EasyEDA to KiCad Conversion: Migrate Projects Both Ways (Step-by-Step)

After working with both EasyEDA and KiCad for nearly a decade, I’ve lost count of how many times I’ve needed to move projects between these two platforms. Whether it’s collaborating with a team that uses different software, accessing LCSC component libraries in KiCad, or taking advantage of EasyEDA’s JLCPCB integration for a KiCad design—the ability to convert between EasyEDA to KiCad and KiCad to EasyEDA is an essential skill for modern PCB designers.

This guide covers every practical method for migrating projects in both directions, including the tools that actually work, the gotchas that will bite you, and the workflow I’ve refined through dozens of conversions.

Why Convert Between EasyEDA and KiCad?

Before diving into the how, let’s address the why. Both tools are excellent, but they have different strengths that make EasyEDA KiCad interoperability valuable.

When to Convert EasyEDA to KiCad

Scenario	Benefit
Complex multi-sheet designs	KiCad handles hierarchical schematics better
Team collaboration	KiCad’s local files work with Git version control
Advanced routing	KiCad’s push-and-shove router is superior
Offline work required	KiCad works without internet
Long-term archival	Open-source format ensures future access

When to Convert KiCad to EasyEDA

Scenario	Benefit
JLCPCB ordering	One-click ordering with automatic BOM/CPL
LCSC parts library	Direct access to millions of in-stock components
Quick prototyping	Cloud-based, no installation needed
Workshop/teaching	Easier for beginners to access
Cross-platform work	Works on any device with a browser

Many professional designers use both tools: KiCad for complex production designs and EasyEDA for quick prototypes destined for JLCPCB assembly. The Easy EDA to KiCad conversion capability lets you leverage each tool’s strengths.

EasyEDA to KiCad: Complete Conversion Methods

There are four main approaches for EasyEDA to KiCad conversion, each suited to different needs.

Method 1: Wokwi Online Converter (Fastest for PCB Only)

The Wokwi online tool is the quickest way to convert an EasyEDA to KiCad PCB file. It runs entirely in your browser—your files never leave your computer.

Best for: Quick PCB-only conversions when you don’t need the schematic.

Step-by-Step Process:

1. In EasyEDA, open your PCB design
2. Go to Document → Export → EasyEDA Source
3. Save the downloaded JSON file
4. Visit wokwi.com/tools/easyeda2kicad
5. Upload your JSON file
6. Download the converted .kicad_pcb file
7. Open in KiCad PCB Editor

Limitations:

• PCB only (no schematic conversion)
• Some text positioning may need adjustment
• Copper pours may require rebuilding (press ‘B’ in KiCad)

Method 2: easyeda2kicad Python Tool (Best for Component Libraries)

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

Best for: Building a KiCad library from LCSC components for JLCPCB assembly.

Installation:

pip install easyeda2kicad

Basic Usage:

easyeda2kicad –full –lcsc_id=C2040

This creates:

• Symbol in .kicad_sym file
• Footprint in .pretty folder
• 3D model in .3dshapes folder (WRL and STEP formats)

Batch Conversion Example:

easyeda2kicad –full –lcsc_id=C2040    # ESP32-WROOM-32easyeda2kicad –full –lcsc_id=C14663   # STM32F103C8T6easyeda2kicad –full –lcsc_id=C965     # AMS1117-3.3

KiCad Library Configuration:

Setting	Path
Windows	C:/Users/YourName/Documents/Kicad/easyeda2kicad/
Linux/Mac	/home/YourName/Documents/Kicad/easyeda2kicad/

In KiCad:

1. Go to Preferences → Configure Paths
2. Add environment variable EASYEDA2KICAD pointing to your folder
3. Go to Preferences → Manage Symbol Libraries
4. Add: ${EASYEDA2KICAD}/easyeda2kicad.kicad_sym
5. Go to Preferences → Manage Footprint Libraries
6. Add: ${EASYEDA2KICAD}/easyeda2kicad.pretty

Method 3: easyeda2kicad6 (Complete Project Conversion)

For full project migration including both schematic and PCB, the easyeda2kicad6 TypeScript tool is the most comprehensive option for EasyEDA KiCad conversion.

