• State Resolved
  • Locked Locked
  • Replies 8 replies
  • Subscribers 49 subscribers
  • Views 598 views
  • Users 0 members are here
Support feedback
Options
Options
Similar topics

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.

Original question:

THS4541: OPA657 + THS4541 circuit review and OPAmp for negative rail

OPA657: OPA657 as TIA output noise/osillates

Follin Ju
Prodigy 195 points
Part Number: OPA657
Other Parts Discussed in Thread: OPA818

Hello!

I'm testing the design mentioned in 

And the final circuit diagram:

And I fnd the output of the OP657 has a noisy output. The maximum value will be around 40mVp-p. (I used a axial cable with 100Ω isolate resistor, and the waveform is same as the result of ADC output ,so it's credible)

I've confirmed all the power supply, the ripple/noise are all below 3-5mV.

And then I removed the feedback capacitor but it still kept the same.

Then I changed the gain resistor to 1k and 100k, then the result:

1k - 0.5mVpp pretty well;

100k - 1.47mVpp 

400k -  9.6mVpp 

It seems there's some current noise on the input side of OPA657 and amplified.

And I doubt with the environment so I also have another channel of Scope using same axial cable connected to nothing but near the PCBA (NC in the below waveform).

So I guess the spikes are from the environment.

But drop the spikes, there seems to be a  sine waveform on the output of TIA.

I did the phase margin simulation and also tried different feedback capacitor, but they didn't work.

And there's trace without sold mask to install the steel shielding case, but I'm still waiting for the delivery.

Before I get the sheilding parts, what else can I try?

Thanks!

Layout:

  • 0 in reply to kai klaas69
    Prodigy 195 points

    Hi Kai,

    I've looked through the thread you mentioned.

    And I noticed there're several points I didn't follow:

    1. It seems I removed too many GND copper on out layers and inner layers. 

    2. Need to add more GND vias of the coupling capacitors.

    3. The length of the trace from APD connector to OPAmp is little long. This is because the shielding trace between the four sets of same circuits. Which benefits more? Is the isolation usually necessary? I'd very like to remove the "isolation" shielding trace to short all the APD trace if it benefits more ( better for stability, anti-interference) .

    4. On the datasheet the Rf and Cf are placed under the TIA but in your scheme just place it near it.

    Would you mind helping check again and see if I missed something?

    I post the detailed schematics and layout here.

    TOP01

    INNER02(GND)

    INNER03

    INNER04 (PWR)

    INNER05 (GND)

    BOTTOM06

    Total:

    Thank you so much.

  • 0 in reply to Follin Ju
    Guru 140200 points

    Hi Follin,

    there's another really big issue:

    You urgently need to have a decoupling cap closest to pin 1 of APD connector. It's not only the connection from pin 3 to the -input of OPAmp which is way too long, but also the connection from pin1 to signal ground (through the decoupling cap).

    By the way: Connectors means that the photodetectors are not directly mounted to the PCB? Do they see any cabling?? I hope not? I really don't think that the OPA657 is accepting any cabling at its -input.

    Follin, the OPA657 is a decompensated 1.6GHz OPAmp. You cannot treat this "beast" like a standard low frequency OPAmp. It does not forgive even the least mistake. Only connection lengths in the millimeter and sub-millimeter range are adequate. Any longer cabling at the -input of OPA657 may result in a catastrophic failure.

    Kai 

  • 0 in reply to kai klaas69
    Prodigy 195 points

    Hi Kai,

    THe APD is directly inserted into the socket, but the lenth of the APD pin will be around 8mm.

    I modified the layout to make it more like what you did. And will repeat the copper remmoving from 2-4 layer but keep the 5th layer and bottom layer GND.

    Also moved the coulping capacitor to the 1 pin of APD. 

       

    In the first version I have no GND copper but only the bared trace for sheilding to avoid parasitic capacitor/leakage current as possbile - it seems that doesn't make sense. But I've seen a lot of same design on the boards of high precision instruments.

