<schematicsymbol />

Overview

<schematicsymbol /> renders a symbol from the tscircuit symbol library. It is a schematic-only element and does not create a PCB component or footprint.

Use it in either of these ways:

• Render a standalone schematic symbol.
• Show a library symbol as an additional schematic representation of an existing physical <chip />.

Render a Standalone Symbol

Set symbolName to a name from the symbol library.

export default () => (
  <board width="10mm" height="10mm" routingDisabled>
    <schematicsymbol name="D1" symbolName="diode_right" />
  </board>
)

A standalone <schematicsymbol /> can participate in schematic connections, but it has no physical representation on the PCB.

Represent a Physical Chip

Use chipRef together with connections to make the symbol represent ports from an existing physical chip:

• chipRef selects the physical <chip />.
• Each connections key identifies a port exposed by symbolName.
• Each value selects the matching physical port on the referenced chip.

Every port exposed by the symbol must have exactly one connection.

export default () => (
  <board width="20mm" height="12mm">
    <chip
      name="Q1"
      footprint="soic8"
      noSchematicRepresentation
      pcbX={0}
      pcbY={0}
      pinLabels={{
        pin1: "G1",
        pin2: "S1",
        pin3: "G2",
        pin4: "S2",
        pin5: "D2",
        pin6: "D2",
        pin7: "D1",
        pin8: "D1",
      }}
    />

    <schematicsymbol
      name="A"
      chipRef=".Q1"
      symbolName="n_channel_e_mosfet_transistor_horz"
      connections={{
        gate: "Q1.G1",
        source: "Q1.S1",
        drain: "Q1.D1",
      }}
      schX={0}
      schY={0}
    />

    <resistor
      name="R1"
      resistance="10k"
      footprint="0402"
      pcbX={-5}
      pcbY={1}
      schX={-2}
      schY={-0.1}
    />
    <resistor
      name="R2"
      resistance="10k"
      footprint="0402"
      pcbX={5}
      pcbY={1}
      schX={2}
      schY={0.55}
    />

    <trace from=".R1 > .pin2" to=".Q1 > .G1" />
    <trace from=".R2 > .pin1" to=".Q1 > .D1" />
  </board>
)

The connections mapping does not create electrical traces. Normal <trace /> elements still target the physical chip, such as .Q1 > .G1. On the schematic, those traces terminate at the mapped symbol ports. On the PCB, they terminate at the physical Q1 pads.

noSchematicRepresentation hides the chip's default schematic box so only the library symbol is shown. The physical chip still appears once on the PCB.

Pair chipRef with connections

chipRef and connections only take effect when both are provided. If either prop is used by itself, it is ignored and tscircuit emits a source_property_ignored_warning.

Port labels are not matched automatically.

Show Multiple Symbols for One Chip

Multiple <schematicsymbol /> elements can represent different port groups from one physical chip. For example, a dual MOSFET can use symbols named A and B while keeping a single physical Q1:

<chip
  name="Q1"
  footprint="soic8"
  noSchematicRepresentation
  pinLabels={{
    pin1: "G1",
    pin2: "S1",
    pin3: "G2",
    pin4: "S2",
    pin5: "D2",
    pin6: "D2",
    pin7: "D1",
    pin8: "D1",
  }}
/>

<schematicsymbol
  name="A"
  chipRef=".Q1"
  symbolName="n_channel_e_mosfet_transistor_horz"
  connections={{
    gate: "Q1.G1",
    source: "Q1.S1",
    drain: "Q1.D1",
  }}
  schX={-2.5}
/>

<schematicsymbol
  name="B"
  chipRef=".Q1"
  symbolName="n_channel_e_mosfet_transistor_horz"
  connections={{
    gate: "Q1.G2",
    source: "Q1.S2",
    drain: "Q1.D2",
  }}
  schX={2.5}
/>

The name belongs to the schematic representation. The referenced chip keeps its own name and remains the only physical component on the PCB.

To place a representation on a named schematic sheet, set schSheetName on the <schematicsymbol />. Connected schematic components must also be assigned to that sheet. See <schematicsheet />.

Props

Prop	Type	Required	Description
name	string	Yes	Name of this schematic representation. This is currently displayed as its reference text.
symbolName	string	Yes	Symbol name from the tscircuit symbol library.
chipRef	string	No	Selector for the physical chip represented by this symbol. Requires connections.
connections	Record<string, string | string[]>	No	Maps every symbol port label to exactly one port on the chip selected by chipRef.
displayName	string	No	Human-facing name for the schematic representation.
schX	distance	No	X position in the schematic.
schY	distance	No	Y position in the schematic.
schRotation	number | string	No	Schematic rotation in 90-degree increments.
schSectionName	string	No	Schematic section containing the symbol.
schSheetName	string	No	Name of the schematic sheet containing the symbol.