Investigate KiCad DRC errors

Run DRC with the intended settings

1. Keep a review copy and its project/custom-rule files. Record the board revision and KiCad version.
2. In PCB Editor, use Inspect → Design Rules Checker. Refill zones for the check and run DRC. Select each finding to inspect its location and rule.
3. Retain the report and exceptions. The JSON command below provides a repeatable way to save results.

Official KiCad 10.0 DRC tutorial

Optional CLI report example

kicad-cli pcb drc \
  --format json --output board-drc-review.json \
  --severity-all --all-track-errors --refill-zones \
  --exit-code-violations board.kicad_pcb

Replace board.kicad_pcb with your review copy and quote paths with spaces. Choose an unused output filename. This is a documented command example, not a newly executed DRC result. POSIX line continuations are shown; in PowerShell remove the trailing backslashes and use one line.

--severity-all includes errors, warnings and excluded violations; --all-track-errors requests all errors on each track. --refill-zones refills for the check but does not save the board unless --save-board is also supplied. The example leaves --save-board out.

With --exit-code-violations, exit code 0 means no reported violations and 5 means violations were found. Investigate other nonzero codes as execution failures. Read echo $? immediately in a POSIX shell, or $LASTEXITCODE in PowerShell, and verify that the new report exists and can be read. Neither code is fabrication approval. Official CLI options

Unconnected items

Identify the reference/pad, net and reported location. Compare the intended connection with the schematic and inspect the track endpoints and zone connection at that point. Visual overlap alone is not evidence of the intended net connection.

Do not rename the net or add copper merely to silence the finding. Record the intended connection and what remains unexplained.

Clearance or short-circuit findings

Select both reported objects and their layer. Record the required and actual clearance and the applicable rule/net class. Compare that rule with the design and fabrication requirements before changing it.

A universally safe clearance value does not exist for every design/process. Lowering the constraint can hide a real problem.

Zone-related findings after edits

Check the zone net/layer and whether the fill is current. KiCad’s official tutorial demonstrates stale fill causing clearance findings after a footprint moves; refilling resolves that tutorial case. Your finding may have a different cause.

Record the refill state, rerun DRC, and inspect remaining findings against zone settings and the intended connection. This page has not run that example on your board.

Outline or layer problems

Inspect the reported Edge.Cuts elements and their endpoints. Look for gaps, overlaps and an unintended layer assignment, using the intended board dimensions as the reference.

Keep the layer, coordinates and intended geometry. An equal number of outline or track segments is not proof of matching geometry.

Schematic-to-board mismatches

Use the intended schematic revision and project. Review component references, footprint assignments and pin/pad relationships before accepting changes from the schematic.

KiCad CLI offers --schematic-parity as a separate check. Do not treat a missing schematic as verified or assume a board-only DRC ran parity checks.

Excluded, ignored or filtered findings

Review disabled rules and excluded findings alongside the visible list. Keep the reason, applicable revision and reviewer decision for each exception.

Hiding a finding does not repair it. If a report is empty, confirm the scope and enabled rules before interpreting the result.

Recheck after a correction

Keep the earlier report, describe the edit and name the new board revision. Rerun with the intended settings, reconcile each earlier finding and record new findings. Leave unresolved items open with an owner and next check.

Choose your next check

Continue the pre-fabrication checklist

If this board was imported from EAGLE, also compare it back to the original design. Open the migration guide and downloadable worked example

The paid BoardPort product compares supported EAGLE 9.6.2 and KiCad 10.0 file pairs offline under three rules: pad/net mapping, footprint references, and defined outline/routed-segment comparisons. It does not run DRC on a standalone KiCad board. Review the exact comparison scope