generateSemiconductorSubcircuitROM

Generate reduced-order model of semiconductor switch by running SPICE

Since R2025a

Syntax

generateSemiconductorSubcircuitROM(libraryPath,subcircuitName)

generateSemiconductorSubcircuitROM(libraryPath,subcircuitName,Name=Value)

ROMParameters = generateSemiconductorSubcircuitROM(libraryPath,subcircuitName,Name=Value)

Description

The generateSemiconductorSwitchROM function converts a SPICE subcircuit into a MOSFET (Ideal, Switching) or IGBT (Ideal, Switching) block, which represents a reduced-order model (ROM). The SPICE subcircuit can describe any n-type semiconductor device with an integral diode. The function parameterizes the ROM with the on-state tabulated I-V curve and tabulated switching losses for the transistor, and with the on-state tabulated I-V curve and tabulated reverse recovery loss for the associated body diode.

Manufacturers often provide SPICE subcircuits that you can use to parameterize Simscape blocks. One option is to generate a lookup table to parameterize a high-fidelity N-Channel MOSFET or N-Channel IGBT block from a SPICE netlist using the ee.spice.semiconductorSubcircuit2lookup function. ROMs are easier to interpret and run faster than high-fidelity semiconductor switch subsystems. Use ROMs to quickly test and analyze system-level scenarios where the semiconductor switch interacts with other systems.

To use this function, you need a SPICE simulation engine. The function supports:

• SIMetrix 8.4 and beyond — You must be able to run SIMetrix in non-GUI Mode. For more information, see Running in non-GUI Mode (SIMetrix Simulator Reference).

• LTspice XVII and beyond.

generateSemiconductorSubcircuitROM(libraryPath,subcircuitName) generates a ROM from the SPICE subcircuit named subcircuitName in the SPICE subcircuit library file on the path libraryPath.

generateSemiconductorSubcircuitROM(libraryPath,subcircuitName,Name=Value) specifies options using one or more name-value arguments in addition to the input arguments in the previous syntax. For example, generateSemiconductorSubcircuitROM(libraryPath,subcircuitName,OnStateGateSourceVoltage=20) generates a ROM with an on-state gate-source voltage equal to 20 V.

Some of the name-value arguments are the test-circuit conditions. You can set these values based on your detailed circuit conditions or a datasheet. These values are optional, but accurate test-circuit conditions provide you with more accurate ROMs.

ROMParameters = generateSemiconductorSubcircuitROM(libraryPath,subcircuitName,Name=Value) returns a structure that contains the lookup table data for the I-V curve and loss of the semiconductor switch and the diode.

Examples

Generate Reduced-Order Model of Simscape MOSFET from SPICE Subcircuit

Since R2026a

This example shows how to generate a Simscape reduced order model (ROM) from a SPICE defined MOSFET by using the function generateSemiconductorSubcircuitROM. The function runs the necessary simulations using LTspice or SIMetrix software.

In this example, you use the values in the manufacturer data sheet of the MOSFET C3M0032120D to define the input arguments of the generateSemiconductorSubcircuitROM function.

Define Input Arguments

Define the input arguments for the generateSemiconductorSubcircuitROM function based on the SPICE simulation tool and operating system.

Define the name of the library that contains the subcircuit to simulate.

filename = "C3M0032120D.lib";

Define the name of the SPICE subcircuit inside the library file.

subcircuitName = "C3M0032120D";

Define the SPICE software used during the simulation. By default, the function uses SIMetrix.

SPICETool = "LTspice";

Define the path of the executable of the SPICE tool used during simulation. The default value is C:\Program Files\SIMetrix910\bin64\Sim.exe. If you are not using a Windows® operating system, or if the path is not the default specified before, this argument is needed.

