PA100 with DC SERVO?

[peranders]

I agree that it doesn't HAVE to be so complicated. It just makes it better. When I first made the circuit and used it in the original application, there was a measurable increase in output THD under some conditions, without the additional filtering.

How much did the THD increase?

If you have 2 poles you'll get small thump and the closer the second pole is to integrator pole the more damped oscillations you'll get. Inserting even a third pole must increase the unstableness, yes?

 

[gootee]

How much did the THD increase?

Hi, peranders.

I'm sorry. I don't know. It was several years ago and I didn't make notes of that testing. It should be able to be seen with LT-Spice simulations. If I get time, I will try that again.

If you have 2 poles you'll get small thump and the closer the second pole is to integrator pole the more damped oscillations you'll get. Inserting even a third pole must increase the unstableness, yes? [/B]

It would increase the _tendency_ toward instability. But it is not unstable, as I have shown it.

There is a small "thump" and then about 2 cycles of additional overshoot and ringing at the filter output. With the circuit as shown, there might also be up to a few hundred microvolts of very low frequency steady-state oscillations, at the amplifier output.

So maybe it is not as stable as it should be, for this application. But, as I mentioned, for audio applications, the circuit might be able to be improved by lowering the filter's cutoff frequency. (But, CONTRARY to what I said in that same previous post, the integrator's frequency should probably NOT be lowered by the same proportion.)

There are trade-offs to be made, of course, as always. A steeper filter is better at keeping phase-changed audio from feeding back into the amplifier input through the servo loop. But the servo loop must also not cause other problems that might be worse.

For others who might be reading this: It is very simple to simulate an amplifier with a servo loop, with LT-Spice (free from http://www.linear.com), or any other Spice software. By running AC Analysis and Transient Analysis, all of the preformance and stability issues can fairly-easily be assessed and adjusted.

I just now did such a transient LT-Spice simulation, using capacitor values for the three filter capacitors that were approx double the values shown in my original schematic, i.e. 4.7uF, 1uF, and 1uF instead of 2.2uF, 0.47uF, and 0.47uF. The integrator was not changed. With these new values, even all of the very small, very-low-frequency oscillations appear to ge gone.

With a 23mV DC offset in the amp's input signal (a 1 kHz 1 V P-P sine), which would give 22 V P-P out, and, if used without the servo, over 500 mV of DC offset, I see that, at turn-on, the output experiences a 7.2mV downward thump during the first 0.13 seconds, then about one cycle of approx 4Hz ringing (only about 200 uV 0-P). And then the output rises cleanly by 2.5 mV over 4 or 5 seconds, until the offset is within about 0.25 mV of zero. (Well, it also looks like there might be about 2 uV p-p of steady-state output oscillation at about 0.2 Hz or so. But that is insignificant.)

Maybe I should mention that, for my examples, I have been using a non-inverted main amplifier configuration, and have an inverting opamp buffer amplifier between the filter output and the "R1" shown in the servo schematic I posted. The main non-inverting amplifier is simulated with an opamp, and has 10K || 2.2pF from output to - input, and 499 Ohms from - input to ground. R1 in the servo schematic is 10K, for this simulation, connected to the - input of the main amplifier, and follows the inverting buffer amplifier that I mentioned, which is an opamp with 10K || 4.7 pF from out to - input, 10K between - input and filter's output, and 4.99K from + input to ground.

With that configuration, it's possible to measure the filter's true output, i.e. without seeing effects from amp's - input node coming through R1.

Thanks, peranders, for pointing-out the stability issue. I am going to change the schematic, to use the larger capacitances in the post-filter section.

- Tom Gootee

http://www.fullnet.com/~tomg/index.html

 

[DJ Exprice]

What we need now is a FULL schematic

Something we can all go by.

I wanna use this in the BPA300 kit; one that works perfectly with it, but we'll wait on that for now until the BPA300v3 project ITSELF is somewhat more complete.

 

[gootee]

I have replaced the schematic of the DC SERVO, at

http://www.fullnet.com/~tomg/dc_servo.jpg

with a corrected and expanded version, which exactly reflects the schematic on which all of my original discussion and data were based, except that the post-filter's capacitors are now approximately doubled, per my last posted message. (Opamp types are not specified. But in my simulation, I happened to use an OP275 spice model, from Analog Devices' website, for all of the opamps. I also modeled all capacitors' ESRs, mostly as 0.03 Ohms.)

