Circuit VR: A Tale Of Two Transistors

Last time on Circuit VR, we looked at creating a very simple common emitter amplifier, but we didn’t talk about how to select the capacitor values, or much about why we wanted them. We are going to look at that this time, as well as how to use a second transistor in an emitter follower (or common collector) configuration to stiffen the amplifier’s ability to drive an output load.

Several readers wrote to point out that I’d pushed the Ic value a little high for a 2N2222. As it turns out, at least one of the calculations in the comments was a bit high. However, I’ve updated the post at the end to explore what was in the comments, and talk a bit more about how you compute power dissipation with or without LTSpice. If you read that post, you might want to jump back and pick up the update.

Back to Our Program

As a reminder, the LT Spice circuit we started with appears below. You can download that file and others on GitHub.

Output Z

Last time, we went over the design equations and even looked at a spreadsheet for figuring out the values. That spreadsheet assumed you wanted to pick a few items including the normal collector current for the device. In some cases, though, your driving design goal will be a certain output impedance. In that case, pick RC accordingly, and go through the same steps but you’ll compute Ic instead of selecting it and skip step 4. You can use this same procedure when the actual load you are driving is the collector resistor, which isn’t uncommon.

It is easy to see that RC is the output impedance if you do a little logic. Remember, this amplifier inverts. So Q1 is as close to off as it is going to get when the input signal is large. Assume Q1 turned all the way off. What would the output circuit look like then? A voltage divider made up of RC and RL. Like any voltage divider, the maximum power in RL is going to occur when RL=RC. If you have more of an engineering mindset, you can think of it as the amplifier’s Thevenin equivalent is a voltage source with RC as the resistor. Or, if you are more graphical, think of a voltage divider with a 10V input and a 100 ohm “top” resistor (R1). If you try values for the bottom resistor (R2) ranging from 1 to 200, it looks like this:

The voltage in R2 keeps going up, but the current goes down. When R2 is 100 ohms, the power maxes out at about 250 mW. This is why you try to match, say, a transmitter with an antenna or speakers with an amplifier.

You might want to control input impedance as well. For the input impedance case, you would have to control the values of Re, R1, and R2 which is quite a bit harder without setting up a lot of simultaneous equations or just iterating. It also will depend on beta, which is notoriously unreliable. If the product of Re and beta is a large number, you can approximate it as R1 and R2 in parallel, and that’s often good enough.

Note that in the above circuit example I just put a large resistor in as the load so it didn’t affect things much. But what if that resistor had been a 16-ohm speaker, perhaps?

Back to Capacitors

So why are capacitors important? Because the transistor needs a very specific set of DC voltages on its terminals and connecting an input or output to it is going to perturb that. However, we can isolate the circuit from any DC effects using a capacitor on the input and the output. That means we can’t amplify very low-frequency signals well — the capacitors will act like large resistors. But at higher frequencies, it won’t be any problem. You can see that in the simulation where some capacitors guard the inputs and the outputs.

If you want to see the effect in a less distracting way, check out this simulation. Here an input signal is riding a DC level. A voltage divider sets another DC level. With a capacitor between them, the circuit essentially shifts the input to a new DC level, like this:

The reactance of the capacitor, of course, depends on the frequency, according to 1/(2*π*f*C). That means the higher the capacitance, the lower the reactance at a given frequency. In this case, the 100 Hz signal sees the 10 uF capacitor as about 160 ohms of reactance. At 47uF, that drops to about 34 ohms. At 1 kHz, that will divide both of those values by another 10 (16 and 3.4 ohms).


The emitter resistor essentially introduces negative feedback which reduces our dependence on beta and makes things generally more stable. However, it also limits gain. If you suppose you have RE as a short-circuit — 0 ohms — you might think you could get infinite gain. But, in fact, you really just get a small internal resistance that is temperature- and current-dependent. At room temperature, though, it is generally just a few ohms at most. It would still increase the gain quite a bit if we could just short the emitter — in theory, up to the beta of the transistor. But without the negative feedback, we get all the other undesirable features we tried to avoid.

However, just as we use capacitors to isolate the input and output, why can’t we use a capacitor to short the signal to ground even if the DC path is through the resistor? As it turns out, you can. Try adding a capacitor across RE and watch the output go higher. Below, you can see the same output with a 47 uF capacitor across RE. Look at the scales. That 0.2V input signal now produces an output of over 5V, peak-to-peak. That’s a gain of about 25, or 5 times the DC gain.

Gain with bypass cap

The effect varies on the value of the capacitor and, of course, the frequency. Here’s the output with 10uF, 47uF, and 100 uF capacitors (first graph, below). The second graph shows the effect versus frequency. You typically want the reactance of the capacitor to be about 1/10th of the emitter resistance at the frequency where you will accept a 3dB drop off.

