How to Convert Eagle Files to KiCad: Complete Migration Guide

With Autodesk officially discontinuing Eagle CAD support in June 2026, thousands of PCB designers are looking to migrate their projects to KiCad. If you’ve invested years building Eagle schematics, board layouts, and component libraries, the thought of starting over is daunting. The good news is that KiCad has robust Eagle import capabilities that can save you significant time and effort.

I’ve migrated dozens of Eagle projects to KiCad over the past few years, and while the process isn’t perfectly seamless, it’s far from the nightmare you might expect. This guide covers everything you need to know about converting Eagle files to KiCad, from basic project imports to library conversion and troubleshooting the inevitable issues that arise.

Understanding Eagle and KiCad File Formats

Before diving into conversion, understanding the file formats helps you anticipate potential issues and plan your migration strategy.

Eagle File Types

Eagle uses several file types that you’ll encounter during conversion:

File Extension	Description	KiCad Equivalent
.sch	Schematic file	.kicad_sch
.brd	PCB board layout	.kicad_pcb
.lbr	Component library	.kicad_sym + .kicad_mod
.dru	Design rules	Board setup settings
.ulp	User language programs	Python scripts

Eagle Version Compatibility

KiCad’s import function works best with Eagle XML format files, introduced in Eagle version 6. Here’s what you need to know:

Eagle Version	Format	KiCad Import Support
Pre-6.0	Binary	Not directly supported
6.0 – 7.x	XML	Best compatibility
8.x – 9.x	XML	Schematic works, PCB may fail
Fusion 360	XML	Save as 7.x format first

If you have older binary Eagle files from before version 6, you’ll need to open them in a newer Eagle version and save them as XML format before importing into KiCad. For Eagle 9.x files from Fusion 360, saving a copy in Eagle 7.x legacy format often produces better results during import.

KiCad File Structure

KiCad separates schematic symbols and PCB footprints into different library files, unlike Eagle which combines both in a single .lbr file. This fundamental difference means that during conversion, each Eagle library becomes two KiCad libraries: one for symbols (.kicad_sym) and one for footprints (.kicad_mod or a .pretty folder).

Method 1: KiCad Built-in Eagle Project Import

KiCad 7 and 8 include native Eagle import functionality that handles most conversion tasks automatically. This is the recommended starting point for most users.

Step-by-Step Eagle to KiCad Project Conversion

Step 1: Prepare Your Eagle Files

Before importing, run ERC (Electrical Rules Check) and DRC (Design Rules Check) in Eagle to identify any existing errors. Problems in the original design will carry over and potentially cause more issues after conversion.

Step 2: Create a New KiCad Project Location

Create an empty folder where the converted KiCad project will be stored. Keep this separate from your original Eagle files.

Step 3: Import the Eagle Project

In KiCad’s main window:

1. Go to File → Import Non-KiCad Project
2. Select “EAGLE Project”
3. Navigate to and select your Eagle .sch file
4. The corresponding .brd file loads automatically
5. Select your empty destination folder

Step 4: Map Eagle Layers to KiCad Layers

A layer mapping dialog appears showing Eagle layers on the left and KiCad equivalents on the right. Click “Auto-Match Layers” first, then manually review and correct any mismatches.

Common manual mappings needed:

Eagle Layer	KiCad Layer
Milling	Edge.Cuts
Document	User.Drawings
Reference	F.Fab or B.Fab
tRestrict	F.Courtyard
bRestrict	B.Courtyard

Step 5: Review the Imported Files

KiCad creates the converted schematic and PCB files. Open both and visually inspect for obvious problems like missing components, incorrect layer assignments, or scrambled graphics.

Critical: Fixing the Schematic-to-PCB Link

This is where many people run into trouble. After importing, clicking “Update PCB from Schematic” can cause all component footprints to lose their positions and scatter across the board. To prevent this disaster:

1. Open the PCB editor
2. Click “Update PCB from Schematic”
3. In the dialog that opens, check “Re-link footprints to schematic symbols based on their reference designators”
4. Uncheck “Replace footprints with those specified in the schematic”
5. Click “Update PCB”

These checkbox settings tell KiCad to re-establish the schematic-to-footprint links using reference designators rather than replacing existing footprints. After this first update with these settings, subsequent updates will work normally.

Method 2: Eagle ULP Script Conversion

For more control over the conversion process, especially for older KiCad versions or complex projects, the eagle-to-kicad ULP scripts provide an alternative approach.

What the ULP Scripts Do

The eagle-to-kicad ULP (User Language Program) scripts, available on GitHub, run inside Eagle and produce KiCad-compatible output files. These scripts handle several things the native import doesn’t:

• Multi-sheet schematic conversion with proper net labels
• Multi-part symbol conversion
• Via-to-pad conversion for unconnected vias
• Library extraction from schematics
• Reference designator cleanup

Using the Eagle-to-KiCad ULP Scripts

Prerequisites:

• Eagle version 6.x or newer
• Downloaded ULP scripts from GitHub
• Backup of your original Eagle files

Process:

1. Open your Eagle schematic
2. Run the “run-me-first-from-eagle-sch.ulp” script
3. Select a clean target directory for output
4. The scripts run sequentially, converting:
   1. Schematic sheets
   1. Component references
   1. Library symbols and footprints
5. Import the resulting Eagle PCB into KiCad’s Pcbnew separately

The PCB file still requires KiCad’s native import because the ULP scripts focus on schematic and library conversion.

