John: Created page with "{{Tutorial |name=KiCad Tutorial |competency=PCB Design |difficulty=Beginner |time=3-6 hours (spread across multiple sessions) |prerequisites=Electronics Fundamentals - Understanding of circuits, components, schematics |materials=KiCad (free download), computer, practice project (LED breakout board) |next_steps=Design custom board for your robot, study SimpleBot PCB design, order boards from JLCPCB }} '''KiCad Tutorial''' is your complete guide to designing y..."

2025-10-11T20:14:29Z

Created page with "{{Tutorial |name=KiCad Tutorial |competency=PCB Design |difficulty=Beginner |time=3-6 hours (spread across multiple sessions) |prerequisites=Electronics Fundamentals - Understanding of circuits, components, schematics |materials=KiCad (free download), computer, practice project (LED breakout board) |next_steps=Design custom board for your robot, study SimpleBot PCB design, order boards from JLCPCB }} '''KiCad Tutorial''' is your complete guide to designing y..."

New page

{{Tutorial
|name=KiCad Tutorial
|competency=[[PCB Design]]
|difficulty=Beginner
|time=3-6 hours (spread across multiple sessions)
|prerequisites=[[Electronics Fundamentals]] - Understanding of circuits, components, schematics
|materials=KiCad (free download), computer, practice project (LED breakout board)
|next_steps=Design custom board for your robot, study [[SimpleBot]] PCB design, order boards from JLCPCB
}}

'''KiCad Tutorial''' is your complete guide to designing your first printed circuit board (PCB) from start to finish. This tutorial walks you through KiCad, a free and powerful PCB design tool, using a simple LED breakout board project.

By the end of this tutorial, you'll:
* Install and configure KiCad
* Create a schematic with components and connections
* Assign footprints to components
* Layout a PCB with proper trace routing
* Generate Gerber files for manufacturing
* Order your PCB from an online manufacturer

This tutorial is '''hands-on'''. You'll design a complete, manufacturable PCB that you can order and assemble.

== Part 1: Installing KiCad ==

=== Download and Install ===

# Visit [https://www.kicad.org/download/ KiCad Downloads]
# Download the latest stable version for your operating system
# Run the installer (accept defaults)
# Launch KiCad

'''Note''': This tutorial uses KiCad 7.x or 8.x. Interface may differ slightly in older versions.

=== First Launch Setup ===

When you first launch KiCad:
# Select default library paths (click OK/Next)
# KiCad will download symbol and footprint libraries (this may take a few minutes)
# You'll see the KiCad project manager window

=== Understanding KiCad's Interface ===

KiCad has several tools (all launched from the project manager):
* '''Schematic Editor''' - Draw circuit diagrams
* '''Symbol Editor''' - Create/edit component symbols
* '''PCB Editor''' - Layout physical board
* '''Footprint Editor''' - Create/edit component footprints
* '''Gerber Viewer''' - Preview manufacturing files

'''Workflow''': Schematic → Footprint Assignment → PCB Layout → Gerber Export

== Part 2: Creating a New Project ==

=== Project: LED Breakout Board ===

We'll design a simple LED breakout board:
* '''Input''': 5V and GND via screw terminal
* '''Components''': Current-limiting resistor, LED, header pins for output
* '''Output''': LED indicator, 5V/GND headers for connecting to other boards

This teaches fundamental PCB design skills without overwhelming complexity.

=== Create the Project ===

# Click '''File → New Project'''
# Name it: <code>led_breakout</code>
# Choose a location to save it
# Click '''Create'''

You'll see two files created:
* <code>led_breakout.kicad_sch</code> - Schematic file
* <code>led_breakout.kicad_pcb</code> - PCB layout file

== Part 3: Schematic Design ==

=== Launch the Schematic Editor ===

# Double-click <code>led_breakout.kicad_sch</code> in the project manager
# You'll see a blank grid with a title block in the corner

=== Adding Components (Symbols) ===

We need these components:
* 1× LED
* 1× Resistor (220Ω)
* 1× Screw terminal (2-position)
* 1× Pin header (1×3, for 5V/LED/GND output)
* Power symbols (VCC, GND)