SPICEPath = "C:\Users\"+ getenv('USERNAME') + "\AppData\Local\Programs\ADI\LTspice\LTspice.exe";

Define the folder for the generated netlists and SPICE outputs.

netlistFolderPath = "SPICENetlists";

Define the vector of terminal orders. The values of this vector define the ports of the semiconductor device to which each node of the SPICE subcircuit connects. For example, observe the definition of the subckt C3M0032120D d g s Tj Tc subcircuit in the library file. The subcircuit defines the nodes for the drain, gate, source, junction temperature, and case temperatures at the positions 1, 2, 3, 4, and 5, respectively. The generateSemiconductorSubcircuitROM function requires you to use the number 1 for the drain, 2 for the gate, 3 for the source, 4 for the base, 5 for the junction temperature, and 0 for no connection. To obtain a ROM, you do not need the case temperature. Use this vector of terminal orders for this MOSFET.

terminals = [1 2 3 5 0];

Define the device type. In this example, the device is a MOSFET.

deviceType = 'MOSFET';

Define the on-state gate-source voltage. Set this argument equal to the gate driver on-state voltage in the destination circuit. To decide the value of it, look at the manufacturer data sheet. The function assigns the value of this argument to the MOSFET gate node. The value of this argument must be within the data sheet limits and greater than the threshold voltage. The threshold voltage of an C3M0032120D MOSFET is equal to 2.5 V and the maximum operational gate-source voltage is equal to 19 V. You can find the threshold voltage value in the Gate Threshold Voltage parameter in the Electrical Characteristic table, and the gate-source voltage value in the Operational Gate-Source Voltage parameter of the Key Parameters table. Specify a value of 10 V for the on-state gate-source voltage.

VgsOn = 10;

Define the off-state gate-source voltage. Set this argument equal to the gate driver off-state voltage in the destination circuit. It must be less than the threshold voltage and greater than the minimum allowed voltage. By default, this value is equal to 0.

VgsOff = 0;

Define the constant current for threshold voltage. The function uses this current value to obtain the switch threshold voltage by measuring the gate voltage at which a constant drain current is first observed. This current is typically very small. The data sheet specifies a value of 15 mA. You can find this information in the Test Conditions column of the Gate Threshold Voltage parameter in the Electrical Characteristic table.

Icc = 0.0115;

Define the on-state gate resistance. The data sheet specifies a value of 5 $$\Omega$$. You can find this information in the Internal Gate Resistance row of the Electrical Characteristics table.

RgOn = 5;

Define the off-state gate resistance. The manufacturer data sheet does not specify a value for this argument. Specify the same value as the on-state gate resistance.

RgOff = 5;

You must specify values within the manufacturer operating range, which for this device is between -55 and 150°C. For this example, choose temperature points of 25 and 75°C.

TVec = [25 75];

Define the on-state current breakpoints for the tabulated I-V curve. This argument specifies the currents at which the function tabulates the device. The values of this argument must be less than the maximum data sheet values, which you can find in the DC Continuous Drain Current parameter of the Key Parameters table.

Define the on-state current breakpoints for switching losses.

IVec = 5:10:45;

Define the off-state voltage breakpoints for switching losses. These values define the voltage breakpoints at which the function tabulates the device diode. The value of this argument must be less than the maximum values. You can find the maximum value in the Drain-Source Voltage parameter of the Key Parameters table.

VVec = [10 50];

Define the gate voltage rise and fall time. The value should be smaller than the turn-on and turn-off time of the device. You can find the values in the Electrical Characteristics table.

GateVoltageRiseFallTimeForLoss = 10e-9;

Adjust these values depending on the circuit where you will use the device. The data sheet does not specify the leakage inductance or stray capacitance, and the final circuit is undetermined in this case. Assume default values of zero.

Lleak = 0;
Cstray = 0;

Generate Reduced Order Model

Generate the ROM.

generateSemiconductorSubcircuitROM(filename, subcircuitName,...
    "SPICETool", SPICETool, "SPICEPath", SPICEPath, "TestNetlistFolder", netlistFolderPath,...
    "OnStateGateSourceVoltage", VgsOn, "OffStateGateSourceVoltage", VgsOff,...
    "ConstantCurrentForThresholdVoltage", Icc, "OnStateGateResistance", RgOn,...
    "OffStateGateResistance", RgOff, "Temperatures", TVec,  ...
    "OnStateCurrentsForIV", IVec, "OnStateCurrentsForLoss", IVec,...
    "OffStateVoltagesForLoss", VVec, "GateVoltageRiseFallTimeForLoss", GateVoltageRiseFallTimeForLoss,...
    "TestCircuitLeakageInductance", Lleak, "TestCircuitStrayCapacitance", Cstray);

