Hi 5111212,
Here are two options. As Michael indicated, near all op amp can attenuate the input signal in this manner.
If you use OPA277 or OPA2277, please watch out for common mode voltage requirements. If you provide us with your attenuation and op amp requirements, we can check out a circuit for you.
Best,
Raymond
Hi 5111212 ,
The power is the dual supply +-12V and the signal level is +-12V, I want to get 1/8 gain.
Enclosed is a circuit that will meet the above requirements.
I have some questions. THS1209 is ADC with BW is 2MHz. But THS4131 is a high speed FDA with BW of 150MHz. I don't think that you will need 150MHz Op Amp to connect between OPA277 and THS1209 ADC (I think that THS1209 can do single-ended or differential input ADC mode).
Are you using THS1209 in a differential mode? If so, you may use THP210 Op Amp to attenuate the input signal and interface directly to differential input of ADC.
Please let us know if this is what you have in mind.
Best,
Raymond
Hi David,
Here is an example of SE to FDA with attenuation.
THP210 SE to DF Output 03172021.TSC
https://www.ti.com/lit/an/sloa099/sloa099.pdf
If you'd like to use THS4551 HS Op Amp, I can transfer you to the support team tomorrow.
Best,
Raymond
Hello Raymond and David,
Actually, the FDA attenuator is quite simple - if a bit confusing. It should work with any FDA, you just need to choose by desired speed and precision which to use. The design starts by targeting an output Vocm voltage and a +/-swing around that. Running single supply, if you keep the output in range (not clipping into the rails) the non-signal input side is a simple R divider to ground. Since the output feeding that is not going below ground, neither does the fed back input signal - staying in range, here is your sim file simplified to a 1/8 gain (you don't need that R to ground) showing just the output swings - this is taking +/-12V input to the 2.5V output centered swing using single 5V supply, I tried the THP210 here, it was not setting up the output Vocm correctly - I think the part would be fine, but the model was not so I went to the THS4561 model,
And then here are the two summing junction voltages - magically inside the supply voltages and not clipping, Since the differential voltage has to be zero, these are on top of each other.
So you can actually do this function pretty easily with any FDA-This is because of that separate common model loop driving the input common mode voltage swing. . The design starts by setting.
1. desired output Vocm
2. desired +/-V on each side of that on the two outputs
3. that sets the attenuation
4. Then, going further what bandwidth do you want and then do you want any MFB filtering in the FDA stage - pretty easy to do
5. Once you have the RC values set around the part (including any RC into the ADC), check the phase margin
6 If the phase margin is poor, there a couple of easy ways to fix that.
Here is the single 5V 1/8 attenuator design with the THS4561
I went on to look at the SSBW here, yes a little peaky - that is normal as most of these FDA's are nominally design and specified at a signal gain of 1, that is a noise gain of 2, here we have NG of 1.125 so yes, a little lower phase margin - this 6dB peaking implies a 29deg phase margin using Figure 2 in this article, this is all easy to fix, but would be better to get closer to end design and device.
Incidentally, here is an output noise comparison between the two - lot of other things going into this, but using an input divider raises the noise gain giving more gain to the output for the FDA input voltage noise, If that can be avoided, as shown with the THS4561 ckt, normally lower noise can be delivered.
