Update Schematic from PCB

Electronics Designer: Update Schematic from PCB (board title bar, the Project view, or edsnx project update-schematic) is KiCad’s back-annotation: it carries board changes back to the schematic. Footprints are matched to their symbol units by the footprint’s (path …) link (or by reference, an option); the dialog lists every change with a checkbox: references (a re-annotated board), values, footprints (library id → the Footprint field), attributes (DNP, exclude from BOM) and net names (a net renamed on the board renames the local and global labels that name it). Nets named by hierarchical labels or power symbols are reported as warnings, not renamed: a power net is named by the power symbols’ value (change it in the schematic), and a local label next to a hierarchical label of the same sheet would not rename the net. A net that leaves its sheet through a sheet pin is renamed with a warning: the sheet pin and the sub-sheet’s hierarchical label keep the old name. A multi-unit part placed in part (a dual op-amp with only unit A on the schematic) is matched to the units that are placed; the warnings list the pads of the missing units and their nets, which cannot be carried back. Update Schematic applies the ticked changes: sheets open in an editor get one undo step each, closed sheets are written to disk.