Posts tagged Electrical Engineering

Negative Resistor Lesson

This tutorial is going to cover the topic of negative resistance. At first, it might seem like a strange idea that you could have a current flowing in the opposite direction of an applied voltage; but, hopefully by the end of this tutorial you will have a better intuitive understanding of what a negative resistance really is, and how to build a negative resistor out of common circuit components.

  1. What is a Negative Resistance?
  2. Creating a Negative Resistor Using a CCVS
  3. Creating a Negative Resistor Using a VCVS
  4. Creating a Negative Resistor Using Real Components
  5. Example Problem
  6. Summary

What is a Negative Resistance?

Our first step is to try to develop an intuitive notion of what a negative resistance is, and how it would behave in a circuit. The definition of resistance is governed by simple a relationship called Ohm’s Law.

$$R=\frac{V}{I}$$

We can see by looking at this equation, that to create a negative resistance we would need to create a circuit component which develops a negative voltage whenever a positive current is passed through it (assuming passive sign convention). However, rather than thinking about it in terms of mathematics, a simpler way to understand the idea of negative resistance is to consider the resistance of two resistors in series.

From a basic understanding of circuits, we know that the values of resistors add in series. Therefore, if we had a resistor with a positive value of 11 Ohms in series with a resistor with a negative value of -4 Ohms, the equivalent resistance in series comes out to 11 + (-4) = 7 Ohms. In other words, we can think of a negative resistor as a device we can put in series with another resistor to decrease its value.

Example of a negative resistor circuit

Return to Top

Creating a Negative Resistor Using a CCVS

Now that we have an idea of what we are trying to achieve, we can start our quest to create a negative resistor returning to Ohm’s Law and rearranging.

$$R=\frac{V}{I} \Rightarrow V=RI$$

Looking at this equation, we notice that it looks very similar to the equation governing the operation of a current-controlled voltage source (CCVS). In the equation below, $V_{CCVS}$ is the voltage output of the CCVS, $I_c$ is the controlling current, and $r_c$ is the “gain parameter” with units of Ohms—hint, hint!

$$V_{CCVS}=r_c I_c$$

If we make the assumption that the control current $( I_c )$ is flowing into the positive terminal of the CCVS, we can easily calculate the resistance $( R_{CCVS} )$ of the CCVS by once again using Ohm’s Law.

$$R_{CCVS}=\frac{V_{CCVS}}{I_c} = R_c$$

This leads us to the solution that the resistance of a current-controlled voltage source, whose control current is measured at the positive terminal, is simply equal to the gain parameter $( r_c )$ of the CCVS. By utilizing this fact, we can easily create a negative resistor simply by using a CCVS with a negative gain parameter. An example of this method can be seen in the figure below. Here we implement a resistance of -4 Ohms using the CCVS method.

Example of a negative resistor built using using a CCVS

Return to Top

Creating a Negative Resistor Using a VCVS

At this point, some readers might be wondering “why go any further?” Unfortunately, a current-controlled voltage source isn’t a very practical real world circuit component. In fact, many circuit simulation programs (such as LTspice) don’t even include CCVS models! We can, however, overcome this limitation by using a component which is more readily at our disposal: a voltage-controlled voltage source (VCVS).

By looking at the equation governing the operation of a VCVS, we can see that it looks identical to the equation of a voltage amplifier. In the equation below, $V_{out}$ is the voltage output of the VCVS, $V_{sense}$ is the controlling voltage (i.e., the input voltage to an amplifier), and $G$ is the gain parameter (which is a unitless ratio).

$$V_{out}=G V_{sense}$$

With the help of Ohm’s Law (last time, I promise!), we find that we can make the VCVS mimic a CCVS through the use of a sensing resistor $( R_{sense} )$ in series with the VCVS to measure current. The current flowing through $R_{sense}$ will create a voltage which is proportional to the current, and can then be picked up by $V_{sense}$. The proposed setup can be seen in the figure below.

Example of a negative resistor setup using a VCVS

While the above setup gives us a structure that can be used to create a negative resistor, we continue our analysis by developing a set of analytical equations describing this circuit’s operation. The voltage developed across the sense resistor is written below.

$$V_{sense} = I_{sense} R_{sense}$$

We can now take the equation governing the VCVS, make the following substitutions and regroupings, and make the equation look like the equation governing the CCVS.

$$V_{out}=G V_{sense} = G (I_{sense} R_{sense}) = (G R_{sense}) I_{sense}$$

Here we see that $(G R_{sense})$ takes the place of $r_c$ from the CCVS equation. Also, we know from the previous section that $r_c$ is the resistance of the CCVS negative resistor circuit. However, to find the total resistance $R_{total}$ of VCVS circuit we are building, we need to take into account the added resistance of the current sensing resistor $(R_{sense})$.

