So what do you do when you need to make a complex transformer like a 10 turn trifilar winding with a center tap that you might find at the input and output of a diode ring mixer, like the double balanced mixer below? Well you use a Spice Directive. If you have not forgotten everything you have learned so far, you might recall that all the way back in part one of this literary travesty that the last button in our list was the Spice Directive button and like all good men everywhere, our purpose is to push buttons, and with the pushing of this button your entire existence is now complete.

So in the circuit above we have a double balanced mixer, from left to right you have the local oscillator, a 10 turn trifilar winding, the diode ring, another 10 turn trifilar winding and finally the RF input. The IF output is at R1. As well are all experts in the field, we know that a diode mixer likes to have 50 ohm terminations all all its ports. So the LO, RF and IF are all 50R.

So we have a 2MHz input signal, being mixed with a 7MHz local oscillator to give the sum and difference frequencies, 7 + 2 = 9, 7 -2 = 5 so when we run this, we should be able to see 5 and 9MHz peaks which we can then filter out the one we don’t want and keep the other as the IF.

But before we do that, a Spice Directive for transformers always follow the same rules, they are numbered k1, k2, k3 etc followed by the group of inductors you want to make up the transformer, L1 L2 L3 and the final number 1 sets the coupling to perfect, you can of course set this to a number less than one and have imperfect coupling between the windings if you wish to simulate a lower Q than perfection.

So we run a transient analysis on our mixer circuit and we get a bonkers output that looks like this. Now like all good and proper mad scientists you might conclude that something is wrong, that this circuit is a failure and should should be confined to the annals of electronics history where the smoke has escaped and the shmoo released. But you would be wrong of course, because the thinkers out there will have realized that diode mixers are NON LINEAR and that the output will be the Sum and the Difference of the inputs plus all the fart noises, aka Harmonics.

So if we pull up the FFT window we can see then that we have 2 main peaks, one at 5MHz=LO-RF and 9MHz=LO+RF. And you can also see the double balanced action where the LO and RF are attenuated in the output quite substantially, and then in the rest of the spectrum you see those + and – pairs with their harmonics attenuated. It is actually a rather cool way to come to understand what a Double Balanced Mixer does and kind of how its doing it, visually.

So anyway, you now know how to make complex transformers, how to set the turns ratios and all that jazz and do quite a lot now in LT Spice. Perhaps its time to find a circuit that you have used before in a project, lay it out in LT Spice and simulate it and see if it does what it says it does, to see if you can improve it and make it better, or perhaps even find a better solution altogether. And do not forget to have fun.

So anyone who is not living in the 1850’s would have noticed a few years ago a revolution in signal generation with the advent of cheap micro controllers and modules in the way of the Arduino AD9850 DDS VFO. Now cheap and highly accurate signal sources were available to the masses, but they did have some limitations. Firstly the DDS output has a 200 ohms impedance, secondly its output was low, in around 300mv p-p and thirdly its output gain was not uniform across the entire frequency range and if it was being used as a local oscillator feeding a diode ring mixer the output needed to be amplified and buffered.

Alas poor Yorick, the internet came to everyone’s rescue with some eager beaver grabbing a handful of parts and some popcorn transistors and knocking up a buffer amplifier to add to the DDS to bring its output up to ear destroying levels, well -7dbm needed to drive the input of a diode mixer. But, was it any good? We now have enough peanuts in the brain box to test this thing and see if it was really all that up to scratch.

First lets run a transient analysis and take a look at the waveform. Its not very sinusoidal now is it. It is clipping hard on the negative rail and well when any form of clipping happens we make fart noises AKA harmonics. So here is a new trick to add to your LT Spice bag of tricks, we can look at the FFT output and see the harmonic content.

RIGHT CLICK the waveform window, select VIEW->FFT and you will get a nice frequency analysis of the harmonic content, we can see that the 2nd and 3rd harmonic are about -20db down on the fundamental. This might be important in your design and if this was the FFT display of a final amplifier you should be hitting panic buttons because the Law is generally the 2nd harmonic needs to be -50db down on the fundamental. Check with your local authority to be sure to be sure because a clean signal is a nice signal. However, with a DDS buffer, this may or may not be a problem in your design.

Next we can perform an AC Analysis on buffer amp and see its gain over a range of frequencies. We can see there is a large rolloff in gain from about 10Mhz and onward and by 28Mhz we have lost almost -3db gain. Now this might be enough to stop your diode ring mixer from turning on if your -7dbm signal is now more like -10dbm, the mixer will not mix, and that might suck bad for your circuit.

So now you know enough to make simulations on amplifiers and buffer stages to see if they actually do what you want them to and if you are really cleaver you will now be thinking of ways of optimizing this circuit to make it work better, like by rebiasing Q1 by adding a low value resistor from emitter to ground so that its not clipping the negative rail, by adding a low pass filter maybe to clean up the harmonics and by optimizing component values to get a flatter gain response. What you do will depend on your actual needs and implementation. Either way have fun.

