PSpice Modeling Application
Modeling Transient Voltage Suppressors (TVS)
Modeling VCO (Voltage Controlled Oscillators)
Modeling Lightemitting Diode (LED)
Modeling Switches
Use Switch modeling application to create the following type of switches:

Time controlled: These switches change or toggle their state at a specified time. Here specified time is the simulation time.

Voltage controlled: These switches change their state at a specified voltage.

Current controlled: These switches change their state at a specified current.
You can create simple switches or switches with hysteresis. The switch models have builtin checks for dynamic range of parameters.
TOC
Modeling Transient Voltage Suppressors (TVS)
Use the TVS modeling application to create TVS (Transient Voltage Suppressor) or MOV (metal oxide varistor) devices. You specify the datasheet information directly into the application to create a device. The models support temperature effects, tolerances, and package parasitic.
You can specify temperature in either %/C or %/Kelvin.
TVS Definition
A transient voltage suppressor is used to protect electronics circuit against voltage transients such as lightning surges etc. You can connect TVS models in parallel to devices and circuits to protect from voltage surges.
TVS resistance decreases with increase in voltage, acting as a resistance shunt as shown in the following V/I curve.
The equation for a TVS device is given as following: I=KxVα
Where,

I is the current through the device

K is a constant depending on the type of the device

α is the nonlinearity exponent and is a measure of the steepness of the V/I characteristics of a TVS.
The behavior of the TVS device for different current ranges can be derived from the following circuit:
L is the lead inductance
In the circuit,

ROO is the ohmic resistance of the devices and it has very high value

RB is the bulk resistance

C is the capacitance

VR is an ideal varistor
Leakage current region: At a very low current, of the order of less than A, the ideal varistor has infinite resistance and RO determines the behavior of the circuit. The leakage current will increase with temperature. In this region the V/I curve becomes linear.
Normal operating region: At the normal operating range (5 to A) the VR determines the behavior.
High current region: At currents above A, the varistor has zero resistance and RB determines the behavior.
Tolerance: The varistor voltage at °C with 1 mA passed in shown in the figure below. The trace at the center represents the varistor voltage at nominal value and the other two traces represent the values at either side of the tolerance band.
TOC
Modeling Capacitors
Use the Capacitor modeling application to model nonideal capacitors with resistive and inductive parasitic. To create a model, use manufacturer data to specify tolerance and initial conditions. To add a resistance in series and in parallel, specify the equivalent series resistance (ESR) and parallel resistor (RP) values in ohm. To add inductive parasitic, specify either one of the series inductance (ESL) or the self resonant frequency (SRF) mentioned by the manufacturer. The application calculates the other value based on the following equation, and displays the result in a grayed field:
TOC
Modeling Inductors
Modeling of inductors is important for analog applications, especially those involving a wide range of frequency or high DC currents, such as EMI and DC filters, respectively. You can model a nonideal inductor using the DC resistance, wire capacitance, and magnetic core loss to represent the non linear characteristics.
The nonideal behavior of an inductor is because of the DC resistance of the wire and the self
capacitance. This can be represented in a circuit, with a capacitor in parallel (Cp) and a resistance in series (Rdc) with the inductor.
Use the Inductor modeling application to model generalpurpose nonideal RF inductors that exhibit resonance due to parasitic capacitance. The inductor model generated using this application does not include core model; therefore, it will not demonstrate any saturation characteristics. The effect of dc current causing magnetic saturation can be approximately modeled using Current Coefficients. This is explained later in the Examples section.
For this inductor you can configure inductance, DC series resistance, and selfresonant frequency (SRF). Based on these inputs, the application calculates the parasitic capacitance value. You can also configure an additional parallel resistance in the inductor model by selecting it in the application. This is an optional parameter of model.
The parasitic capacitance, Cp, is calculated using the equation:
Where,
SRF is the selfresonant frequency of the inductor, Rdc is the DC resistance, and L is the inductance.
Examples
Following is an example circuit with a nonideal inductor modeled using the application:
The inductor is placed with the following values specified in the Modeling Application form:

Inductance: m

Series Resistance (RDC): m

Self Resonant Frequency (SRF):meg
When the circuit is simulated for impedance, you see the following result.
In nonideal inductors, there is a loss of phase shift because of a high resistive element at low frequencies. The impedance value is constant, dominated by DC resistance, at low frequencies. As frequency increases, the impedance rises to a peak at the resonant frequency and then starts falling. Beyond the resonant frequency, the parasitic capacitance dominates and the inductor behaves like a capacitor.
Phase plot of the same circuit, with and without the parallel resistance is described below.
The Green trace is for simulation with Parallel Resistance (RP) of Meg and the Red trace is without the parallel resistance. Beyond the resonant frequency, the phase lag of 90 degrees (Inductive behavior) swings to a phase lead of 90 degrees (capacitive behavior).
Current coefficient affects the inductance value as per the following equation:
Where,

L is the effective inductance at current I

IL is the linear current coefficient

IL is the quadratic current coefficient
Inductor specification gives the dc current, I, at which the inductance falls to % of its nominal value, L. This can be modeled using current coefficients as:
Assuming IL = 0, this becomes:
The temperature coefficients affect the inductance as per the following formula:
Where,

TC1 is the linear temperature coefficient

TC2 is the quadratic temperature coefficient

Tnom is the nominal temperature
TOC
Modeling Transformers
Use the Transformer diode modeling application to model generalpurpose transformers. The transformer types you can create are:

Two Winding: Models a simple two winding transformer.

