<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. The example below shows a top-layer pour surrounding a chip, with a few traces stitching components back to ground.

export default () => (
  <board
    width="30mm"
    height="20mm"
  >
    <chip name="U1" footprint="soic8" pcbX={-6} pcbY={0} />
    <resistor name="R1" resistance="10k" footprint="0402" pcbX={6} pcbY={4} />
    <capacitor name="C1" capacitance="100nF" footprint="0402" pcbX={6} pcbY={-4} />
    <trace from=".R1 > .pin2" to="net.GND" />
    <trace from=".C1 > .pin2" to="net.GND" />
    <trace from=".U1 > .pin4" to="net.GND" />
    <copperpour connectsTo="net.GND" layer="top" clearance="0.15mm" />
  </board>
)

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"
thermalRelief	Configure spoke width/count when attaching to pads.	{ spokeWidth: "0.3mm", spokeCount: 4 }
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.

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.