Using:
  DeviceType = MOSFET
  Terminals = [1;2;3;5;0]
  OnStateGateSourceVoltage = 10
  OffStateGateSourceVoltage = 0
  ConstantCurrentForThresholdVoltage = 0.0115
  OnStateGateResistance = 5
  OffStateGateResistance = 5
  Temperatures = [25;75]
  OnStateCurrentsForIV = [5;15;25;35;45]
  OnStateCurrentsForLoss = [5;15;25;35;45]
  OffStateVoltagesForLoss = [10;50]
  MaximumSwitchingFrequency = 100000
  GateVoltageRiseFallTimeForLoss = 1e-08
  TestCircuitLeakageInductance = 0
  TestCircuitStrayCapacitance = 0
  Reltol = 0.001
  Abstol = 1e-12
  Vntol = 1e-06
  Gmin = 1e-12
  Cshunt = 0
  SingleSimulationTimeLimit = 100
Extracting switch IV curve ...
Using existing netlist SPICENetlists\C3M0032120D_Vth_I0A0115_T25.net to extract threshold voltage.
Running netlist SPICENetlists\C3M0032120D_Vth_I0A0115_T25.net to extract threshold voltage in SPICE tool LTspice ...
Using existing netlist SPICENetlists\C3M0032120D_SwitchIV_Vg10_I45.net to extract switch current-voltage table.
Running netlist SPICENetlists\C3M0032120D_SwitchIV_Vg10_I45.net to extract switch current-voltage table in SPICE tool LTspice ...
Using existing netlist SPICENetlists\C3M0032120D_Goff_T25.net to extract off-conductance.
Running netlist SPICENetlists\C3M0032120D_Goff_T25.net to extract off-conductance in SPICE tool LTspice ...

Extracting diode IV curve ...
Using existing netlist SPICENetlists\C3M0032120D_DiodeIV.net to extract diode current-voltage table.
Running netlist SPICENetlists\C3M0032120D_DiodeIV.net to extract diode current-voltage table in SPICE tool LTspice ...

Extracting switching loss lookup tables ...
Using existing netlist SPICENetlists\C3M0032120D_Loss_V10_T25.net to extract diode reverse recovery loss table.
Using existing netlist SPICENetlists\C3M0032120D_Loss_V50_T25.net to extract diode reverse recovery loss table.
Using existing netlist SPICENetlists\C3M0032120D_Loss_V10_T75.net to extract diode reverse recovery loss table.
Using existing netlist SPICENetlists\C3M0032120D_Loss_V50_T75.net to extract diode reverse recovery loss table.
Running netlist SPICENetlists\C3M0032120D_Loss_V10_T25.net to extract losses in SPICE tool LTspice.
Running netlist SPICENetlists\C3M0032120D_Loss_V50_T25.net to extract losses in SPICE tool LTspice.
Running netlist SPICENetlists\C3M0032120D_Loss_V10_T75.net to extract losses in SPICE tool LTspice.
Running netlist SPICENetlists\C3M0032120D_Loss_V50_T75.net to extract losses in SPICE tool LTspice.
Running netlist SPICENetlists\C3M0032120D_Loss_V10_T25.net to extract losses in SPICE tool LTspice.
Running netlist SPICENetlists\C3M0032120D_Loss_V50_T25.net to extract losses in SPICE tool LTspice.
Running netlist SPICENetlists\C3M0032120D_Loss_V10_T75.net to extract losses in SPICE tool LTspice.
Running netlist SPICENetlists\C3M0032120D_Loss_V50_T75.net to extract losses in SPICE tool LTspice.

Generate Reduced-Order Model of Simscape IGBT from SPICE Subcircuit

This example shows how to generate a Simscape reduced-order model (ROM) of a SPICE-defined IGBT by using the generateSemiconductorSubcircuitROM function. The function runs the necessary simulations using LTspice or SIMetrix software.

In this example, you use the values in the manufacturer datasheet of the IGBT IKW15N120T2 [1] to define the input arguments of the generateSemiconductorSubcircuitROM function.

Define Input Arguments

Define the input arguments for the generateSemiconductorSubcircuitROM function based on the SPICE simulation tool and operating system.

Define the name of the library that contains the subcircuit to simulate.

filename = "IGBT_1200V_TRENCHSTOP2_L1.lib";

Define the name of the SPICE subcircuit inside the library file.

subcircuitName = "IKW15N120T2_L1";

Define the SPICE software used during the simulation. By default, the function uses SIMetrix.