'''Adding the LED:'''
# Press '''A''' (Add symbol shortcut) or click the "Place Symbol" icon
# Type "LED" in the search box
# Select '''Device:LED''' from the list
# Click to place it on the schematic (middle of the grid)
# Press '''ESC''' to exit placement mode

'''Adding the resistor:'''
# Press '''A''' again
# Type "R" in the search box
# Select '''Device:R''' (resistor)
# Place it to the left of the LED
# Press '''ESC'''

'''Adding the screw terminal:'''
# Press '''A'''
# Type "screw terminal" or "conn_01x02"
# Select '''Connector:Screw_Terminal_01x02''' (2-position terminal)
# Place it on the far left
# Press '''ESC'''

'''Adding the output header:'''
# Press '''A'''
# Type "conn_01x03"
# Select '''Connector_Generic:Conn_01x03''' (3-pin header)
# Place it on the far right
# Press '''ESC'''

'''Adding power symbols:'''
# Press '''P''' (Power symbol shortcut)
# Type "VCC"
# Select '''power:VCC'''
# Place above the screw terminal
# Press '''P''' again
# Type "GND"
# Select '''power:GND'''
# Place below the screw terminal and near the LED

Your schematic should have: screw terminal (left) → resistor → LED → header (right), with VCC/GND symbols.

=== Connecting Components (Wiring) ===

Now connect the components with wires (nets):

# Press '''W''' (Wire tool) or click "Place Wire" icon
# Click on the screw terminal pin 1 (top pin)
# Click on the VCC symbol (creates a connection)
# Press '''ESC''' to exit wire mode

Repeat for all connections:
* Screw terminal pin 1 → VCC symbol
* Screw terminal pin 2 → GND symbol (bottom)
* VCC → Resistor pin 1 (left side)
* Resistor pin 2 (right side) → LED anode (top pin, triangle side)
* LED cathode (bottom pin, bar side) → GND
* VCC → Header pin 1
* LED anode → Header pin 2 (LED output)
* GND → Header pin 3

'''Tips:'''
* Wires connect when you click directly on a pin (pink circle appears)
* Press '''ESC''' to cancel wire placement
* Move components with '''M''' (grab and move)

=== Annotating Components ===

Components need unique reference designators (R1, D1, J1):

# Click '''Tools → Annotate Schematic'''
# Click '''Annotate''' button (uses defaults)
# Click '''Close'''

Your components now have designators:
* J1 (screw terminal)
* R1 (resistor)
* D1 (LED)
* J2 (header)

=== Setting Component Values ===

Assign values to resistor and LED:

# Hover over R1 and press '''V''' (Value shortcut)
# Type "220" (220 ohms)
# Press '''Enter'''
# Hover over D1 and press '''V'''
# Type "Red LED" or just "LED"
# Press '''Enter'''

=== Adding Title Block Information ===

# Click '''File → Page Settings'''
# Fill in:
** Title: "LED Breakout Board"
** Date: (auto-filled)
** Revision: "1.0"
** Company: (your name or "BRS")
# Click '''OK'''

=== Electrical Rules Check (ERC) ===

Check for errors before moving to PCB layout:

# Click '''Inspect → Electrical Rules Checker'''
# Click '''Run ERC'''
# Review any errors or warnings
# Fix errors (warnings about unused pins are usually OK)
# Click '''Close'''

'''Common errors:'''
* Unconnected pins - Make sure all wires connect to pins (pink circle at connection)
* Missing power flags - Can ignore for this simple circuit

=== Save Your Schematic ===

# Press '''Ctrl+S''' or click '''File → Save'''

Your schematic is complete! Next: assign footprints.

== Part 4: Footprint Assignment ==

=== Understanding Footprints ===

'''Schematic symbols''' show logical connections (how components connect).
'''Footprints''' show physical layout (where pads/holes are on the PCB).

