<connector />

Overview

A <connector /> represents a physical connector on your board, such as a USB receptacle, wire terminal, or board-to-board header. It behaves similarly to <chip /> for placement and footprint handling, but is specialized for connector use cases.

Connectors support:

• Custom pin naming via pinLabels
• Explicit internal shorting via internallyConnectedPins
• Schematic pin styling and arrangement controls
• Optional connector standard hints for USB-C, M.2, and common JST families

Standard Connector Examples

USB-C

export default () => (
  <board width="30mm" height="20mm">
    <connector name="J_USB" standard="usb_c" />
  </board>
)

JST connectors

For a JST connector, set standard to the connector family and pinCount to the number of electrical circuits. When you do not provide a footprint, the parts engine uses both values to select a compatible part.

export default () => (
  <board width="30mm" height="20mm">
    <connector name="J1" standard="jst_ph" pinCount={2} />
  </board>
)

The supported JST families are:

standard value	JST family	Nominal pitch
"jst_sh"	SH	1.0 mm
"jst_gh"	GH	1.25 mm
"jst_zh"	ZH	1.5 mm
"jst_ph"	PH	2.0 mm
"jst_xh"	XH	2.5 mm
"jst_vh"	VH	3.96 mm

The family determines the pitch, so use the exact family-only value. For example, "jst_sh_2mm" is invalid. pinCount must be a positive integer. To select a specific connector instead of allowing automatic part selection, set manufacturerPartNumber or provide an explicit footprint; an explicit footprint takes priority over standard-based selection.

Custom Footprint Example

export default () => (
  <board width="40mm" height="40mm">
    <connector
      name="J1"
      manufacturerPartNumber="AF_QTZB1_0"
      pinLabels={{
        pin1: ["VCC"],
        pin2: ["D_NEG"],
        pin3: ["D_POS"],
        pin4: ["GND"],
        pin5: ["EH1"],
        pin6: ["EH2"],
      }}
      footprint={
        <footprint>
          <hole pcbX="-2.5mm" pcbY="-2.125mm" diameter="1.3mm" />
          <hole pcbX="2.5mm" pcbY="-2.125mm" diameter="1.3mm" />
          <smtpad
            portHints={["pin1"]}
            pcbX="-3.5mm"
            pcbY="1.575mm"
            width="1.1mm"
            height="3.8mm"
            shape="rect"
          />
          <smtpad
            portHints={["pin2"]}
            pcbX="-1mm"
            pcbY="1.575mm"
            width="1.1mm"
            height="3.8mm"
            shape="rect"
          />
          <smtpad
            portHints={["pin3"]}
            pcbX="1mm"
            pcbY="1.575mm"
            width="1.1mm"
            height="3.8mm"
            shape="rect"
          />
          <smtpad
            portHints={["pin4"]}
            pcbX="3.5mm"
            pcbY="1.575mm"
            width="1.1mm"
            height="3.8mm"
            shape="rect"
          />
          <smtpad
            portHints={["pin5"]}
            pcbX="7.15mm"
            pcbY="-1.475mm"
            width="1.8mm"
            height="4mm"
            shape="rect"
          />
          <smtpad
            portHints={["pin6"]}
            pcbX="-7.15mm"
            pcbY="-1.475mm"
            width="1.8mm"
            height="4mm"
            shape="rect"
          />
        </footprint>
      }
    />
  </board>
)

This example is adapted from the core test for connector cable insertion center behavior: connector-cable-insertion-center.test.tsx.

Cable insertion center

When a connector footprint is rendered, tscircuit computes pcb_component.cable_insertion_center for the connector in circuit JSON. This gives a useful reference point for cable entry direction, annotation, or automation workflows.

In the linked test, the computed cable insertion center is validated and then visualized as a small PCB note rectangle.

Properties

The TypeScript interface for <connector /> is defined in @tscircuit/props:

export interface ConnectorProps extends CommonComponentProps {
  manufacturerPartNumber?: string
  pinLabels?: Record<
    number | SchematicPinLabel,
    SchematicPinLabel | SchematicPinLabel[]
  >
  schPinStyle?: SchematicPinStyle
  schPinSpacing?: number | string
  schWidth?: number | string
  schHeight?: number | string
  schDirection?: "left" | "right"
  schPortArrangement?: SchematicPortArrangement
  internallyConnectedPins?: (string | number)[][]
  standard?:
    | "usb_c"
    | "m2"
    | "jst_sh"
    | "jst_gh"
    | "jst_zh"
    | "jst_ph"
    | "jst_xh"
    | "jst_vh"
  pinCount?: number
}

Property	Type	Description
manufacturerPartNumber	string	Manufacturer part number for the connector.
pinLabels	Record<number | SchematicPinLabel, SchematicPinLabel | SchematicPinLabel[]>	Maps connector pins to one or more net labels.
schPinStyle	SchematicPinStyle	Schematic rendering style for pins.
schPinSpacing	number | string	Pin spacing in schematic symbol.
schWidth	number | string	Schematic symbol width.
schHeight	number | string	Schematic symbol height.
schDirection	"left" | "right"	Direction of the connector symbol pins.
schPortArrangement	SchematicPortArrangement	Schematic port layout strategy.
internallyConnectedPins	(string | number)[][]	Pin groups treated as internally shorted.
standard	ConnectorStandard	Connector interface or product family. See the supported values above.
pinCount	number	Number of electrical circuits. Must be a positive integer.

Like most components, <connector /> also accepts common placement and PCB props from CommonComponentProps such as pcbX, pcbY, rotation, and footprint.