Converting Eagle Libraries to KiCad

If you have extensive custom Eagle libraries, converting them separately ensures you have a KiCad library for future projects, not just embedded symbols in converted designs.

Method A: KiCad Library Import

KiCad can directly import Eagle .lbr files:

1. Open KiCad’s Symbol Editor
2. File → Import Symbol → EAGLE Library
3. Select your .lbr file
4. Choose destination library
5. Repeat in Footprint Editor for footprints

This method imports symbols and footprints but may not preserve all attributes like LCSC part numbers or custom fields.

Method B: eagle-lbr2kicad ULP

The standalone eagle-lbr2kicad-1.0.ulp script converts Eagle libraries to KiCad format:

1. Open Eagle (any project)
2. Run → eagle-lbr2kicad-1.0.ulp
3. Select the .lbr file to convert
4. Choose output directory
5. Script generates .kicad_sym and .kicad_mod files

Method C: Online Converters

SnapEDA offers a free Eagle to KiCad library converter that handles many library files without needing Eagle installed. Upload your .lbr file and download KiCad-compatible libraries.

Library Conversion Comparison

Method	Requires Eagle	Preserves Attributes	Batch Processing
KiCad Import	No	Partial	No
ULP Script	Yes	Good	No
SnapEDA Online	No	Limited	Yes
eagle2kicad CLI	No	Good	Yes

Common Eagle to KiCad Conversion Problems and Solutions

Even with careful conversion, issues arise due to fundamental differences between the tools.

Problem: Footprint Positions Reset After Schematic Update

Cause: KiCad uses UUIDs (Universally Unique Identifiers) to link schematic symbols to PCB footprints. Immediately after import, these links don’t exist.

Solution: During the first “Update PCB from Schematic” operation, enable “Re-link footprints to schematic symbols based on their reference designators” and disable “Replace footprints with those specified in the schematic.”

Problem: Copper Zone DRC Errors

Cause: Eagle and KiCad handle copper pour clearances differently. Imported zones may have incorrect or zero clearance values.

Solution: Select each zone, open properties (double-click or use Properties panel), and set appropriate clearance values (typically 0.25mm to 0.5mm).

Problem: Keepout Regions Block Everything

Cause: Eagle keepout areas may convert with settings that prevent all copper, not just pours.

Solution: Edit the rule area properties and adjust which items are restricted.

Problem: Text Size Mismatches

Cause: Eagle and KiCad use different default text sizes. Imported text may appear larger or smaller than native KiCad components.

Solution: Use Edit → Edit Text & Graphics Properties in the schematic editor to batch-change text sizes. For precise control, search-and-replace specific size values in the .kicad_sch file (it’s a text file).

Problem: Missing or Broken Component Links

Cause: Eagle stores symbol-to-footprint associations differently than KiCad.

Solution: Use Tools → Edit Symbol Library Links in the schematic editor to reassign symbols to KiCad library versions.

Problem: Unconnected Pin Errors (ERC)

Cause: KiCad flags pins without connections as potential errors. Eagle was more permissive.

Solution: Add “No Connect” flags (press X) to intentionally unconnected pins to clear ERC warnings.

Problem: Old Binary Eagle Files Won’t Import

Cause: KiCad only imports XML-format Eagle files (version 6+).

Solution: Open the file in Eagle 6.x or newer and save it, which converts to XML format. Alternatively, use Fusion 360’s free tier to open and re-save old Eagle files.

Differences Between Eagle and KiCad Workflow

Understanding workflow differences helps you work effectively after migration.

Symbol and Footprint Association

In Eagle, symbols and footprints are tightly coupled in device definitions within libraries. In KiCad, symbols and footprints are separate entities, linked during design via the “Footprint” field. This means:

• Converting Eagle libraries creates two separate KiCad library files
• You have more flexibility in KiCad to use different footprints with the same symbol
• The association must be explicit in KiCad, which can catch mismatches that Eagle allowed

Net Naming

Eagle allows wires to connect by touching endpoints. KiCad requires explicit connections using wire endpoints, junction dots, or net labels. Some Eagle designs may need additional net labels after conversion to ensure proper connectivity.

