Moving from Eagle to KiCad: importing boards, schematics and libraries

Autodesk has retired Eagle. How to import Eagle .sch, .brd and .lbr files into KiCad, what the importer converts, and the checklist to run before ordering boards.

For two decades Eagle was the default PCB tool for hobbyists and small companies, and a huge amount of open hardware — plus countless part libraries — exists only in Eagle format. With Autodesk ending Eagle in 2026 and pointing users to Fusion, KiCad is where most of those designs are moving. The good news: KiCad has a built-in Eagle importer, and it does most of the work.

What you can import

Eagle file	Becomes in KiCad	How
`.sch` + `.brd`	A complete KiCad project	Project manager: the Import Non-KiCad Project command (File menu), then pick the Eagle `.sch`
`.brd` only	A PCB file	PCB Editor: File → Import → Non-KiCad Board File
`.lbr` library	A footprint library you can use directly	Add it in Manage Footprint Libraries with the Eagle library type

Before you import

KiCad reads Eagle's XML format, used since Eagle 6. Files saved by Eagle 5 or older are binary — they have to be opened and re-saved in Eagle 6 or newer first.
Keep the .sch and .brd with the same base name in one folder. The importer pairs them, so the schematic and board stay linked and later changes can be pushed from one to the other.
Write down the design rules (the .dru file) and layer count — you'll re-enter some of them by hand.

What the importer converts

Every symbol and footprint used in the design is extracted into project libraries named after the project, so the imported design no longer depends on the original .lbr files. Nets and net labels, buses, multiple sheets, tracks, vias, polygons (as KiCad zones), text and silkscreen come across. What usually needs attention is everything that was a setting rather than an object: design rules, net classes, and some text styling.

Post-import checklist

Refill zones. Press B in the PCB Editor. KiCad recalculates copper pours with its own rules, and they may differ slightly from Eagle's.
Recreate design rules. Set clearances, track widths and via sizes in Board Setup, and set up net classes for power and signal nets.
Run ERC and DRC. Expect a batch of warnings on the first run — typically unconnected pins that Eagle tolerated, or silkscreen overlapping pads. Work through them; don't just silence them.
Check the text. Eagle's vector font and ratio settings don't map one-to-one, so silkscreen sizes and positions can shift. Tidy it before fabrication.
Verify footprints on paper. Especially parts from old third-party libraries: print 1:1 and place the real components on the printout.
Compare Gerbers. If you have Gerbers made from the original Eagle design, open both sets in KiCad's Gerber viewer and toggle layers — any difference jumps out.

Reusing whole Eagle libraries

Many Eagle library collections were never redrawn for KiCad — connector families (Molex, Phoenix, WAGO, Harting, Weidmüller), relays, transformers, displays, odd packages. To reuse one:

Add the .lbr as an Eagle-type footprint library to browse and place its footprints right away.
To make a footprint editable, open it in the Footprint Editor and save it into one of your own .pretty libraries.
For symbols, check whether your KiCad version lists an Eagle option under Manage Symbol Libraries. If it doesn't, importing any Eagle schematic that uses the parts gives you a project symbol library you can copy them from.
Tidy while you go: KiCad's library conventions (pin 1 marker, courtyard, fabrication layer, reference placement) are stricter than most Eagle libraries.

Next step: organise the converted parts properly — see KiCad libraries, footprints and 3D models.