Best for: Complete project migration when you need synchronized schematic and PCB.

Step-by-Step Workflow:

Export from EasyEDA:

1. Open your project in EasyEDA
2. For PCB: Document → Export → EasyEDA Source → save as ProjectName_PCB.json
3. For Schematic: Document → Export → EasyEDA Source → save as ProjectName_SCH.json

Convert PCB First:

1. Run: node dist/main.js “ProjectName_PCB.json”
2. Open the generated .kicad_pcb file in KiCad
3. Review conversion remarks (displayed on the PCB)
4. Add EasyEDA.pretty to your Footprint Libraries (Project Specific)
5. Go to File → Export → Export Footprints to Library
6. Choose “EasyEDA” as library and click OK

Convert Schematic:

1. Run: node dist/main.js “ProjectName_SCH.json”
2. Ensure the schematic file is in the same directory as the PCB
3. Open the .kicad_sch file in KiCad
4. Add the generated .sym file to Symbol Libraries
5. Run Tools → Annotate Schematic (keep existing annotations)
6. Update PCB from Schematic to sync everything

Post-Conversion Checklist:

Task	Why It Matters
Run DRC	Catch conversion errors
Check copper pours	May need rebuilding
Verify text positions	Often shifts during conversion
Review multi-part symbols	May need manual combining
Check power connections	Verify VCC/GND nets

Method 4: KiCad Plugin (GUI-Based Component Import)

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

Installation:

1. In KiCad, go to Plugin and Content Manager
2. Search for “EasyEDA”
3. Install the KiCAD-EasyEDA-Parts plugin
4. Restart KiCad

Usage:

1. Open the plugin from Tools menu
2. Enter an LCSC part number (e.g., C2040)
3. Click Download
4. Component appears in your library

This is essentially a GUI wrapper around easyeda2kicad.py with the same capabilities.

KiCad to EasyEDA: Import Process

Converting KiCad to EasyEDA is more straightforward because EasyEDA has built-in import functionality.

Supported KiCad Versions

KiCad Version	EasyEDA Support	Notes
v4.x	Full support	Direct import
v5.x	Full support	Use archive function
v6.x	Full support	Requires zip packaging
v7.x	Partial	May need v6 re-save
v8.x	Check docs	Use format converter

Step-by-Step KiCad to EasyEDA Import

Prepare Your KiCad Project:

1. Open your project in KiCad
2. Go to File → Archive Project
3. This creates a ZIP file with all dependencies included
4. Alternatively, manually ZIP your .kicad_pcb, .kicad_sch, and symbol library files

Import into EasyEDA Standard:

1. Log into EasyEDA
2. Go to File → Import → KiCAD
3. Select your ZIP file
4. Wait for processing (may take a minute for large projects)
5. Review the imported project

Import into EasyEDA Pro:

1. Open EasyEDA Pro
2. Use the Format Converter tool (recommended for newer KiCad files)
3. Or import directly from the start page
4. Select your archived project ZIP

Common KiCad to EasyEDA Issues

Issue	Cause	Solution
Import fails	Cyrillic/special characters	Remove non-ASCII from filenames
Missing symbols	Symbols not in ZIP	Use KiCad Archive function
Power flags imported as symbols	EasyEDA interprets differently	Delete or convert manually
Design rules lost	Not supported in import	Recreate in EasyEDA
Version incompatibility	KiCad too new	Re-save in older KiCad version

Best Practices for Successful Conversion

After many EasyEDA to KiCad and KiCad EasyEDA conversions, I’ve developed these practices:

Before Any Conversion

Action	Purpose
Run DRC in source tool	Don’t import existing errors
Document component list	Track LCSC part numbers
Export fresh files	Avoid stale cached versions
Back up original	Never convert without backup

