TINA/Spice/OPA549-HIREL: Composite amplifier for OPA549-HiRel using OPA192 with improved DC accuracy and drift

Hi Byliu,

Can you please describe the issues you are having? When I run the file you have provided I do not run into convergence issues.

Composite amplifiers are generally used when you need an amplifier with good dc precision and either strong drive capability or good AC performance as well. Because the loop of the first amplifier is closed around the output of the second, the dc error arises entirely from the front amplifier. Thus your drift and dc performance will derive from OPA192 and your output drive capability from OPA549.

The trick is in making sure that both amplifiers are stable. Since the OPA549 output is fed back to the OPA192 and subsequently to the non-inverting input of the OPA549, there are 2 feedback loops to contend with when conducting a stability analysis.

For the OPA192, there is an amplifier with gain in the feedback loop, and this creates an unusual case where your feedback factor can be greater than one. You need to have a local feedback loop (cap from input to output) to compensate for this.

If you simulate this circuit you will see that it is very unstable with excessive ringing on the output and ~8dB of gain peaking in the AC response.

If you aren't very familiar with amplifier stability analysis, here are two presentations that go through various analysis techniques!

3056.Solving Op Amp Stability 2015_TG.pptx

3441.Dual FB Beta_plus and Beta_minus RevD.pptx

Best,

Zak

Thank you for your reply.

I found that the simulation oscillates when the signal goes from positive to negative. I changed the first stage to a unit-gain follower, but the instability is still there. I found that this phenomenon is related to the Rload (R4). For example, if I change R4 to 20 Ohm or higher, the simulation is ok. If R4=5 Ohm or lower, the simulation went wrong.  So, I guess maybe it is related to the current limiting feature of OPA549?

My concern is

1. should I trust the simulation? If I fabricate such circuit, will it be unstable when R<5 Ohm and stable when R>10 Ohm?

2. Will the choice of OPA192 improves the overall DC performances? We want to design a high drive buffer for a DC motor, the RMS current requirement is 3A and the peak current might be 5A or more. We choose OPA549 and a 18/20 bit precision DAC for our application. In the datasheet of OPA549-HiRel, the voltage offset and the voltage offset temperature drift is too high (also the voltage noise) for a 18/20 bit DAC. We want to build a composite amplifier to mitigate the DC errors, especially the temperature drift. Your helps are greatly appreciated.

Thanks!

6114.opa549_composite.tsc

Hello all, thanks for the TINA file, that makes it trivial to set up and run a LG phase margin sim,

This circuit is well known but hazardous as all get out. Essentially you have injected a huge prop delay inside the loop. At an IC design level whenever we want to introduce a high power output stage (see the THS3491) we get into a lot of prop delay issues that hurt phase margin - same here.

Anyway, couple of key points

1. The power stage needs to be powered up and stable before the input stage comes up, I might tie a 1k to ground on the V+ input of the OPA549 to give it a reference point powering up. If not, you get into an odd stability issue we used to call motorboating as the whole thing tries to find a DC operating point. I often run an RC pole on the supplies from the output stage back to the input stage to enforce this.

2. Your current circuit is way unstable - couple of ways to fix this, but the easiest comes along with running inverting - is that an option???????

Composite ckt with OPA549 and OPA192.docx

Original LG sim.TSC

Thank you (I still could not open your tsc file, but the drawings in the word file is fine, can you open my tsc?).

1. Inverting is OK for me. I modify the circuit, add R10 to the inverting input, add R6 to the non-inverting port of OPA192. Add R11 of non-inverting port of OPA549 to ground, add a snubber circuit at the output. This circuit works when R4=11 or more, but it get unstable (in the tina simulation) when I changed R4 to 10 Ohm or less, i.e., 4 Ohm. I do not know where this instability comes from when R4=4 Ohm, is it because of the spice model of OPA549? is it about the architecture of Tina? or it is unstable in the final PCB board?

2. Should I give up the composite amplifier architecture? I am really not good at analyzing the stability of OPA192 + OPA549. And what's more, if I build this PCB, will it get the desired dc performance of OPA192 (low voltage offset, low voltage temperature drift) and the high current driving capability of OPA549?

6472.6114.opa549_composite.tsc

This would be the step response:

And this would be the frequency resposne:

Kai

And here comes the phase stability analysis:

byliu.TSC

Kai

Hi Michael,

if I don't use the voltage divider at the input of OPA549, I get a nasty overshot:

Kai

I think the slew rate this composite circuit is limited by OPA549. We want to have a lower temperature drift, offset voltages and noise.

We drive OPA192 with an 18/20 bit DAC, the update rate is 2.5 us, and generating a signal from DC to 20KHz. The signal is below 100 KHz, most of the time, its frequency is far below 10KHz. OPA549 is driving a DC motor, and we placed a shunt resistor at the output of OPA549 for current monitoring. 

yes, the other thing to always consider in these circuits is the relative slew rates - I was using a divide by two in R7 and R12 to divide the 20V/usec of the OPA192 down more closely to the 9V/usec of the OPA549. With that low 9V/usec slew rate, you probably don't want too much BW in the solution to stay out of slew limiting on a large step -that is a path to disaster as a slew limited output opens the loop up during slew, composite circuits have trouble recovering from that.

the 1k-1k divider seems ok to me.

