This thread has been locked.

If you have a related question, please click the "Ask a related question" button in the top right corner. The newly created question will be automatically linked to this question.

OPA2832: Gain stage to drive 8.9Vpp into 50 ohm from LMH6517 VGA

Part Number: OPA2832
Other Parts Discussed in Thread: LMH6517, THS4541, THS3217, THS3215, OPA691, OPA2677, OPA2695

 Hello,

I need to drive a 50 ohm load up to 8.9Vpp (23dBm) 5 MHz to 30 MHz from the output of a LMH6517 programmable gain amplifier. The LMH6517 can produce max 5.9Vpp differential. I have power rails of 5V and 3.3V. I used an OPA2832 in a bridge for gain. My approach is distorted when I crank up the Vpp output. Can someone suggest a chip that I can put after the LMH6517 or a correction to my approach?

 

On both differential outputs of the LMH6517, I put OPA2832 op amp as non-inverting amplifier of gain of 2 with GND and 5V on the supply rails. The OPA28322 is spec 75MHz BW for gain of 2. The datasheet says it can do 4.9Vpp for 5V supply and further it talks about an output range of 0.3V to 4.6V with 150 ohm load. It is not talking about a 50 ohm load anywhere so my part selection is possibly wrong because I need to drive 50 ohm. 

 I tied both op amp outputs to a mini circuits ADTT1-1+ transformer. The sine wave is not round at high frequency and high amplitude. For example, at 10MHz 3Vpp output, it is no longer fine at the output pin 1 of the op amp. Below 3Vpp, it is a nice sine. I took a photo of an analog scope. The bottom curve is the op amp output at 1V/div. The top curve is the mini-circuit transformer output after an 50 ohm attenuator. What part can I use to drive closer to the rails?

Thanks,

Frank

 

  • Maybe a THS4541 could do this on 5V supply. Diff I/O - I think you do need buildout resistors into the balun. 

    The other part, but not 5V only is the THS3215 and THS3217 

  • Hi Frank,

    I don't know your transformer. But when loading the output with 50R wouldn't this mean that each of the OPA8232 would see an effective output load of 25R? As the OPA8232 is specified for a 150R load, wouldn't 25R look like a short-circuit?

    Why not using a much higher supply voltage or even better a bipolar supply voltage? Then you could design a circuit which is able to drive a 100R load. This would allow you to use the circuit in a true 50R system (50R source impedance, 50R cable and 50R load impedance).

    Kai

  • Hello Frank,

       For a 9Vpp 30MHz sin wave signal output, you are going to need an amplifier that can support a slew rate of at least 1700V/us. Michael suggestions would work, and Kai brings up a good point on the load and voltage supplies. But if you can not move to dual supply +/-5V, here are some more suggestions with +5V or below supply with high slew rate: link.

    Thank you,

    Sima

  • First of all Frank, I stand corrected you can drive into the balun with zero source R, here is that sim for just the ADT1-1WT, 

    And then here is this file V9

    ADT1 model.TSC

    At one time I was spending a lot of time with that (and other) baluns for FDA characterization and ADC interface work, here is one of several articles, 

    https://www.eenewsanalog.com/content/extending-useable-frequency-span-11-wideband-transformers-used-distortion-measurements

    The THS4541 would be right on the edge if 30MHz 9Vpp into a 50ohm differential load is required, 

    4.5Vp*30MHz*6.28 = 850V/usec and the part has about 1500V/usec

    4.5V/50ohm = 90mA (that would be +/-90mA in each polarity)

    On 5V supply, probably not enough headroom under load for a 4.5V diiff output. The no load headroom is right at 0.25V max so can just barely make 4.5V diff out. With load current that will increase the headroom so you would perhaps have to provide something like 5.4V supply tightly toleranced to have a chance 

    There are not many RR output stages that can deliver 90mA with <0.25V headroom on each side as a single 5V supply would require. Higher supply would make this a lot easier. 

  • And then putting in the THS4541 to drive the transformer - I did a lot of the original modeling work on this at release, so I am using the RTM model - there might be an update you want to check as well, 

    And then trying to set up a 30MHz 8.9Vpp at the load, if I start with a 4.5Vpp target, looks ok, 

    Doubling that, it falls apart, and I had a lot of convergence issues - not sure what is going on, had to raise the supplies to get it to run at all, 

    And this file, 

    THS4541 gain of 2 to transformer 50ohm load.TSC

  • Hello Michael,

    I got an error when I try to to open the TSC file. It just says error: Unable to open . I downloaded the TSM from https://www.ti.com/product/THS4541?keyMatch=THS4541&tisearch=search-everything&usecase=GPN and recopied your circuit. I had the same convergence complaints you got.

    THS4541 redone from ground up.TSC

    The simulation seems to clip at 6Vpp when using the max rated supply voltage of 5.4V. It is clipping at the output at 1.2V from the rails. I need 8.9Vpp.

    >There are not many RR output stages that can deliver 90mA with <0.25V headroom on each side as a single 5V supply would require. >Higher supply would make this a lot easier. 

    On the board I input 12V DC and generate various positive voltages between 5V and 1.8V. I could just add another LDO regulator to get say a 10V rail. I would prefer not to add and debug a negative power supply.

    We used over here an OPA691 for a different application. I don't have much experience with current feedback amplifiers. It doesn't seem to want to go to 8.9Vpp either.I didn't think about AC coupling capacitors at the input of the 2x gain amplifier.

    II tried also inverting with DC blocking capacitors.The bias voltage does not have the effect I was hoping for. Both op amps outputs are not centered at the half power supply.

    Ideas, suggestions?

    Frank

  • So your topology looks good, we did all those parts back in the early 2000 time frame, if you switch to the OPA2677 dual, it will do this easily on a single 7.5V supply. Those DSL drivers were not RR out, but can crank a lot of output current with minimal headroom loss. 

