

Official Tutorials

Autodesk’s free video courses for beginners

YouTube: Learn Fusion 360

Comprehensive channel with project-based learning

Fusion 360 Shortcuts

Essential shortcuts:

E: Extrude
R: Rectangle
C: Circle
L: Line
D: Dimension
S: Sketch
Shift+S: Section view

Community Forum

Ask questions and share designs

SolidWorks

SolidWorks Tutorials

Built-in tutorials: Help → SolidWorks Tutorials

YouTube: SolidWorks

Official channel with tips and techniques

CSWP Certification

Certified SolidWorks Professional exam for students (free via RMIT)

GrabCAD Library

Download free CAD models (motors, sensors, fasteners)

Next Steps

CAD Design Guide

Step-by-step mecanum chassis design tutorial

Mechanical Assembly

Assemble 3D printed and laser-cut parts

Bill of Materials

Complete parts list for the robot

PCB Design

Learn EasyEDA for electrical design

References

Fusion 360 Documentation
SolidWorks Help
McMaster-Carr CAD Library - Download 3D models of standard parts
Thingiverse - Community 3D printing models

Hardware

Software Tools

ROS2 Concepts

Code Examples

​Overview

Fusion 360

SolidWorks

​Autodesk Fusion 360

​Installation

​Interface Overview

​Basic Workflow

​Mecanum Chassis Example

​Export for Manufacturing

​Collaboration

​SolidWorks

​Installation (RMIT Students)

​Interface Overview

​Basic Workflow

​Design Best Practices

Design Intent

Parametric Modeling

Assembly Efficiency

File Management

​Simulation (Optional)

​CAD Comparison

​Common CAD Tasks

​Creating Motor Mount

​Creating Wheel Assembly

​Bill of Materials (BOM)

​Troubleshooting

​Learning Resources

​Fusion 360

Official Tutorials

YouTube: Learn Fusion 360

Fusion 360 Shortcuts

Community Forum

​SolidWorks

SolidWorks Tutorials

YouTube: SolidWorks

CSWP Certification

GrabCAD Library

​Next Steps

CAD Design Guide

Mechanical Assembly

Bill of Materials

PCB Design

​References

Overview

Autodesk Fusion 360

Installation

Interface Overview

Basic Workflow

Mecanum Chassis Example

Export for Manufacturing

Collaboration

SolidWorks

Installation (RMIT Students)

Interface Overview

Basic Workflow

Design Best Practices

Simulation (Optional)

CAD Comparison

Common CAD Tasks

Creating Motor Mount

Creating Wheel Assembly

Bill of Materials (BOM)

Troubleshooting

Learning Resources

Fusion 360

SolidWorks

Next Steps

References