How to Convert Altium & Eagle Projects to KiCad (Step-by-Step)

If you’ve spent any time in the PCB design world, you know the frustration of dealing with projects stuck in proprietary formats. Maybe you inherited an old Eagle design from a colleague, received reference files from a vendor in Altium format, or simply want to migrate your entire library to an open-source solution. Whatever your situation, converting Altium to KiCad or Eagle to KiCad doesn’t have to be a nightmare.

I’ve been through this process dozens of times—importing TI reference designs, rescuing legacy boards from defunct Eagle installations, and helping clients move their entire portfolios to KiCad. In this guide, I’ll walk you through everything you need to know about EDA project conversion, including the native methods, third-party tools, and the gotchas that nobody tells you about until you’re knee-deep in broken netlists.

Why Engineers Are Moving to KiCad

Before diving into the how, let’s briefly address the why. KiCad has transformed from a hobbyist tool into a legitimate professional PCB design suite. With the release of KiCad 7 and the substantial improvements in KiCad 8 and 9, the import capabilities have expanded dramatically.

The biggest drivers for migration include:

The discontinuation of standalone Eagle by Autodesk (scheduled sunset in 2026) has left thousands of engineers scrambling for alternatives. Altium Designer’s subscription costs can be prohibitive for small teams or independent consultants. KiCad offers unlimited board size, layer count, and schematic complexity—no artificial limitations like Eagle’s free version had.

Understanding File Formats Before Conversion

Getting familiar with the file extensions you’re dealing with saves headaches later. Here’s what you’ll encounter:

Altium Designer File Formats

File Extension	Description	KiCad Equivalent
.SchDoc	Schematic document	.kicad_sch
.PcbDoc	PCB layout file	.kicad_pcb
.PrjPcb	Project file	.kicad_pro
.SchLib	Symbol library	.kicad_sym
.PcbLib	Footprint library	.kicad_mod
.IntLib	Integrated library	.kicad_sym + .kicad_mod

Eagle File Formats

File Extension	Description	KiCad Equivalent
.sch	Schematic file	.kicad_sch
.brd	Board layout file	.kicad_pcb
.lbr	Library file (symbols + footprints)	.kicad_sym + .kicad_mod

KiCad Native Formats

Understanding KiCad’s own formats helps when troubleshooting:

File Extension	Purpose
.kicad_pro	Project file
.kicad_sch	Schematic
.kicad_pcb	PCB layout
.kicad_sym	Symbol library
.kicad_mod	Single footprint (inside .pretty folder)

Converting Altium Designer Projects to KiCad

Method 1: Native KiCad Import (Recommended)

Since KiCad 7, the built-in Altium importer has become remarkably capable. KiCad 8 added symbol library support, and KiCad 9.0.3 introduced direct .PrjPcb project file import. This is now the preferred method for most Altium to KiCad conversions.

Step 1: Prepare Your Altium Files

Make sure you have clean, uncorrupted source files. If possible, open them in Altium first and verify everything renders correctly. Note any custom fonts or special characters that might not translate.

Step 2: Import the PCB Layout First

Open KiCad and go to File → Import Non-KiCad Project → Altium Project (for KiCad 9.0.3+) or import files individually:

1. In the PCB Editor, select File → Import → Non-KiCad Board File
2. Choose your .PcbDoc file
3. Select a destination folder for the converted project
4. When the layer mapping dialog appears, click “Auto-Match Layers” first
5. Review each layer assignment—pay special attention to mechanical layers

Step 3: Handle Layer Mapping

This is where many engineers trip up. Altium uses different naming conventions:

Altium Layer	KiCad Equivalent
Top Layer	F.Cu
Bottom Layer	B.Cu
Top Overlay	F.SilkS
Bottom Overlay	B.SilkS
Top Solder	F.Mask
Bottom Solder	B.Mask
Top Paste	F.Paste
Keep-Out Layer	Edge.Cuts
Mechanical 1-16	User.1-User.9 or Dwgs.User

Step 4: Import Schematics

For hierarchical designs, start with the top-level schematic:

1. In the Schematic Editor, go to File → Import → Non-KiCad Schematic
2. Select the top-level .SchDoc file
3. KiCad will automatically pull in sub-sheets for hierarchical designs

Step 5: Verify and Clean Up

Run the Design Rules Check (DRC) in both the schematic and PCB editors. Common issues include unconnected nets where the importer couldn’t match components, missing footprint associations, and DRC rules that didn’t transfer (these need to be recreated manually).

Method 2: Using altium2kicad Converter

For older KiCad versions or complex designs where the native importer struggles, the altium2kicad Perl scripts provide an alternative path.

