<copperpour />

Overview

The <copperpour /> element lets you quickly create a copper pour (groundplane) that is connected to a specific net. Groundplanes improve signal integrity by giving high-frequency and return currents a short path, reduce electromagnetic interference, and act as a thermal sink for heat-producing components.

A copper pour automatically flows around component keep-outs and pads while maintaining a clearance gap that you control.

Basic Usage

Add a copper pour to any board by connecting it to a net—most commonly net.GND. Set useThermalReliefs to connect same-net plated holes through thermal spokes instead of merging each hole directly into the surrounding copper. The example below shows two grounded through-holes with thermal reliefs beside two unconnected holes.

export default () => (
  <board width="18mm" height="10mm">
    <pinheader
      name="J1"
      pinCount={4}
      footprint="pinrow4"
    />
    <trace name="J1_GND_1" from=".J1 > .pin1" to="net.GND" />
    <trace name="J1_GND_2" from=".J1 > .pin2" to="net.GND" />
    <copperpour
      connectsTo="net.GND"
      layer="top"
      padMargin="0.45mm"
      useThermalReliefs
    />
  </board>
)

Thermal reliefs currently use four 0.3mm spokes. Unconnected plated holes and plated holes on other nets continue to receive the normal clearance from the pour.

Copper Pour Properties

Property	Description	Example
`connectsTo`	Net that the pour is tied to. Often `net.GND` or `net.VCC`.	`"net.GND"`
`layer`	PCB layer for the pour (`"top"`, `"bottom"`, or an inner layer name).	`"top"`
`clearance`	Default minimum distance between the pour and other features (e.g. pads, traces, board edge). This is used as a fallback for specific margin properties. Defaults to `0.2mm`.	`"0.3mm"`
`padMargin`	Minimum distance from component pads. Overrides `clearance`.	`"0.4mm"`
`traceMargin`	Minimum distance from traces on other nets. Overrides `clearance`.	`"0.1mm"`
`boardEdgeMargin`	Minimum distance from the board edge. Overrides `clearance`.	`"2mm"`
`cutoutMargin`	Minimum distance from board cutouts. Overrides `clearance`.	`"0.1mm"`
`useThermalReliefs`	Connect same-net plated holes through four thermal spokes instead of solid copper.	`true`
`outline`	Optional polygon describing a custom pour boundary.	`[{ x: -10, y: -8 }, { x: 10, y: -8 }, ...]`

Creating Pours on Multiple Layers

You can add separate pours for different layers to create stitched groundplanes or dedicated power planes.

Use vias tied to the same net to stitch pours between layers and further reduce impedance.

Relationship to Automatic Pours and Autorouting

automaticPoursEnabled is a board-level convenience that generates implicit pours for nets marked or recognized as power or ground. Those pours are generated after PCB traces have been routed, and the feature is skipped when PCB routing is disabled. They do not cause the autorouter to skip power-net traces or treat an entire layer as a dedicated plane.

Use <copperpour /> instead when you need to choose the exact net, layer, outline, or clearance. Avoid defining an explicit pour over a region that is also filled by an automatic pour unless the overlap is intentional.

To make source-only power connections—traces with one component endpoint and one net endpoint—from a dense package terminate on an inner plane, combine explicit pours with a fanout routing phase:

<autoroutingphase
  autorouter="fanout"
  fanoutRoutingLayers={["top", "bottom"]}
  fanoutPourNetMap={{ inner1: "GND", inner2: "V3_3" }}
/>
<copperpour connectsTo="net.GND" layer="inner1" />
<copperpour connectsTo="net.V3_3" layer="inner2" />

See <autoroutingphase /> for details.

Tips for Effective Groundplanes

Keep sensitive signal traces short and route them over solid groundplane areas when possible.
Use consistent clearances—tight enough to maximize copper, but wide enough to satisfy fabrication rules.
Add stitching vias between pours on different layers to reduce loop area.
Consider splitting pours if you need isolated analog and digital ground regions, connecting them at a single point.

<copperpour /> makes it easy to drop in broad ground coverage with sensible defaults, while still giving you the control needed for detailed PCB layout.

Overview​

Basic Usage​

Copper Pour Properties​

Creating Pours on Multiple Layers​

Relationship to Automatic Pours and Autorouting​