Composite amplifier: LM3886 + LME49710

Status
This old topic is closed. If you want to reopen this topic, contact a moderator using the "Report Post" button.
Hi,

After reading tons of threads on this forum and all the info from the Neurochrome website I thought to give it a chance and design a composite amplifier using the LM3886 and the LME49710. I have some hobby level electronics experience and this would be my 4th serious electronics project (2 digital ones before, some RF involved and an electronic load where I learned about op-amps)

My goals are:
- 80-100W range for 8 ohm
- The lowest THD+N I can achieve
- Use the LM3886 instead of going discreete as it's my first amp
- Stability
- I want to design it to specs instead of just ending up with something that works accidentally.


I settled on a 4 chip parallel/bridged config with the same components as the Modulus-686 (if they work there, they will work for me as well :).

My first step was to learn the LM3886 so I started simulating it in TINA-TI to get it to be stable and learn the feedback loop, gain and phase margins and stability in general.
This was the easy part as I followed mostly the info here: LM3886 Chip Amp Stability Analysis

The next step was to add a LME49710 in front of it. This was trickier to stabilize as the whole thing tends to oscillate at around 5Mhz.
Getting the right phase and gain margins was a very interesting game of whack-a-mole for around one week.
After experimenting with various compensation components and adding a DC servo, here's what I have:
non-inverting.png

It's the non-inverting part. The input is setup so that I can inject bias voltages (that's why the cap is bypassed) and to measure the settle time of the servo.

The inverting part is this:
inverting.png

Here is the bandwidth of the inverting side. The non-inverting is the same:
bw.png

The noise says around 32uV at 20KHz for a 60V swing, so 0,000053333%? Am I doing this correctly?
noise.png

Step response. I did this with a 1K voltage generator with 1nS rise time:
step.png
step-zoom.png

My questions are:
- Does the schematic and compensation makes sense?
- How can I simulate noise over output power in TINA?
- The servo takes 15-20 seconds to eliminate a bias of 400mV. This is a long time and I don't want to mute the amp for this duration. Is this normal?
- What else could I simulate before I start doing the PCB layout?

[EDIT]
Check post #90 for the result:
Composite amplifier: LM3886 + LME49710
 
Last edited:
Member
Joined 2009
Paid Member
Looks like you're building a composite bridged amp. Sweet! If you're aiming for 80-100 W into 8 Ω, why the ±40 V supply? Not that it matters greatly for the simulation, but it does make a rather big difference in reality. If you're bridging the two amp halves, you only need about ±26-27 V to get 100 W into 8 Ω.

Also note that if you ever want to drive a 4 Ω load with this amp, you'll need two LM3886es in parallel per side. That opens up another can of worms as LM3886es in parallel don't always play nice. I've started to include circuits in my parallel designs (Modulus-286 and Modulus-686) that prevent the LM3886es from latching up if one supply lags the other on startup.

The THD you simulate in TINA-TI is mostly an indicator that your circuit isn't fundamentally broken. THD is not included in the LM3886 macro model, so the THD results will always be optimistic. I regularly simulate stuff in the 0.000001 % range in TINA. :)

A composite bridge/parallel amp would not be my first choice as a first amplifier project, fourth overall electronics project. There are quite a few pitfalls and trap doors in such a design and many of these are not covered by the simulation models. At least it looks like you're building two half-circuits, so you can test each half independently, which is a smart move. You can also always bypass the composite loop and test the LM3886s by themselves.

Before you build the circuit, I suggest looking at the open loop response. I'd also look at both small signal and large signal transient response with capacitive load.

Tom
 
Last edited:
I agree with Tom regarding the power supply voltage. The latch up problem likely will not be an issue if traditional linear supplies are used. An rc delay on the mute pin should help alleviate the possibility of latch up as well. Any issues that are not identified during simulation can be dealt with during the prototype phase. This is normal design practice.
I may jump on here and try some of your simulations as well
 
@wallyboy - no reason actually, I didn't know about the LME49724. I will definitely check it out, thanks for the hint!

