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.

Suggestions For a Radar Pulse Amplifier

Other Parts Discussed in Thread: OPA847, LMH6629, OPA684, BUF602, OPA4820

In my application, I have a voltage signal that is like a radar pulse. 

It is at a 5MHz sine wave, lasts a few microseconds, and is (as far as I can tell) about 1uV in amplitude. I need to amplify it to 1.0 volt or so.  

I can not determine the source impedance but I think it is quite low. 

I have tried a few variations of amplifers and can get the signal high enough but the noise is killing me.  So I thought I would use a low noise first stage with a gain of 10 then maybe three more stages with voltage gains of V/V=20 (21.5 to be exact).  I thought that if each of the three stages had 2 pole BP filters on them I might get the noise low enough.  Any supply voltage other than 5.0 would be a problem I hope to avoid. 

Please comment on my plans.  Also suggest a circuit and components if possible.

Thanks In Advance,


  • Hello Peter,

    I looked at the previous post in the Spice model forum to get to speed faster.

    Since you are intending to use for a +5V supply, the simplest would be to start with a decompensated amplifier such as the LMH6629.  The OPA847 is another option, but you will need to generate a -5V supply as well.

    To achieve the best possible noise peformance while limiting the input drive requirement of you low impedance stage, I would recommend using the LMH6629 in a non-inverting gain configuration and have the gain as high as possible.  As John mentioned in the Spice Model forum, the feedback resistor cannot be selected to be too high.  For these high GBWP amplifier I would limit it to 1.5kohm.  The LMH6629 on page 10 shows the frequency response for each package with feeback resistor value varying between 240ohm to 1.5khm.  The peaking is most likely due to the feedback resistor parasitic capacitance interacting with the open-loop gain and the inverting input capacitance.


    Since you are looking at a 5MHz BW, achieving ~50MHz -3dB BW would be sufficient, so the maximum gain you can achieve is ~78V/V on the input stage only.  Let's target 50V/V for the first stage to avoid component value to be too small or too large.  In an non-inverting configuration of 50V/V, Rf = 500ohm, Rg = 10.2ohm.  With 50V/V gain, you will achieve 78MHz bandwidth.

    Since the first stage will dominate the noise contribution, any subsequent stage can be designed to be capable of providing high gain.  For high gain, high BW configuration, I would recommend using the OPA684.  Each amplifier can be configured at a gain of 100V/V and achieve 70MHz BW. 

    The 3 gain stage structure above will then have 500000V/V and 36.8MHz BW.

    Your example showed a gain of 100kV/V and your requirement shows 1MV/V, so I settled to 500kV/V.

    Now the hard part of the design will be to make sure that it is stable.  As each satge has high gain, there is a possibility of positive feedback through the power supply.  The best approach to minimize the risk is to power the last amplifier in the signal chain first and insert a inductor between the stage (n+1) and the previous stage (n).6644.High Gain Signal Chain.TSC

    I attached a possible solution in the TINA file above.  Note that I showed only the inductor in the positive supply, The negative supply voltage if not low enough impedance may require the same inductor.  Also, since the amplifier is used in non-inverting configuration, a mid-point reference buffer such as the BUF602 may be needed as well to avoid any pickup in the GND pin through the gain resistor.

    For filtering, since you have multiple stage, inserting an RC filter after each stage may be the most effective and least complicated way of implementing it.  If you want to implement filtering in the OPA684, consider the Sallen-Key as the op-amp is a current feedback amplifier.  Sallen-Key filter will allow you to have gain in the filter stage as well.





  • Xavier,

    Thank you.

    Note, I made a mistake.  My input signal is around 10.uv not 1.0uv.  So a gain of 100kV/V should be enough. 

    I tested your circuit and, if I interpret TINA correctly,  it achieves 114 db or more than the 500kV/V you shot for.  One thing I did to get TINA to run faster was change the 100uf capacitors, C1, C2, and C3 to 100nf.  Before that change there was no output for the first 1us of simulation because things were settling out.  I also gave VG1 a 2.5V offset to bias U2. 