Will I get the desired dc accuracy and temperature drift using this composite amplifier?

I also tried this circuit with an inverting and a follower mode of OPA192:

In the follower arch of OPA192, there is overshoot. In the inverting mode of OPA192, it is ok.

Are these circuits stable?

And if I want to have better DC accuracy (low voltage offset, low-temperature drift) and low noise, which one

1. non-inverting input, gain=2,

2. non-inverting inputy, follower,

3. inverting

should I use?

Hello, just got back from breakfast, 

1. It is best to start at your desired output swing. What is the maximum voltage step desired and rise time or settling time desired under that maximum condition. 

2. From there, can assess implied slew rate and start working backwards on the solution. 

3. So you are heading in the right direction, as you build these different ideas, could you insert the TINA file so we can easily pick up the evalution - thanks.

And here is that LG sim I tried to send earlier, I have to manually pick V9 so you can open it - if you need V7 I have that too.

7838.Original LG sim.TSC

Hi Byliu,

I wouldn't use a 1k 1k voltage divider:

And the bandwidth isn't higher, either. Also, the "spike" in the sine becomes visible again.

I would use my original circuit, but change C3 from 3n3 to 2n2. See my post above.

Kai

So Kai, the reason I am suggesting 1k divider with gain of 2 in the OPA549 is to not throw away loop gain unncessarily - there has been no linearity discussion yet, but LG is your friend in precision as long as you can keep good phase margin. And yes, this is inside the loop of a very linear amplifier - generally, total HD is the linearity of the output stage corrected by the LG of the overall composite. The big divider you have could certainly work and it definitely shifts the required swings out of the OPA192 way down - which can be useful, but seems extreme in your case.

I do no think the spikes have to do with slew rate. I changed OPA192 with OPA191, which is 5.5V/us, the spikes are still there with 1k - 1k divider.

OPA191_OPA549 kai.TSC

Hi Byliu,

when you run a noise analysis you will see that the noise is about three times higher.

Have you thought about running the OPA549 with a DC servo using the OPA192? This would at least eliminate the output offset voltage of OPA549. What is your lowest AC drive frequency?

Kai

Hi Kai,

Can I remove the overshot completely without using 1k-10k divider and amplifier?

Does the first stage amplifier (OPA192 or OPA210) is in a decomposed mode? Where the stable gain should be more than 1?

Benyuan

OPA210_OPA549 kai.TSC

Ok so that 10V at 20kHz is what I was looking for,

The attached runs through tuning in a non-inverting and then inverting design - few key points,

1.The input edge rate needs to be slow enough to stay out of slew limiting - if you do that, the step responses are pretty nice.

2. The OPA549 model appears to show a very distinctive negative going xover deadzone - is that real?

3. For precision, the 1k's setting the gains (overall loop, not inside the loop) need to be precision matched - those are available as matched pairs.

I can only attach one TINA at a time, here is the non-inverting one, easy to adjust to inverting.

Some composite power amplifier circuits.docx

updated closed loop.TSC

Thank you for your detailed analysis in the word document. I like the non-inverting solutions. And there is indeed crossover distortions and overshot, I do not know whether it has to do with the SPICE model of OPA549 or it does exist in the IC chip.

I remember that you once said that the first amplifier is in decomposed mode? should the overall gain (outer loop) be greater than 1?

Hi Michael,

but if you dedrease the load to 2R the overshot is still there, even when heavily decreasing the slew rate of input signal:

Kai

You are correct Kai, at 2ohm load the SSBW looks great still on the non-inverting but even a smaller step shows a major hitch in the getalong going negative 

I don't think that is a loop thing, that is an output stage negative going transition opening the loop at that deadzone, then trying to catch up - if real, probably need to think about a different power amplifier - that is now a product line question as we can't look inside their output stages too effectively. 

The questions

1. Is the modelled deadzone going negative in the part (might be in the datahseet?) 

2. Is there similar part that does not have this effect. 

Thank you, Michael.
I need bipolar output for driving the DC motor forward and reversely. I think a peek into the spice model or some comments from TI about crossover might be more appropriate.

In the past, we were using LM3886 for the power stage, and now considering the series of power amplifiers (OPA54x) as an alternative. Maybe, I should also try a precision amplifier (such as OPA211, OPA192) plus a current boost stage using discrete NPN, PNP solutions, though, this also includes mitigating the crossover distortions by pre-biasing the BJT.

Hi Byliu,

build it up now and check it with measurements! And don't forget that connecting a real load to the output like a motor with all its parasitic impedances can change everything...

Kai

Yes Byliu, it would be nice if TI apps would just run a simple OPA549 non-inverting gain of 2 into a 2ohm load with say +/-1V output into 2ohms. The sims of that show a clear crossover deadzone where the output then tries to catch up and slews with overshoot to the negative level. If that is physically there, I would not waste much more time on this device - and try to find a device without such a poor transition from sourcing to sinking current. In sim, the issue seems to be the load R not the Iout. +/1V into 2ohm is only +/-500mA. It might also be a lower negative slewing issue. If I slow the edge rate down and go to100ohm load, it is perfect on the negative going edge, same edge rate and 2ohm, and it is hideous.

OPA549 alone.TSC

Yes, a comment from TI officially would be much more appropriate. I also simulate OPA549, OPA548 alone, both exist this problem when Rload=2 Ohm.