**Lab 12: PSpice: Time Domain Analysis**

**Objectives**

- Use PSpice Circuit Simulator to simulate circuits containing capacitors and inductors in the time domain.Use PSpice Circuit Simulator to simulate circuits containing capacitors and inductors in the time domain.
- Practice using a switch, and a Pulse & Sinusoidal voltage source in R-L and R-C circuits.

**Equipments**

- PSpice Program

**Background**

The inputs to an electric circuit have generally been independent voltage and current sources. PSpice provides a set of voltage and current sources that represent time varying inputs. “Time Domain (Transient)” analysis using PSpice simulates the response of a circuit to a time varying input. Time domain analysis is most interesting for circuits that contain capacitors or inductors. For the capacitor, the part properties of interest are the capacitance and the initial voltage of the capacitor (the “Initial Condition”). For the inductor on the other hand, the part properties of interest are the inductance and the initial current of the inductor (the “Initial Condition”).

In this lab we consider three examples. The first example illustrates transient analysis of a R-L circuit with s single switch; the second and third circuits analyzed are the response of an R-C circuit to a Pulse voltage source and a sinusoidal voltage source.

We will again use a five-step procedure to organize circuit analysis using PSpice.

**Procedure**

#### Exp #1: Transient Analysis of an R-L Circuit with a Switch

Time varying voltages and currents can be caused by opening or closing a switch. PSpice provides parts to represent Single-Pole Single-Throw (**SPST**) switches in the parts library. These parts are summarized below:

**PSpice Component Name:** **Sw_tCLOSE****Description**: The switch will be closed at **t = TCLOSE****Library**: **eval.olb**

**PSpice Component Name:** **Sw_tOPEN****Description**: The switch will be opened at **t = TOPEN****Library**: **eval.olb**

**PSpice Problem**

The circuit shown is at steady state before the switch closes at time ** t = 0**.

The current in the inductor before the switch is closed is * i_{L}*(t = 0) = 40 mA. Find the current of the inductor as a function of time after the switch closes. That is, use PSpice to simulate the circuit after the switch closes.

Analytical Solution:

set * i_{L}*(0−) = 40 mA and

*= 60 mA.*

**I**_{SC}\({i_L}(t) = {I_{SC}} + \left( {{i_L}({0^ - }) - {I_{SC}}} \right){e^{ - t/\tau }} = (60 - 20{e^{ - 40000t}})\;mA\)

Where \(\tau = \frac{L}{{{R_{TH}}}} = 25\mu S\)

**Formulate**a circuit analysis problem

After the switch closes the circuit’s time constant is 25 μs. Plot the inductor current,, for the first 150 μs (6 time constants) after the switch closes.**i**_{L}(t)**Describe**the circuit using Capture- Place all parts on the schematic page.
- The polarized inductor can be found in
library and it has terminal points 1 & 2 that indicate a positive and negative polarity, respectively. Set the initial condition**analog_p.olb**. That is, double click on the inductor. The property editor will open. The column labeled "*i*_{L}(0^{−}) = 40 mA**IC**" (for Initial Condition) is used to enter the initial inductor current. Enterin this column, then close the property editor.**40mA**

**Simulate**the circuit using PSpice- Select
**PSpice ➤ New Simulation Profile**. Name the profile "**Transient**". Select "**Time Domain (Transient)**" for the**Analysis Type**. - There are several other information settings for the transient analysis.
is the length of time that the simulation will run. The simulation starts at time zero and ends at the "**Run to time**". In this case, specify the "**Run to time**" as \(6{\tau _{RL}} = 150\mu S\) and run it.*Run to time* - Do not change the default setting of
**zero**for the time that the data starts being saved. - Click
**OK**.

- Select
**Probes**Before running the simulation, we need to mark the voltages and/or currents that we want to display with probes.- Select
**PSpice ➤ Markers ➤ Current Into Pin**, and place the prob that appears at the top of the inductor. - Your circuit should now appear as shown in the following diagram:

- Select
- Running and Displaying the Results of the
**Simulation**- After a successful simulation, a Probe window will automatically open.
**Delete Trace**

Click on the**I(L1)**icon (the text) at the bottom left of the simulation windows, and press**delete**key to delete it.**Adding Trace and Plotting Expression**

We will add black the trace for**I(L1:1)**to show another way of plotting traces.