  • my simulation had a typo. One the voltage supply at the bottom left, It is written incorrectly Vbias' instead of Vbias.

  • So we get this:

    frank_opa691.TSC

    Kai

  • yea I fixed that, your input swing, and set the gain to 2 for a OPA2677 on single 8V supply with 4V midscale, with 500ohm load, looks about right on output Vpp, but when I drop that to 50ohms I lose Vpp - kind of perplexing for the high output device where I am giving it 2V headroom on each side. 

    Here is 50ohm and the file, I am at 30Mhz here , I suppose the closed loop zo of each side is causing the reduced swing, Another form of rolloff to the load, getting about 8.5Vpp now, 

    And the V9 file, 

    OPA2677 AC coupled inverting.TSC

  • Here I modified this to do a SSBW test and indeed the 50ohm load rolls off much faster than 500ohm, that is the closed loop output impedance coming up with frequency on the op amps - true of any part, even these fairly fast ones, at 30Mhz, this is where I am losing that swing when I was expecting 9Vpp. I am working from memory (always hazardous) that 30MHz was your max? 

    And this modified file

    OPA2677 AC coupled inverting SSBW sim.TSC

  • Incidentally, this file is using the 2002 transistor level OPA2677 model by Rea Schmid. At that time, I was managing the marketing/apps part of the group and Rea and I both preferred using a simplified transistor level model - these do a very good job of I/O impedances and most other things. There is likely a later macromodel that hopefully emulated the open loop output impedance for the device. All of these circa 2000 high speed parts used an internally closed loop output stage which helps a lot for keeping the over frequency closed loop Zout low. 

  • So I got to wondering what part might do better on flatness through 30MHz. That would be the OPA2695, the fastest CFA we did back then with apparently enough output current for this requirement. This circuit hits 6dB gain at the load flat across 5Mhz to 30Mhz adjusting for two midband gain errors, 

    1. The DC open loop gain  for this >1GHz part is relatively low, that gives a 1/(1+LG) error that can be compensated with higher nominal gain in the stage. 

    2. The measured ADT1-1WT shows a midband insertion loss of 0.4dB. I had at one time tried to include that in the model, but it messed other things up. That also can be tuned out increasing the nominal gain. That does mean more swing the actually desired at the load needs to appear at the device output pins. 

    Here is the SSBW with a 50ohm load, look pretty good across 5Mhz to 30MHz. The OPA2695 will have more headroom loss under load so I went to 10V supply with 5V midbias. And of course this has plenty of slew rate margin, 

    V9 file, 
    OPA2695 AC coupled inverting 2009 model.TSC

  • And making those changes on the 30MHz sine wave sim, pretty clean looking sine waves close to the right Vpp, 

    And file, 

    5684.OPA2695 AC coupled inverting 2009 model.TSC

  • The flatness of 5MHZ to 30MHz does not need to be corrected in the analog domain.  The GUI has fields for the desired frequency and output power. I already have a corrections table in the CPU that produces and adjustment according to frequency. The main criteria is just to make the output to have the strong fundamental much better than the harmonics.

    We have the LMH6517 two outputs splitting out into three paths. One channel of the LMH6517 goes to 2 SMA outputs. The low power one looks nice on the spectrum analyser. Only the higher power one was very bad looking.

  • Hello Michael,

    So, we are getting close to resolved.

    At the output of the op amps, there is a little distortion at half of the supply voltage.We use this circuit for phase detection in a laser system so it could count. After the transformer, the distortion does reduce in significance.

    Could it be  cross over distortion by the rail-to-rail output stage where the top transistor stops sourcing and the bottom transistor starts sinking? What would your best recommendation be?

    This is what I tried: I biased the non-inverting op amp input higher on the inverting op amp circuit. I loose headroom from the top. I trade off headroom for avoiding the problem area. I like to understand if this work around is for the right root cause.

    OPA2695 AC coupled inverting 2009 model, output distortion at 5V bias.TSC

    I don't think the inverting topology with the chosen resistors in current feedback op amp is the cause. I don't design much in current feedback op amp.  I don't have much trouble shooting experience with the inverting input low impedance input. I just tried a few simulations in buffer op amp circuit topology.  Only taking the DC blocking capacitor thus forcing the top transistor to source current makes any difference.

    OPA2695 buffer circuit, dc block cap, output distortion.TSC

    OPA2695 buffer circuit, no dc block cap, no output distortion.TSC

    Thanks so much for your simulations!

    Frank

  • I think you are pointed to that little wiggle on the rising edge of each half waveform. The OPA2695 is not a RR output device, but a class AB output (called a diamond buffer sometimes). Not sure what is causing that, normally I would be trying to add some class A current into or out of the stages to see if that helps, but you don't have much room for more output current. 

    Not sure about the other examples you show, the inverting mode is the highest slew rate and your gain of 1 examples probably exceed what theLMH6517 can deliver. 

  • >Not sure about the other examples you show, the inverting mode is the highest slew rate and your gain of 1 examples probably exceed what theLMH6517 can deliver. 

    I was testing different conditions around the OPA2695 to see when the distortion disappears.

  • Since there is something visible in the time waveform, the fourier series will produce a result, here I am still set up to compensate for the insertion loss, few tricks inside of here, but about 4.5% THD or -27dBc. This is a pretty tough requirement if less than -40dBc THD is desired. I am not sure what is causing that little hitch in the getalong, but its simulating so off to fourier. 

    Let's assume I can add some class A current for the moment,Pulling some out to ground helped a little, 

    Let's back off on the gain as you have go down to 20Mhz, yea this is better at 2.6% or -32dB. 

  • Thanks for your help! We can close the thread.

  • You bet, good luck