Quick Start Guide

​

Launch KiCad and Create Project

1. Open KiCad Project Manager
   • Launch KiCad from your applications menu
   • You’ll see the main Project Manager window
2. Create a New Project
   • Click File > New Project or press Ctrl+N (Windows/Linux) / Cmd+N (macOS)
   • Choose New Project (not “New Project from Template” for now)
3. Name Your Project
   • Navigate to your desired project directory (e.g., ~/Documents/kicad_projects/)
   • Enter project name: led_blinker
   • Click Save

​

Project Structure

led_blinker/
├── led_blinker.kicad_pro      # Project settings
├── led_blinker.kicad_sch      # Main schematic (created)
├── led_blinker.kicad_pcb      # PCB layout (created later)
├── fp-lib-table               # Footprint library table (created later)
└── sym-lib-table              # Symbol library table (optional)

• Schematic file (.kicad_sch)
• PCB file (.kicad_pcb)

​

Open Schematic Editor

1. Launch Eeschema
   • In Project Manager, double-click led_blinker.kicad_sch
   • Or click the schematic editor icon in the toolbar
   • Eeschema opens with a blank schematic sheet
2. Configure Schematic Settings
   • Click File > Schematic Setup
   • Under General, set:
     • Sheet size: A4
     • Title: LED Blinker Circuit
     • Revision: 1.0
   • Click OK

​

Add Components to Schematic

3. Add the 555 Timer IC
   • Press A (Add Symbol) or click the “Add Symbol” button
   • In the search box, type: 555
   • Select Timer:NE555 from the list
   • Click OK
   • Move mouse to place component, click to place
   • Press Esc to exit placement mode
4. Add a Capacitor (C1 - Timing)
   • Press A again
   • Search for: C
   • Select Device:C (generic capacitor)
   • Place it to the right of the 555 timer
   • Press Esc
5. Add Another Capacitor (C2 - Bypass)
   • Press A, search for C
   • Place below the 555 timer
   • Press Esc
6. Add Resistors
   • Press A, search for R
   • Select Device:R (generic resistor)
   • Place three resistors:
     • R1 and R2: Near pins 7 and 6 of 555
     • R3: For LED current limiting
   • Press Esc
7. Add an LED
   • Press A, search for LED
   • Select Device:LED
   • Place near R3
   • Press Esc
8. Add Power Connector
   • Press A, search for Conn_01x02
   • Select Connector:Conn_01x02 (2-pin connector)
   • Place in upper left corner
   • Press Esc
9. Add Power Symbols
   • Press P (Add Power Port)
   • Search for VCC
   • Place near the positive supply pins
   • Press P again, search for GND
   • Place near ground connections
   • Press Esc

​

Wire the Components

10. Connect Components with Wires
    • Press W (Begin Wire) or click the wire tool
    • Click on pin 8 of the 555 (VCC)
    • Click on a VCC power symbol
    • Continue wiring according to standard 555 astable circuit: 555 Timer Connections:
    • Pin 1 (GND) → GND
    • Pin 2 (TRIG) → Pin 6 (THRES)
    • Pin 3 (OUT) → R3 → LED → GND
    • Pin 4 (RESET) → VCC
    • Pin 5 (CTRL) → C2 (0.01µF) → GND
    • Pin 6 (THRES) → R2 → Pin 7
    • Pin 7 (DISCH) → R1 → VCC
    • Pin 8 (VCC) → VCC
    To connect wires, click once to start, click again to create corners, and click on the destination pin to complete the connection.

​

Add Component Values

11. Edit Component Values
    • Hover over R1, press V (Edit Value)
    • Type: 10k
    • Press Enter
    • Repeat for all components:
      • R1: 10k
      • R2: 100k
      • R3: 330
      • C1: 10µF
      • C2: 0.01µF
      • LED: Red
12. Add Reference Designators
    • KiCad auto-assigns references (R1, R2, C1, etc.)
    • To manually edit, hover over component and press E
    • These will be automatically numbered later

​

Annotate Schematic

13. Assign Reference Designators
    • Click Tools > Annotate Schematic
    • Select Use entire schematic
    • Keep default settings: Sequential numbering
    • Click Annotate
    • Click OK to confirm changes

​

Run Electrical Rules Check (ERC)

