Audio power amplifier improvement

Question

I need someone to revise/suggest improvement for the audio power amplifier I am designing. This PA is going to be used for driving the horn speaker (8ohm 100W). I decided to start design from scratch instead of just copy/paste existing design (of course this is still not something new, you can find the same topology on Internet, Hitachi has similar concept in app note). As you can see, it is composed of two stage differential amplifier. The first differential amplifier uses Wilson current mirror as a current source, and the second the "standard" current mirror as a load. The second differential amplifier provides bias voltage and drives the output stage. For the output stage, I selected mosfet approach that is composed of 4 mosfet transistors (complementary). I must emphasize that I am not much in analog design field, so does not have strong sense if this design is any good. This is the part of bigger project with the rest of digital logic. The main aims of this PA is to be stable, and to use in wide temperature range (preferably in range of -20°C - 75°C), if possible. Therefore, I need your revision and improvement suggestion. I highlighted a couple of design doubts:

1. I am not sure about this kind of bias (the red circled resistor would be potentiometer). Is this stable and safe (not get in situation to blow up mosfets while adjusting bias)?
2. Is this design stable (not oscillate)? Of course, I am planning to add Boucherot cell (Zobel network) at the output.
3. How to improve temperature operating range?

Please note that I used available bjt transistors from the LTspice lib. Maybe some improvement can be done also in that part.

The following are screenshots of schematic, transient analysis, and FFT analysis performed in LTspice.

EDIT: According to my simulations, I noticed that the mosfet bias current change with temperature is mostly caused due to change of emitter current of driving differential amplifier (that also changes the voltage drop on R4 and sets mosfet bias). I decided to implement current source based on current in emitter of the driving differential amplifier instead of simple resistor. I got better results in therm of bias stability, if I am correct. There are also some changes due to suggestions. The revised schematic is following:

Answer 1

To find out, if something runs stable, you can add:

.step temp 0 100 20

Explaination:

.step what start end incement

This will run the simulation multiple times and you will see, if it is stable over a wide temp range.

The problem with a sim is, that the parts are ideal in most ways. For example: components will not die in simulation. That means, if your potentiometer is rated for 50mW and you run 100mA at 20V through it, it will insta-fry (well, actually, it sometimes can take a few seconds and smells horrible. Ask me how i know)

Important questions to answer when designing an amplifier with push pull configuration:

• View both mosfets currents - do they overlap? There should of course be no time, where both are not conducting any current at all. It might be stable enought, if the lowest current is 10mA - just try to change the temperature, if this changes anything
• will your components dissipate the heat? Just hover over the component after simulating to a stable point and it will show the power dissipation (on the bottom, if I remember correctly). Otherwhise, measure the waveforms and calculate the TDP of each part. This is absolutely mandatory of course. I mean, you could also just build it like most people do, but risk frying something.

About the stability with mosfets: It does not matter at ALL. No need to balance anything. Mosfets conduct less current, when they get hot, which means, they cool down. This basically creates an equilibrium. They are self balancing. Just do not take < 20mOhm mosfets, as they could be so far unbalanced, that one conducts all current from the start (if everything is cold) and therefore fries itself because a bond wire fails or so. Relatively unlikely however.

But there is still one problem: if the temp changes, Vgs(th) also changes. This will move the bias point. So try to fix this in simulation. You absolutely have to simulate with different temperatures. If you don't do so, it will often yield in problems. Big problems. And the more complex the circuit gets, the more you risk that.

Just pretend something for a second: If your amp has a frequency range of 100kHz or higher, the bias might not matter that much. Why? Well, you just could add a 30kHz low pass with 4 stages. This would remove basically ALL the "switching" noise - if your input differential amplifier can handle such aprupt changes. It is possible, but not the best solution.

Just a question: Why even use Mosfets at all? NPN Quasi and NPN/PNP complimentary push/pull is somewhat preferable in most cases. Why? Well, it first is simpler to implement, second it has much more stable bias and third, at higher frequencies you do not need to fear the gate capacity as much. I had some circuits with mosfets - at 20kHz the signal was totally crappy, because the gate charge was far to high. Like an order of magnitude to high! Keep that in mind.

If you want to know, how to really test the performance of the amp, do the following 4 things: - Simulation with 20kHz in and lowest input voltage (like if you use 1Vpp, use 100uV) Is the signal still clean and recognizable? Is the gain the same as full volume? Do the math.

• Simulating with 20kHz and max amplitude - this shows, if the main circuit really is able to sustain the gate drive in a clean way.

• Simulate at lowest frequency and max amplitude - will it be clean?

• simulate at lowest frequency and lowest amplitude - will it be clean?

the last 2 are not to undereastimate! The switching, I was talking about, can be invisible at higher frequencies. It will show at lower frequencies however. Now add that to the lowest amplitude. If this also is stable and has the same gain as always, it absolutely runs smooth.

This is mandatory!

But you are not done! Repeat that at least with the following temps:

• 0°C
• 20°C
• 40°C
• 70°C

This is also mandatory!

What else to recommend?