Each component needs a footprint:
* LED → 5mm through-hole LED footprint
* Resistor → Axial resistor footprint
* Screw terminal → 5mm pitch screw terminal
* Header → 2.54mm pin header

=== Open Footprint Assignment Tool ===

# In schematic editor, click '''Tools → Assign Footprints'''
# You'll see a list of components on the left, libraries in the middle, footprints on the right

=== Assigning Footprints ===

For each component, select it (left column), then double-click the footprint (right column):

'''J1 (Screw Terminal):'''
# Select J1 in left column
# Middle column: scroll to '''TerminalBlock_Phoenix'''
# Right column: double-click '''TerminalBlock_Phoenix_MKDS-1,5-2_1x02_P5.00mm_Horizontal'''
# This is a 2-position, 5mm pitch screw terminal

'''R1 (Resistor):'''
# Select R1
# Middle column: scroll to '''Resistor_THT'''
# Right column: double-click '''R_Axial_DIN0207_L6.3mm_D2.5mm_P10.16mm_Horizontal'''
# This is a standard through-hole resistor footprint

'''D1 (LED):'''
# Select D1
# Middle column: scroll to '''LED_THT'''
# Right column: double-click '''LED_D5.0mm'''
# This is a standard 5mm LED footprint

'''J2 (Header):'''
# Select J2
# Middle column: scroll to '''Connector_PinHeader_2.54mm'''
# Right column: double-click '''PinHeader_1x03_P2.54mm_Vertical'''
# This is a 3-pin, 2.54mm pitch (0.1") header

=== Verify Assignments ===

All components should now have footprints listed in the left column. If any show "No Footprint", assign one.

# Click '''OK''' to save footprint assignments
# Close the footprint assignment window

=== Save and Update PCB ===

# In schematic editor, press '''Ctrl+S''' to save
# Click '''Tools → Update PCB from Schematic''' (or press '''F8''')
# Click '''Update PCB'''
# Click '''Close'''

This generates a netlist and sends it to the PCB editor.

== Part 5: PCB Layout ==

=== Open PCB Editor ===

# In project manager, double-click <code>led_breakout.kicad_pcb</code>
# You'll see a blank workspace

=== Import Components from Schematic ===

If you followed the "Update PCB from Schematic" step, components should already be imported. If not:

# In PCB editor, click '''Tools → Update PCB from Schematic'''
# Click '''Update PCB'''
# All components appear in a cluster near the origin

=== Setting Up the Board ===

Before placing components, set up the PCB:

'''Set design rules:'''
# Click '''File → Board Setup'''
# Left panel: click '''Constraints'''
# Set minimum values (for JLCPCB/PCBWay standard):
** Minimum Clearance: 0.2mm
** Minimum Track Width: 0.2mm
** Minimum Via Diameter: 0.8mm
** Minimum Via Drill: 0.4mm
# Click '''OK'''

'''Select layers:'''
For this beginner project, use 2 layers (F.Cu = top, B.Cu = bottom).

=== Drawing the Board Outline ===

Define the physical board shape:

# Select '''Edge.Cuts''' layer (dropdown in top toolbar)
# Click '''Draw a Rectangle''' tool (right toolbar)
# Click to start at (0, 0)
# Click to end at (40mm, 25mm) - creates a 40mm × 25mm rectangle
# This is your board outline

'''Tips:'''
* Grid helps with alignment (default 1mm is fine)
* Switch to '''mm''' units if needed (bottom status bar)

=== Placing Components ===

Arrange components logically on the board:

# Switch to '''F.Cu''' layer (top copper)
# Press '''M''' (move) and click a component to move it
# Press '''R''' while moving to rotate component

'''Suggested layout:'''
* J1 (screw terminal) - Left edge, centered vertically
* R1 (resistor) - Middle, horizontal orientation
* D1 (LED) - Right of resistor, vertical orientation
* J2 (header) - Right edge, vertical

'''Layout strategy:'''
* Inputs (screw terminal) on one side
* Outputs (header) on opposite side
* Flow left-to-right matches schematic

=== Routing Traces (Connecting Components) ===

'''Ratsnest lines''' (thin white lines) show which pads need to be connected.

# Select '''F.Cu''' layer
# Press '''X''' (Route tracks tool)
# Click on a pad to start a trace
# Follow the ratsnest line to the destination pad
# Click on destination pad to complete connection
# Press '''ESC''' to finish

Route all connections:
* J1 pin 1 → R1 left pad (this is the VCC net)
* R1 right pad → D1 anode (top pad)
* D1 cathode → J1 pin 2 (GND net)
* Branch VCC to J2 pin 1
* Branch LED anode to J2 pin 2
* Branch GND to J2 pin 3

'''Trace width:'''
* For this low-current circuit, default 0.25mm traces are fine
* To change: Press '''W''' while routing to cycle through widths

