How to Convert EasyEDA to KiCad: Complete Migration Guide (2025)

Introduction

Switching between PCB design tools is a common challenge for electronics engineers. Whether you're moving to KiCad for its powerful open-source features, collaborating with a team that uses different software, or simply want to keep a backup in another format, converting your EasyEDA designs is essential.

This comprehensive guide covers every method available for converting EasyEDA projects to KiCad format in 2025. You'll learn to migrate complete projects including schematics, PCB layouts, and component libraries while avoiding common pitfalls that can derail your conversion.

Why Convert from EasyEDA to KiCad?

Both EasyEDA and KiCad are excellent PCB design tools, but they have different strengths. Here are common reasons engineers migrate from EasyEDA to KiCad:

Many engineers use both tools: EasyEDA for quick prototypes with JLCPCB assembly, and KiCad for complex projects requiring advanced features. Being able to convert between them gives you the best of both worlds.

Conversion Methods Overview

There are four main methods to convert EasyEDA designs to KiCad format. Each has different strengths depending on your needs:

Method 1: Wokwi Online Converter

The Wokwi EasyEDA2KiCad online tool is the fastest way to convert EasyEDA PCB files to KiCad format. It runs entirely in your browser, so your files never leave your computer.

Step-by-Step Instructions

1. Export from EasyEDA: In EasyEDA, go to Document > Export > EasyEDA Source... and download your project as JSON.
2. Open the converter: Visit wokwi.com/tools/easyeda2kicad
3. Upload your file: Click to select your EasyEDA board JSON file.
4. Download the result: The converted KiCad PCB file will download automatically.
5. Open in KiCad: Open the .kicad_pcb file in KiCad's PCB editor.

Method 2: easyeda2kicad.py (Python)

The easyeda2kicad Python package is the most popular tool for converting LCSC/EasyEDA components to KiCad format. It generates symbols, footprints, and 3D models in full color.

Installation

Install the package using pip:

pip install easyeda2kicad

Basic Usage

Convert a component using its LCSC part number:

# Convert everything (symbol + footprint + 3D model)
easyeda2kicad --full --lcsc_id=C2040

# Convert only symbol and footprint
easyeda2kicad --symbol --footprint --lcsc_id=C2040

# Convert symbol only
easyeda2kicad --symbol --lcsc_id=C2040

# Convert footprint only
easyeda2kicad --footprint --lcsc_id=C2040

# Convert 3D model only
easyeda2kicad --3d --lcsc_id=C2040

# Use legacy KiCad v5 format
easyeda2kicad --symbol --lcsc_id=C2040 --v5

# Custom output path
easyeda2kicad --full --lcsc_id=C2040 --output ~/libs/my_lib

KiCad Library Setup

After converting components, configure KiCad to use the generated libraries:

1. Set environment variable: In KiCad, go to Preferences > Configure Paths and add a new variable:
   Name: EASYEDA2KICAD
   Path: C:/Users/YourName/Documents/Kicad/easyeda2kicad/ (Windows) or/home/YourName/Documents/Kicad/easyeda2kicad/ (Linux)
2. Add symbol library: Go to Preferences > Manage Symbol Libraries, click the Global Libraries tab, and add:
   Nickname: easyeda2kicad
   Path: ${EASYEDA2KICAD}/easyeda2kicad.kicad_sym
3. Add footprint library: Go to Preferences > Manage Footprint Libraries, click the Global Libraries tab, and add:
   Nickname: easyeda2kicad
   Path: ${EASYEDA2KICAD}/easyeda2kicad.pretty

Method 3: easyeda2kicad6 (Node.js)

The easyeda2kicad6 tool is a TypeScript/Node.js converter that handles complete project conversion including both schematics and PCBs. It's the most comprehensive option for full project migration.

Installation

1. Install Node.js (v16 or later)
2. Download easyeda2kicad6 from GitHub
3. Extract the downloaded zip file
4. Open a terminal in the extracted folder and run:

   npm install uuid

5. Verify installation:

   node dist/main.js

   This should display usage information.

Full Project Conversion Workflow

Converting a complete project requires several steps to maintain schematic-PCB synchronization:

1. Export from EasyEDA:
   • Open your project in EasyEDA
   • Go to File > Export > Export Footprints to Library...
   • Choose "EasyEDA" as the library format and click OK
   • Export both schematic and PCB as JSON files
2. Convert the PCB first:

   node dist/main.js "MyProject_PCB.json"

3. Open in KiCad and add footprint library:
   • Open the generated .kicad_pcb file in KiCad
   • Go to Preferences > Manage Footprint Libraries
   • Add the generated EasyEDA.pretty folder as a project-specific library
4. Convert the schematic:

   node dist/main.js "MyProject_SCH.json"

5. Add symbol library:
   • Go to Preferences > Manage Symbol Libraries
   • Add the generated .sym file as a project-specific library
6. Annotate and sync:
   • Open Tools > Annotate Schematic...
   • Enable "Keep existing annotations"
   • Click Annotate
   • Go to Tools > Update PCB from Schematic
   • Select only "Relink footprints to schematic symbols based on their reference designators"
   • Click Update PCB
7. Verify:
   • Run ERC (Electrical Rules Check) on the schematic
   • Run DRC (Design Rules Check) on the PCB
   • Press "B" to rebuild copper pours
   • Save both files

Method 4: KiCad Plugin

The KiCAD-EasyEDA-Parts plugin provides a convenient interface directly within KiCad for downloading and converting LCSC components.

