New Class A, Super-A, Non-Switching : need a revival ?

[dadod]

Hi Dadod

Sorry some how I missed your post until Valery mentioned this.

I just simulated, it looked strange. Can you explain how does this work? You have a voltage and a current generator.

I have to read the new stuffs you added like the image attached. I never get this advanced.

Thanks

Tha is Tian probe. Just ran simulation, click on output and then change shown plot with -1/(1-1/(2*(I(Vi)@1*V(x)@2-V(x)@1*I(Vi)@2)+V(x)@1+I(Vi)@2)) .
that is on .asc file too.
To plot the Loop Gain you need just part of dot commands:
.step param prb list -1 1 ; set prb=0 to turn off probe
;.param prb=0
.ac dec 1k 1 1G

Better take a look LTspice example loop2.

I suggest to study LTspice a bit more, you can't just jump in the middle of it without better understand.

 

[Audiocrase]

Hi Dadod

I am studying the LTSpice right now. What Tian probe? I don't understand and I only found one article on web but it's more explaining in spice derivatives which I don't understand. LTSpice does not have anything on this either.

I want to know how the two generators work in the loop. What Valery showed make sense to me but it failed in the simulation. This I don't understand.

Thanks

 

[dadod]

Hi Dadod

I am studying the LTSpice right now. What Tian probe? I don't understand and I only found one article on web but it's more explaining in spice derivatives which I don't understand. LTSpice does not have anything on this either.

I want to know how the two generators work in the loop. What Valery showed make sense to me but it failed in the simulation. This I don't understand.

Thanks

LTspice has it in examples: LTC/LTspiceIV/examples/Educational/LoopGain2

 

[vzaichenko]

Tha is Tian probe. Just ran simulation, click on output and then change shown plot with -1/(1-1/(2*(I(Vi)@1*V(x)@2-V(x)@1*I(Vi)@2)+V(x)@1+I(Vi)@2)) .
that is on .asc file too.
To plot the Loop Gain you need just part of dot commands:
.step param prb list -1 1 ; set prb=0 to turn off probe
;.param prb=0
.ac dec 1k 1 1G

Better take a look LTspice example loop2.

I suggest to study LTspice a bit more, you can't just jump in the middle of it without better understand.

I made it working. Damir - thank you for a hint

 

[Audiocrase]

Here is the Loop Gain simulated with Tian probe, PM=62 dB, GM= 4 degree. I changed some models as I don't have them.
You have to work on it a bit more.

I simulate with your modified file, it does not look right. So I try with a known opamp LT1360. I attached the .asc for LT1360 which is just your program with the LT1360 substituted in. I also attached the open loop gain of LT1360 from datasheet and the graph of your simulation. They don't look that same at all. You have the green trace of phase going to -400deg also.

 

[vzaichenko]

I simulate with your modified file, it does not look right. So I try with a known opamp LT1360. I attached the .asc for LT1360 which is just your program with the LT1360 substituted in. I also attached the open loop gain of LT1360 from datasheet and the graph of your simulation. They don't look that same at all. You have the green trace of phase going to -400deg also.

Audiocrase, attached is what your model shows.

1) Copy the blue formula at the bottom (Ctrl+C);
2) Run the simutation;
3) Press "A" - Add to plot dialog will open;
4) Paste the formula into the dialog (Ctrl+V);
5) Press "OK" - see the plot.

Cheers,
Valery

 

[vzaichenko]

These curves are different from the datasheet plot you attached earlier, as they are different by nature - the ones in the model show the feedback loop response with the loop closed, the ones in the datasheet are just open loop. Those will always be different. For analyzing stability you need to look at the feedback loop curves with the loop closed. Open loop curves don't give you this info.

 

[Audiocrase]

Audiocrase, attached is what your model shows.

1) Copy the blue formula at the bottom (Ctrl+C);
2) Run the simutation;
3) Press "A" - Add to plot dialog will open;
4) Paste the formula into the dialog (Ctrl+V);
5) Press "OK" - see the plot.

Cheers,
Valery

Thanks, I got it. What is the point in the schematic is this? Can you explain this?

-1/(1-1/(2*(I(Vi)@1*V(x)@2-V(x)@1*I(Vi)@2)+V(x)@1+I(Vi)@2))

What section to read to do this in the LTSpice?

Thanks

 

[Audiocrase]

Hi Valery

This is the plot per your instruction. This is a loop gain plot with the loop closed.

So you want to look at the loop gain trace at the point crossing the 0dB line. If the phase at that pointis >=180 degrees, then it's not stable.

The phase is about -200 deg, so it's not stable, I need to make the phase at 0dB less than 180deg?

 

[Bob Cordell]

I cannot make the open loop test suggested by Valery. I attached the .asc. I don't know what I did wrong. It won't give me result. Please help.

Thanks

2 things. You do not have the feedback network in place. With the inductor method, you should be simulating loop gain, not open-loop gain. Keep the feedback network in place (e.g., something like 19k in series and 1k shunt to ground) and put the inductor in series with the feedback network. Then inject the AC signal into the junction of the inductor and feedback network series resistor. This allows any excess phase effects at the feedback input to the IPS to be properly taken into account. Also, for simulation purposes, especially for transient and distortion, don't keep the feedback network capacitor in the circuit. Just short it. Otherwise, it introduces a long time constant that can affect the simulation.

Secondly, you are simulating a TMC compensated amplifier. Just simulate a conventional Miller-compensated amplifier until you get things working right and build confidence.