'''Tips:'''
* Route on F.Cu (top) layer when possible
* Use vias to switch layers if traces cross (press '''V''' while routing)
* Press '''/''' while routing to switch between 45° and free-angle modes

=== Adding a Ground Plane (Copper Pour) ===

A ground plane improves power distribution and reduces noise:

# Select '''F.Cu''' layer
# Press '''Ctrl+Shift+Z''' (Add filled zone tool) or click "Add Filled Zone" icon
# Click to start zone around the board edge
# Follow the board outline (click each corner)
# Double-click to close the zone
# In the dialog:
** Net: select '''GND'''
** Clearance: 0.3mm
** Minimum width: 0.2mm
# Click '''OK'''

The ground plane fills all unused copper with GND connection.

# Press '''B''' to rebuild all copper zones

Repeat for bottom layer (B.Cu) if desired (also connect to GND).

=== Adding Mounting Holes ===

Mounting holes let you attach the PCB to a chassis:

# Press '''Ctrl+Shift+A''' (Add footprint) or click "Add Footprint" icon
# Type "MountingHole"
# Select '''MountingHole:MountingHole_3.2mm_M3'''
# Place in four corners (inside the board outline)

Press '''ESC''' when done.

=== Adding Text (Silkscreen) ===

Add labels to identify the board:

# Select '''F.Silkscreen''' layer (front silkscreen)
# Press '''Ctrl+Shift+T''' (Add text) or click "Add Text" icon
# Type "LED Breakout v1.0"
# Click to place near top edge
# Press '''ESC'''

Add polarity labels:
* "+" near VCC connections
* "-" near GND connections
* "LED OUT" near J2 pin 2

'''Tips:'''
* Keep silkscreen text away from pads (0.5mm clearance)
* Use F.Silkscreen for top, B.Silkscreen for bottom

=== Design Rule Check (DRC) ===

Check for errors before manufacturing:

# Click '''Inspect → Design Rules Checker'''
# Click '''Run DRC'''
# Review errors and warnings:
** Errors (red) - Must fix
** Warnings (yellow) - Review, may be OK
# Fix any errors:
** Traces too close? Reroute with more spacing
** Unconnected nets? Route missing traces
# Re-run DRC until no errors
# Click '''Close'''

=== 3D Preview ===

View your board in 3D:

# Click '''View → 3D Viewer''' (or press '''Alt+3''')
# Rotate view with mouse (left-click drag)
# Inspect component placement and board appearance
# Close 3D viewer when satisfied

== Part 6: Generating Gerber Files ==

=== Understanding Gerber Files ===

'''Gerber files''' are the industry-standard format for PCB manufacturing. They describe:
* Copper layers (traces and pads)
* Soldermask (green coating)
* Silkscreen (white text)
* Board outline (cut shape)
* Drill holes

=== Exporting Gerbers ===

# In PCB editor, click '''File → Fabrication Outputs → Gerbers (.gbr)'''
# In the dialog:
** Output directory: <code>gerbers/</code>
** Layers to export: Check these:
*** F.Cu (front copper)
*** B.Cu (back copper)
*** F.Paste (front solder paste - optional)
*** B.Paste (back solder paste - optional)
*** F.Silkscreen (front silkscreen)
*** B.Silkscreen (back silkscreen)
*** F.Mask (front soldermask)
*** B.Mask (back soldermask)
*** Edge.Cuts (board outline)
** Format: 4.6, unit mm (defaults are fine)
** Check "Use Protel filename extensions" (JLCPCB/PCBWay prefer this)
# Click '''Plot'''
# Click '''Generate Drill Files'''
** Format: Excellon (default)
** Units: Millimeters
** Zeros: Decimal format
# Click '''Generate Drill File'''
# Click '''Close'''

You now have Gerber files in the <code>gerbers/</code> folder.

=== Zipping Gerber Files ===

Manufacturers need all Gerbers in a single ZIP file:

# Navigate to your project folder → <code>gerbers/</code> subfolder
# Select all .gbr and .drl files
# Right-click → Send to → Compressed (zipped) folder
# Name it: <code>led_breakout_gerbers.zip</code>

This ZIP file is ready to upload to a manufacturer.