During Conversion

Practice	Reason
Convert PCB before schematic	Footprint libraries must exist first
Keep files in same folder	Tools expect co-located files
Use project-specific libraries	Avoid polluting global libraries
Note conversion remarks	Tools flag known issues

After Conversion

Verification	Method
Visual PCB comparison	Open both side-by-side
Run ERC and DRC	Let target tool catch issues
Print critical footprints 1:1	Verify dimensions physically
Check all net connections	Especially power nets
Verify copper pours	Often need rebuilding

Conversion Tools Comparison

Here’s how the main EasyEDA KiCad conversion tools compare:

Tool	Direction	Schematic	PCB	Libraries	3D Models	Difficulty
Wokwi Online	EasyEDA→KiCad	No	Yes	No	No	Easy
easyeda2kicad.py	EasyEDA→KiCad	No	No	Yes	Yes	Medium
easyeda2kicad6	EasyEDA→KiCad	Yes	Yes	Yes	No	Medium
EasyEDA Import	KiCad→EasyEDA	Yes	Yes	Yes	No	Easy
LC2KiCad	EasyEDA→KiCad	Yes	Yes	Yes	No	Advanced

Essential Resources

Here are the key resources for EasyEDA to KiCad and KiCad to EasyEDA conversion:

Resource	URL	Purpose
Wokwi Converter	wokwi.com/tools/easyeda2kicad	Online PCB conversion
easyeda2kicad.py	github.com/uPesy/easyeda2kicad.py	Component library conversion
easyeda2kicad6	github.com/yaybee/easyeda2kicad6	Full project conversion
LC2KiCad	github.com/RigoLigoRLC/LC2KiCad	Alternative converter
EasyEDA Import Docs	docs.easyeda.com/en/Import/Import-KiCAD	Official KiCad import guide
EasyEDA Pro Import	prodocs.easyeda.com/en/import-export/import-kicad	Pro version guide
PyPI Package	pypi.org/project/easyeda2kicad	Python package page
KiCad Forum	forum.kicad.info	Community support

Frequently Asked Questions

Can I convert an EasyEDA project to KiCad and maintain perfect synchronization between schematic and PCB?

Yes, but it requires careful workflow. Use easyeda2kicad6 and convert the PCB first, then the schematic. After importing both into KiCad, run “Update PCB from Schematic” with the option to relink footprints based on reference designators. This reconnects the schematic symbols to PCB footprints. However, expect to spend time manually fixing annotation mismatches and verifying all connections. The conversion isn’t perfect—always run DRC and visually inspect critical areas before trusting the result for manufacturing.

Why do my copper pours disappear or look wrong after EasyEDA to KiCad conversion?

KiCad handles copper pours (zones) differently than EasyEDA. After conversion, you often need to press ‘B’ in KiCad to rebuild all zones. If they still look wrong, check the zone priority settings—the converter may assign incorrect priorities when multiple zones overlap. Also verify that zone net assignments are correct; sometimes the conversion loses the net connection and you’ll need to reassign GND or power nets manually. For complex boards with many zones, budget extra time for zone cleanup.

Is there a way to convert just specific components from EasyEDA/LCSC to use in KiCad without converting an entire project?

Absolutely—this is actually the most common use case. Use easyeda2kicad.py with the LCSC part number to download individual components. For example, easyeda2kicad –full –lcsc_id=C2040 creates a complete KiCad library entry for the ESP32-WROOM-32 including symbol, footprint, and 3D model. You can then use this component in any KiCad project while still ordering from LCSC. Many designers maintain a personal library of converted LCSC parts specifically for this workflow—it gives you access to JLCPCB’s parts inventory without being locked into EasyEDA.

What gets lost or broken during conversion that I should watch out for?

