Why should KiCad Gerbers be reviewed even after DRC passes?

Open the actual exported files and verify the board outline, copper layers, solder mask, silkscreen and drills. Check dimensions and units, not only the visual appearance. A correct board file cannot compensate for an omitted output layer or an old file accidentally included in the upload archive. Generate into a clean revision-specific folder to avoid mixing exports.

Inspect plated and non-plated holes, connector cutouts and the relationship between drill positions and copper pads. Confirm that copper fills were regenerated before export. Review silkscreen around pads and polarity marks, especially where the editor hides overlaps through display settings. The manufacturer's preview is useful, but keep an independently reviewed copy of exactly what was submitted.

For assembly, check reference designators across the BOM, placement file and drawing, plus component rotation, board side and omitted parts. Confirm the supplier's accepted origin and rotation convention rather than assuming every assembler interprets the file identically. DRC checks the design against configured rules; fabrication and assembly review check whether the delivered package communicates the intended product.