Altium Designer PCB Design Tutorial: Step-by-Step Guide for Beginners

When someone asks me which PCB design software they should learn for a career in electronics, my answer depends on their goals. For hobbyists, KiCad or EasyEDA makes sense. But if you’re aiming for a job in professional product development—especially in aerospace, medical devices, or consumer electronics—Altium Designer is often the expectation.

I’ve used Altium for over eight years across dozens of commercial products. It’s not the cheapest option (not even close), but there’s a reason it dominates professional PCB design. The unified environment, the component management, the MCAD integration—everything works together in ways that save serious time on complex projects.

This tutorial walks you through Altium Designer from project creation to manufacturing files. By the end, you’ll have designed a complete PCB and understand the workflow that professionals use daily.

What is Altium Designer?

Altium Designer is a comprehensive PCB design platform developed by Altium Limited. Unlike some tools that separate schematic capture and PCB layout into different applications, Altium integrates everything into a single unified environment.

The software handles:

Schematic capture: Creating electrical diagrams with component symbols and connections

PCB layout: Physical placement of components and copper trace routing

Component management: Libraries with real-time supply chain data

Simulation: SPICE-based circuit simulation

Signal integrity: Analysis tools for high-speed design

MCAD integration: Bi-directional communication with SolidWorks, Fusion 360, and other mechanical CAD tools

Manufacturing output: Gerber files, drill files, assembly documentation

Altium Designer Licensing and Cost

Let’s address the elephant in the room: Altium Designer is expensive. Current pricing runs approximately $7,000+ per year for a subscription or $12,000+ for a perpetual license.

However, several options exist for those who can’t justify the full price:

License Type	Cost	Best For
Full Subscription	~$7,000/year	Professional engineers, companies
Perpetual License	~$12,000+	Long-term users, companies
Student License	Free (6 months)	University students
Trial	Free (15 days)	Evaluation

Students can apply for a free educational license through Altium’s academic program. If you’re learning, this is the way to go.

Setting Up Altium Designer

Before diving into design, let’s configure the environment properly.

Installation and Licensing

Download Altium Designer from altium.com. During installation, you’ll need to sign in to your Altium account and activate your license. The software requires a stable internet connection for initial activation, though offline work is possible afterward.

Connecting to Altium 365 Workspace

Modern Altium workflows leverage Altium 365, a cloud platform for component management, collaboration, and design sharing. While you can work offline with local libraries, connecting to a Workspace provides significant advantages:

• Managed component libraries with verified footprints
• Real-time collaboration with team members
• Version control for design files
• Supply chain data integration

For this tutorial, we’ll assume you’re connected to a Workspace with sample data. If you’re working standalone, the steps remain similar, but you’ll use local libraries.

Configuring Preferences

Before starting, configure your environment:

1. Go to DXP > Preferences
2. Under Data Management > File Types, verify file associations
3. Under Schematic > General, set your preferred sheet sizes
4. Under PCB Editor > General, configure display options
5. Under System > View, adjust grid and cursor settings

Take time to explore the preferences. Small adjustments—like enabling push-and-shove routing or setting default trace widths—pay dividends later.

Creating Your First Altium Project

Every Altium design begins with a project. The project container holds all related files: schematics, PCB layout, libraries, output configurations, and documentation.

Step 1: Create a New PCB Project

1. Select File > New > Project > PCB Project
2. A new project appears in the Projects panel (PCB_Project1.PrjPcb)
3. Right-click the project and select Save Project As
4. Choose a location and name your project meaningfully

For this tutorial, we’ll design a simple LED flasher circuit—the classic astable multivibrator using two transistors.

Step 2: Add a Schematic Sheet

1. Right-click your project in the Projects panel
2. Select Add New to Project > Schematic
3. A blank schematic sheet opens
4. Save it immediately (File > Save As) with a descriptive name

The schematic editor opens with a blank sheet. The main menu bar and toolbars adapt to schematic editing mode—this context-sensitive interface is one of Altium’s strengths.

Schematic Capture in Altium Designer

Schematic capture is where your circuit takes shape. You’ll place component symbols and connect them with wires to define electrical relationships.

Configuring the Schematic Sheet

Before placing components, set up your sheet:

1. Right-click on the sheet and select Document Options
2. Set the sheet size (Letter or A4 for simple designs)
3. Configure the title block with your information
4. Set the grid (typically 10 mil for placement)

Finding and Placing Components

Altium provides multiple ways to access components:

Manufacturer Part Search (recommended):

1. Open Components panel (View > Panels > Components)
2. Type a part number (e.g., “2N3904” for an NPN transistor)
3. Browse results showing availability, pricing, and datasheets
4. Drag the component onto your schematic

Workspace Libraries:

1. In the Components panel, select your Workspace
2. Browse or search the managed library
3. Place components directly

Local Libraries:

1. Access via Design > Browse Libraries
2. Search installed libraries
3. Place components

For our multivibrator, we need:

• 2× NPN transistors (2N3904)
• 2× Resistors (470Ω for LED current limiting)
• 2× Resistors (47kΩ for base bias)
• 2× Capacitors (10µF for timing)
• 2× LEDs
• 1× 2-pin header (power input)

Placing Components

To place a component:

1. Select the component in the Components panel
2. Drag it onto the schematic sheet, or click Place button
3. Press Spacebar to rotate before placing
4. Press X to flip horizontally, Y to flip vertically
5. Click to place

Pro tip: Press Tab before placing to edit component properties (designator, value, etc.) without placing first.