== Part 7: Ordering Your PCB ==

=== Choosing a Manufacturer ===

Recommended beginner-friendly manufacturers:
* '''JLCPCB''' - $2 for 5 boards, fast shipping (1-2 weeks)
* '''PCBWay''' - Similar pricing, good quality
* '''OSH Park''' - USA-based, $5 per sq inch, purple boards

This tutorial uses JLCPCB (most popular for hobbyists).

=== Ordering from JLCPCB ===

# Visit [https://jlcpcb.com/ JLCPCB.com]
# Click '''Instant Quote'''
# Click '''Add Gerber File''' and upload <code>led_breakout_gerbers.zip</code>
# JLCPCB auto-detects settings:
** Size: 40mm × 25mm (from your board outline)
** Layers: 2
** Quantity: 5 boards (default minimum)
# Select options:
** PCB Color: Green (cheapest), or choose Blue/Red/Black (+$2)
** Surface Finish: HASL (default, fine for through-hole)
** PCB Thickness: 1.6mm (default)
# Review price (typically $2-5 for 5 boards)
# Add shipping (varies by location, $5-20)
# Click '''Save to Cart'''
# Checkout and pay

=== Waiting for Delivery ===

* Production: 1-3 days
* Shipping: 1-2 weeks (standard), 3-7 days (expedited)
* Tracking: Emailed when shipped

== Part 8: Assembling Your PCB ==

When your boards arrive:

=== Gather Components ===

Order components to match your design:
* 1× 220Ω resistor (1/4W through-hole)
* 1× 5mm red LED
* 1× 2-position 5mm screw terminal
* 1× 1×3 pin header (2.54mm pitch)

'''Where to buy:'''
* Mouser, Digikey (exact parts, fast shipping, minimum order fees)
* Amazon, eBay (component kits, slower shipping, no fees)

=== Soldering Components ===

Follow [[Soldering]] tutorial for technique. Assembly order:

# '''Resistor''' - Bend leads, insert, solder, trim
# '''LED''' - Mind polarity! Long leg = anode (+), short leg = cathode (-)
# '''Screw terminal''' - Insert, solder (requires more heat)
# '''Pin header''' - Insert, solder

=== Testing ===

# Connect 5V power supply to screw terminal (+ to top, - to bottom)
# LED should light up
# Measure voltage at header pins with multimeter:
** Pin 1: ~5V (VCC)
** Pin 2: ~2V (LED forward voltage)
** Pin 3: 0V (GND)

'''Troubleshooting:'''
* LED not lighting? Check polarity, test LED separately
* No voltage? Check solder joints for cold joints (dull, not shiny)
* Short circuit? Check for solder bridges between pads

== Part 9: Next Steps ==

Congratulations! You've designed, ordered, and assembled your first PCB. Next:

=== Design a Custom Board for Your Robot ===

Apply your skills to a real project:
* Design a sensor breakout board for [[SimpleBot]]
* Create a motor driver board
* Design a main board integrating MCU, sensors, and power

=== Study Existing Designs ===

Learn from production-quality PCBs:
* [[SimpleBot]] PCB design (files in <code>./simplebot/kicad/</code>)
** Study component placement strategy
** Observe trace routing and ground plane usage
** Note silkscreen labeling

=== Learn Advanced Techniques ===

Expand your PCB design skills:
* '''SMD components''' - Surface-mount devices for compact boards
* '''4-layer boards''' - Internal power and ground planes
* '''High-current traces''' - Calculate trace width for motor drivers
* '''Impedance control''' - High-speed signal integrity
* '''PCBA services''' - Let manufacturers assemble SMD boards

=== Share Your Design ===

Contribute to the BRS community:
* Document your PCB on the wiki
* Share KiCad files on GitHub
* Write an Implementation page
* Help others learn PCB design

== Common Beginner Mistakes ==

* '''Wrong footprint dimensions''' - Always verify footprints with calipers or datasheets before ordering
* '''Forgetting board outline''' - No Edge.Cuts layer = manufacturer can't cut your board
* '''Missing connections''' - Run DRC to find unrouted nets
* '''Traces too narrow''' - Use at least 0.2mm (wider for high current)
* '''No ground plane''' - Increases noise, makes routing harder
* '''Overlapping silkscreen''' - Text on pads won't print correctly
* '''Reversed component polarity''' - Double-check LED, capacitor, IC orientation
* '''Forgetting mounting holes''' - Can't attach board to chassis

