The editor

Board layout

The board editor places real footprints, routes copper with a walk-and-shove router, pours and fills zones with thermal reliefs, and checks its own work with DRC — the same board data that goes to fabrication and into the 3D view.

The board editor with the Layers panel open, listing F.Cu, B.Cu, F.Silkscreen, B.Silkscreen, F.Fab, B.Fab, F.Courtyard, B.Courtyard, Cmts.User and Edge.Cuts, plus a Board Setup panel with grid and track-width controls and a Layer stackup link. — The board editor — the Layers panel lists all ten default layers; Board Setup sits opposite.

Footprints

Press A to place a footprint. The chooser searches the installed footprint library — 15,124 footprints across 155 libraries — the same real KiCad .pretty libraries the app ships with, so a footprint's pads, drills and 3D model are the ones the library actually defines, not a redrawn approximation.

Update Board from Schematic, in the Tools menu, brings footprints across from the schematic with their connections as ratsnest lines — the airwires that show what still needs to be routed.

Routing

Press X to route a track and V to drop a via. The router has two modes, walk and shove: walk routes around whatever is in the way, shove pushes existing tracks aside to make room. Switching modes cancels any route in progress, so the next one starts clean in the new mode. Step the active grid with N / ShiftN and the track width with [ / ].

The board editor's floating tool dock: select, place footprint, route a track, place a via, draw a copper zone, draw a board outline and the ruler, with a command-palette chip at the end. — The board dock — eight tools: footprint, route, via, zone, outline and the ruler.

Differential pairs

The diff-pair router shares the same walk/shove toggle as single-track routing. Once a pair is routed, selecting a track on either rail exposes length and skew tuning: a target length for the pair, and a maximum allowed skew between the two rails.

Zones and pours

Press Z to draw a copper zone and B to fill every zone on the board. A filled zone pours copper up to its clearance from everything around it and connects to through-hole pads and vias with thermal relief spokes rather than solid copper, so the pad can still be hand-soldered.

The stackup

The stackup manager describes the board as a real physical cross-section — copper layers, prepreg, solder mask — rather than just a layer count. A new board starts as two copper layers on a 1.6 mm-thick board; layers can be added and the manager keeps the dielectric thickness consistent with the total board thickness you set.

The Board Stackup dialog: 2 copper layers, F.Cu and B.Cu each 0.035 mm, an FR4 dielectric core 1.51 mm thick, and a computed board thickness of 1.6 mm at the bottom. — The Board Stackup dialog — two copper layers, an FR4 core, and the board thickness computed from them.

DRC

Design Rule Check runs against the whole board and returns violations positioned in millimetres, so each one can be selected and jumped to directly. It is not a command you run. There is no Run DRC and no DRC dialog: the check is recomputed with the board on every read, so the count in the status bar and the list in the Violations tab of the properties dock are always current. The agent's run_drc tool reads the same result. A deeper pass — fab producibility, net classes, current, decoupling, return paths, impedance — runs one level above DRC and is described on the agent page.

Bringing in existing work

Rivet PCB reads real .kicad_pcb files and real Altium board files on import. Like the schematic importer, this is read-only: it maps the file into the app's own project format once, on open, rather than keeping a live link back to it.