Wiring the Schematic

With components placed, connect them with wires:

1. Select Place > Wire or press Ctrl+W
2. Click to start a wire at a component pin
3. Click to add corners
4. Click on the destination pin to complete the connection
5. Press Esc to exit wire mode

Altium automatically creates electrical connections when wires touch pins at the proper points. Watch for the small “X” that indicates a valid connection point.

Read more different PCB Design services:

Adding Net Labels

For complex schematics, net labels eliminate long wire runs:

1. Select Place > Net Label or press P, N
2. Type the net name (e.g., “VCC”, “GND”)
3. Place on the wire or pin

All net labels with the same name are electrically connected, even if they’re not visibly wired together.

Design Verification

Before moving to PCB layout, verify your schematic:

1. Run Project > Compile PCB Project
2. Review the Messages panel for errors and warnings
3. Fix any issues (unconnected pins, duplicate designators, etc.)

Common schematic errors:

• Floating input pins (use “No ERC” directive if intentional)
• Missing power connections
• Duplicate reference designators

PCB Layout in Altium Designer

With a verified schematic, you’re ready to create the physical board layout.

Step 1: Add a PCB Document

1. Right-click your project in the Projects panel
2. Select Add New to Project > PCB
3. Save the new PCB document

Step 2: Define the Board Shape

Every PCB needs a defined outline:

1. Select Design > Edit Board Shape
2. Click to place corners defining your board outline
3. Right-click and select Close when done

For a simple design, a 2″ × 2″ (50mm × 50mm) board works well.

Alternatively, use Design > Board Shape > Define from Selected Objects to create a board from a drawn rectangle or imported DXF.

Step 3: Configure the Layer Stack

Define your layer structure:

1. Go to Design > Layer Stack Manager
2. For a simple 2-layer board, the default works fine
3. For more layers, use the Add Layer tools
4. Set dielectric thicknesses and copper weights

A typical 2-layer stack:

• Top Layer (signal)
• Dielectric (core)
• Bottom Layer (signal)

Step 4: Import the Design

Transfer your schematic to the PCB:

1. Select Design > Import Changes From [Project Name]
2. The Engineering Change Order (ECO) dialog appears
3. Review the changes (component additions, net connections)
4. Click Validate Changes to check for errors
5. Click Execute Changes to import

Your components appear in a cluster near the board, connected by thin “ratsnest” lines showing required connections.

Step 5: Set Design Rules

Design rules ensure your board can be manufactured:

1. Open Design > Rules
2. Key rules to configure:
   1. Clearance: Minimum spacing between copper objects (typically 6-10 mil)
   1. Width: Trace widths (minimum and preferred)
   1. Routing Via Style: Via size and hole diameter
   1. Solder Mask Expansion: Mask clearance around pads

For prototype boards from services like JLCPCB or PCBWay:

Rule	Typical Value
Minimum Clearance	6 mil (0.15mm)
Minimum Track Width	6 mil (0.15mm)
Via Hole Size	0.3mm
Via Diameter	0.6mm
Annular Ring	0.15mm

Step 6: Component Placement

Good placement determines routing success. Strategy:

1. Place fixed components first: Connectors at board edges, LEDs where visible, mounting holes at corners
2. Place major components: ICs, transistors—the parts with the most connections
3. Place supporting components: Decoupling capacitors near ICs, resistors near their related components
4. Optimize: Minimize ratsnest line crossings

To move components:

• Click and drag
• Press Spacebar to rotate
• Press L to flip to the opposite layer

Use View > Fit Board to see your entire layout.

Step 7: Routing

Connect components with copper traces:

Interactive Routing (recommended):

1. Select Route > Interactive Routing or press Ctrl+W
2. Click on a pad to start routing
3. Move the mouse to define the trace path
4. Click to place corners
5. Click on the destination pad to complete

Routing tips:

• Press Spacebar to toggle trace angles (45° vs. 90°)
• Press Shift+Spacebar to change corner modes
• Press Tab to access routing options
• Use Backspace to undo the last segment
• Press + or – to change layers (through a via)

Push and Shove Routing: Enable in routing options to have traces push existing traces aside rather than blocking. This speeds up dense layouts significantly.

Step 8: Copper Pours (Ground Planes)

Add ground planes for better performance:

1. Select Place > Polygon Pour
2. Draw the polygon boundary
3. In the Polygon Pour dialog, set the Net to GND
4. Click OK, then Repour to fill

Ground planes reduce EMI, provide return paths for signals, and help with thermal management.

