EAGLE to KiCad migration: import, then verify.

BEFORE IMPORT

Is this .brd an EAGLE XML board?

The .brd extension alone does not establish compatibility. Inspect a copy in a local text editor without saving changes. The following is an abbreviated, authored example of the structure this product expects.

<?xml version="1.0" encoding="utf-8"?>
<eagle version="9.6.2">
  <drawing>
    <board>
      <!-- board data omitted -->
    </board>
  </drawing>
</eagle>

1. Look for readable XML tags: an eagle element and a board inside drawing. A schematic or a library is a different input.
2. Read the version on eagle, not the XML declaration. Here, 9.6.2 is the EAGLE version; XML 1.0 is not. BoardPort supports the fixed EAGLE 9.6.2 profile.
3. If the text is unreadable or the structure or version is missing or different, treat BoardPort compatibility as unconfirmed. Binary files and other versions are outside this product. Renaming the extension or changing the version text does not convert a file.

Recognizing these markers does not validate the whole XML file or guarantee that KiCad can import it. Preserve the original, import a copy in KiCad, then save the destination as .kicad_pcb. BoardPort does not convert or repair files.

IMPORT WITH KICAD

How to import EAGLE .brd and .sch files into KiCad

KiCad supports importing EAGLE 6.x and later XML projects. That is broader than BoardPort’s EAGLE 9.6.2 comparison profile: a file outside BoardPort’s scope may still be importable with KiCad. KiCad project import documentation

1. Make a working copy. Keep the original project, libraries and any existing manufacturing outputs together. Use a separate destination folder and record which files were imported.
2. For the complete project: In the KiCad project manager, choose File → Import Non-KiCad Project and the EAGLE option. Keep the .sch and .brd with the same base filename together, then choose the destination folder.
3. For a board on its own: Open the PCB Editor and choose File → Import → Non-KiCad Board File. Select the EAGLE file type and your .brd. Review any layer mapping offered and save the result as .kicad_pcb.

Menu names above use the English KiCad 10.0 documentation; labels can differ by language or release. Keep the first saved import before further cleanup. PCB import documentation

kicad-cli pcb import --format eagle \
  --output imported.kicad_pcb \
  --report-format json --report-file import-report.json \
  source.brd

Schematic, PCB and libraries: decide what you are migrating

A board that opens in KiCad is not a complete migrated project. Inventory the files you have, then choose the matching import path. The following is a planning checklist grounded in KiCad 10.0 project documentation; this article did not execute a schematic or library conversion.

KiCad stores used symbols and footprints in the schematic and board files, while important design settings also live in .kicad_pro. Keep that project file when transferring a complete design. Library paths and 3D model locations may depend on environment variables; record any external assets needed on another computer. KiCad: project import, file storage, paths and libraries

Before updating a migrated PCB from a schematic, keep a copy and review the proposed additions, removals and net changes. Record reference, pin/pad and footprint assignments that you have not checked. BoardPort does not verify that relationship and a PCB PASS cannot close this task.

AFTER IMPORT

Five items to review before further editing

1. Keep both files. Keep the original .brd and the first saved .kicad_pcb together. Note their versions and the import date so later edits are distinguishable.
2. Check readability and scope. Use the free compatibility check for the pair. Record unsupported features and warnings; a successful read is not a successful migration audit. Open free compatibility check
3. Review connections and references. For a changed pad-to-net mapping or an added or missing reference, compare the intended design with both source files. The example below shows U1 / 2 and U2.
4. Inspect outline and routing. Inspect the board outline and routing in KiCad. BoardPort only compares the defined normalized outline topology and routed-segment counts; equal counts do not prove identical routes.
5. Keep unresolved checks separate. Record each DIFF and NOT CHECKED with the next action. Run KiCad checks, inspect manufacturing outputs and complete human review separately.

Save these steps as a blank checklist · See what PASS / DIFF / NOT CHECKED mean

DOWNLOADABLE REAL DESIGN

A five-footprint pressure module: from archived import to a traceable difference

This example uses the publicly licensed UCLA locomote Pressure module design. It contains five footprint references and eight connected pads. Download the original EAGLE board, the archived KiCad import and both complete reports without registering or buying BoardPort.

The KiCad 10.0.6 import was recorded on 31 August 2026 at 21:42:40 UTC. On 13 September 2026, we verified the archived file hashes and recomputed the BoardPort reports. We did not rerun KiCad, manufacture the board or test its electrical operation for this article.

A controlled change makes the limit visible. In a separate copy of the destination, we changed only PAD2 pad 1 from N$3 to N$4. The result becomes 2 PASS / 1 DIFF / 0 NOT CHECKED. Footprint references and outline still pass. This edited copy is a test case, not a defect observed in KiCad’s importer.