Several things commonly need attention after conversion. Text positioning often shifts—both on silkscreen and in schematics. Multi-part components (like quad op-amps) may split into separate symbols requiring manual recombination. Design rules don’t transfer, so you’ll need to recreate your clearance and trace width rules. PCB art and logos convert to polylines that may need cleanup. Arcs in symbols sometimes malform due to format differences. And critically, always verify power connections—net names like “VCC” and “3V3” may not map correctly between tools. Never trust a conversion blindly; systematic verification is essential.

Can I go back and forth between EasyEDA and KiCad on the same project?

Technically yes, but I strongly advise against treating it as a regular workflow. Each conversion introduces small errors and losses. After a few round-trips, your design accumulates enough issues to cause real problems. Instead, pick one tool as your “source of truth” for each project. If you need to use both tools, maintain the master in one platform and treat conversions as one-way exports. If you must do round-trip development, keep meticulous notes about what changes in each conversion and manually verify everything after each direction change.

Troubleshooting Common Conversion Problems

Even with the best tools, EasyEDA to KiCad conversions can hit snags. Here are solutions to the most common issues I encounter.

Conversion Fails Completely

Symptom	Likely Cause	Fix
“Invalid JSON” error	Corrupted export	Re-export from EasyEDA
Tool crashes	File too large	Split into smaller sections
Empty output	Wrong file type	Ensure you exported “EasyEDA Source” not Gerber
Missing components	Incomplete export	Export schematic and PCB separately

Partial Conversion Issues

Problem	Cause	Solution
Footprints missing	Library not linked	Add EasyEDA.pretty to Footprint Libraries
Symbols not found	Symbol library missing	Add .sym file to Symbol Libraries
Net connectivity lost	Conversion error	Run Update PCB from Schematic
Wrong layer assignments	Layer mapping issue	Manually reassign in KiCad

Visual Differences After Conversion

Some visual differences are expected and don’t affect functionality:

Difference	Impact	Action Needed
Text position shifted	Aesthetic only	Manually adjust if needed
Silkscreen size changed	May affect readability	Verify before ordering
Via appearance	None	KiCad renders differently
Zone fill pattern	None	Press ‘B’ to rebuild

Advanced Conversion Tips

Handling Large Projects

For projects with multiple sheets or boards exceeding 100 components, I recommend this approach:

1. Export each schematic sheet separately
2. Convert PCB first to establish footprint library
3. Convert schematic sheets one at a time
4. Reassemble hierarchy in KiCad
5. Run comprehensive DRC after full assembly

Preserving Design Intent

To maintain design integrity across KiCad EasyEDA conversions:

Aspect	Preservation Method
Trace widths	Document before conversion, verify after
Clearances	Recreate design rules manually
Net classes	Must be recreated in target tool
Via sizes	Check and adjust if needed
Board stackup	Verify layer count and order

Version Control Integration

If you’re using Git for version control:

For EasyEDA projects: Export JSON files regularly and commit them—these are text-based and diff well.

For KiCad projects: The native .kicad_pcb and .kicad_sch files are already text-based and version-control friendly.

For converted projects: Maintain the original files alongside converted versions, with clear naming conventions indicating which is the source of truth.

Conclusion

The EasyEDA to KiCad and KiCad to EasyEDA conversion ecosystem has matured significantly over the past few years. What once required tedious manual recreation can now be accomplished with automated tools that handle most of the heavy lifting.

For component library conversion, easyeda2kicad.py is the gold standard—it lets you access the entire LCSC inventory from within KiCad. For quick PCB conversions, the Wokwi online tool can’t be beat for convenience. And for complete project migration, easyeda2kicad6 provides the most comprehensive solution, though it requires more manual cleanup afterward.

Going the other direction, EasyEDA’s built-in KiCad import works well for most projects. Just remember to use the Archive function in KiCad to ensure all dependencies are included, and watch out for special characters in filenames.

Whichever direction you’re converting, the key to success is systematic verification. Run DRC, check your power nets, verify critical footprints, and never trust a conversion for manufacturing without thorough review.

The ability to move between EasyEDA KiCad platforms gives you the flexibility to use the best tool for each situation—and that’s a competitive advantage worth having.