SIMPLIS IGBT Models

Show extracted PWL waveforms option

Beginning in version 8.2, there is now an option to plot the extracted parameters as a set of PWL curves. To enable this option, select the Show extracted PWL waveforms checkbox and extract the model. After the model is extracted, a set of curves will be generated comparing the extracted PWL curves against the simulated SPICE curves. The curves displayed will depend on the model level being extracted.

Below is a typical PWL approximation of the charge vs. voltage characteristic of the Collector-Emitter capacitor. As SIMPLIS uses the charge vs. voltage in a simulation, this characteristic curve is used to curve fit the non-linear capacitance. As a result, the capacitance is piecewise constant, and is calculated from the charge vs. voltage characteristic. The SPICE curves are shown in red and the PWL curves in blue.

Level 0 Model

Level 0 models a switch with on/off resistance values, an anti-parallel diode, and gate capacitance. The Level 0 Model can be used  for AC Bode plots and for simulating output voltage during load and line transients when the actual switching waveform shapes are not critical.

• The conduction region is modeled with an on and off resistance.
• CGE capacitance is modeled with a linear capacitor and has a parallel 10Meg resistor.
• Internal gate resistance is modeled with RG.
• The anti-parallel diode is modeled with a 2- or 3-segment resistor; the number of segments is specified in the SIMPLIS Options dialog.
• There is no output (CCE) or reverse capacitance (CCG).

Below is a schematic view of a Level 0 model:

Level 0 models these circuit elements	Level 0 Schematic
QQ1: Switch with on and off resistance and saturation voltage CGE: Linear capacitance RGE: 10Meg Ω resistor RG: Internal gate resistor !R_AP_DIODE: Anti-parallel diode modeled by PWL resistor

Level 1 Model

Level 1 models a switch with on/off resistance values, anti-parallel diode, and gate capacitance, plus a lumped-linear Coss capacitance across collector and emitter terminals. The Level 1 Model can be used for power stage simulations, including Quasi-resonant, LLC, and phase-shifted bridge topologies,as well as for AC Bode Plots and for simulating output voltage during load and line transient.

• The conduction region is modeled with an on and off resistance.
• CGE capacitance is modeled with a linear capacitor and has a parallel 10Meg resistor.
• Internal gate resistance is modeled with RG.
• The anti-parallel diode is modeled with a 2- or 3-segment resistor; the number of segments is specified in the SIMPLIS Options dialog.
• There is no reverse capacitance (CCG).
• The bulk COSS capacitor is the parallel CCG and CCE capacitors with the value as follows:

  COSS = (QCCE1 - QCCE0)/(VCCE1 - VCCE0)

Below is a schematic view of a Level 1 model:

Level 1 models these circuit elements	Level 1 Schematic
QQ1: Switch with on and off resistance and saturation voltage CGE: Linear capacitance RGE: 10Meg Ω resistor RG: Internal gate resistor !R_AP_DIODE: Anti-parallel diode modeled by PWL resistor COSS: Lumped linear output capacitance

Level 2 Model

Level 2 models a switch with forward transconductance gain, a anti-parallel diode, and gate capacitance, plus a nonlinear Gate-Collector, Collector-Emitter, and Gate-Emitter capacitors. The active region is modeled by a linear transconductance gain (ICE is proportional to VGE - VT0). The Level 2 Model can be used for switching losses, IGBT voltage and current stresses, and all simulations covered by Level 0 and Level 1 models.

• Forward conduction is modeled with a two-segment gain. The following gain information assumes that the device is being switched from an off state to an on state:
• • Below the threshold voltage (VT0 - HYSTWD/2), the gain is 0.
  • Above the threshold, the gain is GAIN = ICE2/(VGE2 - VT0 - HYSTWD/2) units: A/V (transconductance)
• Internal gate resistance is modeled with RG.
• The anti-parallel diode is modeled with a 2- or 3-segment resistor; the number of segments is specified in the SIMPLIS Options dialog.
• This model level implements non-linear capacitors for all three capacitors (CGE , CCG and CCE). The Model Extraction algorithms determine the number of segments for each capacitor. Typically the Gate-Emitter capacitor is linear, while the Collector-Gate and Collector-Emitter capacitors have four segments.
  Note: The actual capacitor used is determined by the CGE_NSEG , CDE_NSEG and CDE_NSEG parameters.
• • If one of these parameters is set to 0, the capacitor at that  location will be an open circuit.
  • If the number of segments is set to 1, a linear capacitor is implemented with capacitance: Cxx = (Qxx1 - Qxx0)/(Vxx1 - Vxx0)

    where "xx" is the capacitor GE, CG, or CE.

