Engineering Differential amplifier confusion (BJTs + Operational Amp)

[LvW]

To complete my analysis of the circuit under discussion here are my simulation results:

* Baluncore`s circuit (post#22) with all values as given in the figure.
* Opamp modell (PSpice) LT1022/LT
* Transistors BC549
* Loop gain analysis indicates instability up to a closed-loop gain of at least Acl=50 (34dB).
That means: Stable for closed-loop gains above 34 dB only.
(Note: To verify instability in the time domain we must check "skip initial transient solution" or switch on (at least one of the) power supplies at t=0).
* The circuit was stabilized lowering the gain of the long-tailed pair using negative feedback with two additional resistors (100 ohms) between the emitter nodes and the current source (still 10mA).
* Now the circuit works stable down to a closed-loop gain of app. Acl=4 (12 dB, stability limit, opamp feedback resistors 1k, 0.250 k). That means: Stable for closed-loop gains > 12dB.
* Similar results for OP-27/LT

 

[alan123hk]

@LvW
Your approach of adding two resistors to the emitter is perfectly fine.
I think of another method as shown in the figure below, adding a capacitor between the collector and base of Q2. Although the bandwidth and stability of my method are slightly worse than yours, it still seems to be able to keep the circuit in a stable working state.

It would be interesting to try to compare the stability of the two approaches.

 

[LvW]

Ala123hk - I am sorry but I cannot confirm your findings.
Perhaps you have used another OP-27 model?
I have used OP-27/LT (but similar results for OP-27/AD ) with two 1k feedback resistors.
How did you simulate the loop gain?
I have used an ac source between the opamp output and the first resistor (in your diagram R4).
My results:
* With two 100 ohms in the emitter legs: PM=-10 deg and GM=-3dB
* With C1=200pF (without the 100 ohm resistors): GM=-40dB (PM not applicable because the phase crosses the 0 deg-line twice).

Most remarkable: In my simulation, the loop gain settles app. at -60dB above 100 MHz (in your simulation it goes down to max. -20dB and rises again).

EDIT: OK - using a simple model called OP-27 my results are very close to yours.
This is another proof that modelling of the 2nd and 3rd pole is very important in the case under discussion.

 

[Baluncore]

If you do not add sufficient noise, numerical stability can be a problem with any SPICE. You must kick the SPICE model of a bicycle, clean out of the tram tracks, before it will actually become real and show it's true colours.

Do not trust SPICE, always build a prototype. Simple models often produce results that are too good to be true. The reverse can also happen.

If I drop a universal op-amp onto the LTspice sheet, but make no connections to it, the global internal connections appear to allow the model to be included without flagging any connection error. But then the analysis of a previously working circuit, that uses another op-amp, may be corrupted by the presence of the disconnected universal op-amp. Ground any terminal of the universal op-amp, and the problem goes away.

 

[alan123hk]

using a simple model called OP-27 my results are very close to yours.
This is another proof that modelling of the 2nd and 3rd pole is very important in the case under discussion.

I just pulled this OP27 from the parts library provided by LTSpice. I don't know how complex its internal structure is, like how many poles it has etc. If you mean it's a simple OP27 model, where can I find better or more sophisticated OP27 models?

 

[LvW]

Do not trust SPICE, always build a prototype. Simple models often produce results that are too good to be true. The reverse can also happen.

Of course, I agree. I am aware that there is a difference between model and hardware. Nevertheless, simulation programs are a very efficient tool at the beginning (the first step !) of a design phase.

If I drop a universal op-amp onto the LTspice sheet, but make no connections to it, the global internal connections appear to allow the model to be included without flagging any connection error.

As mentioned already in an earlier post - one must be very careful when interpreting simulation results.
Simple example: Universal opamp model with inadvertently added positive resistive feedback. All simulations (ac, dc, TRAN) will not reveal instability.
Error of the simulation program? No ! The program is not responsible - it has worked properly.
The user is the source of errror. He did not know that such a system can be stable (theoretically!) because there is absolutely no external disturbance.
Mechanical analogy: Two balls lie vertically on top of each other - without any mechanical interference from the outside.

 

[alan123hk]

LTSpice has several functions that can generate noise.
Link Removed

 

[alan123hk]

Sorry, I found the stability analysis Bode plot I uploaded a little bit inaccurate. Below are the corrected results that I think should be accurate enough.
It can be seen that the results obtained by the two methods of improving stability are almost the same.

Both have a flat bandwidth of about 5 MHz and good stability.

 

[LvW]

Sorry, I found the stability analysis Bode plot I uploaded a little bit inaccurate. Below are the corrected results that I think should be accurate enough.
It can be seen that the results obtained by the two methods of improving stability are almost the same.
...
Both have a flat bandwidth of about 5 MHz and good stability.

Hi Alan,

in order to interprete your results it is important to know which circuit you have simulated - the circuit in post#52?
Which opamp model?
Which kind of correction?
How did you simulate the loop gain?

 

[alan123hk]

in order to interprete your results it is important to know which circuit you have simulated - the circuit in post#52?
Which opamp model? Which kind of correction? How did you simulate the loop gain?

Of course, I just use the OP27 model provided by the parts library of the LTSPice, because it is very convenient.
For my suggestion to improve stability, the correction I said is to first change the single capacitor into a resistor and a capacitor in series, place it between the collector and base of the transistor Q2, and then move the injection voltage from the previous position to the output of op amp U1.
The image below says it all.

By the way, unfortunately for amateur electronics enthusiasts like me, due to limited resources, we can only do a simple loop gain simulation analysis of the linearization circuit using free software.
But for the laboratories of large companies and universities with deep pockets, in addition to computer simulations, they also have very advanced instruments to perform this analysis on real circuits.