== Troubleshooting Tips ==

* '''Ratsnest lines everywhere?''' Press '''N''' to show/hide ratsnest (airwires)
* '''Can't route a trace?''' Switch layers with '''V''' (via) or rearrange components
* '''DRC errors won't clear?''' Zoom in closely - errors are marked with small icons
* '''Gerber upload fails?''' Ensure Edge.Cuts layer is included (board outline)
* '''Board too expensive?''' Reduce size to <100mm × 100mm for cheapest pricing
* '''Components don't fit?''' Verify footprints - measure physical parts with calipers

== KiCad Keyboard Shortcuts Reference ==

=== Schematic Editor ===
* '''A''' - Add symbol (component)
* '''P''' - Add power symbol
* '''W''' - Wire (connect components)
* '''L''' - Label net (name wires)
* '''M''' - Move component
* '''R''' - Rotate component
* '''V''' - Edit value (resistor value, etc.)
* '''Ctrl+S''' - Save
* '''F8''' - Update PCB from schematic

=== PCB Editor ===
* '''M''' - Move component
* '''R''' - Rotate component
* '''X''' - Route track (trace)
* '''V''' - Add via (while routing)
* '''W''' - Change track width (while routing)
* '''/''' - Change routing mode (45° / free angle)
* '''Ctrl+Shift+Z''' - Add filled zone (copper pour)
* '''B''' - Rebuild all copper zones
* '''N''' - Toggle ratsnest display
* '''Alt+3''' - 3D viewer

== Tools and Resources ==

=== Essential Software ===
* '''KiCad''' (Free) - [https://www.kicad.org/download/ Download]
* '''PDF reader''' - View component datasheets

=== Component Suppliers ===
* '''Mouser''' - [https://www.mouser.com/ mouser.com] (USA)
* '''Digikey''' - [https://www.digikey.com/ digikey.com] (USA)
* '''LCSC''' - [https://www.lcsc.com/ lcsc.com] (China, cheap, slow shipping)

=== PCB Manufacturers ===
* '''JLCPCB''' - [https://jlcpcb.com/ jlcpcb.com] ($2 for 5 boards)
* '''PCBWay''' - [https://www.pcbway.com/ pcbway.com]
* '''OSH Park''' - [https://oshpark.com/ oshpark.com] (USA-based)

=== Learning Resources ===
* [https://docs.kicad.org/ KiCad Official Documentation]
* [https://www.youtube.com/c/Contextualelectronics Contextual Electronics] - KiCad video tutorials
* [https://www.youtube.com/playlist?list=PLy2022BX6EspFAKBCgRuEuzapuz_4aJCn Phil's Lab] - PCB design tutorials
* [https://www.eevblog.com/forum/kicad/ EEVblog KiCad Forum] - Community support

== Design Files for This Tutorial ==

If you want to compare your work or download a complete reference design:

* LED Breakout KiCad project (schematic, PCB, Gerbers)
* Available in BRS repository: <code>./pcb_examples/led_breakout/</code> (if created)

== Expanding Your Skills ==

After mastering this tutorial, try these progressively challenging projects:

=== Beginner+ ===
* '''Power indicator board''' - Add multiple LEDs, different colors
* '''Sensor breakout''' - IR sensor + headers
* '''Button array''' - 4 buttons + pull-up resistors + header

=== Intermediate ===
* '''Motor driver board''' - TB6612FNG IC + terminal blocks + logic inputs
* '''Voltage regulator board''' - LM7805 IC + capacitors + heatsink
* '''Sensor array''' - 4× IR sensors + multiplexer IC

=== Advanced ===
* '''Robot main board''' - MCU + sensors + motor driver + power (like SimpleBot)
* '''SMD practice board''' - Recreate LED breakout with 0805 resistor, SMD LED
* '''Programmable board''' - ESP32 module + USB-to-serial + sensors

== See Also ==

* [[PCB Design]] - Full competency overview
* [[Electronics]] - Understand circuits before designing PCBs
* [[Soldering]] - Assemble your PCBs after ordering
* [[SimpleBot]] - Study a production robot PCB design

[[Category:Tutorials]]
[[Category:PCB Design]]
[[Category:Beginner]]

KiCad Tutorial - Revision history