14. Check for Errors
    • Click Inspect > Electrical Rules Checker
    • Click Run ERC
    • Review any errors or warnings:
      • ✅ No errors: Great! Continue to next step
      • ⚠️ Warnings: Review each warning, most are informational
      • ❌ Errors: Fix these before proceeding Common warnings you can ignore:
    • “Power pin not driven by any output”
    • “No input pin on net”
15. Save Your Schematic
    • Press Ctrl+S (Windows/Linux) / Cmd+S (macOS)
    • Or click File > Save

​

Link Symbols to Physical Footprints

1. Open Footprint Assignment Tool
   • In Eeschema, click Tools > Assign Footprints
   • Or click the footprint assignment icon in toolbar
   • The CvPCB window opens
2. Assign Footprints to Components Select each component on the left and assign footprints:
   555 Timer (U1)

   Resistors (R1, R2, R3)

   Capacitors (C1, C2)

   LED (D1)

   Connector (J1)

   Package_DIP:DIP-8_W7.62mm
   (or Package_SO:SOIC-8_3.9x4.9mm_P1.27mm for SMD)
   
   Through-Hole vs. SMD:

   • THT (Through-Hole): Easier for hand soldering, good for prototypes
   • SMD (Surface Mount): Smaller, better for production, requires more skill

   For your first project, use Through-Hole (THT) components.
3. Apply and Save
   • Click Apply, Save Schematic & Continue
   • Close the footprint assignment window
   • Return to Eeschema
4. Verify Footprint Assignments
   • In Eeschema, hover over each component
   • Press E to edit
   • Check that the Footprint field is populated
5. Save Schematic Again
   • Press Ctrl+S / Cmd+S

​

Import to PCB Editor

1. Open Pcbnew
   • In Eeschema, click Tools > Update PCB from Schematic
   • Or press F8
   • The Update PCB from Schematic dialog opens
2. Import Components
   • Click Update PCB
   • New components are highlighted in green
   • Click Close
   • Pcbnew opens with all components floating

​

Define Board Outline

3. Draw Board Edge
   • Select Edge.Cuts layer from the Layers panel (right side)
   • Press Ctrl+Shift+P or click Place > Draw Rectangle
   • Draw a rectangle approximately 50mm x 40mm
   • This defines your board physical size
   The Edge.Cuts layer (magenta/pink) defines where the PCB manufacturer will cut the board.

​

Position Components

4. Arrange Components on PCB
   • All components initially appear in a cluster
   • Press M to move components
   • Arrange them logically:
     • J1 (connector) at the edge for easy access
     • U1 (555 timer) in the center
     • Arrange R, C components around U1
     • LED near the edge for visibility
   Press F while hovering over a component to flip it to the bottom layer. Press R to rotate.
5. Check Ratsnest
   • Thin white lines (airwires/ratsnest) show electrical connections
   • Minimize crossings by optimal component placement
   • Try different arrangements to reduce trace complexity

​

Route Traces

6. Set Up Design Rules
   • Click File > Board Setup
   • Under Design Rules > Constraints:
     • Minimum track width: 0.25mm (typical for DIY)
     • Minimum clearance: 0.2mm
   • Click OK
7. Route Copper Traces
   • Press X to start routing
   • Click on a pad to start a trace
   • Click to create corners
   • Click on destination pad to complete
   • Press Esc to cancel current route
   Routing Tips:
   • Route power (VCC, GND) with wider traces (0.5mm or more)
   • Route signal traces with default width (0.25mm)
   • Avoid sharp angles (use 45° turns)
   • Keep traces as short as practical
   Layer Usage

   Via Placement

   F.Cu (Front Copper) - Top layer traces
   B.Cu (Back Copper) - Bottom layer traces
   (Switch layers during routing with 'V' key)
   
8. Add Ground Plane (Optional but Recommended)
   • Select B.Cu layer
   • Press Ctrl+Shift+Z or Place > Add Filled Zone
   • Click corners to define zone (usually entire board)
   • Right-click and select Close Zone Outline
   • In dialog:
     • Layer: B.Cu
     • Net: GND
     • Clearance: 0.3mm
   • Click OK
   • Press B to rebuild filled zones
   Ground planes improve electrical performance and reduce routing complexity by providing a common ground connection.