Custom Tap: Models a custom tap transformer.

Center Tap: Models a center tap transformer.

Flyback: Models a single ended flyback converter transformer.

Forward: Models a single ended forward converter transformer.

Forward with Reset Winding: Models a single ended forward converter transformer with auxiliary reset winding.
TOC
Modeling Zener Diodes
Use the Zener diode modeling application to model generalpurpose zener diode. To create a model, configure Zener voltage and temperature coefficient of Zener breakdown voltage (TCBV) given as αVZ. These parameter values can be obtained directly from the Zener diode datasheet.
You can select one of the following units for TCBV:

mV/°C

%/°C
This application internally converts and uses TCBV in mV/°C. This conversion is based on the following equations:
TOC
Modeling VCO (Voltage Controlled Oscillators)
VCO is simply an oscillator having an output whose frequency is proportional to an applied voltage. VCOs are widely used in a variety of applications such as Function Generators, PLLs, Frequency Synthesizers, and so on.
The modeling application allows you to create VCOs with sinusoidal, triangular, and square waveforms as output. You can enter the following parameters to define your model:

Maximum Operating Frequency

Minimum Operating Frequency

VCO Sensitivity (Hz/V)

Maximum Controlling Voltage

Initial Phase (PHASE)
Example
Assume you need a VCO to operate in the frequency range Fmin=MHz, Fmax=MHz. The controlling voltage is in the range of V to V. This gives sensitivity of.8MHz/V.
Enter the parameter values in VCO user interface as below:

Maximum Operating Frequency = E6

Minimum Operating Frequency = E6

VCO Sensitivity (Hz/V) = .8E6

Maximum Controlling Voltage =

Initial Phase =
The application circuit is shown below with Ramp (ranging from V to V) at input and load R1 at output.
Output waveforms show VCO frequency changing with Input Voltage.
The maximum time step value for simulation is at .005µ to get a smooth output.
The minimum frequency comes out to be at V input. Zooming the output curve from µs to µs. Time period=µs
Frequency comes out to be /1µs= MHZ
Similarly, you can find out the expected frequency for a given input, say at V, for the following given values:
Fmin=MHz, Vmin=V, Sensitivity=.8MHz/V
This gives expected freq (at 8V) = + (3*1.8) = .4MHz.
To measure the frequency from simulation results, zoom the area around V input. Time period (with the help of cursor) = .4574µ – 4.2998µ = .1576µ Frequency comes out to be /0.1576µ = .345MHz.
Measured frequency comes close to expected frequency. For the measured frequency to be exactly same as expected frequency, you need to provide step in input at V.
Similarly, the maximum frequency of MHz comes out to be at V Input.
VCO output amplitude is fixed at V. This can be modified by using E device from analog.olb, specifying a suitable GAIN value, and placing it after VCO.
Modeling Lightemitting Diode (LED)
You can use the LED model to represent generalpurpose LED devices in your schematic design. To create a model of a LED, you need to define the following parameters using datasheet values:
 Forward Voltage
 Forward Current
 Reverse Voltage
 Leakage Current
 LED Resistance
 Power Dissipation
 Maximum Forward Current
This LED model supports the following analysis in PSpice Advance Analysis:
 Smoke Analysis
 Sensitivity and MonteCarlo Analysis
To understand the relation between the forward characteristics of the LED devices and the LED model, define the forward voltage as 2.25V in the LED model. In the following figure, you can notice that the forward voltage rises after 2.25V, which was defined in the LED device model.
Figure 5 LED Forward Voltage
TOC
Modeling Independent Sources
In this application, the following types of sources are supported along with the wave types:
 Pulse: Step, Pulse, Square, Ramp, Sawtooth, Reverse Sawtooth, and Triangular Sine: Sine, Cosine, and AC Source
 DC: Ideal DC and DC
 Exponential FM
 Impulse: 1.2/50 µSec, 4/10 uSec,4/20 uSec, 8/20 µSec, 10/350 µSec, and 10/1000 µSec. Three Phase (Only voltage): DELTA and STAR configurations.
 Noise Sources
 Impulse Sources
A lightning impulse voltage rises very quickly, in a few microseconds, to its peak value and then falls to relatively slowly. You can use lightning impulse voltages to test the effect of external source of high voltages such as lightning stroke on your designs. Designs, such as power supply systems, are often required to be qualified against effect of such transient. These sources, modeling critically damped lightning impulses, are available as both current and voltage types.
A sample representation of a lightning impulse voltage is shown in the following figure. The maximum voltage reached, P, is the peak voltage. The intersection of the straight line that connects the points where the rising wave reaches .9 and .3 of the peak voltage is the virtual origin. The time between the origin and the virtual origin is the delay, D. The part of the wave from the virtual origin to P is the front and the trailing part of the wave is termed tail. The time taken for the impulse to reach the peak from the virtual origin, T1, is the front time. Similarly, the time taken to fall to half the peak value, T2, is the half time.
The following table lists the voltage and current waveform sources and the corresponding Front and Half times.
Wave (In µ seconds) 
Front Time (T1) 
Half Time (T2) 
1.2/50 
1.2 µs 
50 µs 
4/10 
4 µs 
10 µs 
4/20 
4 µs 
20 µs 
8/20 
8 µs 
20 µs 
10/350 
10 µs 
350 µs 
10/1000 
10 µs 
1000 µs 
Three phase Sources
This application enables you to quickly generate balanced three phase sources. You can select either delta or star connected voltage source. You can define the following parameters for these sources.
Line voltage: The voltage or potential difference between two lines of different phases. The line voltage in three phase systems exists between the RY, RB, and YB phases.

