simple bjt amp stage/low THD?

[questron]

hi guys,

i'm not building anything right now, and since i stumbled upon this simple BJT amp stage circuit topology, i'd like to explore it, aiming at having control over achieving the lowest THD. so i tried the following different circuit topologies, where Rb is used to set the gain, and all of them are set to be around 30, in order to facilitate comparison. all questions regarding practicality are purposely ignored.

a plain one, no shunt bias even, used as a reference point for comparision. power supply is 6v.


shunt bias.

worse than just plain.

NFB.

the NFB is done through emitter degeneration, although it is better than the shunt bias case, but still a lot worse than just plain.

12v shunt bias.

the best so far. maybe emitter degeneration is not as effective as raising the supply voltage?

24v shunt bias.

the best so far. this is the first time we can say that's a considerable improvement.

24v shunt bias, Long Tail Pair  input.

that's a much better THD number, absolutely the best in this study.

here is a summary

(note: the 12v roll is wrong, the THD in the schematic is correct, it should be 0.0858%, not 0.858%)

Observations:
1) shunt bias messes up the THD, the negative feedback provided with this topology does not help THD, it only seems to do the opposite.
2) raising the supply voltage high enough helped significantly.
3) long tail pair input helped a whole lot!

Question background:

in the long tail pair input case, i got this low THD number, 0.000446%, only by trial and error. values of the long tail resistor, R2, and the feedback resistor, R8, are both very sensitive. a change in value within 1% either way will royally mess up the THD number, so this doesn't seem to be the right way of doing a circuit.

also, Vc of the long tail pair is way to close to the supply voltage, 23.61v vs 24v. i'd like to have it closer to the the mid-point of the supply, but when i try change the resistor values, i was not able to get the THD down to the lowest ever achieved, 0.000446%, not even close, off by 100x or even 1000x.

plus this circuit is ugly, i don't know how i should bias the long tail pair, and DC blocking capacitors are everywhere, etc..

Questions:
1) how could i have control over the long tail pair's Q-point, without sacrificing THD?
2) what are the better ways of biasing them?
3) people say the long tail pair cancels out all even order harmonics, but the 2nd harmonic is still prominent, as seen in the FFT, as is the 3rd harmonic. what techniques can be utilized to at least significantly lower the 2nd harnonic?


4) generally speaking, are there other techniques of lowering THD of this circuit topology?

thank you for all inputs/comments/suggestions/helps!
 

[Jay_Diddy_B]

Hi,
I would have expected to see R5 and R6 connected to GND instead of the +ve rail in the long-tailed pair circuit.

If you run the simulation longer and set the maximum time step to 1us, you will get more accurate THD and FFT analysis.


.tran 0 50m 0 1u

Regards,

Jay_Diddy_B

[fcb]

I would have expected to see R5 and R6 connected to GND instead of the +ve rail in the long-tailed pair circuit.

Connecting R5 & R6 to GND won't work, his supply is single rail.

[Jay_Diddy_B]

I would have expected to see R5 and R6 connected to GND instead of the +ve rail in the long-tailed pair circuit.

Connecting R5 & R6 to GND won't work, his supply is single rail.

Oops !!

Missed that.

Jay_Diddy_B

[Jay_Diddy_B]

Hi,
I tried this variation on the circuit:



I obtained 0.000352% THD with Vin = 10mV peak.

Note: THD increases with signal amplitude. This is shown in this thread:
https://www.eevblog.com/forum/beginners/simple-bjt-amp-stage/

This is the FFT:



I have attached a zip file with the LTspice model.

Regards,

Jay_Diddy_B

[Jay_Diddy_B]

Hi,

This will also work:



It has similar THD.

Regards,

Jay_Diddy_B

[questron]

thank you Jay!
what are the gains of these two variations?

[fcb]

Gain is determined by the feedback network R4/R9.