​

Add Text and Graphics

9. Add Silkscreen Text
   • Select F.Silkscreen layer
   • Press Ctrl+Shift+T or Place > Add Text
   • Type: “LED Blinker v1.0”
   • Position on an empty area
   • Press E to edit size if needed
10. Add KiCad Logo (Optional)
    • Place > Add Footprint
    • Search for: KiCad-Logo
    • Select appropriate size
    • Place on silkscreen layer

​

Run Design Rule Check (DRC)

11. Check for Errors
    • Click Inspect > Design Rules Checker
    • Click Run DRC
    • Review results:
      • ✅ No errors: Perfect! Ready for manufacturing
      • ❌ Errors: Fix each error before proceeding Common DRC errors:
    • Clearance violation: Traces too close
    • Unconnected items: Missing traces
    • Track width: Trace too narrow
12. Save Your PCB
    • Press Ctrl+S / Cmd+S
    • File > Save

​

Verify Physical Design

1. Open 3D Viewer
   • In Pcbnew, press Alt+3 or View > 3D Viewer
   • A 3D window opens showing your PCB
2. Inspect the 3D Model
   • Rotate view: Click and drag
   • Zoom: Mouse wheel
   • Check:
     • Component placement looks correct
     • No physical collisions
     • Board dimensions are appropriate
     • Mounting holes aligned (if added)

3. Export 3D Model (Optional)
   • File > Export > STEP
   • Save for mechanical CAD integration
   • Useful for enclosure design

​

Create Gerber Files for Fabrication

1. Open Plot Dialog
   • In Pcbnew, click File > Plot
   • The Plot dialog opens
2. Configure Gerber Output
   • Output directory: gerbers/ (relative to project)
   • Plot format: Gerber
   • Include layers:
     • ✅ F.Cu (Front Copper)
     • ✅ B.Cu (Back Copper)
     • ✅ F.SilkS (Front Silkscreen)
     • ✅ B.SilkS (Back Silkscreen)
     • ✅ F.Mask (Front Soldermask)
     • ✅ B.Mask (Back Soldermask)
     • ✅ Edge.Cuts (Board Outline)
   For a 2-layer board, you only need F.Cu and B.Cu. 4+ layer boards require additional internal layers.
3. Plot Settings
   • ✅ Use Protel filename extensions (recommended for most manufacturers)
   • ✅ Include netlist attributes
   • ✅ Subtract soldermask from silkscreen
   • Coordinate format: 4.6, unit mm
4. Generate Plot Files
   • Click Plot
   • Gerber files are created in gerbers/ folder
   • Click Generate Drill Files
5. Generate Drill Files
   • In the Drill Files dialog:
     • Drill units: Millimeters
     • Zeros format: Decimal format
     • Drill file format: Excellon
   • Click Generate Drill File
   • Click Close

​

Verify Gerber Files

6. Open GerbView
   • Return to KiCad Project Manager
   • Click the GerbView icon
   • File > Open Gerber Plot File(s)
   • Select all .gbr files in the gerbers/ folder
   • File > Open Excellon Drill File(s)
   • Select the .drl file
7. Inspect Gerbers
   • Toggle layers on/off in the Layers panel
   • Verify:
     • All copper traces present
     • Silkscreen readable and not on pads
     • Soldermask openings correct
     • Drill holes in correct positions
     • Board outline complete

​

Create Assembly Files

8. Generate BOM (Bill of Materials)
   • In Eeschema (schematic editor)
   • Click Tools > Generate BOM
   • Select an export plugin (CSV recommended)
   • Click Generate
   • Save as led_blinker_bom.csv
9. Generate Pick-and-Place File
   • In Pcbnew
   • File > Fabrication Outputs > Component Placement (.pos)
   • Choose format: CSV
   • Generate separate files for top and bottom

• JLCPCB - Low cost, fast shipping
• PCBWay - Good quality, reliable
• OSH Park - US-based, purple PCBs
• Aisler - EU-based, good for small batches

1. Visit manufacturer website
2. Click “Quote Now” or “Instant Quote”
3. Upload your Gerber zip file
4. Specify:
   • Layers: 2
   • Dimensions: Detected automatically
   • Quantity: 5 (minimum for most)
   • Thickness: 1.6mm
   • Copper: 1 oz
   • Color: Green (or your preference)
   • Surface finish: HASL or ENIG

• Review the auto-detected board dimensions
• Check pricing
• Add to cart and checkout
• Typical lead time: 1-2 weeks