Anyone who has the older version of my DC SERVO schematic should note that it was actually incorrect: Without an inverting buffer in the loop, the integrator would have to have been re-configured to be non-inverting. (I guess that means that no has bothered to try to simulate it, yet!)

In case anyone is interested, I can try to post an additional version, without an inverting buffer in the loop, as well as the files needed to run LT-Spice simulations of them.

- Tom Gootee

http://www.fullnet.com/~tomg/index.html

 

[AndrewT]

Hi Tom,
the advantage of your original schematic was the DC accurate filter, even though we don't quite understand on what topology it is based.

Your new posting has inserted an opamp into the circuit. What has happened to the DC accuracy as a result? I suspect the output opamp (U1) sends it's output offset to the amplifier.

Why don't you post two versions on your site.
1) the original requiring the inverting amplifier.
2) a version with non-inverting integrator (without any extra inverting opamps).

 

[gootee]

Hi, AndrewT.

Yes, the additional inverting opamp buffer would not be good for a practical implementation, since, at best, its' offset drift would probably compound any offset drift problem.

I used it in this version of the circuit because it made it convenient to measure the voltage at the output of the post-filter and I just happened to already have an LT-Spice circuit with the integrator set up as shown. And then I wanted to post the exact circuit I had been simulating and referring to in my previous posts.

I will go ahead and put up a version without the inverting stage, with a non-inverting main amplifier. Eventually, I'll also post the same thing but with an inverting main amplifer example. I might as well also post the LT-Spice files for them, while I'm at it, since those will be so much more utile, for many people. But it will all have to wait until later today or possibly tomorrow, since it's not quite 8:30 AM, Saturday, here, right now, and I have some Curve Tracer DIY Kit orders to try to finish and get to the Post Office by noon, and then have some other things that need some attention. Sorry about the delay.

- Tom Gootee

http://www.fullnet.com/~tomg/index.html

 

[AndrewT]

Hi Gootee,
who's putting pressure on you by specifying time scales?
You're being good to us with all this research.
I and I'm sure a few others will be gratefull no matter how long it takes.
Thanks.

 

[gootee]

Hi, AndrewT,

No worries. Apparently I was putting pressure on myself.

I guess I've gotten better at that, now that I've been my own boss, for a while. I'll have to try to remember that my employee only works about 16 hours a day, and will try to put absolutely no pressure on him, ALL the rest of the time.

I do like doing the research, and "trying" to do design engineering. And it's somehow gratifying to share it, when I can (Must be a "character flaw". .

But I also get a benefit from that: I get the "peer review" process' results, which help me to improve my processes of research, analysis, and design, et al. i.e. I get critiques, and ideas, and knowledge, in return, also, which are sometimes very, very valuable (not to mention a bit of socializing, too). It's good situation, all things considered.

I'll try to let some air out of that "gas bag" employee, so he won't have so much pressure.

Thanks.

- Tom

 

[gootee]

I have made the LTspice schematic for the DC SERVO, in a version that has only a non-inverting integrator and a "DC-Accurate" third-order post-filter.

I went ahead and just added it to the new webpage I have for the LTspice stuff that I come up with and decide to share.

It's at:

---------------------------------------------------------

http://www.fullnet.com/~tomg/gooteesp.htm ,

---------------------------------------------------------

right after the transformer-measuring/modeling section.

I hope I didn't "go overboard". (This was BEFORE I realized I was putting too much pressure on the employee who I forced to do this for me. But, I like to include certain parasitics in my Spice models, now. And I think that it is especially-important for everyone to learn the best ways to run ground returns, which I am still always trying to learn more about, and "get my head around", better. And I think it would be helpful for people to realize that Spice can GIVE them most of the answers, about that stuff, without the amount of work they might be imagining, if they just set it up in their models. Yes, I'm talking about "The Dreaded PCB Trace and Wire Parasitics". Well, anyway, I set up this LTspice DC SERVO schematic to also be an example of one easy way to start to look at those effects. Or not. It works either way. Most of the relevant setup is separate from the actual schematic. That helps the schematic, for those who are only interested in that. But it also makes a nice base for trace/wire parasitics "beginners", because it should be easy to copy and paste it mostly all at once, to their own LTspice schematics.

Cheers! It's Saturday night! I'm outta here!