    Question.  Why do you have AM2? What does that tell you?

    Now my problem is the noise.  I think TINA is showing me -1.4 db S/N in a 10MHz bandwidth. As you say, I need filters. 

    Over the last few days, I was doing some experiments using an OPA4820 (I have you Eval board with one of these on it) with TINA and I discovered I could get the S/N way down with High Pass filters.  I used Sallen Key, gain of 1, -3db at 4MHz and was getting a 68db S/N in 10Mhz.  Does that make sense at all?  I was always trying Bandpass or LPF to get rid of noise.


    Thanks Again,


  • Peter,

    AM2 was a leftover from another circuit.  It has no use at all.  I apologize for the confusion.

    I kept the 100uF and did not see the settling issue you had.  I attached my simulation with the result for reference.

    From a nosie perspective, the limit is going dictated by the input stage (LMH6629).  Considering that only the voltage noise contribute to the output (a valid simplification due to the high gain and small resistances used), the callculate output voltage noise density comes out to ~39nV/rtHz at 1MHz.  Simulating it it comes out to be 40nV/rtHz.  Moving onto the SNR simulation, this give ~15dB at 5MHz.

    4370.High Gain Signal Chain.TSC

    Note that I inserted RC filter after each stage to limit the ferquency response to ~10MHz.  I would also recommend loading each amplifier with 100ohm to GND in practice.

    68dB SNR for teh OPA4820 seems reasonnable at unity gain configuration, but in this case, the use of high-pass filter does not make sense to get rid of the noise as the broadband noise dominates.  Due to the low frequency range, low pass filter filter would be best.  Bandpass filter is another possibility but I do not expect the increase complexity of the filter to provide significant improvement over the low pass filter.


  • Xavier,

    That is a miracle to me.  The circuit looks perfectly (assuming a 10 to 15 db S/N is as good as it sounds to me).

    You don't know how many different circuits, opamps, filters, biasing circuits, etc. I tried over the last week or so.  Every attempt seemed to get better in some area and far worse in others. 

    I spent many hours last night with a MATLAB filter program making 2 pole Sallen Key filters that all were worst than what you just whipped up.  You didn't leave anything for me to do.  Probably a good idea ;-)

    The lesson I learned....rely on the professional.

    Great job, thanks again,


  • Xavier,

    I saw your article in "Analog Wire",  "High-gain, high-bandwidth… how can I get it all?". 


    I have this circuit running on the bench right now.

    I didn't want to make a public comment with that article.

    Right now, the noise out is too high for me.  I don't know if I am exceeding the TINA prediction, meeting it, or am below it.

    I am measuring +/- 1.25 volts (2.5 P-P) about the 2.5 volt level.  I measure this by AC coupling the output of the last stage into my scope.  Then I DC, positive trigger the scope and slowly raise the trigger level while watching the scope trace on the 50ns per division setting.  As the trigger level gets higher the scope triggers less and less and then finally doesn't trigger.  I barely lower the trigger level then and note the peak voltage where it barely triggers.  +1.25 volts. 

    I then repeat with the trigger level set to negative trigger.  It barley triggers at -1.25 (AC Coupled).

    I do this with no input and the input connected to ground through a 100nf cap.


  • Peter,

    Thank you.

    I have an EVM for this circuit that should arrive within the next few days, so I will be able to verify this on the bench.

    You may have an oscillation in the circuit.  Have you looked at the performanc eof the first stage by itself?

    The input of the LMH6629 cannot be connected to ground as the bias current will charge the cap.  I would expect a resistor in parallel with the 100nF cap, say 100ohm.

    Best regarsd,


  • Pete,

    The circuit works.  We achieve ~100dB of gain.  See attached results.

    In order to evaluate it on the bench, we had to place a bandpass filter at the frequency of interest on the output of the arbitrary waveform generator, followed by two 40dB attenuator to get the signal low enough.

    To isolate the sinewave, we averaged it 512x.  See results for 1MHz and 5MHz.  Another 1MHz result shows the noise in the signal.