SPICETool = "LTspice";

Define the path of the executable of the SPICE tool used during simulation. The default value is C:\Program Files\SIMetrix910\bin64\Sim.exe. If you are not using a Windows® operating system, or if the path is not the default specified before, this argument is needed.

SPICEPath = "C:\Users\"+ getenv('USERNAME') + "\AppData\Local\Programs\ADI\LTspice\LTspice.exe";

Define the folder for the generated netlists and SPICE outputs.

netlistFolderPath = "SPICENetlists";

Define the vector of terminal orders. The values of this vector define the ports of the semiconductor device to which each node of the SPICE subcircuit connects. For example, observe the definition of the .SUBCKT IKW15N120T2_L1 C G E PARAMS: TJ= {TEMP} subcircuit in the library file. The subcircuit defines the nodes for the drain, gate, source, junction temperature, and case temperatures at the positions 1, 2, 3, 4, and 5, respectively. The generateSemiconductorSubcircuitROM function requires you to use the number 1 for the drain, 2 for the gate, 3 for the source, 4 for the base, 5 for the junction temperature, and 0 for no connection. To obtain a ROM, you do not need the case temperature and you cannot assign the junction temperature for this IGBT device. Use this vector of terminal orders for this IGBT.

terminals = [1 2 3];

Define the device type. In this example, the device is an IGBT.

deviceType = 'IGBT';

Define the on-state gate-source voltage. To decide the value of this argument, look at the manufacturer datasheet. The function assigns the value of this argument to the IGBT gate node. The value of this argument must be within the datasheet limits and greater than the threshold voltage. For an IGBT, the source is called emitter. The threshold voltage of an IKW15N120T2 IGBT is equal to 6.4 V and the maximum operational gate-source voltage is equal to 20 V. You can find the threshold voltage value in the Gate-emitter threshold voltage parameter in the Electrical Characteristic table, and the gate-source voltage value in the Gate-emitter voltage parameter of the Maximum Ratings table. Specify a value of 10 V for the on-state gate-source voltage.

VgeOn = 15;

Define the off-state gate-source voltage. This argument must be less than the threshold voltage and greater than the minimum allowed voltage. By default, this value is equal to 0.

Define the constant current for threshold voltage. The function uses this current value to obtain the switch threshold voltage by measuring the gate voltage at which a constant drain current is first observed. This current is typically very small. The datasheet specifies a value of 0.6 mA. You can find this information in the Conditions column of the Gate-emitter threshold voltage parameter in the Electrical Characteristic table.

Icc = 0.6e-3;

Define the on-state gate resistance. The datasheet specifies a value of 41.8 ohms. You can find this information in the conditions from Figure 1 of the datasheet.

RgOn = 41.8;

Define the off-state gate resistance. The manufacturer datasheet does not specify a value for this argument. Specify the same value as the on-state gate resistance.

RgOff = 41.8;

Define the temperature point at which the device is tabulated. You must specify the values of this argument within the manufacturer operating ranges. In this example, you cannot parameterize the device over the temperature because the input terminals do not include the junction temperature. Specify values close to 27 °C, which is the default value for LTspice.

TVec = [25 30];

Define the on-state current breakpoints for the tabulated I-V curve. This argument specifies the currents at which the function tabulates the device. The values of this argument must be less than the maximum datasheet values, which you can find in the DC collector current parameter of the Maximum Ratings table.

IVec = [0:0.5:2, 5:5:20];

Define the on-state current breakpoints for switching losses.

Define the off-state voltage breakpoints for switching losses. These values define the voltage breakpoints at which the function tabulates the device diode. The values of this argument must be less than the maximum values.

VVec = 10:200:610;

Define the leakage inductance and stray capacitance of test circuit. The datasheet specifies the leakage inductance of 315 nH and stray capacitance of 34 pF. You can find the information in the Conditions column of the IGBT Characteristic table.