[Jay_Diddy_B]

Hi,
FCB is correct for the second version.

in the first version the gain is

Gain = R9 / (R4//R6)

where R4//R6 is the parallel combination of R4 and R6

The gain of the first circuit is

620 / 39 //39 = 31.79

and the gain of the second circuit is

620 /20 = 31

So the gains are essentially the same.

Regards,

Jay_Diddy_B

[questron]

If you run the simulation longer and set the maximum time step to 1us, you will get more accurate THD and FFT analysis.
Jay_Diddy_B

thank you Jay!
very interesting point. i'm just wondering, is there an industry standard for frequency and time when simulating ciruicts for say radio/audio applications? if not, what is a reasonable frequency/time combination to use for such applications?

[questron]

thank you Jay, good work again, that's a much cleaner circuit, and a much better Q-point as well!
appreciate the help from fcb and you on the gain!

a few questions if you don't mind:
1) what's the advantage of a "voltage-divider" biasing scheme v.s. just the upper half of it, i.e. R6 and R7 only?
2) what's the advantage of using a gain-network v.s. just a resistor, R9? what does C3 do?
3) maybe it not possible to further suppress the 2nd and 3rd harmonics, but i'm curious about what could be done to them, comments/ideas?

[fcb]

1. divider allows you to set the input to cope with maximum swing - similar to split rail applications
2. both versions have a gain network..  C3 sets the gain at DC to unity - minimises DC error in direct coupled applications.
3. the cell you have on the schematics is the basis for most audio amplifiers, I suggest looking though schematics of some of the exotica out there (e.g. Krell) - good place to start is improving the current sources and perhaps looking at cascode transistors on the long tail pair, perhaps darlingtonify Q4 and understand miller effect?

[Jay_Diddy_B]

Hi,

I am going to add a few more pieces to the puzzle.

So far we have been concentrating on reducing THD. I am going to look at some other properties.

Square Wave Response

In this model I have replaced the 1kHz sine wave source with a 10 kHz square wave:



The results are not very good, there is a lot of ringing on the leading and trailing edge of the square wave:




This is normally an indication of poor phase margin in a servo system. The amplifier is really a servo, we are trying to reproduce the input with gain.

AC Analysis

We can break the control loop and inject a disturbance to measure the loop gain of the amplifier like this:



By plotting V(Va) / V(vb) we can see a Bode plot of the loop gain. We find that there is very little phase margin:




Adding a Dominant Pole

A pole can be added to the amplifier, in the form a capacitor between the base and collector of the transistor Q4:





 If I repeat the ac analysis I get this result:



The Bode plot shows that we have 60 degrees of phase margin.

If I now repeat the square wave test I get a much improved result:




The amplifier schematic now looks like this:




The THD at 1kHz with a 10mV peak signal is 0.000369%



Regards,

Jay_Diddy_B

[T3sl4co1l]

Note that R2 is superfluous -- however, open-loop gain can be increased by approximately the same factor again by replacing R1-R2 with a current mirror (R2 is the input side, R1 is the output side).

Add a follower output and you've got essentially a complete op-amp, as such!

My most recent example: http://seventransistorlabs.com/Images/Theremin_PLL.png
Note the similarities to the above circuit: diff pair, PNP gain stage output, feedback path to -in.  And the differences: current mirrors 'below' rather than fixed current sinks (because of different requirements, in this example), the feedback path has an R+C in it (this is an error amplifier, used to control the "Varactor"  line such that the "Mixer" line remains constant, so the DC gain should be as large as possible, whereas for a plain old signal amplifier, the gain is usually fixed), and this circuit has a MOSFET follower output, rather than nothing.

It's a powerful and flexible little circuit.  You can stack things on to extend gain, bandwidth, distortion, operating range and more.  The same basic circuit shows up in everything from jellybean op-amps to huge power amplifiers and analog computers.

Tim

[Jay_Diddy_B]

Hi Group,

Note that R2 is superfluous -- however, open-loop gain can be increased by approximately the same factor again by replacing R1-R2 with a current mirror (R2 is the input side, R1 is the output side).

Add a follower output and you've got essentially a complete op-amp, as such

Snip ...