Design Rules

Eagle design rules (.dru files) don’t convert. You’ll need to manually configure KiCad’s Board Setup with your design rules, including:

• Clearances
• Track widths
• Via sizes
• Net classes

Post-Conversion Cleanup Checklist

After converting an Eagle project to KiCad, work through this checklist:

Schematic:

• Run ERC and address all errors
• Verify all net connections
• Add “No Connect” flags where needed
• Check text sizes for consistency
• Verify power and ground symbols are correct

PCB:

• Run DRC and address all errors
• Verify board outline on Edge.Cuts layer
• Check copper zone clearances
• Verify all drill sizes
• Confirm layer stackup settings
• Check design rules match your manufacturer requirements

Libraries:

• Verify critical footprints match datasheets
• Check pad sizes and shapes
• Confirm 3D model associations if used

Useful Resources for Eagle to KiCad Migration

Software Downloads

Resource	URL	Description
KiCad	kicad.org	Free PCB design software
eagle-to-kicad ULP	github.com/lachlanA/eagle-to-kicad	Conversion scripts
eagle2kicad CLI	teuniz.net/eagle2kicad	Standalone converter

Library Resources

Resource	URL	Description
SnapEDA Converter	snapeda.com	Online library converter
KiCad Official Libraries	gitlab.com/kicad/libraries	Standard KiCad libraries
Ultra Librarian	ultralibrarian.com	Component library downloads
Component Search Engine	componentsearchengine.com	Multi-format library source

Documentation

Resource	URL	Description
KiCad Documentation	docs.kicad.org	Official KiCad docs
KiCad Forums	forum.kicad.info	Community support
Element14 Eagle Import Guide	community.element14.com	Detailed tutorial

When to Convert vs. Redesign

Not every Eagle project is worth converting. Consider these factors:

Convert when:

• The design is complex with many components
• Layout is optimized and validated
• You need to maintain the exact design
• Quick modifications are needed

Redesign when:

• The original design has issues you’d fix anyway
• It’s a simple design that’s quick to recreate
• You want to use KiCad-native library components
• The Eagle design used features that don’t convert well

Many experienced engineers report that for simple designs, recreating in KiCad takes less time than cleaning up a converted project. For complex, validated designs, conversion makes sense even with cleanup required.

Frequently Asked Questions About Eagle to KiCad Conversion

Can I Convert Eagle Files Without Having Eagle Installed?

Yes, for most Eagle 6.x and newer XML-format files, KiCad’s native import works without Eagle. For binary format files (pre-6.0), you’ll need Eagle to first convert them to XML format. Alternatively, SnapEDA’s online converter handles library files without Eagle.

Will My Eagle Libraries Work Directly in KiCad?

Eagle .lbr files cannot be used directly in KiCad, but they can be converted. KiCad can import Eagle libraries through File → Import, or you can use conversion scripts. The converted libraries work well but may need minor adjustments for pin assignments and attributes.

Why Do My Footprints Move When I Update the PCB from the Schematic?

This happens because KiCad hasn’t established UUID links between schematic symbols and PCB footprints after initial import. The fix is to enable “Re-link footprints to schematic symbols based on their reference designators” during the first update. After that, positions remain stable.

Can I Convert Eagle 9.x Files from Fusion 360?

Eagle 9.x schematics usually import correctly, but PCB files often fail silently. The workaround is to save the design in Eagle 7.x legacy format (File → Save Copy for EAGLE 7.x) in Fusion 360 before importing into KiCad.

Is the Conversion Perfect or Will I Need to Fix Things?

Expect to spend time on cleanup. Copper zone clearances, text sizes, keepout regions, and design rules all need attention after conversion. For complex boards, plan for 30 minutes to several hours of cleanup depending on board complexity. Simple two-layer boards convert with minimal issues; complex multilayer designs require more work.

Best Practices for a Smooth Eagle to KiCad Migration

Based on years of helping engineers migrate from Eagle to KiCad, these practices minimize frustration:

Back up everything first. Before any conversion attempt, copy your entire Eagle project folder. Conversion scripts can modify source files, and you don’t want to lose your original work.

Convert one project at a time. Resist the urge to batch-convert all your Eagle projects at once. Each conversion may reveal unique issues, and addressing them one project at a time is more manageable.

Verify critical dimensions. After conversion, measure key dimensions in the KiCad PCB editor and compare against your Eagle originals. Conversion should preserve geometry, but verification catches rare conversion bugs.

Test with a simple fabrication. Before committing to a production run, consider ordering a prototype from your converted KiCad files. This validates that your conversion and any modifications produce a manufacturable board.

Document your conversion process. Keep notes on issues you encounter and solutions that worked. Future conversions will go faster with your own troubleshooting guide.

Join the KiCad community. The KiCad forums at forum.kicad.info are incredibly helpful. Many members have gone through Eagle migrations and freely share solutions to common problems.

Conclusion

Converting Eagle files to KiCad is a practical solution for designers facing Eagle’s end of life. KiCad’s native import handles the heavy lifting for most projects, and the eagle-to-kicad ULP scripts provide additional options for complex conversions.

The key to successful migration is understanding what converts well and what requires manual attention. Schematic connectivity and PCB geometry transfer accurately. Design rules, copper zone settings, and schematic-to-PCB links need manual configuration.

For designers with extensive Eagle history, the migration is worthwhile. KiCad 7 and 8 have matured into capable tools that match or exceed Eagle’s functionality in most areas. The push-and-shove router alone makes the transition rewarding, and the active development community ensures KiCad will continue improving.

Start with a simple project to learn the process, then tackle your more complex designs with confidence. Your years of Eagle work aren’t lost—they’re just moving to a new home in KiCad.