Prerequisites:

• Perl installed on your system
• Git for downloading the converter
• Optionally: FreeCAD for 3D model conversion

Conversion Process:

git clone https://github.com/thesourcerer8/altium2kicad/cd altium2kicadperl unpack.plperl convertschema.plperl convertpcb.pl

The converter unpacks Altium’s compound document format and translates each element. Keep in mind that design rule settings won’t transfer—you’ll need to recreate them manually.

Converting Eagle Projects to KiCad

Eagle to KiCad conversion is generally smoother than Altium, largely because KiCad has had Eagle import support for longer. However, there are still quirks to navigate.

Native KiCad Import for Eagle Projects

Step 1: Access the Import Function

In KiCad’s main window, go to File → Import Non-KiCad Project → Eagle Project. Select your .sch file—KiCad will automatically locate the corresponding .brd file if they share the same base name.

Step 2: Map Custom Layers

Eagle users often create custom layers for documentation or manufacturing notes. When the layer mapping dialog appears, you’ll need to manually assign these:

• Eagle Milling layer → KiCad Edge.Cuts
• Eagle Document layers → KiCad Dwgs.User or Cmts.User
• Eagle Reference layers → KiCad Fab layers

Step 3: Address the Component Position Issue

Here’s something that catches many engineers off guard: after importing, if you click the “Update PCB from Schematic” button, all component positions reset. The footprints scatter off the board outline because the imported project lacks the UUID links that KiCad uses to maintain schematic-to-PCB relationships.

The workaround involves either avoiding that button until you’ve established proper links through manual annotation, or using a Python script to save and restore component positions.

Converting Eagle Libraries to KiCad

If you have a substantial Eagle library that you want to bring into KiCad, you have several options:

Option 1: eagle-lbr2kicad ULP Script

This runs from within Eagle and converts .lbr files directly:

1. Download the eagle-to-kicad-libs repository from GitHub
2. Open Eagle and run the eagle-lbr2kicad-1.0.ulp script
3. Select your .lbr file and specify the output directory
4. The converter generates KiCad .lib and .mod files

Option 2: SnapEDA Converter

SnapEDA offers a free online Eagle to KiCad library converter. Upload your .lbr file, and it generates KiCad-compatible symbol and footprint libraries. This works well for smaller libraries and eliminates the need to have Eagle installed.

Option 3: Direct Import (KiCad 8+)

Recent KiCad versions can open Eagle library files directly, though in read-only mode. For long-term use, you’ll want to migrate these to native KiCad format using the library migration feature under Preferences → Manage Symbol Libraries.

Working with BRD Files in KiCad

The .brd extension gets confusing because both older KiCad versions and Eagle used it. Here’s how to handle different scenarios:

Eagle .brd Files

Import through File → Import → Non-KiCad Board File and select “Autodesk Eagle Board Files” from the file type dropdown.

Legacy KiCad .brd Files

If you have old KiCad projects (pre-version 4) with .brd extensions, modern KiCad opens these automatically. The file will be converted to .kicad_pcb format when you save.

Identifying the Source

Not sure what created a .brd file? Open it in a text editor. Eagle .brd files are XML (version 6+) or binary (older versions). Old KiCad .brd files start with “PCBNEW-BOARD Version”.

Converting from KiCad to Altium or Eagle

Sometimes you need to go the other direction—sending files to a client who uses Altium or collaborating with a team stuck on Eagle.

KiCad to Altium

Altium Designer includes a native KiCad import wizard:

1. In Altium, go to File → Import Wizard
2. Select “KiCad Design Files” (may require enabling the extension under Extensions & Updates)
3. Add your .kicad_sch and .kicad_pcb files
4. Map symbols and footprints as prompted
5. Configure output directories and click Finish

The import quality varies—complex designs may require cleanup, and custom footprints sometimes need adjustment.

KiCad to Eagle

Unfortunately, Eagle never implemented KiCad import functionality. Autodesk’s support team has acknowledged requests for this feature but hasn’t delivered it. Your options are limited to:

• Exporting Gerbers from KiCad and importing those into Eagle (layout only, no editability)
• Manual recreation of the design
• Third-party conversion services (use with caution)

Allegro to KiCad Conversion

Cadence Allegro uses proprietary binary formats that KiCad doesn’t natively support. However, there are workarounds:

Using the System76 Converter

System76 developed a Rust-based Allegro to KiCad converter for their internal use and released it as open source:

git clone https://github.com/system76/kicad-allegrocargo build –release./target/release/allegro2kicad input.brd output.kicad_pcb

This handles Allegro extract files but may not support all features.