@tomchr - first of all thanks a lot for the wealth of info you put on your website and on this forum.
After posting this I went and changed the power supply to ±28 as you recommend on your website.
I do intend to parallel 2 LMs on each side but I didn't include them in this simulation as it was slowing down TINA and I saw no benefit to keep them in the simulation at this stage.
My first step was indeed to simulate the open loop response for both the LM3886 and then the composite one. The bare-bone, no compensation composite schematic was resulting instability until I added the C2 3.3p capacitor and R5/R12 divider plus the C17 33p cap.
This took one week of tweaking and TBH I don't understand the need for the divider.
I get an intuitive feeling that high frequencies pass through C17 and get attenuated less than lower freq so this changes the frequency response but I'm not sure if it's the right way to compensate this beast.
Also - I'm not sure what that divider will do to the input impedance of the LM3886 and if the LM49710 can actually drive that.

Since it was my first simulation for Phase and Gain margin, I followed the methodology you posted here (LM3886 Chip Amp Stability Analysis) and targeted PM > 60 and GM < -10dB. I didn't get exactly there, I got something more like PM ~43 deg and GM < -15dB which I considered good enough.


Good to know that the TINA model doesn't include the THD of the LM3886. Where do distortions come from in this simulation then? Passives tolerances? Phase distortion?

I didn't know that the LMs can latch up. What do you mean by one supply lagging the other? Can this happen due to PCB layout issues - like different lengths for the supply tracks for each of the paralleled LM3886?

Cheers!
 
I'm pretty new to this too but I may be able to help a bit... I'm sure someone will jump in and correct me if I'm wrong :).

I think you need to look at the closed loop response. I think you'll find you have <0˚ phase margin. That means you'll get positive feedback in the high frequencies which will result in oscillation - I think it's possible to get around 80˚margin with this composite.
I'd also look at behaviour at clipping point, your design will clip the 3886 first which will drive the 49710 to try to compensate, the distortion will be pretty nasty... I'd adjust the gain structure. I think you'll find that lower overall gain and lower bandwidth will be easier to design and keep stable.
It may be worth considering how you can accommodate the stability components from the 3886 datasheet.
Lastly I'd suggest you take into account you may need to go through more than one iteration of PCB to get this working... design the layout so that you can get the soldering iron in to change the components around if you need to.

Like I said, I'm no expert but some of that may help.
 
Last edited:
@wallyboy - that makes sense, I forgot that this is dual-supply :)
So that makes it official - I'll go for a linear PSU.
If you want the TINA-TI files to run simulations, let me know. I'll be glad to send them to you.

@simonra - Actually my first PM/GM were with the loop closed and I was unable to get both right. Either PM was really good but GM was bad or the opposite, and the step response showed this clearly: there were always some oscillations of around 4-5Mhz. It seemed like the universe conspired to make this really unstable.
Then I re-read tomchr's page on stability and I noticed he measured the open loop response. After doing the same I managed to get both the PM and GM under control (it wasn't easy either, but doable) and the oscillations (with the loop closed) were gone.

So it's not clear for me at all: do I have to do the PM > 60 deg (or at least 0 deg) and GM < -10dB (or at least 0 dB) with both the loop closed and open?
That seems impossible :)

Good point with the clipping. So you're saying that I should choose the inner/outer gain so that the 49710 will clip first?

Regarding the PCBs, I'm prepared for that. Doing the PCB layout is actually super fun for me and I enjoy every second of it. It's also cheap and fast to get them from china (I'm using JLCPCB) so no worries there.
 
@tomchr - first of all thanks a lot for the wealth of info you put on your website and on this forum.

You're welcome. I'm glad you found it useful.

I do intend to parallel 2 LMs on each side but I didn't include them in this simulation as it was slowing down TINA and I saw no benefit to keep them in the simulation at this stage.

Fair enough.

My first step was indeed to simulate the open loop response for both the LM3886 and then the composite one.

Good plan.

I don't understand the need for the divider.

If you don't need it, why include it?

Also - I'm not sure what that divider will do to the input impedance of the LM3886 and if the LM49710 can actually drive that.

The input impedance of a non-inverting LM3886 is high, so the LME49710 is only loaded by the divider. You have 2 kΩ there total. The LME49710 can drive that just fine.

Since it was my first simulation for Phase and Gain margin, I followed the methodology you posted here (LM3886 Chip Amp Stability Analysis) and targeted PM > 60 and GM < -10dB.

