<spicemodel />

Overview

<spicemodel /> attaches a SPICE .subckt model to a source component for analog simulation. Use it when a component needs behavior that is not covered by the built-in SPICE output, such as a vendor model, an op-amp macro-model, or a custom diode model.

The model is usually passed through the parent component's spiceModel prop. During simulation, tscircuit maps the .subckt pins to the parent component's ports and emits a subcircuit instance into the generated SPICE netlist.

const rectifierDiodeModel = `
.subckt RECTIFIER_DIODE ANODE CATHODE
D1 ANODE CATHODE DGEN
.model DGEN D
.ends RECTIFIER_DIODE
`

export default () => (
<board routingDisabled>
  <voltagesource
    name="V1"
    voltage="5V"
    frequency="60Hz"
    waveShape="sinewave"
  />
  <chip
    name="D1"
    footprint="0402"
    pinLabels={{
      pin1: "ANODE",
      pin2: "CATHODE",
    }}
    spiceModel={<spicemodel source={rectifierDiodeModel} />}
  />
  <resistor name="RLOAD" resistance="1k" />

  <trace from=".V1 > .pin1" to=".D1 > .ANODE" />
  <trace from=".D1 > .CATHODE" to=".RLOAD > .pin1" />
  <trace from=".RLOAD > .pin2" to=".V1 > .pin2" />

  <voltageprobe name="VP_IN" connectsTo=".V1 > .pin1" />
  <voltageprobe name="VP_OUT" connectsTo=".RLOAD > .pin1" />
  <analogsimulation duration="100ms" spiceEngine="ngspice" />
</board>
)

Properties

Property	Description	Example
source	SPICE source text containing a .subckt declaration.	`.subckt LM358 1 2 3 4 5 ...`
spicePinMapping	Optional map from .subckt pin names to parent component port names. Use this when the SPICE model pins do not match the tscircuit port names.	{{ "1": "pin1", "2": "pin2" }}

Pin Mapping

If a .subckt pin name matches a parent component port name, no mapping is needed. In the diode example above, ANODE and CATHODE match the chip's pinLabels.

Use spicePinMapping when the model uses different pin names or numeric pins:

const lm358Model = `
.subckt LM358 1 2 3 4 5
RIN 2 3 10Meg
.ends LM358
`

export default () => (
  <board>
    <chip
      name="U1"
      footprint="soic8"
      pinLabels={{
        pin1: "OUT",
        pin2: "IN-",
        pin3: "IN+",
        pin4: "V-",
        pin5: "V+",
      }}
      spiceModel={
        <spicemodel
          source={lm358Model}
          spicePinMapping={{
            "1": "pin1",
            "2": "pin2",
            "3": "pin3",
            "4": "pin4",
            "5": "pin5",
          }}
        />
      }
    />
  </board>
)

Every .subckt pin must resolve to exactly one parent port. If a mapped SPICE pin is not present in the .subckt, or if a pin cannot be resolved to a port, tscircuit reports a source_invalid_component_property_error for spiceModel.