If you want to know, if the signal really is perfect: add a resistor between the input signal and the reference ground. You can show both the current of this resistor and the output voltage. If they perfectly overlap, the signal is clean. this works, because LTspice scales the... scale ...in a "perfect" way. You will instantly see any differences. If the signal is inverted... Just duplicate the input signal and reverse the polarity. Just remember, to change both frequencies and voltages at the same time, or you will have a missmatch.

That is, how I create or test amplifiers with the most precision. Also good:

If your sine wave looks very choppy (like there are not enought polygons in a game), change the "Maximum timestep" variable, till it is a nice balance between precision and speed. LTspice sometimes calculates to few steps, if the circuit is to easy to simulate. Why waste resources? But this of course limits your ability to evaluate the waveforms.

Hope, I could help you with that advices. Most of it is very important.

Answer 2

For the output stage, I selected mosfet approach that is composed of 4 mosfet transistors (complementary).

It's weird to use TO-247 IRFP240 with TO-220 IRF9640. If you use MOSFETs in pairs, the reason would be dissipation, so it would make sense to pick both transistors in TO-247 which has much better thermal properties. This is mostly due to the increased metal surface area on the back which allows use of a larger surface area of thermal interface material, which is the weak link.

Besides that, IRFP240/IRFP9240 is a good choice.

I must emphasize that I am not much in analog design field, so does not have strong sense if this design is any good.

You should read this book. You can also get it as an ebook. It will save you a lot of money in burned MOSFETs.

I am not sure about this kind of bias (the red circled resistor would be potentiometer). Is this stable and safe

This will not work. From the datasheet:

FETs have positive RdsON tempco which means RdsON increases with temperature. This is great for switching as this means they can be paralleled easily and current will be shared between the FETs. However when used in linear mode as in an audio amp, at low currents the temperature coefficient is the other way around, just like a bipolar. Threshold voltage goes DOWN with increasing temperature, which means current bias increases.

This means your parallel FETs will not share current equally: the hotter one will get more current, so it'll heat more, and take even more current. Also your FETs will not be matched, unless you buy a lot of them and match them manually, so you need to add source resistors to parallel them. This will not appear in simulation, because simulated FETs are all perfectly identical, unlike real world FETs.

Also your bias will be unstable: since the bias circuit does not compensate for temperature, and the FET threshold voltage goes down with increasing temperature, bias current will vary a lot over temperature, and it can also go into thermal runaway and burn your fuses or the FETs. Hopefully you'll have a fuse on the transformer primary.

So, if you are interested in learning how to design an amp, I'd recommend reading Cordell's book.

If you want to build an amp without spending time on learning and design, get a MOSFET amp kit, or use a LM3886 or TDA7294 which are both excellent and easy to use chips. A Class-D amp module is also an option.

Answer 3

I like the circuit. With 2mA tail current in the first stage (90 volts / 44Kohm), you have 4 volts across R3 and R1, thus about 3 volts across the 220 ohm in second stage, producing 6mA thru the 900 ohms. OK. thus about 5 volts to bias on the output FETs.

I'd use emitter resistors in Q10//11 as you did in Q2/3 to ensure base-voltage need not be well matched.

I'd add emitter-degeneration resistors in that first diffpair, to expand the "linear range" from just a few milliVolts to 500 milliVolts. This produces lower distortion.

The first diffpair will have some thermal distortion (your diffpair transistors are in separate packages, so are not thermally tracking); maybe add common-base devices biased at -5 or -6 volts with a Zener, to cut the self-heating by 10:1 and improve the low-frequency upconversion. Otherwise, bass tones will be upconverted and become AM sidebands on your higher tones; you won't like the result. Doug Self's book on amplifier design discusses this.

Have you examined an open-loop gain-phase (BODE) plot?

I'd place a 1nF cap across that 900 ohms. If not bigger.

Also, the large C_gate_drain capacitors will slow down the slewrate. That allows lots of high-frequency distortion.

Answer 4

Short answer: I build the circuit. Change the bias from 900 to 1k. This made it stable from 0°C. Before it only was stable above 20°C. It would sound bad at low volumes. With 0.1mV I get 3.5mV and 1V in gets 35V out. Congrats. With this small change it should work. It does not seem to increase current draw with higher temp, so I would consider building it. It looks very promising. I will save this circuit for a hobby project later maybe.

Only thing to do:

Maybe use other components. Changing to cheaper components for mass production or even for hobby is good in most cases. I try to find the cheapest part and stay at <50% of the power rating and <80% Voltage rating. Do not risk cheaper parts however or somthing could fail. And also remember: Measure the voltage peaks at the components. Remember: Some components get 90Vdc! Not just 45Vdc - since it might sweep through all the voltage range.

Have fun. A nice ciruit, it seems. Good work.

Edit: With the sentence "...so I would consider building it." I meant, try even without potentiometer. I am a cheap-ass. I usually do not use a pot. I do not care, if the bias current is 10mA or 40mA. As long as it does not draw to much current in idle. But just for fun it does not need that perfection. I mean... usually! This circuit does not seem to benefit from a pot - others might of course!

Edit again: The other guy said "This will not work", meaning the bias resistor. Yes, it does! It actually works perfectly to my surprise. I was very surprised. It seems very stable. And at least with 10kHz it performs great.