# Basic Tutorial Lesson 7: Analyzing the Frequency Response of Multistage BJT Amplifiers

 Tutorial Project: Analyzing the Frequency Response of Multistage BJT Amplifiers Objective: In this project, you will use the Bode Plotter to simulate the frequency response of BJT amplifiers with different device models. Concepts/Features: Bipolar Junction Transistor Common Emitter Amplifier Voltage Gain Frequency Response Bode Plotter Data Manager Imported Model Negative Feedback Minimum Version Required: All versions ' Download Link: Analog Lesson 13

## What You Will Learn

In this tutorial you will build and test two-stage common emitter amplifiers using different BJT devices and examine their frequency response. You will learn how to import an external device model and use it in your circuit. You will also become familiar with RF.Spice's Bode Plotter virtual instrument.

## Building a Two-Stage BJT Amplifier & Examining Its DC Bias

The following is a list of parts needed for this part of the tutorial lesson:

Part Name Part Type Part Value
Vcc Vcc DC Bias Source DC, 15
VS Voltage Source AC Amplitude = 1mV, Phase = 0
R1 Resistor 200k
R2 Resistor 50k
R3 Resistor 12k
R4 Resistor 3.6k
R5 Resistor 120k
R6 Resistor 30k
R7 Resistor 6.8k
R8 Resistor 3.6k
RS Resistor 150
RL Resistor 10k
C1 - C3 Capacitor 10u
C4 Capacitor 15u
C5 Capacitor 25u
Q1 - Q2 Q2N2222 NPN BJT Defaults
IN, OUT Voltage Probe Marker N/A

In this tutorial lesson, you will analyze a two-stage common emitter amplifier. Place and connect all the parts as shown in the figure below:

 The schematic of a two-stage common-emitter BJT amplifier.

The voltage source VS is an small-signal AC source with a peak amplitude of 1mV. Let's first take a look at the DC bias of the amplifier. You can run a DC Bias Test of your amplifier to find the operating point parameters of Q1 and Q2. Or you may simply run a live simulation of your circuit and enable circuit animation using "Show Voltage Text". The figure below shows the DC voltage at the operating point:

 The operating point DC voltages in the two-stage common-emitter BJT amplifier.

## Using a Bode Plotter Virtual Instrument

In Tutorial Lesson 3, you ran an AC Frequency Sweep to get the frequency response of your simple BJT amplifier. You can certainly do the same thing here, too. However, RF.Spice A/D provides a quick virtual instrument for this purpose. It is called the Bode Plotter and you can place one from the Instrument Panel on the right side of the screen. First, you have to set up your virtual instrument. Click the Setup button and open the Input/Output tab of the drop-down panel. Set your input between Nodes 0 and 1 and set your output between Nodes 10 and 0. Set the Signal Amplitude equal to 1mV and keep the default zero value of Signal Offset. In the Sweep tab of the drop-down panel, set the Start and Stop frequencies to 10Hz and 20MHz, respectively. Set the value of Step / Interval equal to 50 and choose the "Decade" option for Interval Type.

 Setting up the Bode Plotter virtual instrument: the Input/Output page. Setting up the Bode Plotter virtual instrument: the Sweep page.

You are now set!! Click the Run Sweep button of the instrument, and the frequency response is immediately plotted. Note the Bode Plotter, by default, plots the gain of your circuit define as V(out)/V(in). As you can see from the figure below, your two-stage amplifier provide a high gain of 80dB, but the frequency response rolls off below 10kHz. Your amplifier cannot be used for higher frequencies!

 The Bode plot of the two-stage common-emitter amplifier using two 2N2222 BJTs.

## Importing a New BJT Model

In the previous part, you picked a commercial BJT part from RF.Spice's extensive parts database. In many cases, you may need to use a new device model that doesn't already exist in RF.Spice's database. You can define a new device model from the ground up, or you may import new device models from external text files. In RF.Spice A/D, a device or part is the combination of a simulation or process model and a symbol. You can build a complete new device and store it to the parts database. You can also use an existing part and simply change the model behind it.

