<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>
)

Board Properties

Prop	Type	Description
`width`, `height`	`string \| number`	Define the board's bounding box dimensions in millimeters.
`borderRadius`	`string \| number`	Round the corners of rectangular outlines by the specified radius.
`layers`	`1 \| 2 \| 4 \| 6 \| 8`	Specify the number of copper layers in the board stackup. Defaults to 2 layers.
`autorouter`	`'auto' \| 'sequential-trace' \| 'auto-local' \| 'auto-cloud' \| 'laser_prefab' \| AutorouterConfig`	Select a built-in autorouter preset or provide a configuration object.
`routingDisabled`	`boolean`	Skip routing to speed up development.
`schematicDisabled`	`boolean`	Skip schematic generation for boards that only need the PCB view.
`outline`	`Array<{ x: number, y: number }>`	Supply a custom polygon to replace the default rectangular outline.
`outlineOffsetX`, `outlineOffsetY`	`string \| number`	Offset a custom outline relative to the bounding box origin.
`material`	`'fr4' \| 'fr1'`	PCB substrate material. Defaults to 'fr4'.
`thickness`	`string \| number`	Board thickness in millimeters.
`title`	`string`	Title for the board, displayed in documentation and exports.
`solderMaskColor`	`string`	Color applied to both top and bottom solder masks.
`topSolderMaskColor`	`string`	Color of the top solder mask.
`bottomSolderMaskColor`	`string`	Color of the bottom solder mask.
`silkscreenColor`	`string`	Color applied to both top and bottom silkscreens.
`topSilkscreenColor`	`string`	Color of the top silkscreen.
`bottomSilkscreenColor`	`string`	Color of the bottom silkscreen.
`doubleSidedAssembly`	`boolean`	Whether the board should be assembled on both sides. Defaults to false.
`boardAnchorPosition`	`{ x: number, y: number }`	Moves the board's anchor point to the specified coordinates.
`boardAnchorAlignment`	`'center' \| 'top_left' \| 'top_right' \| 'bottom_left' \| 'bottom_right' \| 'center_left' \| 'center_right' \| 'top_center' \| 'bottom_center'`	Sets which part of the board the anchor point refers to.
`defaultTraceWidth`	`string \| number`	Default width for traces within this board.
`minTraceWidth`	`string \| number`	Minimum allowed trace width for routing.

Customizing the Size of the Board

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

Disabling Routing with `routingDisabled`

The routingDisabled prop is a powerful development speed optimization. When working on component placement and circuit design, autorouting can slow down your iteration cycle. Set routingDisabled={true} to skip the routing step and see your changes instantly:

<board width="20mm" height="20mm" routingDisabled>
  <chip name="U1" footprint="soic8" pcbX={5} pcbY={0} />
  <resistor name="R1" pcbX={-5} pcbY={0} resistance={100} footprint="0402" />
  {/* Traces will show as unrouted ratsnest lines */}
  <trace from=".U1 > .pin1" to=".R1 > .pin1" />
</board>

Why use routingDisabled?

Faster development - Skip routing calculations during component placement
Instant feedback - See layout changes immediately without waiting
Focus on placement - Perfect for optimizing component positions before routing
Better performance - Especially helpful with complex boards that have many traces

Simply remove routingDisabled or set it to false when you're ready to see the final routed board. This workflow significantly speeds up the iterative design process.

Board Material and Colors

You can customize the appearance and manufacturing properties of your board:

Material Selection

Set the material prop to specify the PCB substrate:

"fr4" (default) - Standard fiberglass epoxy laminate
"fr1" - Paper-based phenolic resin (lower cost)

Solder Mask Colors

Customize the solder mask appearance:

solderMaskColor - Sets both top and bottom mask colors
topSolderMaskColor - Sets only the top mask color
bottomSolderMaskColor - Sets only the bottom mask color

Common colors include: "green", "red", "blue", "purple", "black", "white", "yellow"

Silkscreen Colors

Control the silkscreen layer colors:

silkscreenColor - Sets both top and bottom silkscreen colors
topSilkscreenColor - Sets only the top silkscreen color
bottomSilkscreenColor - Sets only the bottom silkscreen color

Example with custom colors:

<board 
  width="30mm" 
  height="20mm"
  material="fr4"
  solderMaskColor="black"
  silkscreenColor="white"
  thickness="1.6mm"
>
  <chip name="U1" footprint="qfn32" pcbX={0} pcbY={0} />
</board>

Double-Sided Assembly

For boards that require components on both sides, set doubleSidedAssembly={true}:

<board width="40mm" height="30mm" doubleSidedAssembly>
  <chip name="U1" footprint="soic8" pcbX={0} pcbY={5} layer="top" />
  <chip name="U2" footprint="soic8" pcbX={0} pcbY={-5} layer="bottom" />
</board>

This informs manufacturing that components will be placed on both the top and bottom layers 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>
)

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>
)

Board Thickness

The board thickness can be specified using the thickness prop (e.g., thickness="1.6mm"). This is important for mechanical fit and impedance control considerations.

Controlling Trace Width

You can set default and minimum trace widths for all traces within a board:

defaultTraceWidth - Sets the default width for all traces (e.g., "0.25mm")
minTraceWidth - Sets the minimum allowed trace width during routing (e.g., "0.15mm")

<board 
  width="30mm" 
  height="20mm"
  defaultTraceWidth="0.3mm"
  minTraceWidth="0.2mm"
>
  <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>

These settings help ensure your traces meet manufacturing requirements and handle the expected current loads.

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
autorouter="laser_prefab" - Reserve prefabricated vias that can be reassigned during routing. Ideal for rapid-turn PCBs produced with laser ablation and mechanical drilling templates. See the Biscuit Board Laser Ablation guide for a complete walkthrough.

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>
)

Learn more about the Autorouting API here

Disable schematic output for mechanical fixtures

Set schematicDisabled when the schematic view would add clutter to the editor or slow down complex mechanical assemblies. The prop is a simple boolean, so you can add it without a value just like any other JSX attribute.

export default () => (
  <board width="20mm" height="20mm" schematicDisabled>
    <fabricationnotetext
      name="Label"
      text="PCB Fixture"
      anchorAlignment="center"
      pcbX={0}
      pcbY={0}
    />
  </board>
)

With schematicDisabled set, the schematic tab shows a placeholder instead of attempting to lay out symbols or connections.

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 },
  ]}
/>
)

Offsetting 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>
)

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>
)

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!

Board Properties​

Customizing the Size of the Board​

Disabling Routing with routingDisabled​

Board Material and Colors​

Material Selection​

Solder Mask Colors​

Silkscreen Colors​

Double-Sided Assembly​

Rounding Board Corners with borderRadius​

Configuring the Layer Stack with layers​

Board Thickness​

Controlling Trace Width​

Setting the autorouter​

Custom Board Outlines​

Offsetting the board origin​

Board Anchor Properties​

Try Different Alignments​

How Anchoring Works​

Flexible PCBs​