- Select
**Trace ➤ Add Trace...**, or right click on the curve line and select**Add Trace**or click button on the toolbar. - Add trace
(the current through inductor**I(L1:1)**through node 1)**L1**

- Select
- To remove grid lines from the plot, right-click on the plot and select
**Settings...**. Under the**X Grid**and**Y Grid**tabs, select**None**on**Major**and**Minor**grid. - Using
**Cursors**

Cursors can be used to determine precise simulation values.

- To active the cursors, click on the
**Toggle Cursor**icon at the top of the simulation window. - At the bottom of the window you may have to resize the cursor window to display data. There are two cursors Y1 and Y2. Y1 is controlled with the left mouse and Y2 with the right.
- Click on the
**Search Cursor**icon, then type in the commands:**SFXV(***xvalue***)**for X-Values or**SFLE(***yvalue***)**for Y-Values. For example: type**SFXV(**.*30.405uS*) - Crosshairs will be shown on the screen. X and Y values for this trace at the position of the cross hairs are displayed in the small Cursor window previously uncovered.

- To active the cursors, click on the

- To change the color or thickness of a line, you can right click on the curve line and select
**Trace Property**. - To copy this plot go to the “Window” tab on the tool bar and select “copy to clipboard” and paste into your document.

**Verify**that the simulation results are correct

The initial response of the inductor current isand its final state current is*i*_{L}(0^{−}) = 40 mA. Verify that the plot agrees with the mathematical prediction.*I*_{SC}= i_{L}(∞) = 60 mA

To ask a more detail questions such as what is the value of ** i_{L}(t)** at a time of 30.405 μs, there are several tools that are at our disposal: the Probe cursor button and Mark Data points & adjust value buttons allow one to select a particular data value on the curve.

To find the current at ** t = 30.405 μs**, one can find that the plot indicates that

**when**

*i*_{L}(t) = 53.592 mA**. Substituting**

*t = 30.405 μs***into the complete natural response gives**

*t = 30.405 μs***, a difference of 0.5%. The simulation results are correct.**

*i*_{L}(t) = 54.073 mA

#### Exp #2: The Response of an RC Circuit to a Pulse Input

**PSpice Problem**

The source voltage and R-C circuit are

Use PSpice to simulate the voltage source and the capacitor’s voltage * v_{C,PS}(t)* and compare it to theoretical prediction

\({v_{C,thy}}(t) = \left\{ \begin{array}{l} 4 \times (1 - {e^{ - 1000t}}) & ,0 < t < 2ms\\ - 1 + 4.46{e^{ - 1000(t - 0.002)}} & ,2ms < t < 10ms \end{array} \right.\)

**Formulate**a circuit analysis problem

Plot three voltages simultaneously:,**v**_{S}(t)and**v**_{R}(t)vs**v**_{C}(t).**t****Describe**the circuit using Capture

Place the parts, adjust parameter values and wire the parts together.- From the
parts library, choose the**source.olb****VPULSE**part and place it in the schematic drawing window. Or you can add it from**Place ➤ PSpice Component... ➤ Source ➤ Voltage Sources ➤ Pulse**.**V1**— Initial voltage voltage level**V2**— Voltage after the switch (Note: V2 can be less than V1)**TD**— Delay time before the first transition from V1 to V2**TR**— Rise time in going from V1 to V2. (It is still TR, even if the V1 > V2)**TF**— Fall time in going from V2 to V1**PW**— Pulse width: time that the voltage is at the V2 level**PER**— Period: the time for one cycle of the pulse wave form. The source will repeat the pulse for as long as the simulation runs, as defined in the simulation set up.- The plot of
shows making the transition from**v**_{S}(t)to**-1 V**instantaneously. Zero is not an acceptable value for the parameters*4 V*or*TR*. Choosing very small value for*TF*and*TR*will make the transitions appear to be instantaneous when using a time scale that shows a period of the source waveform. In this example, the period of the source waveform is*TF*so*10 ms*is a reasonable choice for the values of**1 ns**and*TR*.*TF* - Set
, the delay before the periodic part of the waveform, to zero. Then the values of*TD*and*V1*are*V2*and**-1**, respectively. The value of*4*is the length of time that*PW*, so**V2 = 4V**in this example. The value of per is the period of the pulse function,*PW = 2 ms***10 ms**