Lleak = 315e-9;
Cstray = 34e-12;

Generate ROM

If you have a supported SPICE simulation tool installed, generate the ROM.

generateSemiconductorSubcircuitROM(filename,subcircuitName,...
    SPICETool=SPICETool,SPICEPath=SPICEPath,TestNetlistFolder=netlistFolderPath,...
    DeviceType=deviceType,Terminals=terminals,OnStateGateSourceVoltage=VgeOn,...
    ConstantCurrentForThresholdVoltage=Icc,OnStateGateResistance=RgOn,...
    OffStateGateResistance=RgOff,Temperatures=TVec,...
    OnStateCurrentsForIV=IVec,OnStateCurrentsForLoss=IVec,...
    OffStateVoltagesForLoss=VVec,TestCircuitLeakageInductance=Lleak,...
    TestCircuitStrayCapacitance=Cstray);

Using:
  DeviceType = IGBT
  Terminals = [1;2;3]
  OnStateGateSourceVoltage = 15
  OffStateGateSourceVoltage = 0
  ConstantCurrentForThresholdVoltage = 0.0006
  OnStateGateResistance = 41.8
  OffStateGateResistance = 41.8
  Temperatures = [25;30]
  OnStateCurrentsForIV = [0;0.5;1;1.5;2;5;10;15;20]
  OnStateCurrentsForLoss = [0;0.5;1;1.5;2;5;10;15;20]
  OffStateVoltagesForLoss = [10;210;410;610]
  MaximumSwitchingFrequency = 100000
  TestCircuitLeakageInductance = 3.15e-07
  TestCircuitStrayCapacitance = 3.4e-11
  Reltol = 0.001
  Abstol = 1e-12
  Vntol = 1e-06
  Gmin = 1e-12
  Cshunt = 0
Extracting switch IV curve ...
Using existing netlist SPICENetlists\IKW15N120T2_L1_Vth_I0A0006_T25.net to extract threshold voltage.
Running netlist SPICENetlists\IKW15N120T2_L1_Vth_I0A0006_T25.net to extract threshold voltage in SPICE tool LTspice.
Using existing netlist SPICENetlists\IKW15N120T2_L1_SwitchIV_Vg15_I20.net to extract switch current-voltage table.
Running netlist SPICENetlists\IKW15N120T2_L1_SwitchIV_Vg15_I20.net to extract switch current-voltage table in SPICE tool LTspice.
Using existing netlist SPICENetlists\IKW15N120T2_L1_Goff_T25.net to extract off-conductance.
Running netlist SPICENetlists\IKW15N120T2_L1_Goff_T25.net to extract off-conductance in SPICE tool LTspice.

Extracting diode IV curve ...
Using existing netlist SPICENetlists\IKW15N120T2_L1_DiodeIV.net to extract the diode current-voltage table.
Running netlist SPICENetlists\IKW15N120T2_L1_DiodeIV.net to extract diode current-voltage table in SPICE tool LTspice.

Extracting switching loss lookup tables ...
Using existing netlist SPICENetlists\IKW15N120T2_L1_Loss_V10_T25.net to extract losses.
Using existing netlist SPICENetlists\IKW15N120T2_L1_Loss_V210_T25.net to extract losses.
Using existing netlist SPICENetlists\IKW15N120T2_L1_Loss_V410_T25.net to extract losses.
Using existing netlist SPICENetlists\IKW15N120T2_L1_Loss_V610_T25.net to extract losses.
Using existing netlist SPICENetlists\IKW15N120T2_L1_Loss_V10_T30.net to extract losses.
Using existing netlist SPICENetlists\IKW15N120T2_L1_Loss_V210_T30.net to extract losses.
Using existing netlist SPICENetlists\IKW15N120T2_L1_Loss_V410_T30.net to extract losses.
Using existing netlist SPICENetlists\IKW15N120T2_L1_Loss_V610_T30.net to extract losses.
Running netlist SPICENetlists\IKW15N120T2_L1_Loss_V10_T25.net to extract losses in SPICE tool LTspice.
Running netlist SPICENetlists\IKW15N120T2_L1_Loss_V210_T25.net to extract losses in SPICE tool LTspice.
Running netlist SPICENetlists\IKW15N120T2_L1_Loss_V410_T25.net to extract losses in SPICE tool LTspice.
Running netlist SPICENetlists\IKW15N120T2_L1_Loss_V610_T25.net to extract losses in SPICE tool LTspice.
Running netlist SPICENetlists\IKW15N120T2_L1_Loss_V10_T30.net to extract losses in SPICE tool LTspice.
Running netlist SPICENetlists\IKW15N120T2_L1_Loss_V210_T30.net to extract losses in SPICE tool LTspice.
Running netlist SPICENetlists\IKW15N120T2_L1_Loss_V410_T30.net to extract losses in SPICE tool LTspice.
Running netlist SPICENetlists\IKW15N120T2_L1_Loss_V610_T30.net to extract losses in SPICE tool LTspice.
Running netlist SPICENetlists\IKW15N120T2_L1_Loss_V10_T25.net to extract losses in SPICE tool LTspice.
Running netlist SPICENetlists\IKW15N120T2_L1_Loss_V210_T25.net to extract losses in SPICE tool LTspice.
Running netlist SPICENetlists\IKW15N120T2_L1_Loss_V410_T25.net to extract losses in SPICE tool LTspice.
Running netlist SPICENetlists\IKW15N120T2_L1_Loss_V610_T25.net to extract losses in SPICE tool LTspice.
Running netlist SPICENetlists\IKW15N120T2_L1_Loss_V10_T30.net to extract losses in SPICE tool LTspice.
Running netlist SPICENetlists\IKW15N120T2_L1_Loss_V210_T30.net to extract losses in SPICE tool LTspice.
Running netlist SPICENetlists\IKW15N120T2_L1_Loss_V410_T30.net to extract losses in SPICE tool LTspice.
Running netlist SPICENetlists\IKW15N120T2_L1_Loss_V610_T30.net to extract losses in SPICE tool LTspice.

