I have been working for quite a few days now on a simple project using the OPA549. I have already posted some issues regarding distortion in the post "OPA549 heat generation problem?" which I now consider to be resolved. I have now experienced a new problem related to the OPA549 when loaded, and was actually surprised to find no information about it on this forum nor on the web (as far as my search went). To illustrate the problem, I built a simple follower circuit as shown below :
I simulated this circuit with TINA-TI, which posses the model of the OPA549. I also built this circuit in practice and recorded the following waveforms :
Adding a 4.7 Ohms load gives the following result :
There thus seems to be a problem at the zero crossing. Things get even worse at 50 kHz :
Now, back to 20 kHz and adding an offset to the input signal, I measured :
Thus, it seems that the problem is related to the current at zero crossing on the negative slope. At first I suspected my circuit to have some defect or undesirable effect somewhere, but after testing out four independant Op-Amps from different wires and power supplies, I came to the conclusion that the problem might not be related to my design. I first noted the problem when the load was a simple snubber circuit (10 Ohms in series with 10 nF). The glitches (small but present) appeared just past the peak of Vout, exactly when the output current crossed zero.
Only a few days later did I simulate this circuit on TINA-TI and discover that the problem was related to the OPA549 themselves, and was in fact normal, but yet unwanted. The following graphs were generated from TINA-TI and the same circuit (see the first figure) :
These are literally identical to my measurements. I tried to design a compensative RC circuit to minimize this effect, as for capacitive loads, but couldn't succeed to a satisfactorily degree. There seems to be no indication about this effect on the OPA549 datasheet. As any of you ever encountered a similar problem before? Is there a way to obtain a clean sinusoïdal output at 20 kHz (and below) and full current with this Op-Amp?
Thank's for your help
Just to make sure it's the output stage, can you change the load and see what the behavior is? Is it different now?
Thank's for your interest into this problem. There has been no reply (besides yours) since my original post so I did much of the investigation by myself. Changing the load changes the output behaviour. As I showed for example, at no load the output is very clean and undistorted at up to 50 kHz (for Vpp <= 5 V). Glitches start to appear at approximately 5 kHz as the load current (zero-mean sinusoïdal waveform, resistive load ) increases. On my recorded waveforms (and also on that of the simulations), you can see that severe glitches are present when the output current just reaches a little bit more than 1 Amp peak, which is still far from the 10 Amp peak capability of the chip. For capacitive loads, glitches tend to appear in the same way at the top of the waveform after zero crossing of the current. Small capacities cause output instability and need to be compensated adequately, which is a known concern.
Since the past days, I tried to design several compensation circuits to try to alleviate this glitch phenomenon when the Op-Amp is loaded. I came up with some interesting solution that gave good results on TINA-TI, but which I still need to test in practice. If it works, I will post the schematic here in hope that it helps anyone designing with the OPA549. Meanwhile I simulated my circuits with a different Op-Amp, the OPA541, and found that it behaves much better than the OPA549. I ordered some of these chips to see what they really give in practice. I will update this thread as soon as I get concluant results.
I attached a presentation from a Power Amplifier Seminar regarding crossover distortion. I hope this will help answer your question.
Christopher Hall | Δ-Σ Data Converter ApplicationsTI.com | Selection Guide | Technical Documents | Tools & Software | Design Notes | E2E Site Map
Thank-you for this presentation. It was very insightful and I now have a clear understanding of the problem. In this seminar, a definitive solution was proposed to eliminate crossover distortion : the use of a pull-down resistor. I have past the last hours trying to apply this technique to my OPA549 circuit, but it does not seem to work. The seminar presents a simple approach to compute the pull-down resistor value (Rpd), but it does not justify the value of the pull-down current based on the circuit or the Op-Amp at use. I took it to be 200 mA as it was a close value to the 190 mA used in the presentation. The circuit and my calculations for Rpd are as follow :
(15 + 5) / Rpdmax = 200m => Rpdmax = 100 Ohms
(15 - 5) / Rpdmin = 200m => Rpdmin = 50 Ohms
Here are the waveforms I obtained for Rpd values in this range and outside :
It seems that a pull-down resistor cannot solve the problem. I may be wrong however in my calculation of Rpd. It could be that I_pd has to be in the same range as I_Load, as it seems to be the case in the presentation (I_Load = 140 mA, I_pd = 190 mA). Applying this reasoning for the above circuit and a high output current leads to a Rpd of about 5 Ohms and less, which cannot be practical. In this vein, the simulation produces a clean output for Rpd = 3 and R_Load = 2. The seminar was clear and very well made, but the provided solutions do not seem to work for the OPA549.
I did a simulation in Tina-TI and was not able to replicate your results; I didn't see any distortion. Do you mind attaching your simulation file that you used in your previous post where you weren't able to remove the crossover distortion with a pull-down resistor?
I attached my simulation where I didn't see any distortion.
I tried to join my simulation file in my last post but couldn't find how to do it from the reply form menu. Even now, when I click the "Insert Media" button, browse for my simulation file and click the "Insert" button, the window remains idle and an eventual timeout occurs. Is there another way to join a file that is not a picture?
Anyway, I made some tests with your simulation file and could reproduce the clean output as you mentionned. However, I found it strange that the output was not lagging the input, as observed in my simulation and also in practice. So I raised the frequency to 50 kHz and saw if the lag increased. There was still none. I then set the frequency to 100 kHz and realized to my amazement there was still no lag, as the load remained at 600 mOhms. I then set the input voltage amplitude to 20 V instead of 5 V, and for the same frequency (100 kHz), the output remained perfectly clean with no distortion and again a zero lag on the input (the slew rate 12.6 V/μs, which should have cause great visible distortion). This cannot be the OPA549. If this chip really exists, I would buy many of them for sure!