IDF Export/Import

For board outline and component placement, you can export from Allegro as IDF (Intermediate Data Format) and import into KiCad. This won’t bring in traces or routing but gives you a starting point.

Common Conversion Issues and Solutions

Missing Footprints After Import

Problem: Components appear in the schematic but lack footprint assignments in the PCB.

Solution: Open Symbol Editor, locate the affected symbols, and manually assign footprints using the footprint field. Run “Update PCB from Schematic” to sync.

Broken Net Connections

Problem: The DRC shows unconnected items that were connected in the original design.

Solution: This often happens with power symbols and global labels. Check that net names match exactly, including case sensitivity. KiCad treats “VCC” and “Vcc” as different nets.

Layer Misalignment

Problem: Copper pours or tracks appear on wrong layers.

Solution: Review your layer mapping and re-import if necessary. For minor issues, select affected objects and use Edit → Change Layer.

3D Model Conversion

Problem: STEP files from Altium don’t appear in KiCad’s 3D viewer.

Solution: KiCad prefers WRL (VRML) format for 3D models. Use FreeCAD to batch-convert STEP files:

• Open FreeCAD and load the STEP file
• Export as VRML (.wrl)
• Update the footprint’s 3D model path in KiCad

Best Practices for Successful Migration

Based on my experience with hundreds of conversions, here’s what works:

Always convert a test project first. Don’t migrate your most complex board on day one. Start with something simple to understand the quirks.

Keep original files intact. Conversion is one-way. Store your Altium or Eagle files somewhere safe before starting.

Document your layer mapping. If you establish a consistent mapping scheme, create a reference document for future projects.

Verify against Gerbers. Generate Gerber files from both the original and converted designs, then overlay them in a Gerber viewer to spot discrepancies.

Update libraries post-migration. Don’t just use imported libraries indefinitely. Gradually replace them with native KiCad symbols and footprints to avoid compatibility issues in future KiCad versions.

Useful Resources and Tools

Official Downloads and Documentation

Resource	URL
KiCad Official Download	https://www.kicad.org/download/
KiCad Documentation	https://docs.kicad.org/
KiCad Forum	https://forum.kicad.info/
KiCad GitLab (Issue Tracker)	https://gitlab.com/kicad/code/kicad

Conversion Tools

Tool	Purpose	Link
altium2kicad	Perl-based Altium converter	https://github.com/thesourcerer8/altium2kicad
eagle-to-kicad	Eagle schematic/library converter	https://github.com/lachlanA/eagle-to-kicad
eagle-to-kicad-libs	Eagle library converter	https://github.com/lachlanA/eagle-to-kicad-libs
SnapEDA Converter	Online Eagle library converter	https://www.snapeda.com/
Futureware Converter	Online Altium converter	https://www2.futureware.at/KiCad/
kicad-allegro	Allegro to KiCad converter	https://github.com/system76/kicad-allegro

Component Libraries

Library	Description
KiCad Official Libraries	https://kicad.github.io/
SnapMagic (SnapEDA)	Free symbols/footprints
Ultra Librarian	Multi-format CAD models
Component Search Engine	Manufacturer-verified models

Frequently Asked Questions

Can I convert Altium projects to KiCad without owning Altium?

Yes. KiCad’s native importer reads Altium files directly without needing Altium installed. The altium2kicad converter also works independently. You only need access to the source files (.SchDoc, .PcbDoc, etc.).

Will my design rules transfer during conversion?

Generally, no. Design rules (trace width, clearance, via sizes) rarely survive conversion intact between any EDA tools. Plan to manually recreate your DRC rules in KiCad after importing the layout. This is actually a good opportunity to review and update your design rules.

How do I handle multi-sheet schematics from Eagle or Altium?

KiCad supports hierarchical schematics. When importing, select the top-level schematic file, and KiCad will attempt to pull in referenced sub-sheets. For flat multi-sheet designs, you may need to import each sheet separately and then establish the hierarchy in KiCad.

My converted PCB shows DRC errors everywhere. Is this normal?

Some DRC errors after import are expected. Missing net connections, clearance violations, and unconnected pins often result from format differences. The key is distinguishing between false positives from import artifacts versus genuine design issues. Review each error type systematically.

Is there a way to automate batch conversion of multiple projects?

For Eagle projects, the ULP scripts can be modified for batch processing. For Altium, you’d need to script around the command-line import options or use the altium2kicad Perl converter with shell scripting. The KiCad community forum has several threads with batch conversion solutions that others have shared.