Star connection

Phase voltage = Line voltage / √3

Phase Current = Line Current


Delta Connection

Phase Voltage = Line Voltage

Phase Current = Line Current / √3


Frequency

o Frequency of operation

Phase sequence: The order in which the phase voltages reach their maximum magnitude. If the Phase sequence is RYB, then Phase voltage at R will reach its maximum value first, followed by Y, and then B. In the following figure (Figure 1 Phase Sequence), the top plot shows the waveform for phase sequence RYB and the bottom plot shows phase sequence RBY.
Figure 1 Phase Sequence
Figure 2 Phase Lag
Noise Sources
This application enables you to add random noise models for most of the standard sources in the schematic design. It supports both voltage and current noise sources. The voltage and current noise sources are further classified as DC, Sine, Pulse, Exponential, and Random Noise, which is an independent random transient noise source.
You can specify Noise Amplitude and various other noise parameters depending on the noise source you select. Noise Amplitude can be defined as the difference between the maximum voltage limit (5.5V) and minimum voltage limit (4.5V). For example, as seen in the following figures, if the voltage magnitude is 5V and Noise Amplitude is 1V, the output of the noise source will fluctuate in the range of 5.5V and 4.5V.
Figure 3 DC Voltage Noise
Figure 4 Sine Voltage Noise
TOC
Modeling PWL Sources
Use the PWL Sources modeling application to model timedependent PWL sources. You can specify time and amplitude relationship to define a model with a large set of data points.
The application allows you to define time and analog value pairs along with signaling factors and repetitions through a user interface with the following fields:

PWL File: Select to specify a file that lists the timevalue pairs. A time and value pair must be separated by a space.

PWL Points: Select to enable the fields under Analog Value Time Pairs to specify the time and value pairs in the user interface.

Analog Value Time Pairs: Enabled if you select PWL Points. Contains five pair of fields that can be increased by clicking Add Additional PWL Points. A least one pair of values must be entered for simulation source.

Signal Repetitions: Specify the number of periodic repetitions for the given set of points. You can select any one of the following:

None: Select to specify no repetitions.

Repeat Forever: Select to periodically repeat the complete PWL signals from the start until the end of simulation.

Repeat: Select and specify a whole number to set the number of repetitions. By default the value is 2.


Advance Options: Specify the following optional advanced options:

Value Scaling Factor: Specify the factor by which the value in each PWL pair will be multiplied. Note that Value Scaling Factor or VSF is sometimes referred to as Voltage Scaling Factor in context of Voltage PWL sources. Refer to PSpice Help online help document.

Time Scaling Factor: Specify the factor by which the time in each PWL pair will be multiplied.

AC: Specify the AC magnitude for an AC sweep analysis.

DC: Specify the DC voltage magnitude for a bias point and transient analysis.

TOC
Accessing the Applications
To access any of the modeling applications to create a new model, perform the following steps.

From the Place menu in OrCAD Capture, choose PSpice Component – Modeling Application

Select the submenu corresponding to the device for which the model is to be created.
For example, to create a new Zener model, choose:
Place – PSpice Component – Modeling Application – Zener
Note: To create a PWL (Piecewise Linear) source model, choose Place – PSpice Component – Source – PWL Sources
Important: The Transformer, Zener, Inductor, and Capacitor applications are accessed from OrCAD Capture Market Place and will open the Market Place page in Capture, in case these are not already installed on your system. You can download the application from this page. The rest of the applications are installed with the latest HotFix.
To access modeling application to edit an existing model, perform the following steps.

In OrCAD Capture, open the schematic page with the device instance to be modified.

Select the device.

Rightclick the device instance.

From the popup menu, choose More – Edit PSpice Component.
Applications discussedin this document are accessible only for Analog or Mixed A/D project types in schematic page context.