Three values of bypass cap
Three different frequencies

Note that the capacitor works so well, that at some frequencies, we go beyond the allowable gain and clip (see the last graph). Depending on your design goals, you may need to be careful with that.

Selecting Coupling Capacitors

To know what value to assign the coupling capacitors, you need to know the impedance of the amplifier. That’s fairly easy to estimate, but with LT Spice we can do better. If you look at V2, you know it is putting out 50 mV and you can measure the current drawn from it. Ohms law will tell you that .05 divided by that current must be the resistance V2 “sees.” With C1 set ridiculously high (1F) and V2’s internal resistance set to zero, the circuit draws about 1.75 mA from V2. That’s about 28.6 ohms. So if you know the 3dB frequency you want you simply have to compute the capacitance using the familiar 1/(2*π*f*R) formula. Assume we want 10 kHz as the 3dB point. Since R is 28.6 you need at least 0.6 uF of capacitance. Of course, you can also reverse the formula and determine what your 3 dB point should be given a certain value of capacitor.

Here’s a little WolframAlpha tip. If you try to do the above calculation, you get the answer in scientific notation: 5.56 x 10-7. Sure, you can just shift the decimal point two to the right to get the exponent to -9… or is that to the left? However, you can also just add the words “engineering form” to your query, and you’ll get the answer to the nearest exponent that’s a multiple of 3.

Output Loading

The other problem you’ll often see is that you need to drive a low impedance load which can limit your gain since matching that impedance will prevent you from using a large RC. One answer is to use an output transistor as an emitter follower or common collector amplifier. This is a very simple setup where the input to the base appears practically unchanged on the emitter. So the gain of the stage is nearly 1. That might not seem like a great thing until you realize that the output impedance of such an amplifier is roughly the source impedance divided by beta. Remember, lower output impedance is good because you can drive a wider range of load.

Suppose your RC in the main amplifier is 1600 ohms and you would like to drive a 16-ohm speaker. If the emitter follower beta is 100, the effective impedance seen from the main amp will be 1.6K ohms and the output impedance of the stage will be very low. But because in this case, the emitter resistor is probably the load itself, you won’t want to put a capacitor in the output because it would block the path to ground.

Have a look at this design:

This is very nearly the same amplifier as before, but there’s no coupling capacitor on the output. In addition, the component values changed a bit. When Q1 is turned off, the maximum voltage will go to the load and this will transfer the most power when RL=RC so the output impedance at Q1 is 1600 ohms. This is a poor match for a 16 ohm speaker, but Q2 can get us in the neighborhood in the emitter follower configuration. It is true that beta isn’t reliable, so the match probably won’t be perfect, but it should be good enough for most purposes.

Here’s the output:

Compare that with the output of the original amplifier driving a 16-ohm load. You’ll need to reduce the input drive down to 50mV, but even then the output from the original circuit will be very disappointing.

Of course, Q2 is going to need to be a power transistor. You won’t be able to quite get all 15V on the base of Q2, but you could get close. After the emitter drop, you could have a Ve of about 14V and that’s a little less than 900 mA or around 13 plus watts. Picture a big device with a heat sink. Luckily, the simulation doesn’t care. But, of course, that’s also one of the dangers of simulation is that you can overstress the models and they don’t care.

The End?

As much as we’ve talked about the common collector amplifier, there’s a lot more to it. What if the collector load is a tuned circuit? Or the emitter bypass? You can construct lots of things including multistage amplifiers using this as a building block.

By the way, you might think that bipolar transistors are old-fashioned compared to FETs, but they do have their uses. Also, all of these amplifier configurations have corresponding FET designs. The ideas are the same but, of course, the design equations are a bit different. FETs operate on voltages and there are other peculiarities. For example, some types of FETs are normally on, so you’ll need a negative bias voltage to get them to turn off. FETs — especially MOSFETs — have very high input impedance which makes input circuits easy to design. However, they also introduce capacitance which can be tricky at higher frequencies. But that’s a topic for a future Circuit VR.

Circuit VR: Starting an Amplifier Design

Sometimes I wish FETs had become practical before bipolar transistors. A FET is a lot more like a tube and amplifies voltages. Bipolar transistors amplify current and that makes them a bit harder to use. Recently, [Jenny List] did a series on transistor amplifiers including the topic of this Circuit VR, the common emitter amplifier. [Jenny] talked about biasing. I’ll start with biasing too, but in the next installment, I want to talk about how to use capacitors in this design and how to blend two amplifiers together and why you’d want to do that.

But before you can dive into capacitors and cascades, we need a good feel for how to get the transistor biased to start with. As always, there’s good news and bad news. The bad news it that transistors vary quite a bit from device to device. The good news is that we’ll use some design tricks to keep that from being a problem and that will also give us a pretty wide tolerance on component values. The resulting amplifier won’t necessarily be precise, but it will be fine for most uses. As usual, you can find all the design files on GitHub, and we’ll be using the LT Spice simulator.