    I also included the layout we used for the evaluation.  Let me know if you want me to ship you the board used.

    8562.High Gain Layout.pdf.

    Best regards,


  • Xavier,

    I think I am getting similar results. 

    Would it be possible for you to collect samples of the output with no input signal?  I am measuring about +/- 1.25 volts or about 2.5 volts P-P with no input.  To me that is all noise.  Oh, there are no oscillations.  The signal is just random noise.  The image below was collected by triggering on the noise and raising the scope trigger level until it just barely triggers.  It is then triggering on the highest peaks, ~1.25 volts.  So we see just noise unless the noise pulse is higher than 1.5 volts or so.   Note there is no repeating of this signal like it would if there was oscillations.  Pete


  • I forgot to mention two tiny items.  On your spreadsheet, I believe the horizontal axis for the top and bottom graph should be us not +Vin(mV).  Like I said, tiny and minor.


  • Pete,

    Yes I believe that this is noise.  I eliminated the 3rd gain stage (set it to 1V/V) and now only have the first gain stage and second gain stage set at 100V/V for the LMH6629 and 50V/V for the OPA684 for a total of 5000V/V.  The signal below does not exceed ±50mV.

    7750.No Input signal (100V-V LMH6629 + 50V-V OPA684.xlsx

    I will now be looking into noise amplified added by the last stage.



  • Xavier,

    I guess the question comes down to, "Is the measured noise similar to what TINA predicts or is something else happening?".

    I added some things to your excel sheet:

    I multiplied the readings by 40 to get back the gain of the last stage,

    Counted how many samples exceeded +/- 1 volt.  This is an arbitary value but larger than I can accomidate.

    2,356 samples out of 10,000 were > 1 volt or 24% of the time.

    Does that agree with TINA S/N?

    3821.NoInput 200000V-V.xls


  • Pete,

    Looking at the Total noise (RMS output noise) in TINA, I get 15.9mVrms at the output or 2.899uVrms input referred (5482.77V/V).

    Evaluating the same output RMS noise with the socilloscope I get 16.1mVrms at the output or 2.876uVrms (5597.36V/V implementation).

    So there is a strong correleation between noise between TINA and the implementation.

    Best regards,  Note that this was measured for 0ohm source.


  • Xavier

    I'm missing where the 5483 V/V  or 5597 V/V comes from. 

    This is the circuit 4370.HighGainSignalChain[1] right?


    48.9 V/V * 49 V.V * 39 V/V =93676>>>>99db



  • Pete,

    To avoid clipping on the output and eliminate complexity in the measurement, I set the last stage at unity gain.  The first stage was set at a gain of ~100V/V and the second stage at ~50V/V.

    The actual gain simulated was 5483V/V and the gain of the board was 5597V/V.


  • Xavier,
    I get it now.  I made a mistake in the spreadsheet four messages above.  I simulated a gain of 200000 V/V.  I corrected that by multiplying each of your 10000 readings by 100000/5597 to get back to the 100 db range.
    Then I counted how many were above 1 volt (in absolute value) and got 90/10000 or ~1%
    Also, the maximum value you sampled (multiplied by 100000/5597) was 1.39 V.
    My circuit is showing similar results.  Highest peak ~1.25 V.
    So, if my circuit noise matches with TINA, I'm hurting.  This many false alarms is a problem.  Remember, I'm not amplifying a continuous sine wave.  I'm looking for a blast of a few cycles of a 5 MHz sine wave.  Nothing in between.
    I am considering some type of very high speed comparator at the output to eliminate anything below 2 volts.  That would be speaking as AC coupled signals.  It would be "below 4.5 volts" if DC coupled.  Pretty close to the upper rail.
    I attached my spreadsheet of your readings multiplied up.
  • Pete,

    The high speed comparator would certainly help reducing noise susceptibility.  Another method to improve nosie would be to use a transformer at the input, so you can add some noiseless gain.  I was think of using a 1:4 turn ratio (1:16 ohm ratio) as soon as I can get one in.  I was looking at the ADT16-6T from Minicircuit.