Version Compatibility Matrix

Understanding which KiCad version you need matters for successful conversion. Here’s what each major release supports:

Feature	KiCad 6	KiCad 7	KiCad 8	KiCad 9
Eagle Project Import	Yes	Yes	Yes	Yes
Altium Schematic (.SchDoc)	No	Yes	Yes	Yes
Altium PCB (.PcbDoc)	No	Yes	Yes	Yes
Altium Symbol Library (.SchLib)	No	No	Yes	Yes
Altium Footprint Library (.PcbLib)	No	Partial	Yes	Yes
Altium Integrated Library (.IntLib)	No	No	Yes	Yes
Altium Project File (.PrjPcb)	No	No	No	Yes (9.0.3+)
Eagle Library Import (.lbr)	Via script	Via script	Direct	Direct

For the smoothest experience, use KiCad 9 or later. The import capabilities improve significantly with each release, and bug fixes address many edge cases that caused problems in earlier versions.

Real-World Migration Scenarios

Let me share some actual situations I’ve encountered and how to handle them:

Scenario 1: Inheriting a TI Reference Design

Texas Instruments publishes reference designs in Altium format. To use these in KiCad:

1. Download the .zip file from TI’s website
2. Extract and locate the .SchDoc and .PcbDoc files
3. Import the PCB first using KiCad’s native importer
4. Import each schematic sheet
5. Expect to spend time fixing net names—TI uses specific naming conventions
6. Replace TI’s proprietary footprints with standard ones where possible

Scenario 2: Migrating a Company Library

Moving years of accumulated Eagle libraries requires a systematic approach:

1. Audit your existing library—identify what you actually use versus legacy parts
2. Convert high-priority components first using eagle-lbr2kicad
3. Validate each footprint against datasheets (conversion errors happen)
4. Build a verification checklist covering pad sizes, pin numbering, and 3D models
5. Create a library style guide for your team to maintain consistency

Scenario 3: Collaborating with External Teams

When you use KiCad but your manufacturing partner expects Altium files:

1. Export Gerbers and drill files—these are universal
2. Provide ODB++ or IPC-2581 format if they need intelligent data
3. For schematic review, export PDFs with the built-in BOM
4. Consider using Altium 365 Viewer links for interactive collaboration

Troubleshooting Guide for Specific Errors

“Failed to parse” Errors

This typically means the source file is corrupted or uses features the importer doesn’t recognize. Try opening the file in its native application first, saving a fresh copy, and then importing that copy.

Components Scattered Off-Board

After import, footprints sometimes appear at coordinates far from the board outline. This happens when the original design used a different coordinate origin. In KiCad’s PCB Editor, select all components (Ctrl+A) and use Edit → Move Exactly to relocate them to sensible positions.

Net Names with Special Characters

Altium allows characters in net names that KiCad doesn’t handle well. During import, these get mangled or cause connection errors. You may need to rename nets in the original design before converting, or manually fix net names in KiCad after import.

Polygon Pours Not Filling

If copper pours appear empty after import, the zone priority or clearance settings may be wrong. Select the zone, open its properties, and verify the net assignment. Then click “Edit Zone → Fill Zone” or press B to refill all zones.

Post-Conversion Checklist

Use this checklist after every conversion to ensure nothing was lost:

Schematic Verification:

• All components present with correct values
• All net connections intact
• Power symbols properly connected
• Hierarchical sheet references working
• No ERC errors (or only expected ones)

PCB Verification:

• Board outline matches original dimensions
• All layers present and correctly mapped
• Component count matches schematic
• No orphaned vias or traces
• Copper pours properly filled
• Drill files generate correctly

Library Verification:

• Footprint pad sizes match datasheets
• Pin numbering correct
• Courtyard and silkscreen appropriate
• 3D models assigned where needed

Wrapping Up

Converting Altium to KiCad or Eagle to KiCad isn’t just about file formats—it’s about preserving your engineering work while moving to a tool that gives you more control. The process has gotten dramatically easier with recent KiCad releases, and the community continues to improve import capabilities.

My recommendation: if you’re planning a migration, start now while both your old and new tools are available. Convert a few test projects, establish your workflow, and document your layer mappings. The time investment pays off when you eventually need to migrate production designs or collaborate with teams using different tools.

The open-source nature of KiCad means you’re never locked in again. Your designs remain yours, in formats you can read and manipulate without expensive subscriptions or license servers. That freedom is worth the effort of conversion.

Whether you’re moving from EagleCad to KiCad because of Autodesk’s discontinuation, switching from Altium Designer to KiCad to reduce licensing costs, or exploring Allegro to KiCad conversion for specific projects, the path forward is clearer than ever. Start with the native importers, fall back to third-party tools when needed, and always verify your results against the original design.