Record the revision and the evidence you reviewed

Reproduce the example in a separate folder

1. Save the three design files and retain their license notice: EAGLE .brd · archived KiCad import · one-net edited copy · BSD-3-Clause.
2. Compare SHA-256 values with the downloadable manifest. The hashes identify these archived files, not every future KiCad export. File hashes and provenance
3. For your own import, run KiCad in a folder where the new output names do not exist. Use 10.0.6 when comparing with this archived toolchain; newer versions are a separate experiment.

kicad-cli version
kicad-cli pcb import --format eagle \
  --output my-import.kicad_pcb \
  --report-format json --report-file my-import-log.json \
  source.eagle-9.6.2.brd

The archived KiCad log reports 5 footprints, 12 tracks, 0 vias, 0 zones, no warnings and no errors. This is an import log, not a DRC result. Reimports may generate different identifiers or serialization; compare the design and report findings rather than requiring a byte-identical KiCad file. Archived KiCad log

Open both files in KiCad to inspect PAD2 pad 1. In the EAGLE XML, find signal N$3 and its PAD2 / 1 contactref; in the edited KiCad footprint, the pad net is N$4. Review the original design before accepting or correcting this difference. The free compatibility tool can check whether these files are readable; it does not rerun the full comparison. Full BoardPort recomputation requires the product.

Try the free compatibility check · Save all reproduction instructions · PASS JSON · DIFF JSON

Source: UCLA Networked & Embedded Systems Laboratory, locomote, commit 1e199a9. The original design is used under BSD-3-Clause; the KiCad files are converted derivatives and the one-net file has the change described above. The authors do not endorse BoardPort. This example does not include or validate a schematic or a reusable library. Fixed source revision · Import and license record

CONTROLLED COMPARISON · 17 SEPTEMBER 2026

Move PAD2 by 1 mm: all three checks still PASS

A matching net name is not proof of matching placement. Signal & Ship reran the unchanged BoardPort engine on three versions of the publicly licensed Pressure module. Changing PAD2 pad 1 from N$3 to N$4 produced 1 DIFF. Moving only PAD2’s X coordinate from 1.143 to 2.143 mm produced 3 PASS, just like the archived import. This is a measured limit of the comparison rules, not a KiCad DRC result.

The baseline and moved-board findings are identical: eight pad/net mappings, five footprint references, 12 routed F.Cu segments and the four-segment 7.854 × 5.512 mm outline match. The placement edit changes exactly one byte and leaves all track geometry untouched. BoardPort does not compare footprint coordinates; zero NOT CHECKED items means the three supported rules ran, not that every board property was inspected.

Reproduce the edit and inspect the evidence

1. In a new folder, save the archived KiCad file and license. Keep the original unchanged. The original import was made with KiCad 10.0.6 on 31 August 2026, not during this experiment. KiCad A · BSD-3-Clause
2. Find footprint PAD2, UUID 2be6bf36-1879-4222-b6ec-8e6e9ea9ece3. In a copy, change its outer (at 1.143 -1.016) to (at 2.143 -1.016). Do not change the local pad/text coordinates. The downloadable Python helper checks the input SHA-256 and refuses to overwrite an existing output. Edit helper
3. Compare your edited file’s SHA-256 with the manifest and read report C. Full recomputation uses the paid BoardPort product with the same EAGLE original and each KiCad variant. Reading every input/result and reproducing the edit is free; the free compatibility checker only tests readability. Hashes, versions and exact replacement

EAGLE · KiCad B: net edit · KiCad C: placement edit · Save the method and limits

What to do with this result before fabrication

If the net report says DIFF, first locate PAD2 / 1 and establish the intended net from the source. If it says PASS, still inspect the actual footprint position and routing in the reviewed KiCad project. Retain the project/rule version, refill applicable zones, run DRC and investigate its actual findings, then review fabrication outputs. Do not infer any of those outcomes from this comparison.

Scope: one deliberately edited design, not a KiCad importer defect, customer outcome or error-detection rate. The archived generator header is retained to isolate one edit; it does not identify a new KiCad run. No KiCad import/GUI/DRC, schematic test, Gerber generation, manufacturing or electrical test was executed in this experiment. Results use BoardPort 0.1.0-rc.1 and the unchanged engine/rule versions recorded in the manifest. Original authors do not endorse BoardPort.

Method reference: KiCad’s file-format documentation defines at as position/rotation and dimensions in millimeters. This explains the edit; the reports above are the separate executed comparison evidence. KiCad position format

DRC after migration: keep the source comparison separate

The import log, BoardPort comparison and KiCad DRC answer different questions. Preserve the original and first saved import. Use a review copy with its project and custom rules, and check whether the intended stackup, net classes and clearances transferred.