That's a good place to start. You have to open the loop in the right place for the simulation, though. If opening the loop affects the load impedances in the circuit, you won't get valid results.

Where do distortions come from in this simulation then? Passives tolerances?

Have you included the tolerance of the passives in the simulation? How/why would they impact the THD?

You can often see THD in the simulation due to the simulator's choice of time step. You need to make sure you sample exactly one period of the input sine wave with the exact number of samples as you have points in your FFT. Otherwise, you'll get artifacts from discontinuities. I can find a few articles on that on TI's E2E forum.

What do you mean by one supply lagging the other?

One supply starting up before the other.

there were always some oscillations of around 4-5Mhz. It seemed like the universe conspired to make this really unstable.

Welcome to amplifier design. :)

Don't forget to measure the response to overdrive (i.e. soft and hard clipping) once you build the amp.

Tom
 
So it's not clear for me at all: do I have to do the PM > 60 deg (or at least 0 deg) and GM < -10dB (or at least 0 dB) with both the loop closed and open?
That seems impossible :)
My thinking is that the closed loop is what the op amp will see in reality. So if your negative feedback turns positive at a frequency that has >0 gain then it will cause instability.

So you're saying that I should choose the inner/outer gain so that the 49710 will clip first?
It's probably easier for you to simulate than for me to try to explain... send a sine wave at a voltage where the output just starts to clip and monitor the output of both the 3886 & 49710 by running a transient analysis.
When the 3886 hits the rail the 49710 will follow suit because of the imbalance between the input and feedback signals. Then the 49710 recovers quicker than the 3886 so it hits the other rail coming out of clipping.
Now adjust your gain so that the 3886 never hits the rail, this leaves the 49710 in complete control so recovery is smooth.

As I said before I'm new to this too so others may wish to correct me in my thinking or explain it better.

Good luck.
 
My thinking is that the closed loop is what the op amp will see in reality. So if your negative feedback turns positive at a frequency that has >0 gain then it will cause instability.
This was my reasoning when I started the simulations - I went for calculating the PM and GM with the loop closed and I was unable to get it stable for a week.
Then I realized that maybe I'm doing it wrong so I re-read tomchr's page (LM3886 Chip Amp Stability Analysis) and this (Negative Feedback, Part 9: Breaking the Loop) and they both mention the PM/GM of the open loop.

It's probably easier for you to simulate than for me to try to explain... send a sine wave at a voltage where the output just starts to clip and monitor the output of both the 3886 & 49710 by running a transient analysis.
When the 3886 hits the rail the 49710 will follow suit because of the imbalance between the input and feedback signals. Then the 49710 recovers quicker than the 3886 so it hits the other rail coming out of clipping.
Now adjust your gain so that the 3886 never hits the rail, this leaves the 49710 in complete control so recovery is smooth.

For 49710 to clip first I see 2 options:
1. Reduce the gain of the 3886 so that the 49710 has to swing more. This is not a good idea as the 3886 is not stable below 10x gain according to the datasheet
2. Add a voltage divider between the 2 opamps so that the 3886 sees only a fraction of the 49710 swing.

I'll try #2 and see where that takes me.

I'll post back the results.
 
If you don't need it, why include it?
It was the way I found to stabilize the amp. By adding that divider I was able to add the C17 capacitor and the PM got way better.


That's a good place to start. You have to open the loop in the right place for the simulation, though. If opening the loop affects the load impedances in the circuit, you won't get valid results.
I opened the loop exactly as you recommend on your website.
But as simonra was saying - is it enough to simulate PM/GM of the open loop? Don't I have to do the same with the closed loop to get a stable amp?

Screenshot from 2019-02-22 09-44-41.png

For example with the loop closed I get a PM of 131 and GM of 13 which sounds really bad, but the same amp with the loop open was getting way better PM/GM.
What's the correct way to characterize the amp stability?

You can often see THD in the simulation due to the simulator's choice of time step. You need to make sure you sample exactly one period of the input sine wave with the exact number of samples as you have points in your FFT. Otherwise, you'll get artifacts from discontinuities. I can find a few articles on that on TI's E2E forum.
Yes, simulator aliasing seems like a good way to get THD.
 