Cheers,
Bob

 

[Audiocrase]

2 things. You do not have the feedback network in place. With the inductor method, you should be simulating loop gain, not open-loop gain. Keep the feedback network in place (e.g., something like 19k in series and 1k shunt to ground) and put the inductor in series with the feedback network. Then inject the AC signal into the junction of the inductor and feedback network series resistor. This allows any excess phase effects at the feedback input to the IPS to be properly taken into account. Also, for simulation purposes, especially for transient and distortion, don't keep the feedback network capacitor in the circuit. Just short it. Otherwise, it introduces a long time constant that can affect the simulation.

Secondly, you are simulating a TMC compensated amplifier. Just simulate a conventional Miller-compensated amplifier until you get things working right and build confidence.

Cheers,
Bob

Hi Bob

Thanks for the response

I did, that was the first thing I tried and it's still failed. Attached is the one that try to simulate loop gain and phase, not open loop.

All you need is to change the .include experimental_BJT modified.txt to your transistor model file. I use all the transistors in your model file.

I prefer this simulation if I can make it work. I just don't understand the Tian Probe and how it work given by Dadod, also I just don't follow the result and has to plot the trace using. -1/(1-1/(2*(I(Vi)@1*V(x)@2-V(x)@1*I(Vi)@2)+V(x)@1+I(Vi)@2)) to plot.

Thanks

 

[dadod]

Thanks, I got it. What is the point in the schematic is this? Can you explain this?

-1/(1-1/(2*(I(Vi)@1*V(x)@2-V(x)@1*I(Vi)@2)+V(x)@1+I(Vi)@2))

What section to read to do this in the LTSpice?

Thanks

You just don't read what I pointed where to find Tian probe explanation in LTspice: http://www.diyaudio.com/forums/soli...on-switching-need-revival-19.html#post4871699

 

[Audiocrase]

You just don't read what I pointed where to find Tian probe explanation in LTspice: http://www.diyaudio.com/forums/soli...on-switching-need-revival-19.html#post4871699

I could not find it. I open the LTspiceHelp and search every single category. I search for "examples", "educational" and "Loopgain2". Nothing return. Only thing return is "example circuit" which has nothing to do with it. I did spent quite a bit of time on this before I gave up. I looked through the Index for all the words above also.

Obviously searching for "tian" or "tien" did not return anything.

What you have looks like Plot expressions of traces in the help file, but I still don't know the formulas. Seems like you can't get the loop gain plot directly from the circuit you posted, you have to use the values of different nodes to calculate the final plot. It seems like there is a much easier way to set up the circuit to plot directly from a node.

 

[Audiocrase]

At the mean time, I am still playing with the way Valery suggested, but I modified to loop gain plot by adding back the 20K feedback and 1K shunt resistor as shown in the .asc files attached. What Valery shown is open loop gain, but it would run into the same problem like I changed the shunt resistor to 0.1ohm. That will hide the effect of the input capacitance of the LTP. Driving the input with signal generator to the -ve input like Valery suggested also hide the effect of the capacitance as the output impedance of the generator is very low too.

But I ran into problem that my simulation, if failed. For the life of me, I cannot see what is wrong with the circuit and the way I set it up. I have been spending hours on this and what Dadod suggested. Please take a look and point out what I did wrong.

Thanks

 

[Audiocrase]

I found my problem. I need to set the amplitude of the generator on the right side, not just the left side. Attached is the .asc and the loop gain phase plot. This looks a lot more like the ones in the data sheet. This is a modification of Valery's idea.

I label the -3dB point of loop gain and 0dB point of open loop gain(-30dB down in loop gain as closed loop gain is about 30dB).

 

[dadod]

I could not find it. I open the LTspiceHelp and search every single category. I search for "examples", "educational" and "Loopgain2". Nothing return. Only thing return is "example circuit" which has nothing to do with it. I did spent quite a bit of time on this before I gave up. I looked through the Index for all the words above also.

Obviously searching for "tian" or "tien" did not return anything.

What you have looks like Plot expressions of traces in the help file, but I still don't know the formulas. Seems like you can't get the loop gain plot directly from the circuit you posted, you have to use the values of different nodes to calculate the final plot. It seems like there is a much easier way to set up the circuit to plot directly from a node.

It is not part of LTspice help, but in LTspise directory on your hard disk, and I showed where to find it.

 

[Audiocrase]

Thanks Dadod

Now I got it. I've been on the wrong track.

But what do you think about my last post of using the inductor like Valery suggested to open the loop and go to loop gain simulation like Bob suggested?

 

[dadod]

Thanks Dadod

Now I got it. I've been on the wrong track.

But what do you think about my last post of using the inductor like Valery suggested to open the loop and go to loop gain simulation like Bob suggested?

I don't use inductor, it is not good enough method.

 

[Audiocrase]

I don't use inductor, it is not good enough method.

What is wrong with the inductor and the way the circuit is?

 

[dadod]

What is wrong with the inductor and the way the circuit is?

Nothing is wrong with the inductor, just it is not accurate enough. This method is similar with the one used in LoopGain.asc(also explained in the LTspice examples), where you get the loop gain instead open loop gain as with the inductor method. The Tian probe is explain in the LoopGain2.asc :

Here the open loop gain is determined from the closed loop system[1].
The open loop gain can be plotted by plotting the quantity:

-1/(1-1/(2*(I(Vi)@1*V(x)@2-V(x)@1*I(Vi)@2)+V(x)@1+I(Vi)@2))

Alternatively, you add the following line to your plot.defs file:
.func T.et.al() -1/(1-1/(2*(I(Vi)@1*V(x)@2-V(x)@1*I(Vi)@2)+V(x)@1+I(Vi)@2))
And then plot simply T.et.al()

This is an improvement over the technique shown in LoopGain.asc
because it (i) accounts for reverse feedback(it doesn't even
matter if you reverse the direction of the probe -- you still compute
the same open loop response) and (ii) the inserted probe elements
result in a smaller, sparser circuit matrix.