Schematic to PCB: from a KiCad schematic to a board, with nothing lost

Three things, and only three. Each symbol brings the footprint named in its Footprint field. Each pad takes the net of the symbol pin with the same number: KiCad’s documentation puts it in one line, “symbol pins are matched to footprint pads by pin/pad number.” And the reference ties the two together, so later updates find the same footprint again.

Nothing else moves. The footprints arrive with ratsnest lines between pads of the same net; board outline, placement and routing come after. That is why the update itself rarely fails loudly: it only has to copy, and the mistakes it can make are copying something incomplete.

1. Open the project (.kicad_pro) from the KiCad project manager, and open the schematic and the board from there.
2. Tools → Annotate Schematic…, so every symbol has a unique reference.
3. Tools → Assign Footprints… until every symbol that goes on the board has a footprint.
4. Run ERC and fix what it finds: the board can only be as connected as the schematic.
5. Tools → Update PCB from Schematic… (F8), from either editor. Read the report, then press Update PCB.

The dialog has six options. Their labels are KiCad’s; the descriptions follow KiCad’s documentation.

The first time, leave them as they are. Later, after you change a part’s footprint in the schematic, tick “Replace footprints with those specified by symbols”, or the board keeps the old one.

These are KiCad 9’s own messages, word for word; ‹ › marks the parts that change. Most are in the report that Update PCB from Schematic shows before it changes anything.

Connector shells are where pin and pad numbers drift apart most often, because every library numbers them its own way. In KiCad 9’s own libraries, the footprint and the symbol agree, and the number changes with the connector family:

Mix a symbol from one source with a footprint from another, one that calls the shell “SH”, “MP” or “SHIELD”, and the shield pin has no pad. The shell lugs are still soldered to the board, just to nothing. On a USB-C board that usually means the shield is not tied to ground, which shows up later as ESD and emissions trouble rather than as a dead board.

Two kinds of pad are meant to have no net: pads with no number at all (the plastic locating pegs on the USB-C and USB-A footprints above are unnumbered) and pins you mark as not connected. Anything else without a net deserves a look.

KiCad has a built-in comparison: in the PCB Editor’s DRC, tick “Test for parity between PCB and schematic”. It reports missing footprints, values that differ from the symbol, pins with no pad, pads with no pin, and pads whose net differs from the schematic. From the command line it is kicad-cli pcb drc --schematic-parity --severity-all --exit-code-violations, which fails the run when anything differs. KiCad AI shows a real run that caught one changed resistor value.

We ran it on a board whose USB-C footprint numbered its shell “SH”. kicad-cli’s report found 0 DRC violations and 0 unconnected pads, and among the parity results, exactly the missing connection:

[net_conflict]: No pad found for pin S1 (GND) in schematic.
    Local override; warning
    @(18.7000 mm, 23.5000 mm): Footprint J1

The parity test compares net names as well as connections. A board that went through another tool can therefore show net_conflict lines for nets that are wired right but named differently (“SCL” for KiCad’s “/SCL”), and for unused pins whose pads have no net where KiCad expects an “unconnected-(…)” one. Read the message: “No pad found for pin” is a missing connection; “Pad net (A) doesn’t match net given by schematic (B)” may only be a name.

To separate naming from wiring, take KiCad’s own netlist (kicad-cli sch export netlist) and compare which pads share a net on the board. These are the nets of the board below, as the netlist names them; on the exported board every one has exactly these pads:

The row worth checking first is GND: J1.S1 is there, and on the board all four of J1’s shell lugs carry it. The last row is just as important the other way round: the USB data and sideband pins and the regulator’s NC pin are unused in this design, and they must stay without a net.

The step KiCad leaves to you, placing and routing, is the one an AI PCB tool takes over. In PCBEditor you drop every .kicad_sch of a KiCad 6 to 9 project (sub-sheets included, or the zipped project) into Workspace > KiCad Native. The schematic opens with KiCad’s connections and your footprints, and Approve → Generate PCB builds the board from it.

The schematic here is a USB-C powered BME280 breakout drawn in KiCad 9: 12 parts, an AP2112K-3.3, 5.1 kΩ on each CC pin, 4.7 kΩ I²C pull-ups and a four-pin header. The generated board is two layers, 23.54 × 28.34 mm, with every net routed and DRC at 0 errors and 0 warnings. Exported back as a KiCad board, every net has exactly the pads the kicad-cli netlist in the table above gives it, shield included. Two auto-named nets carry different names (Net-(J1-PadA5) for Net-(J1-CC1)), which is why the comparison is by pads, not by name.

Then review it like a colleague’s first pass. On this board the regulator and its two capacitors went on the bottom side, which means a second assembly pass; if you want everything on top, say so and generate again. Also check that connectors sit on the edge you want and that the sensor is away from the regulator’s heat. A matching netlist proves the board is connected as drawn, not that it is placed as you would.