All radios are made up of some rather standard blocks we use over and over, we have filters, amplifiers, mixers, that is is, no rocket surgery required. A product detector is not someone searching for a product to buy, its just a mixer, a beat frequency oscillator is nothing more than an amplifier with positive feedback to make it go bonkers in a controlled manner and filters, well they just filter out the crap we do not want.

Sure this is an over simplification, but it is near enough to being the truth. I know for myself, once i got my head around the nomenclature of radio and started to see things for what they really are, that things started to make sense to me. So in the next few parts, lets take a look at some of the specific things we can do in LT Spice to get a better understanding of the performance of our circuit under test, starting with filters.

So this is a filter I have used in a number of projects before. I think we have all used someone else’s design without really knowing if that design is any good or not. So, now that we can used LT Spice, we can see for ourselves if someone else’s design is actually any good, or if their design is rubbish. And when we look around the net we see these kinds of blocks being copied over and over and this assume that its good, if might just be that everyone is copying the same bad design.

So if you are paying attention to the above schematic you will notice some things different. Previously we have performed Transient Analysis, and now we are doing something different, performing an AC Analysis which will allow us to sweep the circuit under test with a range of frequencies and get a Bode Plot at the end to look at.

We set up our voltage source with an AC Amplitude of 1 and of course 50R series resistance as the filter is 50 ohms impedance in and out.

Next click SIMULATE->Edit Simulation Command and select the AC Analysis tab. Change the type of sweep to Octave, and add in the other details, for the number of sample points, start and stop frequency. Click ok, then run the simulation and let the fun begin.

Now, if you click on the trace number n004 in my case, you can add upto 2 cursors per trace and move them about to to take some measurements. Cursor 1 is showing the center frequency of the filter, 7.150MHz and its at -6db, cursor 2 is at 12MHz and its -54db, 54 minus 6 is 48db DOWN on the bandpass. Which is good information to be able to work out, you can then tell how far attenuated the Image frequency of your mixing scheme is, the IF freq etc etc to see if your filter is good enough for your task.

Now we have only done this with a single Bandpass filter, you can also do the same with the Low Pass Filters on your transmitters and do the same math to work out how great the attenuation is of the 2nd and 3rd harmonics. A clean signal is a good signal. But I will leave that up to you to try. And now you know enough about how to use LT Spice to perform AC Analysis and to design, align and specify the properties of filters. Get out there and have fun, test your designs and make sure your homebrew radios present the cleanest signal they can.

So lets bring everything we have done so far together into 1 project. So we use a new component in this schematic a transistor. To add the transistor select components->npn. The we can right click the component and select a transistor type. For this circuit we will use some rather standard 2n2222 and the 2n2219a.

So in the above circuit we have a voltage source V2 where you will notice the proper use of Label Nets. Anywhere a Label Net has been placed with the value of 12v, the 12 volts from  V2 will be applied. Run a transient analysis with the following values to see for yourself how the Label Net works “.tran 0 0.000001 0.0000001”.

 

Ok, so what is the above circuit. It is a rather poorly designed buffer and amplifier. What is does however is demonstrate everything we have done so far. We have voltage and signal sources, we have the voltage divider R1 and R2, we have DC Blocking caps C2, 3 and 5, we have L1 blocking AC from entering the power rail. Something else you might notice is we are using 200 ohms for the load and source impedance.

So, once you have the circuit built, run a simulation and follow the signal through the circuit. There is so much that can be learned from probing about the circuit. Voltages can be found on the base, emitter and collector of the transistors, the current flowing through the transistors can be found and we can see the amount of total gain of the amplifier.

So for those who have been paying attention, you will have noticed that the input signal is 0.2v p-p, the green trace in the above circuit. And the output at the top of R6 is close to 5v p-p, which means that the gain is close to 27db.

And there you have it, you now know enough to be able to make complex circuits in LT Spice and simulate them and make usable measurements to define some parameters of amplifiers.

Flow control is something we need to do in radio circuits, we want to keep things out, let only some things pass and all that. We certainly do not want the output of our amplifiers being sent out the power jack into the house wiring and turning the house into a giant antenna for our oscillator circuit. Nor do we want DC being passed into our amplifier circuits either, because that adds a DC offset to the signal that is often not desirable. So, what we do is use DC and AC blocking. So lets knock up a circuits that demonstrates these principles. No gimmies this time, you are on your own.

In the above schematic we have a 7mhz signal source consisting of a 1v p-p sine wave with a 5v dc offset. Signal impedance is set to 50 ohms and a 50 ohm load is used.

So when this circuit is run, out-a should show the 1v signal with 5v offset and when probing the other side of the DC blocking cap, all we have left is the 1v p-p signal as the cap blocks the 5dc from passing on in the circuit.

An inductor does the opposite of the dc blocking cap, it blocks the ac signal and allows dc to pass through. The green trace is out-a and the blue trace is out-b. So from the above 2 simulations we have a good demonstration of the DC blocking and AC blocking action of capacitors and inductors. Add in a voltage divider and a transistor to both of these and we have a simple amplifier.

