Moving a legacy Altium or Eagle design into KiCad

You have a board that works. The design files are in Altium or Eagle, the engineer who drew them has moved on, and now a part on it has gone end-of-life or a customer wants a new connector. The license is expiring, or in Eagle’s case the product itself is gone, and the question lands on your desk: can this be moved into KiCad, and what does that actually cost?

The short answer is yes, and the cost is in cleanup, not conversion. The importer takes minutes. Making the result a design you can trust and edit takes days. Most of the pain comes from expecting the first to deliver the second.

What the importer actually converts

KiCad’s importers are real and they have improved fast. The current release, KiCad 10, can import complete projects from Altium Designer (.PrjPcb), Eagle 6 and newer, CADSTAR, EasyEDA, PADS ASCII and gEDA, and can import standalone boards from Allegro, P-CAD, Fabmaster and Solidworks PCB. The full list, with the file extensions, is in the KiCad 10 project manager documentation. The Allegro, PADS and gEDA importers are new in this release, per the KiCad 10.0.0 release notes.

Two caveats in that documentation matter more than the format list:

• Some formats only import as standalone files. The documentation says these “must be manually linked together into a KiCad project.” That linking is where the work is, and it applies to Altium schematics and boards imported separately.
• KiCad has one top-level schematic sheet. A design with several flat top-level sheets has to be imported one sheet at a time and then arranged as hierarchical sheets in a new project. Older Altium and Eagle designs are commonly flat.

For Altium in particular, the documentation recommends importing the board first, saving the project, and then bringing each schematic sheet in afterward. That order is not cosmetic. It gives the schematic a board to link to.

What it silently drops

The converted files open and look right. That is the trap. Here is what typically does not survive, based on the KiCad documentation, the forum reports from this year, and our own experience with imported projects.

The link between symbols and footprints. KiCad ties each schematic symbol to its footprint by a unique identifier, not by reference designator. Imported symbols and imported footprints do not share those identifiers. Until you re-link them, the first “Update PCB from Schematic” can move or delete every part on the board. KiCad has a checkbox for re-linking by reference designator, and the Hackaday walkthrough of Eagle imports shows exactly this failure and the fix. The same workflow, with the footprints exported to a project library first, is what solved the April 2026 kicad.info thread on a KiCad 10 Altium import.

Symbols that are pictures, not parts. The importer embeds symbols and footprints in the schematic and board files rather than putting them in a library. They are editable in place, but they are not in your company library, they carry no datasheet link, and a second board that uses the same part gets a second unrelated copy. A March 2026 kicad.info report on a KiCad 10 release candidate describes imported schematics that look correct but fail the electrical rules check with symbols that are not “real” symbols. Other users in the same thread found current imports usable, but with days of editing afterward. Treat both reports as true: the outcome depends on how the original was drawn.

Intent that lived in the old tool’s rules. Net classes, clearance rules, differential pair definitions, length-matching constraints, the layer stackup and the impedance targets that came from the fab. Some of this converts partially. None of it should be trusted until you have read it back. A design rule check that passes on an imported board with default rules proves nothing.

No-connect markers and power symbols. Pins that were deliberately left open in the source tool show up as errors in KiCad’s electrical rules check because it has no way to tell an intentional open from a mistake. Power symbol conventions differ between tools, so a net that was global in Eagle may become several disconnected nets after import. This one is dangerous because the board still looks fully routed.

Import and clean, or redraw from the import

There are two honest ways to do this job, and the right one depends on what you need the files for.

Import and clean keeps the original copper untouched. You re-link footprints, replace embedded symbols with library parts, rebuild the rules, and add no-connect flags until the electrical and design rule checks are clean. Choose this when the layout must stay identical, for example a product that is already in the field with regulatory test reports tied to that exact board, and the change you need is small.

Redraw from the import treats the imported board as a reference layer. You draw a fresh schematic from library parts, then re-lay the board using the imported copper as a template, keeping the outline, mounting holes and connector positions exact. Choose this when the board is small, the design will keep evolving, or the import is so full of embedded one-off symbols that cleaning them is slower than drawing them. It costs more up front and pays back on the second revision.

The wrong choice is a hybrid: half the symbols replaced, half embedded, rules partly rebuilt. That project will bite the next engineer who opens it.

The checks that prove it matches

Whichever path you take, the imported design is not done until it has been compared with the original by something other than eyesight.

1. Gerber overlay. Generate Gerbers from the KiCad board and compare them layer by layer against the Gerbers the original fab actually built from. The fab files are the ground truth, not the source project. Any difference in copper is a finding to explain.
2. Netlist compare. If the old tool still runs, export its netlist. Diff it against the netlist from the new schematic. Renamed nets are fine. Merged or split nets are not.
3. Bill of materials diff. The import can drop values, tolerances, or manufacturer part numbers that were held in fields the importer did not map. Diff the two BOMs line by line.
4. Footprint audit. Every imported footprint was drawn to someone else’s conventions. Check the ones that matter, fine-pitch packages, QFNs, connectors, against the current manufacturer drawing before you build.
5. Electrical and design rule checks with real rules. Rebuild net classes and clearances from the original fab notes first. Then run the checks. Then read every warning rather than suppressing them in bulk.

Export everything before the license dies

Autodesk states in its EAGLE next steps FAQ that it no longer sells or supports EAGLE as of June 7, 2026, that EAGLE files load directly into Fusion, and that older perpetual licenses keep running on the machine they are installed on. That is the good case. The bad case, which we see more often, is an Altium seat that lapsed years ago or an Eagle install on a laptop nobody can find.

While you can still open the original, export the artifacts that do not depend on any CAD tool. These are what you compare against later, and they are what a fab and an assembler need regardless of which tool the design lives in.

Export from the old tool	Why it matters after the move
Gerbers and drill files as last sent to the fab	The only true record of the built board
Netlist	The reference for the netlist compare
BOM with manufacturer part numbers	Catches dropped fields
Schematic as PDF	Readable by anyone, forever
Board as STEP or 3D PDF	Mechanical fit check for the enclosure
Library files for every part used	Re-importable into KiCad as libraries, not embedded copies
Fab notes, stackup, impedance report	The rules you will rebuild

Keep the original project files too, untouched, in the same repository as the KiCad project. A migration is also the moment to put the design under version control if it is not already.

How we approach it

We take legacy Altium, Eagle and other designs into KiCad as part of obsolete-part redesigns and product updates, and we decide between cleaning the import and redrawing after looking at the files, not before. Send us the original project, the last Gerbers the fab built from, and whatever fab notes you have, and we will tell you which path fits and what the compare will look like when it is done.