I then completely removed Rpd to see if there was some glitches as I observed in my simulation and also in practice. There was none for all the tests I performed. The conclusion is simply that the Op-Amp of your circuit cannot be the OPA549. Strange because it is labeled as so. I would gladly share my simulation file with you if I knew how to attach it here, or you can always give me your email so that I can send it to you directly.
Thank's for the simulation by the way, you took all of the parameters I had in my circuit.
Great, I just found how to join a file. We have to click the "Options" tab at the top of the page. Here is my simulation file.
For the past days I have been trying to obtain clean waveforms using various Op-Amps. Even though TINA-TI simulations of the OPA549 showed that crossover distortion would still occur with a pull-down resistor, I gave it a real try. The circuit I used for both simulation and practice was as follow :
And the real waveforms I recorded were :
Thus, we can see that the practical and simulated waveforms are pretty much identical, with the distortion pattern slightly down compared to what it was without pull-down (see previous posts). I haven't tested other pull-down resistor values, as the ones I had could not sustain the required power, but based on TINA-TI simulations, I have found no acceptable resistor value that could either eliminate or alleviate this distortion. My choice was then to change Op-Amp. Having learned from my mistakes, I decided to first simulate the new model on TINA-TI before purchasing it. In this end, I found that the OPA541 was especially good under a wide frequency range. I purchased four of these chip and built the following circuit :
However, the real recorded waveforms were different :
The frequency content of the distortions is much lower than that of the OPA549, but they are still significant. This was a very bad surprise since the TINA-TI simulation gave no distortion in the same operating conditions. The OPA541 model of the simulator is thus mainly false, unlike the one of the OPA549 which predicted almost identical distortion patterns. The OPA541 model does not even have all the pins of the package as do the OPA549. I repeated the last experiment many times to ensure that there was no problem in my circuit, and all of the measurements were made with initially cold chips such that the operation curves were well within the SOA.
At this point and as far as my experiments went, I can now conclude that :
- The OPA549 and OPA541 are not well suited for high fidelity power amplification designs, and that even for frequencies well inside the audio band.
- The TINA-TI model of the OPA541 is inadequate, unlike for the OPA549.
I will now give a try to the LM3886 and LM3875 chips and see if they give acceptable distortion patterns.
Keep that in mind that neither OPA549 nor OPA541 and LM3886 and LM3875 power OpAmps are suitable for unity gain operation. That is your mistake.
The OPA549 and OPA541 are suitable for unity gain operation. See figure 14 on page 14 of the OPA549 datasheet, and figure 3 on page 7 of the OPA541 datasheet. In both cases a buffered Op-Amp (unity gain) is used as a slave. My practical circuit is almost identical to figure 14 of the OPA549 datasheet. I limit its operation to frequencies lower than 5 kHz, otherwise significant crossover distortion appears. You are right about the LM3886 and LM3875 however, and I knew about this concern. At unity gain, the LM3886's output oscillates at high frequencies. This behaviour is of different nature than the crossover distortion observed for the OPA549 and OPA541.
I've been using the opa549 as an audio amp for the last couple of years with Av=-2 (see schematics ) and my CRO doesn't show artefacts you mention, sinusoidal forms are nice and clean. I didn't try it in unity gain configuration.
This is interesting. My circuit is similar to yours, where I use a 20k potentiometer instead of your 10k, and a 5.1k resistor instead of your 4.7k. I use two Op-Amps and my pins 4,6 and 8 are also tied to ground. The major difference however is that I don't use a bridge configuration as you do. I use a parallel circuit similar to that of figure 14 of the datasheet. Interestingly, this circuit, when simulated on TINA-TI, doesn't exihbits crossover distortion as only one Op-Amp does when simulated independently. In practice, I also observe less crossover distortion in my parallel circuit (compared to one Op-Amp alone), but not as less as the TINA-TI simulation result shows. In your bridge circuit, the Op-Amps are driven differently and it could be that this helps alleviate crossover distortion. I didn't simulate this configuration but I believe that it coud actually work. As a workaround for a single Op-Amp circuit, I have found that adding a very small inductor (< 50 uH) in series with the output and taking the feedback right after it eliminates much of the distortion. This can also be verified in a simulation. However, I couldn't find a way to implement this effectively in a parallel design. Thank's for circuit schematic by the way.
if you look again at my sch. in previous post you'll notice that it's not a simple bridge configuration (note the nested loops). It's based on SuSy idea (google: Supersymmetry Nelson Pass). You can find more details by looking for: 1994—US Patent 5376899: Amplifier with gain stages coupled for differential error correction.
Yes you are right, this is not a simple bridge connexion. I had never seen such a circuit configuration before and after some research, I found that the bridge topology matched it best, so I called it likewise. It is very similar though, but you have some additionnal feedback that goes from the two Op-Amp outputs to the signal Op-Amp. I believe it could work very well, but I haven't taken the time to perform an in depth analysis of it. I could also have used a similar topology for my circuit, instead of the parallel configuration, which would have allowed me to lower Vs and operate more at the left of the SOA curve.
All content and materials on this site are provided "as is". TI and its respective suppliers and providers of content make no representations about the suitability of these materials for any purpose and disclaim all warranties and conditions with regard to these materials, including but not limited to all implied warranties and conditions of merchantability, fitness for a particular purpose, title and non-infringement of any third party intellectual property right. TI and its respective suppliers and providers of content make no representations about the suitability of these materials for any purpose and disclaim all warranties and conditions with respect to these materials. No license, either express or implied, by estoppel or otherwise, is granted by TI. Use of the information on this site may require a license from a third party, or a license from TI.
TI is a global semiconductor design and manufacturing company. Innovate with 100,000+ analog ICs andembedded processors, along with software, tools and the industry’s largest sales/support staff.