Skip to main content
  • Created:
  • Updated:
  • Author:
    Takeshi Takatsudo

Download KiCad Footprints and Symbols

This guide explains how to download KiCad footprints and symbols from LCSC/EasyEDA using the easyeda2kicad.py tool.

Overview​

This project uses easyeda2kicad.py to download KiCad libraries from the LCSC/EasyEDA database. This ensures we have accurate footprints and symbols matching the actual components from JLCPCB.

What you can download:

  • Footprints (.kicad_mod) - Physical PCB pads for PCB layout
  • Symbols (.kicad_sym) - Schematic symbols for circuit design
  • 3D Models (.step, .wrl) - 3D visualization (optional)

Important: Footprints vs Symbols​

You need BOTH for KiCad design:

TypeFile FormatUsed InPurpose
Footprint.kicad_modPCB EditorPhysical component pads on PCB
Symbol.kicad_symSchematic EditorElectrical connections in schematic

Common mistake: Downloading only --footprint without --symbol!

Prerequisites​

Install easyeda2kicad.py​

pip install easyeda2kicad

The tool should be available in your PATH after installation.

Verify Installation​

easyeda2kicad --version

Quick Start: Download Pre-Generated Footprints​

Don't want to generate footprints yourself? Download the complete footprint library directly from GitHub:

🔗 Download Footprints from GitHub

The /footprints/kicad/ directory contains all .kicad_mod files ready to use in your KiCad project.

Finding LCSC Part Numbers​

All component LCSC IDs are listed in the Bill of Materials. You can also search on:

Download Options​

Download footprint AND symbol together:

# Download both footprint and symbol
easyeda2kicad --lcsc_id <LCSC_ID> --footprint --symbol

# Example: STUSB4500 (USB-PD controller)
easyeda2kicad --lcsc_id C2678061 --footprint --symbol

# Example: USB-C connector
easyeda2kicad --lcsc_id C456012 --footprint --symbol

Option 2: Download Only Footprint​

For parts where you'll use KiCad standard symbols:

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

Option 3: Download Only Symbol​

For parts where you already have the footprint:

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

Output Locations​

Footprints​

~/Documents/Kicad/easyeda2kicad/easyeda2kicad.pretty/
└── *.kicad_mod

Symbols​

~/Documents/Kicad/easyeda2kicad/
└── easyeda2kicad.kicad_sym

Important: Symbols are added to a single .kicad_sym file, not separate files like footprints.

Project Structure​

footprints/
├── kicad/
│   └── *.kicad_mod          # KiCad footprint files
├── images/
│   └── *.svg                # Exported SVG images (for documentation)
└── scripts/
    └── clean-svg-refs.py    # Script to clean SVG exports

symbols/
└── zudo-pd.kicad_sym        # Project symbol library (copied from download)

~/Documents/Kicad/easyeda2kicad/  (download location)
├── easyeda2kicad.pretty/
│   └── *.kicad_mod          # Downloaded footprints
└── easyeda2kicad.kicad_sym  # Downloaded symbols (all in one file)

Complete Download Workflow​

1. Download All Project Parts​

Download all components with BOTH footprints and symbols:

# USB-C Connector
easyeda2kicad --lcsc_id C456012 --footprint --symbol

# STUSB4500 - USB PD Controller
easyeda2kicad --lcsc_id C2678061 --footprint --symbol

# LM2596S-ADJ - Buck Converter
easyeda2kicad --lcsc_id C347423 --footprint --symbol

# ICL7660M - Voltage Inverter
easyeda2kicad --lcsc_id C356724 --footprint --symbol

# L7812CV - +12V Regulator
easyeda2kicad --lcsc_id C2914 --footprint --symbol

# L7805ABD2T - +5V Regulator
easyeda2kicad --lcsc_id C86206 --footprint --symbol

# CJ7912 - -12V Regulator
easyeda2kicad --lcsc_id C94173 --footprint --symbol

# SMAJ15A - TVS Diode
easyeda2kicad --lcsc_id C347883 --footprint --symbol

# SD05 - TVS Diode (5V)
easyeda2kicad --lcsc_id C502527 --footprint --symbol

2. Copy to Project​

# Create symbols directory
mkdir -p /Users/takazudo/repos/personal/zudo-pd/symbols

# Copy footprints
cp ~/Documents/Kicad/easyeda2kicad/easyeda2kicad.pretty/*.kicad_mod \
   /Users/takazudo/repos/personal/zudo-pd/footprints/kicad/

# Copy symbols
cp ~/Documents/Kicad/easyeda2kicad/easyeda2kicad.kicad_sym \
   /Users/takazudo/repos/personal/zudo-pd/symbols/zudo-pd.kicad_sym

3. Add Libraries to KiCad​

Add Symbol Library:

  1. Preferences → Manage Symbol Libraries
  2. Click "Project Specific Libraries" tab
  3. Add library:
  • Nickname: zudo-pd
  • Library Path: ${KIPRJMOD}/symbols/zudo-pd.kicad_sym
  • Plugin Type: KiCad

Add Footprint Library (if not done yet):

  1. Preferences → Manage Footprint Libraries
  2. Click "Project Specific Libraries" tab
  3. Add library:
  • Nickname: zudo-pd
  • Library Path: ${KIPRJMOD}/footprints/kicad/zudo-power.pretty

4. Verify Files​

# Check footprints
ls -l /Users/takazudo/repos/personal/zudo-pd/footprints/kicad/*.kicad_mod

# Check symbols
ls -l /Users/takazudo/repos/personal/zudo-pd/symbols/zudo-pd.kicad_sym

Footprint File Format​

KiCad footprint files (.kicad_mod) are text files in S-expression format:

(footprint "QFN-20_L3.0-W3.0-P0.40-BL-EP1.7"
  (layer "F.Cu")
  (attr smd)
  (fp_text reference "REF**" (at 0 -2.5) (layer "F.SilkS"))
  (fp_text value "CH224D" (at 0 2.5) (layer "F.Fab"))
  (pad "1" smd rect (at -1.4 -1.0) (size 0.25 0.6) (layers "F.Cu" "F.Paste" "F.Mask"))
  ...
)

Troubleshooting​

Problem: "easyeda2kicad: command not found"​

Solution: Ensure pip installed the package correctly and it's in your PATH:

which easyeda2kicad
# Should show: /path/to/python/bin/easyeda2kicad

If not found, try:

python -m easyeda2kicad --version

Problem: "Part not found"​

Solution:

  • Verify the LCSC ID is correct
  • Check if the part exists on LCSC.com
  • Try using the EasyEDA part number instead

Problem: Download fails or times out​

Solution:

  • Check internet connection
  • Try again (server might be temporarily down)
  • Use --full flag for more detailed error messages: 
    easyeda2kicad --lcsc_id C3975094 --footprint --full

Advanced Options​

Download Symbol and 3D Model​

# Download footprint, symbol, and 3D model
easyeda2kicad --lcsc_id C3975094 --footprint --symbol --3d

Specify Output Directory​

easyeda2kicad --lcsc_id C3975094 --footprint --output /custom/path/

Download by EasyEDA ID​

easyeda2kicad --easyeda_id <EASYEDA_ID> --footprint

Next Steps​

After downloading footprints:

  1. Create Footprint SVG Files - Export SVGs for documentation
  2. Review footprints in KiCad PCB editor
  3. Add footprints to your PCB design

References​

Last updated on by Takeshi Takatsudo