References

[1] Infineon. “IKW15N120T2. TrenchStop® 2nd generation Series.” Accessed Jan 9, 2024. https://www.infineon.com/assets/row/public/documents/60/49/infineon-ikw15n120t2-datasheet-en.pdf?fileId=db3a304412b407950112b426d2d43acd.

Input Arguments

libraryPath — Path to SPICE subcircuit library file

string | character vector

Path to the SPICE subcircuit library file that the function uses to generate the ROM, specified as a string or character vector. This library file can contain multiple subcircuits.

subcircuitName — Name of SPICE subcircuit model

string | character vector

Name of the SPICE subcircuit model that the function uses to generate the ROM, specified as a string or character vector.

Name-Value Arguments

Specify optional pairs of arguments as Name1=Value1,...,NameN=ValueN, where Name is the argument name and Value is the corresponding value. Name-value arguments must appear after other arguments, but the order of the pairs does not matter.

Example: generateSemiconductorSwitchROM(libraryPath,subcircuitName,DeviceType="MOSFET",OnStateGateSourceVoltage=10,OnStateGateResistance=2);

SPICETool — Name of SPICE simulation engine

'SIMetrix' (default) | 'LTspice'

Name of the SPICE simulation engine, specified as 'SIMetrix' or 'LTspice'.

SPICEPath — Path to SPICE simulation engine executable file

"C:\Program Files\SIMetrix910\bin64\Sim.exe" (default) | string | character vector

Path to the SPICE simulation engine executable file, specified as a string or character vector.

Terminals — Vector of terminal orders

[1 2 3 5 0] | vector of integers in the range [0,5]

Vector of terminal orders in the SPICE subcircuit. The values of this vector define the ports of the semiconductor device that each node of the SPICE subcircuit connects to:

• 0 — No connection

• 1 — D for MOSFET or C for IGBT

• 2 — G for MOSFET and IGBT

• 3 — S for MOSFET or E for IGBT

• 4 — B for MOSFET

• 5 — Tj for MOSFET and IGBT

The size of this vector must match the number of nodes specified in the subcircuit.

For example, if your SPICE subcircuit is .SUBCKT IAUC100N04S6L014 drain gate source Tj Tcase, then define this vector as [1 2 3 5 0]. If your SPICE subcircuit is .SUBCKT IAUC100N04S6L014 drain gate source , then define this vector as [1 2 3].

DeviceType — Option to specify semiconductor device type

"MOSFET" (default) | "IGBT"

Option to specify the semiconductor device type inside the semiconductor switch subsystem, specified as "MOSFET" or "IGBT".

OnStateGateSourceVoltage — On-state gate-source voltage

10 (default) | positive scalar

On-state gate-source voltage, in volts, specified as a positive scalar.

OffStateGateSourceVoltage — Off-state gate-source voltage

0 (default) | scalar

Off-state gate-source voltage, in volts, specified as a scalar.

ConstantCurrentForThresholdVoltage — Constant current for threshold voltage extraction

0.1 (default) | positive scalar

Constant current that the function uses to extract the threshold voltage, in amperes, specified as a positive scalar.

OnStateGateResistance — On-state gate resistance

2 (default) | positive scalar

On-state gate resistance, in ohms, specified as a positive scalar. This value contributes to loss values. Estimate this value based on your circuit conditions.