  • Otherwise, if the CXX_NSEG parameter is set to a value greater than 1, the capacitor is implemented with a PWL capacitor. For more information, see See Capacitance Models section below.                          

Below is a schematic view of Level 2 model:

Level 2 models these circuit elements:	Level 2 Schematic
QQ1: Switch with forward transconductance, on and off resistance and saturation voltage RG: Internal gate resistor CGE: PWL capacitance RGE: 10Meg Ω resistor CCG: PWL capacitance CCE: PWL capacitance !R_AP_DIODE: Anti-parallel diode modeled by PWL resistor

Level 3 Model

The Level 3 model extends the Level 2 model to include up to 5 forward transconductance gain segments. The Level 3 model can be used to more accurately model converter losses, and converters which operate over a wide range of currents.

• The level 3 model is the same as the Level 2 model but the Forward Conduction is modeled with a variable number of PWL segments.
• As with the Level 2 model, the first segment has a gain of 0.
• The second segment has a gain of GAIN2 = ICE2/(VGE2 - VT0)  units: A/V (transconductance)
• Further segments have gain values which are defined by the slopes between successive point pairs.

  For example, the third segment has a gain of GAIN3 = (ICE3 - ICE2)/(VGE3 - VGE2) units: A/V (transconductance).

• Up to five segments of gain can be used with this model. The number of gain segments is controlled by the GAIN_NSEG parameter.

Below is a schematic view of a Level 3 Model:

Level 3 models these circuit elements	Level 3 Schematic
QQ1: Switch with forward transconductance, on and off resistance and saturation voltage RG: Internal gate resistor CGE: PWL capacitance RGE: 10Meg Ω resistor CCG: PWL capacitance CCE: PWL capacitance !R_AP_DIODE: Anti-parallel diode modeled by PWL resistor !R_GAIN: PWL forward transconductance gain G1: Converts gate-emitter voltage to a current

User-defined Model Schematic

Models these circuit elements	User-defined Schematic
QQ1: Switch with on and off resistance and saturation voltage CGE: Linear input capacitance RGE: 10Meg Ω resistor RG: Internal gate resistor !R_AP_DIODE: Anti-parallel diode modeled by PWL resistor COSS: Lumped-linear output capacitance

▲ back to top

Customize or Manually Generate IGBT Models

You can customize or manually generate your own IGBT models using a parameter string with multiple PARAM_NAME=PARAM_VALUE key-value pairs. The parameter names and their functions are described in the IGBT Model Parameters section below. You can interpret the SIMPLIS parameter values from device datasheet specifications and curves.

You can compose the parameter string in a text editor, spreadsheet, or script. The order of the parameter names in the parameter string and the capitalization of the parameter names are irrelevant.

You can include a PROTECTED=1 key-value pair to prevent from extracting a model and overwriting your manually generated parameters. The PROTECTED=1 key-value pair is not used in the simulation.  

Note: When you click on the device after adding the PROTECTED=1 key-value pair, the following message box appears to warn you that this is a hand-edited model.

To customize or generate your own IGBT model, follow these steps:

1. Create a parameter string of multiple PARAM_NAME=PARAM_VALUE key-value pairs using your preferred text editor, spreadsheet or script.
2. Add the PROTECTED=1 key-value pair to the parameter string.
3. Extract a IGBT model and place it on a schematic.
4. Right click on the symbol and select Edit/Add Properties....
5. Double click on the PARAM_VALUES property.
   Result: The Edit Property dialog opens.
   At this point, you can change individual parameters in the Value box, or replace the entire default properties with the parameter string that you created in Step 2.
6. To replace the entire string, follow these steps:
   1. Click in the Value box and type Ctrl A to select all of the existing parameter string, and press Delete.
   2. Copy the parameter string you completed in Step 2 and paste into the Value box.
   3. Click Ok.
7. To change the name of your customized model, double click the VALUE property in the Edit Properties dialog, and change the name in the Value box.
8. To return to the schematic, click Ok.

prop PARAM_VALUES parameter_string

IGBT Model Parameters

The following tables detail the parameters which define the electrical behavior of the IGBT model. Several other parameters in the PARAM_VALUES property have no effect on the electrical behavior of the model. These parameters are used to populate the Extract IGBT Parameters dialog box.

IGBT Parameters

Gain Model Parameters (LEVEL = 2 and 3 only)

Anti-parallel diode Model Parameters