$$R_{total} = R_{sense}+r_c$$

Making the substitution $r_c = (G R_{sense})$, we obtain:

$$R_{total}= R_{sense}+G R_{sense} = R_{sense}(1+G)$$

From this equation, we can solve for the gain parameter of the VCVS that we would need to create any desired resistance in our circuit.

$$G = \frac{R_{total}}{R_{sense}} – 1$$

Using the set of equations we have developed, we now have the tools to create a negative resistor of any value by using only a VCVS along with a sensing resistor. As an example, we now create a negative resistor with a value of -4 Ohms. By arbitrarily choosing $R_{sense} = 2 \: Ohms$, we can calculate the required gain parameter of the VCVS by using the previous equation.

$$G= \frac{R_{total}}{R_{sense}} – 1 = \frac{-4}{2} – 1 = -3$$

The completed example circuit can be seen below.

Example of a -4 Ohm resistor built using using a VCVS

Return to Top

Creating a Negative Resistor Using Real Components

Now that we have created a theoretical circuit describing a negative resistor, our final step is to create a practical implementation using real world components. To reiterate from the previous section, a VCVS is nothing more than a voltage amplifier with differential input and differential output. To simplify the circuit design, we will make the assumption that one of the terminals of our negative resistor will always be connected to ground. This assumption allows us to use a voltage amplifier which has differential inputs, but only a single ended output. I’ve attached a schematic for an inverting amplifier like this as a reference in the figure below.

A differential input, single sided output, inverting amplifier

The gain of this amplifier is set by the ratio of resistors $R_f$ and $R_1$.

$$G=-\frac{R_f}{R_1}$$

Therefore the input-output relationship of this amplifier is governed by the following equation.

$$V_{out}=-\frac{R_f}{R_1}(V_{in+}-V_{in-})$$

The similarity to the equation governing the VCVS $(V_{out}=G V_{sense})$ is easy to see if we make the following substitutions.

$$G = -\frac{R_f}{R_1}$$

$$V_{sense} = V_{in+}-V_{in-}$$

This allows us to directly substitute for the VCVS in the negative resistor circuit with our differential amplifier circuit. We can solve for the required ratio of $R_f$ to $R_1$ by using the equation used to calculate the required gain of the VCVS in the previous section. The equation is repeated below.

$$G=\frac{R_{total}}{R_{sense}} – 1$$

$$-\frac{R_f}{R_1}=\frac{R_{total}}{R_{sense}} – 1$$

$$\frac{R_f}{R_1}=-\left( \frac{R_{total}}{R_{sense}} – 1 \right)$$

By directly replacing the VCVS from the previous section with the circuit above, we obtain the final schematic for the negative resistor seen below.

A negative resistor implemented using differential amplifier

We find the overall resistance of the circuit by substituting the gain equation of the differential amplifier circuit into the equation for calculating $R_{total}$ of the VCVS circuit developed in previous section.

$$R_{total} = R_{sense}(1+G) = R_{sense}\left(1+ -\frac{R_f}{R_1} \right) $$

Return to Top

Example Problem

To make sure that everything discussed is correct and checks out, we will work out a single example problem and simulate it.

Example: Create a negative resistor with a value of -4 Ohms. Use $R_{sense}=2\: Ohms$, and keep both $10\: kOhms \leq R_1 \leq 1\: kOhms$ and $10\: kOhms \leq R_f \leq 1\: kOhms$. Using Spice, calculate the equivalent series resistance of the negative resistor in series with an 11 Ohm resistor, using a 5 V DC voltage source as the test voltage. The total equivalent resistance should be equal to 11 – 4 = 7 Ohms.

We start by calculating the required gain of the amplifier.

$$G = \frac{R_{total}}{R_{sense}} – 1$$

$$G = \frac{-4}{2} – 1 = -3$$

Now that we know the gain, we can calculate the values of $R_1$ and $R_f$ to set the gain of the differential amplifier circuit. To make our calculations easy, we will choose $R_1 = 10\: kOhms$.

$$G=-\frac{R_f}{R_1}$$

$$-3=-\frac{R_f}{10,000}$$

$$ R_f = 3 \times 10,000 = 30,000\: Ohms$$

Now that we have the values of all the components, we can plug them into our circuit. Here is what we get!

completed example circuit

To verify our results, we run the simulation and everything checks out. Because the differential amplifier has a finite input resistance, this will slightly affect the operation of our circuit. We can take this into account while we are designing our circuit; but, I will leave that as an exercise for the reader (don’t you always love it when textbooks do that).

