Skip to main content
Built-in Elements

<board />

The <board /> element is a root element that contains all the chips and traces to create a PCB.

You can think of a <board /> like a <body /> element in HTML. Everything goes in a board!

export default () => (
  <board width="10mm" height="10mm">
    <resistor resistance="1k" footprint="0402" name="R1" />
  </board>
)
PCB Circuit Preview

Board Properties​

Customizing the Size of the Board​

Generally you'll use the width and height properties to define the size of the board.

Rounding Board Corners with borderRadius​

To soften sharp corners on a rectangular board, set the optional borderRadius prop. You can pass the radius as either a number—interpreted in millimeters—or as a string like "2mm". The radius is applied uniformly to all four corners.

export default () => (
  <board width="20mm" height="15mm" borderRadius="3mm">
    <chip name="U1" footprint="qfn32" pcbX={0} pcbY={0} />
    <resistor name="R1" resistance="1k" footprint="0402" pcbX={5} pcbY={3} />
    <resistor name="R2" resistance="10k" footprint="0402" pcbX={-5} pcbY={-3} />
  </board>
)
PCB Circuit Preview

Configuring the Layer Stack with layers​

You can set the layers prop to add additional inner layers to your circuit board. If you specify layers={4}, the "inner1" and "inner2" layers are added automatically and available for routing, while omitting the prop keeps the default two-layer stackup.

The following example enables a four-layer board and shows traces connecting components across that stackup:

export default () => (
  <board
    width="32mm"
    height="20mm"
    layers={4}
  >
    <chip name="U1" footprint="soic8" pcbX={-6} pcbY={0} />
    <chip name="U2" footprint="soic8" pcbX={6} pcbY={0} rotation={180} />

    <trace from=".U1 > .pin1" to=".U2 > .pin5" />
    <trace from=".U1 > .pin2" to=".U2 > .pin6" />
    <trace from=".U1 > .pin3" to=".U2 > .pin7" />
    <trace from=".U1 > .pin4" to=".U2 > .pin8" />
  </board>
)
PCB Circuit Preview

Setting the autorouter​

Boards or subcircuits can specify what autorouter should be used to route any traces within them.

Usually you'll want to use an autorouter preset:

  • autorouter="auto" - Uses the platform configuration. For tscircuit.com this defaults to sequential-trace.
  • autorouter="sequential-trace" - Iterate over each trace and use tscircuit's fast built-in autorouter. This method is fast and deterministic but often fails with over 50 traces.
  • autorouter="auto-local" - Use the platform configuration, but only route locally (do not make API calls)
  • autorouter="auto-cloud" - Use the platform configuration for

For complex boards with over 50 traces, you should use autorouter="auto-cloud" to take advantage of tscircuit's cloud autorouters, which internally use the popular freerouting library.

You can also specify a custom autorouter object to use your own autorouter.

export default () => (
  <board
    width="20mm"
    height="20mm"
    autorouter={{
      serverUrl: "https://registry-api.tscircuit.com",
      serverMode: "job",
      inputFormat: "simplified",
    }}
  >
    <chip name="U1" footprint="soic8" pcbX={5} pcbY={0} />
    <resistor
      name="R1"
      pcbX={-5}
      pcbY={0}
      resistance={100}
      footprint="0402"
    />
    <trace from=".U1 > .pin1" to=".R1 > .pin1" />
  </board>
)
PCB Circuit Preview

Learn more about the Autorouting API here

Custom Board Outlines​

You can specify a custom outline for your board by passing an outline prop. The PCB you get will have this outline cut out, this is great when you want a board that's not a rectangle!

export default () => (
<board
  outline={[
    { x: -22.5, y: 24.5 },
    { x: 22.5, y: 24.5 },
    { x: 22.5, y: 16.5 },
    { x: 20.5, y: 16.5 },
    { x: 20.5, y: 12.5 },
    { x: 22.5, y: 12.5 },
    { x: 22.5, y: 2.5 },
    { x: 18, y: -1.5 },
    { x: 18, y: -18 },
    { x: -18, y: -18 },
    { x: -18, y: -1.5 },
    { x: -22.5, y: 2.5 },
    { x: -22.5, y: 12.5 },
    { x: -20.5, y: 12.5 },
    { x: -20.5, y: 16.5 },
    { x: -22.5, y: 16.5 },
    { x: -22.5, y: 24.5 },
  ]}

  // These are currently required due to this issue:
  // https://github.com/tscircuit/core/issues/564
  width="50mm"
  height="50mm"
/>
)
PCB Circuit Preview

Offseting the board origin​

width and height set the board's bounding box (and thus the pcbX/pcbY coordinate system) even when you're using a custom outline. Add outlineOffsetX and outlineOffsetY—measured in millimeters, whether passed as numbers or strings like "5mm"—to slide that outline relative to the bounding box so (0, 0) lands where you expect. Positive offsets push the outline toward increasing pcbX/pcbY coordinates.

In this example the outline is shifted half the board's width and height so the origin stays at the lower-left corner while the shape itself is centered:

export default () => (
<board
  width="40mm"
  height="30mm"
  outlineOffsetX="20mm"
  outlineOffsetY="15mm"
>
  <chip name="U1" footprint="qfn32" pcbX={5} pcbY={5} />
  <resistor name="R1" footprint="0402" resistance="1k" pcbX={10} pcbY={12} />
</board>
)
PCB Circuit Preview

Board Anchor Properties​

You can control the board's position and alignment using anchor properties:

  • boardAnchorPosition: Moves the board's anchor point to the specified coordinates
  • boardAnchorAlignment: Sets which part of the board the anchor point refers to
export default () => (
 <board 
    width="10mm" 
    height="10mm"
    boardAnchorPosition={{x:0, y:0}} 
    boardAnchorAlignment="bottom_left"
  >
  <resistor resistance="1k" footprint="0402" name="R1" pcbX={2} pcbY={2} />

  <fabricationnotetext text="(5,5)" anchorAlignment="bottom_left" fontSize="0.5mm" pcbX={5} pcbY={5} />
  <fabricationnotetext text="(10,10)" anchorAlignment="bottom_left" fontSize="0.5mm" pcbX={10} pcbY={10} />
  <fabricationnotetext text="(0,0)" anchorAlignment="bottom_left" fontSize="0.5mm" pcbX={0} pcbY={0} />

  </board>
)
PCB Circuit Preview

Try Different Alignments​

// This moves the board's center to position (1,2)
<board 
  boardAnchorPosition={{x:1, y:2}} 
  boardAnchorAlignment="center"  // Try changing this to other values
  width="10mm" 
  height="10mm"
>
  <resistor resistance="1k" footprint="0402" name="R1" />
</board>

How Anchoring Works​

  • The boardAnchorAlignment determines which point on the board is considered the anchor point
  • The boardAnchorPosition moves that anchor point to the specified (x,y) coordinates

Example Alignments:

  • "center" - Board is centered on the anchor point
  • "top_left" - Top-left corner is at the anchor point
  • "top_right" - Top-right corner is at the anchor point
  • "bottom_left" - Bottom-left corner is at the anchor point
  • "bottom_right" - Bottom-right corner is at the anchor point
  • "center_left" - Middle of the left edge is at the anchor point
  • "center_right" - Middle of the right edge is at the anchor point
  • "top_center" - Top center point is at the anchor point
  • "bottom_center" - Bottom center point is at the anchor point

Flexible PCBs​

info

Interested in flexible PCBs? Upvote this issue on Github!