    And I have another verion of OPA818 refered to the datasheet but also moved the chip very close to APD pins.

    May I have your review to ensure I understand your guide correctly?

    Many thanks!

  • 0 in reply to Follin Ju
    Guru 140200 points

    Hi Follin,

    the last picture looks good. The decoupling cap is mounted properly. But isn't the feedback resistor a bit large? What is its package? 1206? It think 0603 would better do. Maximally 0805.

    Follin Ju said:
    THe APD is directly inserted into the socket, but the lenth of the APD pin will be around 8mm.

    This sounds good.

    Follin Ju said:
    3. The length of the trace from APD connector to OPAmp is little long. This is because the shielding trace between the four sets of same circuits. Which benefits more? Is the isolation usually necessary? I'd very like to remove the "isolation" shielding trace to short all the APD trace if it benefits more ( better for stability, anti-interference) .

    It's very difficult (read impossible) to provide real isolation in a HF circuit by using shielding traces or small local ground planes. You introduce so much stray capacitance and parasitic inductances that you may do more harm than good.

    The best shielding is provided by using a (or better several) solid and continuous ground plane(s). Isolated shielding traces or small local isolated ground planes will not do the trick.

    Follin Ju said:
    And there's trace without sold mask to install the steel shielding case, but I'm still waiting for the delivery.

    Adding steel shielding cases is a good idea and can furtherly improve the shielding or better say the channel separation between the different channels.

    If you really want to enhance the channel separation between the different channels, then don't forget to improve the supply voltage decoupling measures. I would replace the RC-filters at each supply voltage pin by CRC- or even CLRC-pi-filters. Pi-filters even allow you to omit the supply voltage planes in very most cases.

    There's one more issue: I think that some of your components are too large. I mean the feedback resistors and half of the decoupling caps. What sort of decoupling caps do you use?

    Kai

  • 0 in reply to kai klaas69
    Prodigy 195 points

    Hi Kai,

    kai klaas69 said:
    There's one more issue: I think that some of your components are too large. I mean the feedback resistors and half of the decoupling caps

    - I used Susumu RG2012P-155-B-T5 , it's 0805 footprint. I read somewhere that using 0805 which has smaller terminal parasitic capacitor compared with 0402/0603 to avoid bandwitdh degration. Is it too large? It affect a bit the layout as the distance increased.

    - The capacitor I use for OPA657 power supply is  the combination of 0402 220nF and 0805 10uF based on following part of datasheet:

     

    0402 220nF X7R  GRM155R71C224KA12D 

    0805 10uF X5R   GJ821BR61E106KE11L

    And I've also read the thread you posted and it's better to use two identical capacitors and usually it needs actual test. The decoupling things always make me conffused a bit.

     

    kai klaas69 said:
    It's very difficult (read impossible) to provide real isolation in a HF circuit by using shielding traces or small local ground planes.

    The traces are copper without soldmask to contact  two pieces of shielding cases. These GND coppers are same at the top and bottom sides and connected by many vias.

     

    I marked the layout of OPA657/656 version, hope that it will be easier for your review. (Except the large components you mentioned, I will modified it later if necessary). 

    And one important question is that：shall I pour the GND on the TOP layer, and expose the copper trace for contact the shileding parts; 

    Or just add more  GND vias connect to decoupling capacitor with small GND copper area, but make the copper trace seems more "independent". Which is mo resonable?

    Thanks again!

  • +1 in reply to Follin Ju
    Guru 140200 points

    Hi Follin,

    Follin Ju said:
    - I used Susumu RG2012P-155-B-T5 , it's 0805 footprint. I read somewhere that using 0805 which has smaller terminal parasitic capacitor compared with 0402/0603 to avoid bandwitdh degration. Is it too large? It affect a bit the layout as the distance increased.

    Ok, a 0805 package should be acceptable for the feedback resistor.