In this part of the tutorial lesson, you are going to import a new BJT model from a text file called "MyNewBJT.TXT". Open a blank text file using any text editor such as Windows Notepad and type in the following text ad save it to the file:

.model MyNewBJT npn is = 2.0e-16 bf = 50 vaf = 100 rb = 5 rc = 1 cje = 0.4p

+ vje = 0.8 mje = 0.4 cjc = 0.5p vjc = 0.8 ccs = 1p

Next, open the RF.Spice A/D Device Manager using the keyboard shortcut Ctrl+D. Open the menu item Menu > File > Import Simulation Model from Text File… Follow the instructions on the screen. Enter the model name and a description for your new model such as "My new NPN BJT model with better frequency response". Use the Windows Explorer's Open Dialog to browse your folders, locate the model text file and open it. The program will prompt that your new model has been added to the database.

 Importing the new BJT process model called "MyNewBJT" in RF.Spice's Device Manager.

## Replacing the BJT Models in Your Circuit

Next, go back to the circuit of the previous part. Open the property dialog of the transistor Q1 and click the Select Model button of that dialog.

 Changing the process model of a BJT device in its property dialog.

The "Select Process Model" dialog opens up where you can search for "MyNewBJTModel". You can use the filter and type in the first few letters of your model's name to quickly locate it in the parts database. Highlight the name of your new model and click the Selet button to replace the old model.

 Importing the new BJT process model called "MyNewBJTModel".

Repeat the same procedure for Q2. Run a new live simulation of your circuit to examine its DC bias. As you can see from the figure below, the collector and emitter voltages of both Q1 and Q2 have changed compared to the previous part.

 The operating point DC voltage in the two-stage common-emitter BJT amplifier with "MyNewBJT" process models.

Get the frequency response of the new updated amplifier circuit using the Bode Plotter. Click the Run sweep button and you will see the plot shown in the figure below. Note that the frequency response of the new amplifier has been significantly extended and its 3dB rolloff frequency is now about 3.48MHz with the imported BJT models. Also, note that the gain of the two-stage amplifier has dropped from 80dB to 60dB. This can be explained by the fact that the forward beta (bf) parameter of 2N2222 was 150, while the new BJT model has a reduced value of bf = 50.

 The Bode plot of the two-stage common-emitter amplifier using two "MyNewBJT" process models.

## Exploiting Negative Feedback

Negative feedback is often used to extend the frequency response of amplifiers. In this part of the tutorial lesson, you will use the circuit of the previous part with your updated BJT models, and will modify it by adding negative feedback from the output to the input of the amplifier. For this purpose, detach the capacitor C5 from the ground and feed it back to the input with a series resistor RF = 25kΩ as shown in the figure below. Keep in mind that you can easily detach parts from your circuit by select a wire or a segment of a wire and deleting it.

 The schematic of a two-stage common-emitter BJT amplifier with shunt series feedback.

Note that the DC operating point of this circuit hasn't change from the last part, because the feedback path is DC-blocked by the capacitor C5. Get a new frequency response of the feedback amplifier circuit using the Bode Plotter. You can see from the figure that the frequency response of the feedback amplifier has been further extended to a rolloff frequency of 13.1MHz but at the expense of a significantly reduced gain of 39.4dB.

 The Bode plot of the two-stage common-emitter amplifier with shunt series feedback.

Keep in mind that you could have got the same simulation results by running an AC Frequency Test of your amplifier circuit. If you are not satisfied with the small size of the Bode plot on the virtual instrument, you can make a graph of it. Open the Export tab of the setup panel of the instrument and click its Copy To Graph button. A new tab opens up in your project workspace with a large graph of the Bode plot. Note that you have to set the right scale type and axis limits for both the horizontal frequency axis and the vertical gain axis.

 The Bode plot exported to a graph in RF.Spice's Data Manager.