easyeda2kicad

easyeda2kicad - Download KiCad Libraries from LCSC/EasyEDA

Download KiCad footprints and symbols from LCSC/EasyEDA for JLCPCB PCBA projects.

Tool Overview

easyeda2kicad.py downloads KiCad libraries from LCSC/EasyEDA database:

• Footprints (.kicad_mod) - Physical PCB pads for PCB Editor
• Symbols (.kicad_sym) - Schematic symbols for Schematic Editor
• 3D Models (.step, .wrl) - Optional 3D visualization

Critical: You need BOTH footprints AND symbols for complete KiCad design.

Installation Check

Before downloading, verify installation:

easyeda2kicad --version

If not installed:

pip install easyeda2kicad

Download Commands

Recommended: Download Both Footprint and Symbol

Always use this for JLCPCB PCBA projects to ensure exact symbol-footprint combinations:

easyeda2kicad --lcsc_id <LCSC_ID> --footprint --symbol

Example:

# CH224D USB-PD controller
easyeda2kicad --lcsc_id C3975094 --footprint --symbol

# USB-C connector
easyeda2kicad --lcsc_id C2927029 --footprint --symbol

# Passive components (capacitors, resistors, LEDs)
easyeda2kicad --lcsc_id C7432781 --footprint --symbol  # 10µF capacitor
easyeda2kicad --lcsc_id C23138 --footprint --symbol    # 330Ω resistor

Overwrite Existing Files

If files already exist:

easyeda2kicad --lcsc_id <LCSC_ID> --footprint --symbol --overwrite

Download Only Footprint or Symbol

# Footprint only
easyeda2kicad --lcsc_id <LCSC_ID> --footprint

# Symbol only
easyeda2kicad --lcsc_id <LCSC_ID> --symbol

Include 3D Models

easyeda2kicad --lcsc_id <LCSC_ID> --footprint --symbol --3d

Download Output Locations

Footprints

$HOME/Documents/Kicad/easyeda2kicad/easyeda2kicad.pretty/
└── *.kicad_mod

Each footprint is a separate .kicad_mod file.

Symbols

$HOME/Documents/Kicad/easyeda2kicad/
└── easyeda2kicad.kicad_sym

Important: All symbols are added to a SINGLE .kicad_sym file (not separate files).

Copying to Project

After downloading, copy files to project directories:

Standard Project Structure

<project-root>/
├── footprints/
│   └── kicad/
│       └── *.kicad_mod          # Copy footprints here
└── symbols/
    └── <project-name>.kicad_sym # Copy symbols here

Copy Commands

# Copy footprints (specific files)
cp $HOME/Documents/Kicad/easyeda2kicad/easyeda2kicad.pretty/<filename>.kicad_mod \
   <project-root>/footprints/kicad/

# Copy symbols (entire file)
cp $HOME/Documents/Kicad/easyeda2kicad/easyeda2kicad.kicad_sym \
   <project-root>/symbols/<project-name>.kicad_sym

Example for multiple footprints:

# Copy all footprints at once
cp $HOME/Documents/Kicad/easyeda2kicad/easyeda2kicad.pretty/*.kicad_mod \
   /path/to/project/footprints/kicad/

Complete Workflow for Multiple Components

When user requests multiple components, use this pattern:

# 1. Change to download directory
cd $HOME/Documents/Kicad/easyeda2kicad

# 2. Download all components
easyeda2kicad --lcsc_id C3975094 --footprint --symbol --overwrite
easyeda2kicad --lcsc_id C2927029 --footprint --symbol --overwrite
easyeda2kicad --lcsc_id C7432781 --footprint --symbol --overwrite
# ... etc

# 3. Copy footprints to project
cp $HOME/Documents/Kicad/easyeda2kicad/easyeda2kicad.pretty/*.kicad_mod \
   <project-root>/footprints/kicad/

# 4. Copy symbols to project
cp $HOME/Documents/Kicad/easyeda2kicad/easyeda2kicad.kicad_sym \
   <project-root>/symbols/<project-name>.kicad_sym

Verifying Downloads

After copying, verify files exist:

# List footprints
ls -lh <project-root>/footprints/kicad/*.kicad_mod

# Check symbol library size
ls -lh <project-root>/symbols/<project-name>.kicad_sym

# Count symbols in library
grep -c '(symbol "' <project-root>/symbols/<project-name>.kicad_sym

Finding LCSC Part Numbers

LCSC part numbers start with 'C' followed by digits (e.g., C3975094).

