Designing Castellated-Edge PCB Modules for Pluggable Daughterboards

Castellated edges — the half-circle plated notches you'll find along the side of an ESP32 module, an nRF52840 breakout, or a Raspberry Pi Pico — let one PCB be soldered directly onto another as if it were a large, oddly-shaped SMD component, without a connector in between. They're the reason tiny modules can be reflow-soldered straight onto a carrier board and still be hand-desoldered and swapped later if needed. Designing your own castellated-edge module is well within reach for a maker using KiCad, but it has a few fabrication-specific gotchas that aren't obvious from datasheet photos alone.

What a Castellation Actually Is

A castellated via is a plated through-hole that sits exactly on the board's edge, so that when the fabricator routs the board profile, the hole is cut in half — leaving a semicircular plated notch on the outside edge of the board. Because the plating runs through the full thickness of the board, that notch carries a solderable copper surface on both the top and bottom of the board edge, which is what lets a reflow fillet form cleanly when the module is placed onto a carrier board pad that extends slightly past the board edge.

Designing the Footprint

In KiCad, castellated pads are built from a plated through-hole placed with its center exactly on the board edge, then given a copper pad shape (and often a matching edge-cut) so the routing operation splits it symmetrically. The practical settings that matter:

ParameterTypical ValueNotes Via/hole diameter0.3-0.6mm drillSmaller holes risk incomplete plating after the board edge is routed away Pad diameterHole + 0.2-0.3mm annular ringNeeds to stay inside standard annular ring tolerances for your fab Pitch between castellations1.27mm (0.05") or 1.0mm minimumTighter pitch increases risk of plating bridging between adjacent castellations Edge clearanceCenter the hole exactly on the board outlineOffsetting the hole leaves a partial, cosmetically uneven castellation and can fail continuity

Most fabricators that support castellated edges (JLCPCB, PCBWay, OSH Park under specific instructions) want the castellation holes placed with their centers precisely on the board edge polygon in your Edge.Cuts layer — if the hole center is even slightly inside or outside the outline, you'll get an asymmetric or missing notch after routing.

Plating-Before-Routing Fabrication Order

The step that makes castellations work reliably is fabrication sequencing: the board must be plated first, then routed along the edge, so the exposed copper inside the via survives the cut with continuous plating around its circumference. If you send a castellated design to a fab that routs before final plating (common on ultra-budget quick-turn runs), you'll get bare, unplated copper exposed at the board edge that oxidizes quickly and solders poorly. When ordering, explicitly flag the board as having castellated holes in your fab notes — most PCB houses have a specific checkbox or note field for this exact purpose, and it changes their process order.

Mechanical and Thermal Considerations

A module relying entirely on castellated-edge solder joints for mechanical retention (no mounting holes or standoffs) is more fragile under flex and vibration than a connector-based interface — fine for a module that's permanently reflow-soldered down, risky for anything that will see repeated mechanical stress or be handled frequently without a surrounding enclosure. If your module needs both electrical and real mechanical strength (for example, a sensor daughterboard on a robot subject to vibration), add a couple of dedicated mechanical-only castellations or a small adhesive/potting step rather than relying on the signal castellations to carry the load.

During reflow, the carrier board's module footprint should extend its copper pad 0.2-0.3mm past the board edge itself, giving the solder paste a path to wick up into the castellation and form a visible, inspectable fillet — a flush, un-overhung pad produces a joint that's much harder to inspect visually or by X-ray.

Testing Continuity Before Committing to a Panel

Before panelizing a design across dozens of modules, order a small test run and check each castellation for plating continuity with a fine-tipped multimeter probe, pressing gently into the notch rather than just touching the surface — a thin, incomplete plating layer can look intact visually while failing continuity under the slight flex of normal handling. It's a cheap check that catches a design/fab mismatch before you've committed a full panel's worth of boards to a bad footprint.

Castellated edges look like a small detail, but getting the footprint geometry and fab instructions right the first time is the difference between a module that drops cleanly onto a carrier board and one that needs manual touch-up soldering on every single unit — worth the extra ten minutes of design review before you hit order.