With Autodesk officially ending support for EAGLE on June 7, 2026[1], many of you are actively searching for a reliable free EDA tool. LibrePCB (v2.0+) has emerged as a strong European open-source option. It is free of charge (without limitations!), has an easy-to-install and easy-to-update integrated library manager and - even better - now also features an EAGLE project and library importer, which makes it easier to switch.
For a comparison with other tools, check out the LibrePCB website.
If you are dreading the learning curve of a new EDA tool, here is the good news: LibrePCB works almost exactly like EAGLE. The library concept will feel super similar to what you are already used to, meaning your mental model for building parts still applies.
Nice to know: LibrePCB fixes one of EAGLE’s most notorious legacy constraints: the fragile forward/backward annotation sync. In EAGLE, you are forced to keep both the schematic and board windows open simultaneously, otherwise you risk a ‘consistency error’ that requires tedious manual checks to fix. LibrePCB eliminates this entirely by using a unified project data structure. The forward annotation is natively automatic, your schematic and board are always in perfect sync behind the scenes, even if you close the board viewer.
The importer does most of the work, but because they are two different software architectures, it isn’t pure “click & wait”. So we collected some information about the concepts and minor quirks you need to understand to make your migration painless.
Architectural Constraints & Import Limits
1. Library Links & Component Updates
Both, EAGLE and LibrePCB, embed used components directly into the project files. During an EAGLE import, this link is severed. The components in the imported project have no connection to a LibrePCB Library. If you later improve a footprint in your library, it will not automatically update in an imported EAGLE project. For manufacturing and archiving this does not matter at all.
2. Schematic Changes
- Multi-Sheet Gates: EAGLE allows you to spread the gates of a single component across multiple schematic sheets. LibrePCB’s architecture currently cannot map this, and the import will fail if you leave them split. Workaround: Before you touch LibrePCB, open your legacy project in EAGLE and manually consolidate all multi-sheet gates onto a single schematic sheet.
- Xref Net Labels: These are converted to standard, normal net labels.
- Any device placed on the EAGLE board, that lacks a matching component in the schematic, will be discarded.
3. Geometry and Visual Data
- Layer Stack: Custom EAGLE “User layers” are completely ignored. Any text or polygons on these layers will disappear.
- Line Styles: Dashed or dotted lines are converted to solid, continuous lines.
- Plane Filling: Copper pours are calculated differently in every EDA tool. LibrePCB’s plane-filling algorithm may yield slightly different thermal reliefs or clearance boundaries than your original EAGLE file. Tip: Always visually verify your planes and re-run the DRC before manufacturing.
- Traces and Vias: Curved traces and flat-caps are converted to straight lines with round caps. Rectangular or octagonal vias are forced into standard round vias. Workaround: Manually replace vias by pads after the import.
Design Rule Mapping & Migration Strategy
The importer will map standard constraints, but highly bespoke rules will be lost:
All Supported Design Rules
- Max. tented via diameter (mlViaStopLimit)
- Automatic via annular ring (rvViaOuter; simplified, not separated by top/inner/bottom)
- Automatic THT pad annular ring (rvPadInner; simplified, not separated by top/inner/bottom)
- Automatic stop mask clearance (mvStopFrame)
- Automatic solder paste clearance (mvCreamFrame)
- Min. copper/copper clearance (mdWireWire)
- Min. copper/board clearance (mdCopperDimension)
- Min. drill/drill clearance (mdDrill)
- Min. copper width (msWidth)
- Min. PTH annular ring (rlMinViaInner)
- Min. PTH/NPTH drill diameter (msDrill)
- Any other configured rules will be ignored and initialised with LibrePCB default values.
To minimise friction on your first layout transfer, stick to this workflow:
- Check the format: Ensure your EAGLE files are v6 or later (XML based). Legacy v5 files must be saved in a newer version first.
- Flatten: Consolidate those multi-sheet gates and check for orphaned layout devices.
- Import & Override: Run the project importer. Because highly customised EAGLE design rules default to LibrePCB’s base values during translation, immediately load a standard constraint profile. (If you manufacture with AISLER, import the
LibrePCB Fab: Standardrules under Board Setup → DRC Settings). - Verify: Run a fresh ERC and DRC.
We have written a 
click-by-click tutorial showing exactly how to navigate the LibrePCB 2.0 import wizards for both your Projects and Libraries.