Tim

This what the circuit looks like with a current mirror as the load for the long tailed pair:



The THD at 1kHz and 10mV has been reduced to 0.000175%  (1.75 ppm !!!) or 1.75mm in 1km

Regards,

Jay_Diddy_B

[fcb]

The THD at 1kHz and 10mV has been reduced to 0.000175%  (1.75 ppm !!!) or 1.75mm in 1km

That's a new measurement for THD.. mm/KM

[Jay_Diddy_B]

The THD at 1kHz and 10mV has been reduced to 0.000175%  (1.75 ppm !!!) or 1.75mm in 1km

That's a new measurement for THD.. mm/KM

The new unit allows you to visualize how accurate the speaker cone excursion has to be 

It is hard to visualize ppm, but we can understand mm/km.

Regards,

Jay_Diddy_B

[fmaimon]

The THD at 1kHz and 10mV has been reduced to 0.000175%  (1.75 ppm !!!) or 1.75mm in 1km

Is it possible to simulate the difference between transistors pairs (Q1/Q2 and Q6/Q7) as they are not matched? It may increase the THD.

[fcb]

You could go in an edit the spice model, but I think the easiest thing ( and more realistic) would be to alter the temperature of one half of the pair.

[Jay_Diddy_B]

Hi,

You can use the LTspice command ako: to generate transistors with modified parameters.

example:

.model 22221 ako:2N2222 BF=350

ako is 'A kind of'

So this means the new model 22221 is 'a kind of' 2N2222 but with the BF=350

BF is forward gain.

By using numbers only in the new model  name, we can use the step command like this:

.step param transistor LIST 22221  22222 22223

This means step the circuit through three variations of a transistor.


Here is the modified model:



If I look at the SPICE error log I see:

Circuit: * D:\projects\BJT amplifier\Long-Tailed pair current mirror.ascGmin stepping succeeded in finding the operating point.

Snip ....


.step transistor=22221
Snip...
Total Harmonic Distortion: 0.000206%


.step transistor=22222

Snip...

Total Harmonic Distortion: 0.000175%

.step transistor=22223
Snip...
Total Harmonic Distortion: 0.000145%


I have sniped out a bunch of stuff.

The model was run three times with different BF for the transistor Q2 and the THD calculated.

Note:

I changed the BF, but other parameters in the transistor can be modified to simulate a mismatch. This gives an indication to sensitivity of THD to a mismatch in gain.


Regards,

Jay_Diddy_B

[David Hess]

I am not convinced that your shunt feedback and transconductance amplifier tests were valid because the input DC biasing did *not* set the output level midway between the supply voltages.  That is going to result in very sensitive bias conditions and the transistor probably operating close to cutoff or saturation.

[Jay_Diddy_B]

Hi,

Here is another set of modifications that further improves the amplifier, the addition of an emitter resistor in Q4 and the reduction of the value of the feedback divider resistors:



This is a Bode plot of the loop gain. The phase margin is about 78 degrees:



The 10 kHz square wave response is excellent:



Regards,

Jay_Diddy_B

[T3sl4co1l]

Q1-Q2 can also be emitter-degenerated, for similar effect.  This reduces loop gain, but is generally considered to improve THD and bandwidth / phase margin.

Theoretically, I don't think this is strictly true to the first order.  But to the second order, it should be a noticeable improvement, and at very high frequencies (where phase shift piles up quickly), it becomes a first-order concern.

Also, Q6-Q7 don't strictly need emitter resistors -- as long as they remain matched -- but in the real world, they will be slightly different, so it can come in handy.  This affects the balance of currents in the diff pair, which in turn affects input offset voltage, which depends on Q1-Q2 matching.  Alternately, you can compensate for a mismatch in Q1-Q2 by applying the inverse imbalance at Q6-Q7, which is how trimmable op-amps do it (those emitter resistors are taken out to pins, so they can be adjusted with a single trimpot).

Tim

[questron]

wow, a lot of good works has been done since i last checked, a lot to learn about, thank you everyone for the good inputs!