OffStateGateResistance — Off-state gate resistance

2 (default) | positive scalar

Off-state gate resistance, in ohms, specified as a positive scalar. This value contributes to loss values. Estimate this value based on your circuit conditions.

Temperatures — Device simulation temperature

25 (default) | scalar | vector of scalars

Device simulation temperature, in Celsius, specified as a scalar or a vector of breakpoint values for the lookup tables.

OnStateCurrentsForIV — On-state current breakpoints for tabulated I-V curve

0:2:90 (default) | vector of nonnegative scalar

On-state current breakpoints, in amperes, for the tabulated I-V curves, specified as a vector of nonnegative scalars.

OnStateCurrentsForLoss — On-state current breakpoints for losses

[10,50,90] (default) | vector of nonnegative scalars

On-state current breakpoints for switching losses, in amperes, specified as a vector of nonnegative scalars. The function uses this parameter value to calculate the turn-on switching loss, Eon, the turn-off switching loss, Eoff, and the reverse recovery loss, Erec.

OffStateVoltagesForLoss — Off-state voltage breakpoints for losses

[70,100] (default) | vector of nonnegative scalars

Off-state voltage breakpoints for losses, in volts, specified as a vector of nonnegative scalars. The function uses this parameter value to calculate the turn-on switching loss, Eon, the turn-off switching loss, Eoff, and the reverse recovery loss, Erec.

MaximumSwitchingFrequency — Maximum Switching Frequency

1e-5 (default) | nonnegative scalar

Maximum switching frequency of your device in your circuit, in Hz, specified as a nonnegative scalar.

GateVoltageRiseFallTimeForLoss — Gate voltage rise and fall times

10e-9 (default) | nonnegative scalar

Since R2026a

Gate voltage rise and fall times in the test circuit, in seconds, specified as a nonnegative scalar. The function uses this value to calculate switching and reverse recovery losses.

You can find the rise time and the fall time of your device on a manufacturer data sheet. These values represent the time it takes for the MOSFET or IGBT to transition between the on and off states. Specify a single value for this argument that describes both the rise time and the fall time. The output of the generateSemiconductorSwitchROM function is not sensitive to the exact value of the argument, only to its order of magnitude. To obtain an accurate ROM, set this argument to a value of the same order of magnitude as the rise time or the fall time, whichever is smaller. You can also use a value one order of magnitude lower than the rise or fall time.

For example, if your data sheet specifies a rise time of 16 ns and a fall time of 13 ns, set GateVoltageRiseFallTimeForLoss to a value between 1 × 10^-9 and 1 × 10^-8.

The function also uses the value of this argument to estimate values for the step time and stop time.

• Step time — Interval at which SIMetrix prints output. If the value of the GateVoltageRiseFallTimeForLoss argument is zero, the step time is 1 x 10^-10 seconds. Otherwise, the step time is 0.1 times the value of the argument. The function needs to estimate the derived step time only if you set the value of the SPICETool argument to 'SIMetrix'.

• Stop time — Total simulation time for the loss extraction test harness. If the value of the GateVoltageRiseFallTimeForLoss argument is zero, the stop time is 2.5 x10^-4 seconds. Otherwise, the stop time is 2.5 x10^-3 times the value of the argument.

You can adjust the step time or the stop time by editing the generated netlist. For more information, see Tips.

TestCircuitLeakageInductance — Leakage inductance of test circuit

0 (default) | nonnegative scalar

Leakage inductance of the test circuit, in henries, specified as a nonnegative scalar.

TestCircuitStrayCapacitance — Stray capacitance of test circuit

0 (default) | nonnegative scalar

Stray capacitance of the test circuit, in farads, specified as a nonnegative scalar.

Reltol — Relative tolerance

1e-3 (default) | scalar

Relative tolerance parameter used in SPICE simulations, specified as a scalar.

Abstol — Absolute tolerance

1e-12 (default) | scalar

Absolute current tolerance parameter used in SPICE simulations, specified as a scalar.

Vntol — Absolute voltage tolerance

1e-6 (default) | scalar

Absolute voltage tolerance parameter used in SPICE simulations, specified as a scalar.

Gmin — Parallel conductance

1e-12 (default) | scalar

Parallel conductance with all nonlinear devices used in SPICE simulations, in 1/Ohm, specified as a scalar.