Return to Top

Summary

As a summary, I will outline our thought process, the steps we took, and the final result so that we can collect our thoughts.

  1. We notice that a current-controlled voltage source has a similar equation to a resistor.
  2. We realize that we can create any value of resistor (both positive and negative) if we use the current flowing into the positive terminal of the CCVS as the sensing current, and choose a suitable gain parameter value.
  3. We can mimic the CCVS using a voltage-controlled voltage source if we use a current sensing resistor.
  4. We can implement a VCVS by using a differential amplifier.
  5. By substituting the VCVS for the differential amplifier, we obtain a practical method to implement a negative resistor.

The negative resistor circuit can be seen below

A negative resistor implemented using differential amplifier

The resistance of the circuit is given by the following equation.

$$R_{total} = R_{sense}\left( 1-\frac{R_f}{R_1} \right) $$

If you have any questions, feel free to either leave a comment below or shoot me an email.

Return to Top

Adding Spice Models to LTspice

Finally… a new tutorial. Who could have ever guessed that life in the real world would be so busy (note the sarcasm!)? This tutorial is going to cover adding custom Spice models into your LTspice simulations and library. While it is very easy once you know how to do it, there are a couple pitfalls that nearly caused me to go crazy and rip my hair out in the past. Hopefully this will save you some time and stress, and possibly a hole in your monitor. Now let’s get started!

  1. Finding and Downloading the Spice Model
  2. Adding the Spice Model to your LTspice Library
  3. Using the Spice Model in a Circuit
  4. Conclusion and tl;dr (too long;didn’t read)

Finding and Downloading the Spice Model

It might seem obvious, but the first thing you need to do is find a suitable Spice model. This can usually be done in one of two ways. The easiest method is to simply Google the phrase “[part I am looking for] spice model”. If the part is popular enough and isn’t some incredibly complex part, your search will usually turn up some hits. The second method is to directly search the part manufacturer’s web page for the part. Sometimes you will have to switch tabs, or it will simply be link on their part’s web page such in the following screenshot:

screenshot of download website

An unfortunate characteristic of the Spice world is that over time it has become fairly fragmented. Different design tools use different versions of Spice, hence, part manufacturers will often have the Spice file for their part available in a couple different formats. The best format to use is the Spice3 model, however the PSpice model will usually work in LTspice as well.

Once you have found the model you want to use, you need to make sure it is in the correct format with the correct extension. A Spice model file is nothing more than a text file with a different extension. In the case of LTspice, if the model file contains only a single model, it should be named with the .sub extension. If the file contains multiple models, then the file should be named with the .lib extension.

I’m not going to go into depth on renaming text file extensions, however one method to do it is to first open up the model in notepad (in Windows 7, right click on the file > open with > notepad). Next, go to file > save as. Where you type the file name in the file name text box, type the exactly desired file name in quotes, and the program will name it exactly that. For example you could type 1N4148.sub. If you tried typing the file name without the quotes you would get 1N4148.sub.txt instead of the desired 1N4148.sub.

Return to Top

Adding the Spice Model to your LTspice Library

For this tutorial we will be using a Spice model for a made up diode called the 1NADAM, named after your beloved engineer, me! You can either download the file here (righ click on link > save as), or simply copy the code below, paste it into a text document, and save it with the .sub (or .lib) extension as explained in the previous section.

*
******************************************
*
*1N4ADAM
*
*
*Spice model for a made up diode used in
*my LTspice adding models tutorial at
*http://www.adamsiembida.com/
*
******************************************
*
.SUBCKT 1NADAM 1 2 
*
*
R1 1 2 5E+9 
D1 1 2 INTDIO
*
.MODEL INTDIO D 
+ IS = 7.0E-9 
+ N = 1.5 
+ BV = 30 
+ IBV = 0.00025
+ RS = 0.20
+ CJO = 5.0E-13 
+ VJ = 0.80 
+ M = 0.030 
+ FC = 0.50
+ TT = 3.0E-9 
.ENDS
*

As you can see, inside of the file for the 1NADAM there are .SUBCKT and .MODEL statements. Most Spice models downloaded from the internet will have .SUBCKT statements, because often time a simple .MODEL statement will not sufficiently model the complex behavior of modern parts. I am assuming that the reader knows the difference between a .SUBCKT and .MODEL (explaining those thoroughly is a topic for another tutorial). In short, however, a .MODEL statement will provide the model for an existing Spice primitive (i.e. a capacitor, resistor, transistor, diode, and so on). While .MODEL statements will work for simple simulations and old parts, it will not be very accurate for newer, smaller parts. For example, transistors have become so small and non-ideal, that the equations which we all learned in textbooks do not provide sufficient accuracy for good simulation results.