- Tom Gootee

http://www.fullnet.com/~tomg/index.html

 

[consort_ee_um]

As an aside another way of paralleling LM3886's here:
http://www.edn.com/contents/images/330071.pdf
Has anyone tried this technique?
I have not seen it mentioned on this forum, or have I not been paying attention!

 

[gootee]

As an aside another way of paralleling LM3886's here:
http://www.edn.com/contents/images/330071.pdf
Has anyone tried this technique?
I have not seen it mentioned on this forum, or have I not been paying attention!

Hi, consort_ee_um,

Thanks for pointing that out!

Yes, that's interesting. I didn't look at it in detail. But each amplifier "cell" looks, to me, like a Howland-topology current source, making a voltage-controlled current source (i.e. a transconductance amplifier).

There actually WAS a thread with a similar configuration (if I read it correctly), in the Chipamps forum, in January 2007, which is at:

http://www.diyaudio.com/forums/showthread.php?s=&threadid=94585

I was one of the few who responded. But the original poster never replied to anyone's questions, and the thread then died.

I still use a similar topology to implement a medium-low power amplfier (15V max/150 mA max) for my Curve Tracer's base/gate drive (see http://www.fullnet.com/~tomg/gooteect.htm ), so that the staircase waveform is user-switchable between calibrated voltage-controlled current and voltage-controlled voltage stairsteps, which it attempts for whatever load the user happens to connect. In that particular amplifier, I have an opamp with a power amp just after it, but with the opamp's feedback loops also encompassing the power amp, using a Howland VCCS topology. In such a setup, the power amp could be anything. But I used a BD139/BD140 BJT push-pull design for the "power" amplifier portion (which I might change to a small chipamp, if it's ever redesigned again, just to save a little PCB real-estate.)

Thanks again, consort_ee_um.

- Tom Gootee

http://www.fullnet.com/~tomg/index.html

 

[AndrewT]

Hi,
that EDN reference (Fig5) looks just like any other inverting topology, but with the output Rs moved inside the global feedback loop.

Does moving Rs inside the FB make this enormous difference to the phase margin?
Or is there some other difference that accounts for change?

Are all inverting topologies transconductance amps since they all have a virtual earth at the inverting input pin (just after the first input resistor)?

 

[JonHarrison]

Hi Tom,

Thanks for your efforts.

I had a look at your website and tried to download the LTSpice file for the servo but got a page not found error instead; same for the plot settings and the models. Can you help ?

Cheers,

Jon

 

[BWRX]

that EDN reference (Fig5) looks just like any other inverting topology, but with the output Rs moved inside the global feedback loop.

It is easier to think of it simply as a differential amplifier. The input signal (voltage difference between Vin and Gnd) gets amplified across Rs. Since Rs is fixed, you have a voltage controlled current source (as Tom mentioned three posts up).

mauropenasa's my_ref design uses an LM3886 based transconductance stage.
http://www.diyaudio.com/forums/showthread.php?s=&threadid=62483

 

[gootee]

Hi Tom,

Thanks for your efforts.

I had a look at your website and tried to download the LTSpice file for the servo but got a page not found error instead; same for the plot settings and the models. Can you help ?

Cheers,

Jon

Jon,

Mea culpa. At the last minute, I uploaded the files without the .txt filename extensions. It should all be working, now.

- Tom Gootee

http://www.fullnet.com/~tomg/index.html

 

[gootee]

Hi,
that EDN reference (Fig5) looks just like any other inverting topology, but with the output Rs moved inside the global feedback loop.

Does moving Rs inside the FB make this enormous difference to the phase margin?
Or is there some other difference that accounts for change?

Are all inverting topologies transconductance amps since they all have a virtual earth at the inverting input pin (just after the first input resistor)?

It's actually quite different from the normal inverting amplifier topology. Notice that it has both positive and negative feedback loops. Rs is basically a current-sensing resistor. You can google "Howland Source", or "Howland current pump" (maybe try http://groups.google.com, first). They're also described in "The Art of Electronics", by Horowitz and Hill. Best results, and best stability (since they tend to be unstable because of the positive feedback loop) are obtained when the four feedback resistors are very carefully matched.

I'm not sure I have answers to your questions. In one sense, any resistor in series with voltage amplifier output could be called a voltage-controlled current source. But the Howland topology tends to create a very linear I vs V response, with the current vs voltage response staying quite linear even with load-impedance variations (probably mostly due to the current-sensing resistor and its feedback).

- Tom Gootee

http://www.fullnet.com/~tomg/index.html