- The plot of
- From the
library, add a resistor and a*analog.olb***PSpice Ground**. Place a polarized capacitor fromlibrary to the schematic, and connect node-1 to positive polarity. Wire all parts together as shown below:**analog_p.olb**

**Nodes**:

Can be given more convenient names using an**off-page connector**component:**OFFPAGELEFT-R**or**OFFPAGELEFT-L**by clicking**Place ➤ Off-Page Connector**, or button. Edit the properties naming each connector with “**SOURCE**” and “**CAP**.”- From the
**Simulate**the circuit using PSpice

- Select
**PSpice ➤ New Simulation Profile**. Name the profile "**ResponsePulse**". Select "**Time Domain (Transient)**" for the**Analysis Type**. - In this case, specify the "
" for two period (*Run to time*).**20ms** - Check "
**Skip initial transient bias point calculation (SKIPBP)**" - Do not change the default setting of
**zero**for the time that the data starts being saved. - Click
**OK**.

- Select
**Display**the results of the simulation, for example, using Probe

Add traces**V(SOURCE)**,**V(CAP)**, and**V(SOURCE)−V(CAP)**.

Go back and change the pulse width to 5 ms. How do the resulting plots look like?**Verify**that the simulation results are correct

To verify the results, label four points (two from each RC curve) and check with the predictions of the complete natural response. I’ve done two of them, now you check the other two listed in the table below.

#### Exp #3: The Response of an RC Circuit to a Sinusoidal Input

**PSpice Problem**

Use PSpice to plot the capacitor’s voltage ** v_{C,PS}(t)** and power

**delivered to the capacitor.**

*P*_{C}(t)where

\(\begin{array}{l} {v_C}(t) = 1.55\sin (2\pi t - 76.6^\circ )\quad V\\ {P_C}(t) = {v_C}(t) \times {i_C}(t) = 3.77\sin (40\pi t - 153^\circ )\quad W \end{array}\)

**Formulate**a circuit analysis problem

Simulate the circuit to determine the capacitor voltage,. Plot the*v*_{C}(t)versus t. Also, plot the power delivered to the capacitor as a function of time.*v*_{C}(t)**Describe**the circuit using Capture

Place a polarized capacitor fromlibrary on the schematic, and connect node-1 to positive polarity.**analog_p.olb****Simulate**the circuit using PSpice

Specify the run to time as 0.8 s to run the simulation for eight full periods.**Display**the results of the simulation

In the Probe window, add the trace V(CAP). One observes that the plot is disappointing for a couple of reasons. First, it's a very rough representation of a sine function. Second, it takes a while for the capacitor voltage to settle down. In other words, the capacitor voltage includes a transient part as well as the steady state response. In this example, we only want the steady state response and so would like to eliminate the transient part of the response.

- To obtain a smoother plot, edit the Simulation Settings and set the "
**Maximum step size**" to smaller step size:.**0.001 s** - The transient part of the capacitor’s voltage can be eliminated by adjusting the initial capacitor’s voltage to:

\({v_C}(t = 0) = 1.55\sin (2\pi t - 76.6^\circ )\quad V = - 1.55\sin (76.6^\circ ) = - 1.506\quad V\)

Set the initial condition (IC) of the capacitor to be this value.

With these two adjustments, the resulting plots are:

- To obtain a smoother plot, edit the Simulation Settings and set the "

**Questions**

- The circuit is at steady state before the switch is thrown at
.*t = 0*- Determine and plot the voltage across the capacitor
and the current**v**_{C}(t)through the 2 kΩ resistor for*i*_{2kΩ}(t). PSpice does not let you plot current and voltage simultaneous since they have different units.*t > 0* - Simulate the circuit, print out the plots and explain (using short concise sentences) the behavior of the capacitor and 2 kΩ resistor using your plots.

- Determine and plot the voltage across the capacitor
- Turn in
**Exp #1**,**Exp #2**and**Exp #3**of the PSpice lab. Make sure that you show your work for verifying the simulation results!