CW RX Update: RF Preamp 2

So i got it all built, for some reason the gain adjust is not working and I need to investigate that to see why but other than that, it seems to be working and the gain is about what was predicted in the simulation as can be seen by the scope output below. So I will fix the few bits that need fixing and then move onto working on the IF filter. I think this will do the job required quite nicely.

Oh and I have worked out whats going on with the variable gain, Q2 is a current source, so it supplies more current to the amp above, not less, so what I need to do is redesign the amp to have the MIN amount of gain required for my circuit, then use Q2 as a gain boost. Now that I understand what is going on, I can redesign the circuit to have 3 to 12db gain swing. More than enough for the kinds of girls I go out with.


CW RX Update: RF Preamp

So i have merged the separate simulations together into the one file now to get a better understanding of how they will work together.

And the simulation looks promising, they seem to be happy working together.

So now I have built the RF Preamp onto the perf board with the bandpass filter. The only testing I have done so far has been checking for continuaty as i go along to make sure A goes to B and does not short to ground hehe. I still have to add in the pot for setting the amount of gain in the amp and to wind the 200 ohm to 50 ohm transformer that goes on the output of Q1. Its actually nice to see this moving along, lets just hope it works. HIHI.


CW Superhet Receiver Project PART-3

RF Pre Amp

So I am back feeling a little better and it is time to move this project alone a little. Some say that for a 40m band receiver an RF Preamp is overkill. In some places it probably is, but where I live most of my contacts are over 1000km away, are weak at the best of times so I think having a little gain ahead of the mixer is a good thing, but it needs to be variable.

My initial thought was to replace an emitter resistor with a potentiometer but that would mean having rf running though cables to the front panel and the chances of things going bonkers increases when you do things like that. Emitter degeneration was still going to be the way to do this, but by using a second transistor as current controller, control the current and control the gain and that can be done with voltage and a pot. So no RF being shipped about the place.

So now for the actual circuit, this was one given to me by Pete N6QW homebrewing legend and all round good guy. Its one of his GOTO circuits, nothing fancy just a BJT amp optimized for bandwidth and as an IF Amp. So I took that and modified it slightly to fit my needs as a 7mhz rf preamp. And like batman off to the batcave, we hit the simulator in LT Spice to confirm that things are close to spec and things will work well within our design parameters.

The circuit is rather straight forward. No rocket surgery required to follow whats going on there.

Ultimate gain is about 9db, and with 3v on the base of Q2 the gain is like 3db or there abouts. Should be good enough for what I require. Now I just have to build it and see if the simulation meets up with reality. Will post an update when I have it built.

Now i also should mention that I was going to compare and evaluate a number of designs for each stage. I did pull some designs out of different schematics on the web and put them through their paces, mostly they were crap. There were some that were better, but they were not popcorn enough for this project. A very notable mention is the front end of the simple ceiver with its dual gate mosfet made from a pair of J310. While i have J310 here in the crap box I am saving them for another project. If I can keep this one to BJT only i will be happy. Anyways, time to melt some solder and see if it works.


LT Spice For Radio Amateurs: PART 7

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.


LT Spice For Radio Amateurs: PART 6

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.


LT Spice For Radio Amateurs: PART 5

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.


LT Spice For Radio Amateurs: PART 4

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.


LT Spice For Radio Amateurs: PART 3

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.


LT Spice For Radio Amateurs: PART 2

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.