And with that, you now know a bit more about electronics fundamentals and a good grounding in some of the fundamental aspects of using LT Spice in using signal sources, voltage sources, dc offsets and making complete circuits. Have a play with values in the above circuits and see what the outcomes might be. As this will demonstrate why certain values are often chosen and used in different designs.

Ok meat and potatoes time. Lets look at some simple circuits that are electronics fundamentals to illustrate the basics of using LT Spice.

FILE: Voltage-Divider

So you built the voltage divider circuit above, or if you were lazy you downloaded the one I have linked above. Either way, you now have a complete circuit that can be simulated. We have a voltage source providing 12 volts to the circuit, we have R1 and R2 forming a voltage divider, we have a ground and we have 2 Net Labels, Out-A and B.

In this instance the net labels are not being used for their proper purpose, but rather to provide a convenient place to probe the circuit under simulation. So, lets run this thing and see if it does what we expect, in proving Ohms Law is true and working HEHE.

So if you assembled the circuit yourself, right click the schematic and select RUN. This will bring up the simulation command window. We will be performing a Transient Analysis, plug in some values as I have above, and click ok. The window will now split and show you the simulation window.

If you move the mouse around in the schematic window you will notice that the cursor will change from cross hairs to a probe when you hover over OUT-A and B and will look like a current meter when you hover over the voltage source. So we can measure the voltages at points A and B and the current flowing in the circuit. And if you look in the above image, you will see 2 traces, the green one is 12v from out-a and the blue one is 6v at out-b, just what we expected for a voltage divider with 2 10K resistors.

Change the value of the resistors and then run the simulation again, notice what effect that has on the voltage at out-b, its going to change, by how much will depend on the value you change it to.

FILE: Pi-Attenuator

Another simple resistor only circuit is the pi attenuator, I think off the top of my head that this attenuator is -3db. Load it up and run it and see if i am right.

This time we are using a voltage source as a signal. Select a sine wave, give it an amplitude of your choice, its value is Peak to Peak, set the frequency of the signal, I gave it 7 megahertz. Now, this is important, all signal sources need to have their impedance set. The Series Resistance box will set the signals impedance, and being that we like to have 50 ohms impedance everywhere, lets set the series resistance to 50R. Also, all circuits need a load impedance also, if you look at the schematic you will note there is a 50R resistor to ground after the circuit under test, this sets our load impedance to 50R also. 50R in, 50R out, with known impedances we should get accurate results.  Click ok, then run the simulation using the transient analysis numbers shown in the above schematic. Probe points A and B and you should have something like the image below.

The green trace is our 1v p-p 7mhz input signal, the blue trace is our attenuated now 700mv p-p signal. And now you know enough about how to use LT spice to test simple circuits, using both DC voltage sources and AC signal sources. Change the values about and see what happens, the good thing is none of this costs any components or solder. Just your time and some self learning.

Ok, so sometime ago I started writing a series of articles for the WIA AR Magazine from a beginner to homebrew persective. Now for various reasons of no real importance to this story part way though i changed my mind and pulled the pin on the whole thing, but I still have my original files and so now seems as good a time as any to edit them up, add some more information and present them here for those who might be looking for a very basic intro into LT Spice.

I am going to assume you know how to download and install the software and get it up and running. And I am only going to gloss over using the interface and get straight into building basic circuits in the program and testing them. For some circuits I will provide the LT Spice files, for others I will not. The whole point about this series is to learn HOW TO DO IT, not just play with the crap I have already done.

So, lets get into it.

The Interface:

Everything you need to know is pretty much in this one picture. So run the program, click FILE->NEW SCHEMATIC and start clicking things.

1. The Scissors: are used to remove components and wires when you stuff things up.
2. The Pencil: is used to connect parts together with wires.
3. Ground: every circuit has to have a ground point. It wont work without one.
4. Label Net: Meh kind of ignore this for now.
5. Resistor: used to place resistors in the circuit.
6. Capacitor: used to place caps in the circuit.
7. Inductor: used to place inductors in the circuit.
8. Diode: used to place diodes in the circuit.
9. Components: components are things like IC’s, transistors, voltage and signal sources.
10. The Hands: used to move things or drag things around in the schematic.
11. Text: to add notes to the schematic.
12. Spice Directive: High end feature used for making complex inductors like bifilar and trifilar windings.

 

When you place a passive component in the schematic it has no value. To set its value you right click on it and this window pops up. You can enter the values in Ohms, Farads or Henry’s and thats ok if you know exponential notation, or you can shorthand things for resistors 10R, 10K, 10M will be 10 ohms, 10,000 ohms and 10 million ohms, capacitors 10pf, 10nf, 10uf for pico, nano and micro farads, and inductors 10nh, 10uh for nano and micro henry’s.

 

Finally, components, the main things we will be placing are NPN transistors, N type MOSFETS and Voltage Sources. Voltage sources can be DC or AV volts like for powering things and they can also be AC Signal Sources.

And with that, you now know how to place components into a schematic and find all the parts for might need to build, test and simulate many different circuit types in LT Spice.