Installation

1. Download from GitHub
2. Copy the plugin to your KiCad plugins folder
3. Restart KiCad
4. Access the plugin from Tools > External Plugins > EasyEDA Parts

Usage

1. Open the plugin in KiCad
2. Enter the LCSC part number (e.g., C2040)
3. Click Download
4. The symbol, footprint, and 3D model are added to your KiCad libraries

Converting Individual Components

Sometimes you don't need to convert an entire project - you just want to use specific LCSC components in KiCad. Here's how to efficiently build your library:

Find the LCSC Part Number

Every component in the EasyEDA/LCSC ecosystem has a unique LCSC part number (e.g., C2040 for the ESP32-WROOM-32). You can find this:

• On the LCSC website product page
• In EasyEDA's component properties
• In your project's BOM

Batch Conversion

Convert multiple components at once by creating a simple script:

#!/bin/bash
# Convert multiple LCSC components to KiCad

PARTS=(
  "C2040"    # ESP32-WROOM-32
  "C14663"   # STM32F103C8T6
  "C2761969" # RP2040
  "C965"     # AMS1117-3.3
)

for part in "${PARTS[@]}"; do
  echo "Converting $part..."
  easyeda2kicad --full --lcsc_id=$part
done

echo "Done! All components converted."

Converting Full Projects

For complete project conversion, follow this detailed workflow:

Step 1: Export from EasyEDA

1. Open your project in EasyEDA (Standard or Pro)
2. For EasyEDA Standard:
   • Go to Document > Export > EasyEDA Source...
   • Download the ZIP file containing JSON files
3. For EasyEDA Pro:
   • Go to File > Export > EasyEDA (Professional)...
   • Export as .epro or .zip format
4. Extract the ZIP file to a working folder

Step 2: Convert PCB

Always convert the PCB first, as it generates the footprint library needed by the schematic:

# Using easyeda2kicad6
node dist/main.js "MyProject_PCB.json"

# Or using the online converter
# Upload the PCB JSON at wokwi.com/tools/easyeda2kicad

Step 3: Convert Schematic

Convert the schematic JSON file:

# Make sure the schematic has the same base name as the PCB
node dist/main.js "MyProject_SCH.json"

Step 4: Sync in KiCad

1. Open the converted project in KiCad
2. Add the generated libraries to your project
3. Run annotation with "Keep existing annotations" enabled
4. Update PCB from schematic with "Relink footprints" option only
5. Run ERC and DRC checks
6. Rebuild copper pours (press "B")

Post-Conversion Checklist

After converting your project, use this checklist to verify everything is correct:

Known Limitations

All conversion tools have limitations. Understanding these helps you plan for manual corrections:

Troubleshooting Common Issues

Footprints Not Found in KiCad

Problem: KiCad shows missing footprint errors after conversion.

Solution: Ensure you've added the generated .pretty folder to your footprint libraries. Check that the library path is correct and the folder exists.

Symbols Missing from Schematic

Problem: Some components appear as question marks in the schematic.

Solution: Add the generated .sym file to your symbol libraries. You may need to manually link orphaned symbols to their footprints.

Copper Pours Not Visible

Problem: Filled zones appear empty after opening the converted PCB.

Solution: Press "B" in KiCad to rebuild all copper pours. This is expected behavior - KiCad doesn't store zone fills in the file.

DRC Errors About Unconnected Items

Problem: Multiple DRC errors about unconnected pads or traces.

Solution: Check zone priorities and rebuild fills. Some traces may need manual connection if they relied on EasyEDA-specific features.

3D Models Not Showing

Problem: 3D viewer shows flat rectangles instead of component shapes.

Solution: Verify the .3dshapes folder path is correctly set in footprint properties. Check that EASYEDA2KICAD environment variable points to the right location.

Python Script Fails with API Error

Problem: easyeda2kicad.py fails with network or API errors.

Solution: The tool queries LCSC/EasyEDA servers. Check your internet connection. Some parts may not be available via API - try a different LCSC ID or use the manual JSON export method.

Best Practices

Before Converting

• Run DRC in EasyEDA first: Fix any errors before exporting to avoid inheriting problems.
• Document your component list: Keep a spreadsheet of LCSC part numbers for reference.
• Export fresh JSON files: Don't use old exports - make new ones right before conversion.

During Conversion

• Convert PCB before schematic: This ensures footprint libraries are available when opening the schematic.
• Keep both files in the same folder: The conversion tools expect them together.
• Use project-specific libraries: Avoid polluting your global libraries with converted components.

After Converting

• Print and verify footprints: Always check critical components at 1:1 scale.
• Run ERC and DRC: Let KiCad catch any issues the conversion missed.
• Manually check power connections: Verify VCC, GND, and other power nets are correct.
• Keep the original EasyEDA files: Never delete your originals until the KiCad version is fully verified.

Conclusion

Converting EasyEDA designs to KiCad is entirely possible with the right tools and workflow. While no conversion is perfect, the combination of automated tools and manual verification ensures you can successfully migrate your projects.

For simple component imports, use easyeda2kicad.py or the KiCad plugin. For quick PCB conversions, the Wokwi online tool is fastest. For complete projects with schematics, use easyeda2kicad6.

Remember: always verify converted footprints against datasheets, run DRC/ERC checks, and keep your original EasyEDA files as backup. With careful verification, you can confidently use converted designs for production.