Where to find them:

• User's Bill of Materials (BOM)
• LCSC.com - Search by part name
• EasyEDA.com - Component library
• User-provided specifications

Common Part Categories

Active Components (Always download both)

• ICs (USB-PD controllers, buck converters, regulators)
• Connectors (USB-C, pin headers)
• Diodes (Schottky, TVS, ESD protection)

Passive Components (Download both for JLCPCB PCBA)

• Capacitors (ceramic, electrolytic)
• Resistors (all values)
• LEDs (indicator lights)

Note: For JLCPCB PCBA, always download both footprint and symbol even for passive components to ensure exact package matching.

Troubleshooting

Error: "easyeda2kicad: command not found"

# Check installation
which easyeda2kicad

# Try Python module form
python -m easyeda2kicad --version

# Reinstall if needed
pip install easyeda2kicad

Error: "Part not found"

• Verify LCSC ID is correct (starts with 'C')
• Check part exists on LCSC.com
• Try EasyEDA ID instead with --easyeda_id

Error: "Footprint already exists"

Use --overwrite flag:

easyeda2kicad --lcsc_id <LCSC_ID> --footprint --symbol --overwrite

Download timeout or failure

• Check internet connection
• Retry (server may be temporarily down)
• Use --full for detailed error messages:

easyeda2kicad --lcsc_id <LCSC_ID> --footprint --full

Error: "Failed to fetch data from EasyEDA API"

Common for passive components (capacitors, resistors, LEDs) - Many JLCPCB parts exist but don't have symbols in EasyEDA's database.

Solution: Use Generic KiCad Symbols

1. Download footprint only (if available):

   easyeda2kicad --lcsc_id <LCSC_ID> --footprint --overwrite
   

2. Use KiCad's built-in generic symbols:

• Capacitors: Device:C
• Resistors: Device:R
• LEDs: Device:LED
• Inductors: Device:L

3. Pair with downloaded footprint:

• Symbol: Generic KiCad symbol (e.g., Device:C)
• Footprint: Downloaded or generic (e.g., C0805.kicad_mod)

Example workflow for 22nF capacitor (C7393941):

# Try to download (may fail for symbol)
easyeda2kicad --lcsc_id C7393941 --footprint --overwrite

# If symbol download fails:
# 1. Use KiCad generic symbol: Device:C
# 2. Use footprint: C0805.kicad_mod (or downloaded footprint)
# 3. Keep LCSC part number C7393941 in BOM for JLCPCB assembly

This is standard practice - Passive components often use generic symbols with specific footprints. The LCSC part number in the BOM ensures correct component ordering for PCBA.

Expected Output

Successful download shows:

-- easyeda2kicad.py v0.8.0 --
[INFO] Created Kicad symbol for ID : C3975094
       Symbol name : CH224D_C3975094
       Library path : $HOME/Documents/Kicad/easyeda2kicad/easyeda2kicad.kicad_sym
[INFO] Created Kicad footprint for ID: C3975094
       Footprint name: QFN-20_L3.0-W3.0-P0.40-BL-EP1.7
       Footprint path: $HOME/Documents/Kicad/easyeda2kicad/easyeda2kicad.pretty/...

Batch Download Example

For a complete stage (e.g., USB-PD stage with 9 components):

cd $HOME/Documents/Kicad/easyeda2kicad

# Download all components for USB-PD stage
for lcsc_id in C3975094 C2927029 C7432781 C49678 C6119849 C705785 C23186 C23138 C2286; do
  echo "Downloading $lcsc_id..."
  easyeda2kicad --lcsc_id $lcsc_id --footprint --symbol --overwrite
done

# Copy all to project
cp easyeda2kicad.pretty/*.kicad_mod <project>/footprints/kicad/
cp easyeda2kicad.kicad_sym <project>/symbols/<project>.kicad_sym

Important Notes for Claude

1. Always download BOTH footprint and symbol unless user specifically requests only one
2. Use --overwrite when downloading multiple components to avoid conflicts
3. Run downloads from $HOME/Documents/Kicad/easyeda2kicad directory for consistency
4. Copy files separately - footprints are individual files, symbols are a single file
5. Verify after copying by listing files in project directories
6. Inform user of symbol names so they can find them in KiCad

Quick Reference

Task	Command
Download both	easyeda2kicad --lcsc_id <ID> --footprint --symbol
Overwrite existing	Add --overwrite flag
Include 3D model	Add --3d flag
Check installation	easyeda2kicad --version
Copy footprints	cp $HOME/Documents/Kicad/easyeda2kicad/easyeda2kicad.pretty/*.kicad_mod <project>/footprints/kicad/
Copy symbols	cp $HOME/Documents/Kicad/easyeda2kicad/easyeda2kicad.kicad_sym <project>/symbols/<name>.kicad_sym

References

• easyeda2kicad.py GitHub
• LCSC Component Search
• EasyEDA Component Library
• KiCad Documentation