I applied your idea simonra and did the simulations again:
Here is the step response:
Screenshot from 2019-02-22 19-31-46.png
Here is the gain peaking:
Screenshot from 2019-02-22 19-31-49.png
And here is the phase margin calculated according to this (https://training.ti.com/ti-precision-labs-op-amps-noise-3)
Screenshot from 2019-02-22 19-44-11.png
This is the schematic used to calculate the phase margin:
Screenshot from 2019-02-22 19-46-12.png

I get a margin of 65 deg, confirmed by the step response which shows no overshoot at all and the gain peaking - which is zero.

Next I will test the clipping characteristics of both configs: clipping handled by the 47910 or by the 3886.

I did the math like this:
1. The 3886 is configured with a gain of 12 and can reach (Vsupply - 3V) on each rail before clipping. For +/- 28v supply, this means I want to drive it to max +/- 25V. Say 24V to make it round. So a gain of +/- 2V and a gain of 12x will result in +/- 24V swing.
2. The 49710 can swing +/-14V before clipping so to get the +/-2V for the 3886, I have to divide it by 7.

Does this make any sense? Did I miss smth?
 
Last edited:
have you read the article from the November 1992 issue of Electronics Magazine on composite amps? It has some decent info on composites. Here is the link:
Internet Archive: Page Not Found

Nope, didn't read it. Very interesting article although I don't really understand the topology in figure 3: where does the gain come from? Does this mean the LM1875 is a current amplifier only and the overall amp has no voltage gain?
Very good read, thanks for the article.
 
Then I realized that maybe I'm doing it wrong so I re-read tomchr's page (LM3886 Chip Amp Stability Analysis) and this (Negative Feedback, Part 9: Breaking the Loop) and they both mention the PM/GM of the open loop.

PM, GM are simulated open loop.

I opened the loop exactly as you recommend on your website.

I don't show any simulations of a composite amp on my website. I show loop simulations of the LM3886.

You always need to make sure that you break the loop in a way that has as little (preferably no) impact on the loop as possible. This generally means that you'll be breaking the loop at a point where the drive impedance is low and the load impedance is high. The "LC way" of breaking the loop that I like to use generally works well enough. There are fancier ways, however, which yield more accurate results. You can see Middlebrook's method for an example. There's a newer analysis by Tian (et al.) that's supposedly better or simpler to implement in the simulator. You can find some good links and references here: Education AC and Stability Analysis in NGSPICE. - Education

If you have access to IEEE (or are willing to pay for the paper), this looks worth checking out: Striving for small-signal stability - IEEE Journals & Magazine

But as simonra was saying - is it enough to simulate PM/GM of the open loop? Don't I have to do the same with the closed loop to get a stable amp?

No. The PM/GM (which are loop parameters, hence simulated open loop) are just one piece of the puzzle.

I start with the loop analysis, because if the loop isn't stable there's no point in simulating anything else. I then simulate the closed loop response to make sure I don't have excessive peaking and to pick out potential issues that I may have missed. I simulate the transient response to see how the amp behaves when slewing, when it reaches clipping, and on hard clipping. I look at the DC operating point to see the DC offset. I look at the noise performance. And take a quick glance at the THD to see if anything is fundamentally broken.

In a production environment I sweep these parameters across supply voltage and temperature as many of these characteristics vary across temperature. I don't recall if the LM3886 macro model takes temperature into account. It might. I know it laughs at the power supply voltage. Nothing power supply related is simulated with the LM3886 macro model.

Once I have a circuit that I feel reasonably confident in, I'll build it. I then correlate reality with simulation. Over time, I've developed a sense of the strengths and weaknesses of the LM3886 model, which allows me to shorten the development time. Basically, I know how far off target to aim in order to hit the target in reality.

Based on your questions so far, I recommend taking half a step back and brushing up on some stability theory. Chapter 8 in Franco is a good place to start. I'm sure there's a corresponding chapter in Yung. You can find the full references here: References.
In general, I highly recommend Franco for anyone interested in working with opamps and amplifiers in general. The latest edition (3rd) is absurdly expensive, in particular since it hasn't changed in 15+ years, but the 2nd edition is every bit as good (there were very few changes between editions) and can be found on the used market for less.

Tom
 
Status
This old topic is closed. If you want to reopen this topic, contact a moderator using the "Report Post" button.