This is one case where a .SUBCKT model becomes very useful. This allows a manufacturer or engineer to create a more complex model using more than a single Spice primitive, which will lead to better results. This also allows manufacturers and engineers to create models which take into account any peculiarities or quirks that the component might have. You will be hard pressed to find a model for a real part which uses a single .MODEL statement for the Spice model. Therefore this tutorial assumes a .SUBCKT type model but will point out the difference where applicable.

Once you have the Spice model on your computer, adding it to your LTspice library is very easy. Simply copy the file to your LTC\LTspiceIV\lib\sub folder. Usually the full path to that directory will be either C:\Program Files (x86)\LTC\LTspiceIV\lib\sub on a 64 bit Windows 7 installation or C:\Program Files\LTC\LTspiceIV\lib\sub on a 32 bit (x86) Windows installation.

screenshot of adding model file to correct folder

Return to Top

Using the Spice Model in a Circuit

Now that the Spice model is in your library, there are a couple things you need to do. The first is make the circuit which will contain our part. For example, here is a simple half-wave rectifier I have tossed together.

simple half wave rectifiersimple half wave rectifier

The next is to let LTspice know that you will be using that the newly added file. You do this by placing a Spice directive (s shortcut key, or the .op button on the toolbar) onto the schematic containing .lib FILENAME, using the entire name of the file containing your model. Make sure to include the file extension! This is the first pitfall I was talking about. Here is an example of how to correctly add our new file:

.lib 1NADAM.sub

While the above way is correct, below you can see a common mistake which will not work:

.lib 1NADAM

Here you can see some screenshots showing how to add the spice directive on to the schematic.

adding the .lib directive

.lib directive placed on schematic

In case some of you are wondering what exactly this does, it includes any models included in the specified file into the Spice simulation file. You might also be wondering what the difference between the .LIB and .INC directives is. The .LIB directive will only add models from the specified file. If you had some other directives in there, for example a .TRAN statement, it would be discarded. The .INC directive will include everything in the specified file into your project, regardless if it is a model, directive, netlist, or anything else. So use .LIB just to be safe in case there is some other junk in there (even though there shouldn’t be).

Now that you have added the file, you can simply use any .MODEL or .SUBCKT included in the file as you would with any of the default components. Just right click on a component’s default model (in this case the D right next to the diode), and change its value to the name of the model inside of the file. Alternatively you can hold ctrl then right-click on the symbol and change the value in the Value row). Usually you have to look inside the file using a text editor to see what exactly the author of the Spice file called the model. For example the model for the 1N4148 diode might not actually be called 1N4148 inside of the file.

changing model for diode

Here is also where the second major pitfall comes in.

If you are using a .SUBCKT type model for a Spice primitive, you need to change the Spice prefix on the component!.

What the Spice prefix does is tells LTspice what kind of model to expect for the part. For example, on a diode, the default will be a D because, well, the part is a diode so it expects a diode model. Remember however that we are not using a regular diode model for our diode; we are using a .SUBCKT model. This means that we need to change the Spice prefix to a subcircuit model instead of a diode model. To do this, hold ctrl and then right-click on the symbol in the schematic. Then just double click in the Value cell next to Prefix, and change the value to an X.

changing the prefix

At this point the file should be ready to simulate and look like this:

schematic ready to simulate

Congratulations, everything should be working now! We can run a simulation to see what comes out. Keep in mind that this circuit not meant to be a good rectifier. I purposely chose the values to make it easy to see what this circuit is actually doing just by looking at the output. Here is the result:

simulation results

Return to Top

Conclusion and tl;dr (too long;didn’t read)

This article was much longer than I initially expected, and probably more than was really needed. However, what inspired me to write this tutorial was that when I was just starting to learn LTspice, I would read instructions people posted on forums, but I didn’t exactly understand what all the steps meant or how to perform them. For example I had no idea what “change the Spice prefix to X” meant, and I had no idea that you had to hold ctrl then right-click on the symbol to do it. In summary, here is a quick tl;dr version for people who might already be familiar with Spice and LTspice, and just want the quick and concise procedure. This will also serve as a good recap for people who read the entire article!

  1. Download and rename the Spice model to something that makes sense
  2. Move the Spice model into the sub folder in your LTspice directory
  3. Add a .LIB FILENAME directive onto your schematic
  4. Change the Value field for your symbol to the name of the model inside of your Spice model file
  5. If you are using a .SUBCKT type model for a Spice primitive, hold ctrl then right-click on the symbol and change the Prefix field to X

Good luck! I hope this was helpful!

Return to Top