Continue reading “Circuit VR: Starting an Amplifier Design”

Circuit VR: An (Almost) Practical Buck Converter

In the last installment of Circuit VR, we walked around a simplified buck converter. The main simplification was using a constant PWM signal. The result is that the output voltage is a fixed fraction of the input voltage. For a regulator, the pulse width will need to depend on the output voltage so that any changes in the output are self-correcting. So this time, we’ll make a regulator, although we’ll still use a few Spice elements you’d have to replace in a practical design. In particular, we’ll assume you can generate a triangle wave, which is easy enough, and produce a stable 2.5 V reference.

The idea is to take a voltage reference and compare it to the output. We’ll think of the difference between the two as an error voltage, and use a comparator combined with a triangle wave generator to produce a PWM signal that is proportional to the error, and thus works to hold the output voltage constant.

Continue reading “Circuit VR: An (Almost) Practical Buck Converter”

Circuit VR: Simple Buck Converters

The first thing I ever built without a kit was a 5 V regulated power supply using the old LM309K. That’s a classic linear regulator like a 7805. While they are simple, they waste a lot of energy as heat, especially if the input voltage goes higher. While there are still applications where linear regulators make sense, they are increasingly being replaced by switching power supplies that are much more efficient. How do switchers work? Well, you buy a switching power supply IC, add an inductor and you are done. Class dismissed. Oh wait… while that might be the best way to do it from a cost perspective, you don’t really learn a lot that way.

In this installment of Circuit VR, we’ll look at a simple buck converter — that is a switching regulator that takes a higher voltage and produces a lower voltage. The first one won’t actually regulate, mind you, but we’ll add that in a future installment. As usual for Circuit VR, we’ll be simulating the designs using LT Spice.

Interestingly, LT Spice is made to design power supplies so it has a lot of Linear Technology parts in its library just for that purpose. However, we aren’t going to use anything more sophisticated than an op amp. For the first pass, we won’t even be using those.

Continue reading “Circuit VR: Simple Buck Converters”

Circuit VR: Sink or Swim with Current Sources

If you got your start in electronics sometime after 1980 your first project might well have been to light up an LED. Microcontroller projects often light up an LED, too, and a blinking LED is something of the “hello world” program for embedded systems. If you tried lighting up your LED with a 9 V battery directly — not that you’d admit to it — you found it would light up. Once, anyway. The excess current blows up the LED which is why you need a current-limiting resistor. However, those current limiting resistors are really a poor excuse for a current source or sink. In many applications, you need a real current source and luckily, they aren’t hard to create.

As always with Circuit VR, we’ll be using LT Spice to examine the circuits. If you need a quick tutorial, start here and come back after that. If you use Linux, don’t be dismayed. I run LT Spice under WINE and it works great. You can find all the Spice files on GitHub.

Continue reading “Circuit VR: Sink or Swim with Current Sources”

Circuit VR: Oscillating Bridges

Circuit VR is where we talk about a circuit and examine how it works in simulation with LT Spice. This time we are looking at a common low-frequency oscillator known as the Wien bridge oscillator.

What makes an oscillator oscillate? A circuit with amplification that gets the same amount of the output signal fed back into its input, in phase, will oscillate. This is the Barkhausen criterion. Here, we’re going to look into what makes an oscillator work in simulation, and gain some insight into what happens when there’s too much feedback and too little.

In particular, we’ll look at the Wien bridge oscillator, a very simple design that originated as a way to measure impedance back in 1891. Modern versions add some additional features, but let’s start with the most simple implementation and work our way up.

Continue reading “Circuit VR: Oscillating Bridges”

Circuit VR: The Dickson Charge Pump

There was a time when taking a low DC voltage — say a single battery — and converting it to a higher voltage was painful. Now, however, cheap and easy-to-use DC to DC converters are readily available. For some small tasks, though, these can seem like overkill. For example, consider a case where you need to supply a higher voltage for a MOSFET gate that doesn’t draw much current. Perhaps you need that higher voltage to trigger a microcontroller’s programming mode and nothing else. The current draw is minimal, and a full-blown DC to DC converter is overkill. For cases like that, it is tempting to use some voltage multiplication scheme. There are many, but for this post, I’m going to take you inside a Dickson charge pump. This is Circuit VR because not only are we going to discuss the circuit, we’ll look at an LT Spice simulation you can try yourself.

The Dickson is interesting because it doesn’t require any AC conversion or transformers. Instead, it uses diodes or other switching elements to transfer charge between capacitors in stages. Each stage will effectively increase the voltage by the supply voltage — in theory. Reality isn’t so kind, though, as we’ll see.

Continue reading “Circuit VR: The Dickson Charge Pump”