Step 9: Design Rule Check (DRC)

Verify your design before manufacturing:

1. Select Tools > Design Rule Check
2. Review the DRC report
3. Fix any violations (clearance errors, unconnected nets, etc.)

Common DRC errors:

• Clearance violations (traces too close)
• Unrouted nets (missing connections)
• Silk screen over pads
• Via too close to SMD pad

Step 10: 3D Visualization

Altium’s 3D view catches mechanical issues:

1. Press 3 or select View > 3D Layout Mode
2. Rotate with Shift + drag
3. Zoom with scroll wheel
4. Check component clearances and overall appearance

This view shows 3D models of components (if assigned) and reveals issues like colliding parts or wrong footprints.

Generating Manufacturing Output

Your design is complete. Now generate files for manufacturing.

Gerber Files

Gerbers are the industry standard for PCB fabrication:

1. Select File > Fabrication Outputs > Gerber Files
2. In the dialog, configure:
   1. Units: Inches or millimeters (match your design)
   1. Format: 2:5 (inches) or 4:3 (mm) precision
   1. Layers: Select all relevant layers
3. Click OK to generate

Standard Gerber layers:

• Top Copper
• Bottom Copper
• Top Solder Mask
• Bottom Solder Mask
• Top Silkscreen
• Bottom Silkscreen
• Board Outline

Drill Files

Generate drill data for holes:

1. Select File > Fabrication Outputs > NC Drill Files
2. Configure format settings
3. Generate files

Bill of Materials (BOM)

Create a component list:

1. Select Reports > Bill of Materials
2. Configure columns and grouping
3. Export to Excel or CSV

Assembly Outputs

For automated assembly:

1. File > Assembly Outputs > Pick and Place Files for component placement data
2. File > Assembly Outputs > Assembly Drawings for visual reference

Altium Designer Tips and Best Practices

After years of use, these practices save time and prevent problems.

Keyboard Shortcuts to Learn

Shortcut	Action
Ctrl+W	Interactive Routing
Ctrl+D	Open Preferences
P	Place menu
G	Set Grid
L	Flip component to other layer
Spacebar	Rotate component
Tab	Edit properties while placing
3	Toggle 3D view
Q	Toggle units (mm/mil)
Shift+S	Toggle single layer mode

Component Management Best Practices

• Use Workspace-managed components when possible
• Verify footprints against datasheets before layout
• Include 3D models for mechanical verification
• Keep BOMs current with supply chain data

Design Efficiency Tips

• Create design rule templates for reuse
• Use room definitions to group components
• Set up output job files for consistent manufacturing data
• Utilize project templates for common board types

Useful Resources for Altium Designer

Official Resources

Resource	URL	Description
Altium Documentation	altium.com/documentation	Complete reference
Altium Academy	academy.altium.com	Video courses
AltiumLive	altiumlive.com	Annual conference recordings

Community Resources

Resource	Description
Phil’s Lab (YouTube)	Excellent practical tutorials
Robert Feranec (YouTube)	High-speed design focus
Altium Forum	Official community support
Reddit r/PrintedCircuitBoard	Community discussion

Learning Path Recommendation

1. Complete the official Getting Started tutorial
2. Work through Phil’s Lab Altium beginner series
3. Design a simple project (LED flasher, sensor breakout)
4. Study the documentation for features you need
5. Tackle increasingly complex projects

Frequently Asked Questions

Is Altium Designer worth the cost?

For professionals whose work generates revenue, yes. The time savings on complex projects justify the investment. For hobbyists, free alternatives like KiCad offer most features you’ll need.

Can I run Altium Designer on Mac?

Not natively. Altium Designer is Windows-only. Mac users can run it via Boot Camp, Parallels, or VMware. Performance in virtual machines varies.

How does Altium compare to KiCad?

KiCad is free and capable, but Altium offers superior component management, better MCAD integration, more advanced routing tools, and professional support. For career development in certain industries, Altium experience is often expected.

Can I import designs from other tools?

Yes. Altium can import from EAGLE, KiCad, OrCAD, and other formats. Import quality varies—complex designs may need cleanup.

What’s the learning curve like?

Expect 2-4 weeks to become comfortable with basic operations, 2-3 months for proficiency, and 6+ months to master advanced features. The interface is logical once you understand the workflow.

Conclusion

Altium Designer is powerful, professional-grade software that rewards investment in learning. The unified environment, comprehensive feature set, and industry acceptance make it a valuable skill for electronics engineers.

Start simple. The LED flasher project in this tutorial demonstrates core workflows without overwhelming complexity. As you grow comfortable, explore advanced features: high-speed design rules, variant management, multi-board design, and simulation.

The cost barrier is real, but student licenses and trials provide entry points. If you’re serious about a career in electronics design, Altium proficiency opens doors.