English is currently available.
KiCad DISCUSSION
KiCad 10.0.6 is a stable bug-fix release with changes across the editors and output paths. What is a sensible regression check for an existing PCB project after installing it?
For a nearly finished board, which artifacts should be compared before generating the next fabrication package? A successful open and save seems too small a test, but repeating the entire design review may be unnecessary.
Reference: KiCad 10.0.6 release notes (https://www.kicad.org/blog/2026/08/KiCad-10.0.6-Release/).
Preserve the previous project and release outputs, then open a working copy in the updated version. Confirm that symbols, footprints and project-specific libraries resolve correctly. Run ERC and DRC and compare findings with the baseline. Look at the release notes for fixes affecting features the project uses, such as importing, plotting or repeated-sheet workflows.
Regenerate copper fills and manufacturing outputs, then inspect them in a viewer independently of the editor. Compare the outline, drills, copper, mask openings and silkscreen placement. Check BOM and position files if assembly is included. Focus the comparison on unexpected changes; intentional edits made since the previous release should already have an explanation in the revision record.
Record the exact KiCad version and library snapshot with the new package. If an issue appears, reduce it to a small example and retain the original file rather than repeatedly saving over it. Stable maintenance updates can fix important defects, but a controlled check is still useful for detecting project-specific regressions or changes in export configuration.