Cshunt — Shunt capacitance

0 (default) | scalar

Parasitic capacitance, in farads, between each node in the SPICE circuit and the ground, specified as a scalar.

SingleSimulationTimeLimit — Time limit when running a netlist

100 (default) | positive scalar

Since R2026a

Maximum SPICE simulation time when running a netlist, in seconds, specified as a positive scalar.

Use this argument to prevent long simulation times. If the simulation time of a netlist exceeds this limit, MATLAB^® outputs the name of the netlist and terminates the simulation. You can then run a standalone simulation for the netlist in LTspice or SIMetrix to debug the SPICE simulation.

Display — Option to display results

true (default) | false

Option to display the results, specified as either true or false.

CreateModel — Option to create Simulink model that contains ROM

true (default) | false

Option to create a Simulink model that contains the ROM, specified as true or false.

TestNetlistFolder — Name of folder for generated netlists

"" (default) | string | character vector

Name of the folder that the generateSemiconductorSubcircuitROM function creates for generated netlists and SPICE outputs in your current folder, specified as a string or character vector.

If you set the value of this argument to "", the software writes the models in the temporary folder specified by the tempdir command.

If you already have a folder with this name in your current folder that contains generated netlists, the generateSemiconductorSubcircuitROM function extracts the parameters from the existing netlists. The function does not overwrite the existing netlists.

Output Arguments

ROMParameters — ROM parameters generated from SPICE subcircuit

structure

ROM parameters that the function generates from the SPICE subcircuit, returned as a structure with these fields.

SwitchParams — Lookup table for I-V curve and switching losses of semiconductor switch

structure

Lookup table for the I-V curve and switching losses of the semiconductor switch, returned as a structure.

DiodeParams — Lookup table for I-V curve and reverse recovery loss of diode

struct

Lookup table for the I-V curve and reverse recovery loss of the diode, returned as a structure.

Tips

• If you set the value of the SPICETool argument to 'SIMetrix', the generateSemiconductorSwitchROM function uses the value of the GateVoltageRiseFallTimeForLoss argument to estimate a value for the interval at which SIMetrix prints output, tstep. If tstep is too small, SIMetrix takes longer to write output and MATLAB takes longer to read it. If tstep is too large, the temporal resolution is too low for the function to extract losses accurately. You can adjust the step time by modifying the value of tstep in the generated netlist. For example, this code block shows a generated netlist with a step time of 2 ns. To modify the step time, replace 2.000000e-09 with the value of the new step time in seconds.

  * SIMetrix syntax to perform a transient analysis
  * .tran tstep tstop 
  * You can adjust 'tstep' to modify the output interval for tabulated results specified by the '.PRINT' statement
  .tran 2.000000e-09 1.000000e-04 sweep single param lossLoadCurrent list 10 20 30 40 50

  After you make manual edits, save the generated netlist.

• The generateSemiconductorSwitchROM function uses the value of the GateVoltageRiseFallTimeForLoss argument to estimate an appropriate stop time for the transient simulation of the loss extraction circuit. However, you can adjust the stop time by editing the generated netlist. In the SPICE directive for transient simulation, adjust the value assigned to stopTime and the value of <Tstop> in the directive for transient simulation. For example, this code block shows a generated netlist with a stop time of 0.1 ms. To modify the stop time, replace both 0.000100 and 1.000000e-04 with the value of the new stop time, in seconds.

  .param stopTime = 0.000100
  *.........*
  .tran 2.000000e-09 1.000000e-04 *.TRAN <Tstep> <Tstop>

  After you make manual edits, save the generated netlist.

Version History

Introduced in R2025a

R2026a: Specify Gate Voltage Rise and Fall Times for More Accurate Loss Extraction

You can now specify the gate voltage rise and fall times in the test circuit, by using the GateVoltageRiseFallTimeForLoss argument. The generateSemiconductorSwitchROM function uses this value to calculate switching and reverse recovery losses with improved accuracy.

R2026a: Set Time Limits for Running Netlists in LTspice or SIMetrix

You can now set a time limit for running each netlist by using the SingleSimulationTimeLimit argument. If the simulation time of a netlist exceeds this limit, MATLAB outputs the name of the corresponding netlist and terminates the simulation. You can then run a standalone simulation of the netlist in LTspice or SIMetrix to debug the SPICE simulation.