Run DRC and investigate unconnected items, clearance and zone findings · Review the full pre-fabrication checklist

For each finding, locate the reference, pad/net and layer in both designs and retain the intended source connection. A clean DRC result does not prove that the original EAGLE design was preserved. BoardPort compares only its three defined rules.

The archived Pressure module import log has zero zones. Its BoardPort results do not demonstrate DRC or manufacturing validation. In a separate later KiCad 10.0.6 run, we changed one track width and confirmed that one finding disappeared while 18 remained. That board-only case does not establish zone-refill repair, schematic parity or fabrication acceptance.

Read the executed DRC correction and raw reports

COMPLETED RECORD · 22 SEPTEMBER 2026

One finding closed, eighteen left open: what to save

The public Pressure module example was rerun with KiCad CLI 10.0.6. Changing one track from 0.1524 to 0.2 mm removed exactly one default-rule finding: 19 became 18, with no new findings. The filled record keeps the input hashes, versions, raw reports, all eighteen open items and the decision to hold fabrication.

This closes that one finding only. The 0.2 mm value is not a universal fabrication requirement. Five disabled checks, the missing schematic/project settings and the intended fabrication requirements remain open. The first-import BoardPort PASS report is not reused as a report on the later edited board.

1. Open the filled record and match its input revision to the raw report. Every unresolved item keeps its type, object UUID and location. Read the completed record · Raw DRC JSON
2. Save the example for reference. For your own design, save the blank template under a new name and fill it from your own files; do not copy its reviewed status. Save a blank template
3. Leave an owner and next check for each open item. Regenerate DRC and outputs after the next edit; keep the earlier record as the history. Follow this board through output generation

Write a review record on this page

The example is free and needs no registration or upload. It was prepared with AI assistance from retained execution evidence. It is not a customer result or a fabrication approval.

Turn one JSON finding into a review action

This is an excerpt from the existing JSON generated from BoardPort-authored synthetic inputs. PAD_NET_MAPPING reports the changed net on U1 pad 2 and the destination-only mapping for U2 pad 1. It does not establish accuracy for your board or normal KiCad import behavior.

{
  "checkId": "PAD_NET_MAPPING",
  "status": "DIFF",
  "summary": "2 pad-to-net difference(s) require review.",
  "details": [
    "Net changed: U1 pad 2 · EAGLE=VCC · KiCad=GND",
    "Destination-only pad mapping: U2 pad 1 → GND"
  ]
}

DIFF means that the differences need review. Compare both files with the intended circuit and record whether each change is intentional, needs correction or remains unresolved. There are two detail entries within this rule; the summary counts one DIFF for PAD_NET_MAPPING.

Read the complete source JSON · Open the same result as HTML

EAGLE to KiCad migration: common questions

Sources, scope and article updates

On 22 September we rechecked the saved KiCad 10.0 project documentation (retrieved 11 September) and CLI/tutorial documentation (retrieved 17 September), the sold reader and the public example reports. Documentation was not fetched again that day. The commands in the new output case were executed with installed KiCad 10.0.6.

• EAGLE 6.x+ XML project import, same-name .sch/.brd, project storage and external libraries: KiCad project documentation. BoardPort has a narrower fixed input profile.
• BoardPort 0.1.0-rc.1: EAGLE 9.6.2 and KiCad generator 10.0 / format 20260206; pad/net mapping, reference set, normalized line outline and routed-segment counts. HTML/JSON preserve input hashes and scope. Input files and complete reports · A position change these rules do not detect
• DRC options, exit codes and output commands: KiCad 10.0 CLI. Project review, rules, zone fills and output-layer choices: KiCad 10.0 tutorial.

Claim-to-evidence mapping, versions and limitations (JSON)

The mapping above records the earlier review. Its unverified full-layer display was followed by a separate Gerbonara display supplement on the same nine output files. The original record is retained; native GerbView drill overlay and fabrication acceptance remain unverified. Read the later display review and limits · Supplement: input hashes and display scope (JSON)

Changes to this article

• 2026-09-26 — Connected the earlier evidence mapping to the later Gerbonara display review and its limits. No new DRC run, display experiment or fabrication approval is claimed.
• 2026-09-22 — Added an editable review record in English and Japanese. It retains the guide, input revision, evidence, open checks and HOLD boundary in copied or saved notes. Empty fields remain unconfirmed; writing a note does not perform a check.
• 2026-09-22 — Added a filled review record to connect one confirmed removal and eighteen unresolved findings to their exact files; rechecked the main technical claims. Linked the same-revision output example and the next unresolved checks.
• 2026-09-17 — Added the executed 19-to-18 DRC case and replay helper; retained the five disabled checks and missing schematic/project conditions.

Prepared with AI assistance by Signal & Ship. Corrections should identify the article section, file/version and the supporting evidence. Correction contact