    You may want to search for specialized HF-SMD-resistors which specify the HF performance and from which you can estimate the terminal-to-terminal parasitic capacitance. But it looks like you already have chosen the feedback resistor and feedback capacitor in a way that they do properly fit together? Then I would not change anything.

    Follin Ju said:
    - The capacitor I use for OPA657 power supply is  the combination of 0402 220nF and 0805 10uF based on following part of datasheet:

    The datasheet is from 2001 and the schematics of datasheet show a polarized cap, very probably a tantal cap. In this case a paralleling with a small ceramic cap would be a good idea, not only because the tantal may be "huge" and impossible to handle HF but also because the tantal shows sufficient ESR to avoid this nasty "antiresonance". A tantal would also allow to be placed a bit farer away from the smaller ceramic cap because its ESR would also allow a bit parasitic inductance between the two caps.

    But if you mount two uneven ceramic caps in parallel with very low ESR you should be cautious. "Antiresonance" is very likely to occur then and should be avoided by all means. I would take only one ceramic high cap, either in 0805 package or better in 0603 package. Parelleling of two 0805 packages would waste lots of board space and may do more harm than good. But two identical 0603 caps could be paralleled.

    I have seen whole boards failing only because of pronounced "antiresonance". Antiresonance is treacherous because the impedance of parallel circuit at the antiresonance becomes very high, as if no decoupling capacitance was mounted at the antiresonance frequency at all. And if the OPAmp has a weak point at the antiresonance frequency, instability and oscillation is very likely to occur.

    A pi-filter can very easily be built by mounting an identical cap directly in front of the 15R series filter resistor (R57). I usually mount this ferrite bead in series to the filter resistor:

    FBMH1608HM601

    Then you can even decrease the series resistor a bit. The series resistor is usually still necessary to avoid the LC resonance.

    Follin Ju said:
    The traces are copper without soldmask to contact  two pieces of shielding cases. These GND coppers are same at the top and bottom sides and connected by many vias.

    Provided they connect to the common solid and continuous ground plane then it is fine.

    Follin Ju said:
    And one important question is that：shall I pour the GND on the TOP layer, and expose the copper trace for contact the shileding parts; 

    Again, provided they connect to the common solid and continuous ground plane then it is fine.

    Follin Ju said:
    Or just add more  GND vias connect to decoupling capacitor with small GND copper area, but make the copper trace seems more "independent". Which is mo resonable?

    The more ground and the more vias the better. in such a HF circuit there's no "independent" copper. When you try to isolate a local ground plane from the common solid and continuous ground plane, you will get problems at the connection point of the local ground plane to the common ground plane. You will add unwanted parasitic inductance and unwanted stray capacitance and the only effect is that common mode noise develops between the local ground plane(s) and the common ground plane. By this you no longer profit from the awesome shiedling effects of solid ground plane but the local ground planes become antennas now injecting common mode noise into other local ground planes. At the end the ultra positive effect of having a solid ground plane is totally lost. You have no longer proper shiedling and your circuit can even result in instability and oscillation.

    If you want real isolation between the APDs, then you have to use entirely independent printed circuit boards, entirely independent supply voltages and entirely independent Faraday cages. But when you plane to use a common printed circuit board for all APDs, the best you can do definitely is to use one (ore more) common solid and continuous ground planes solid and to avoid gaps in the solid ground plane and to avoid the use of local ground planes and to avoid any isolating ground tacks. All this will do more harm than good. And finally you can mount individual Faraday cages for each APD signal path on the top layer and connect them with as many vias as possible to the common solid and continuous ground plane.

    Another remdy to improve the isolation between the channels (or to increase the channel separation) is to move the channels a bit from each other on the printed circuit board, so that more solid and continuous shielding ground plane exists between the channels.

    Kai

  • 0 in reply to kai klaas69
    Prodigy 195 points

    Hi Kai,

    It's perfecty clear! Thank you!