I'm using LTspice XVII (newest version), the simulation model of ADA4625-1 I downloaded from AD's official site.

I'm going to design an inverting voltage amplify circuit with a gain of -10.

enter image description here

The simulation circuits are as below:

  1. Open-loop frequency response test, the result is consistent with the datasheet, with a 0dB cutoff frequency greater than 10MHz. And it's similar to a single-pole ideal opamp with -20dB/dec over a wide frequency range.

enter image description here enter image description here

  1. A model I built for the feedback loop.

ADA4625-1's input capacitance is 20pF (11pF of CM, 9pF of DM), and I added a 10pF stray capacitance of PCB.

To compensate for the pole generated by Cin and Ri, I added a zero by feedback Capacitance, Cf = 0.1 * Cin.

enter image description here

The AC result of Noise gain is plotted below marked as red lines.

And the frequency of the junction is about 1.25MHz, which I think is corresponded to the -3dB cut-off frequency of the closed-loop.

enter image description here

But the closed-loop simulation shows a much lower -3dB(20-3=17dB) cut-off frequency of 50kHz.

enter image description here enter image description here

Which can't satisfy my need for closed-loop bandwidth.

Please tell me what's the problem, is my simulation model not accurate, or is there some bug in ADA4625-1's SPICE model?

If my simulation circuit is wrong, please tell me how to fix it.

Thanks a lot!

simulation source file


  • 3
    \$\begingroup\$ When you run an ac analysis in SPICE, always check the dc operating point, e.g. what is the output voltage of your op-amp in your configuration? Make sure the op-amp dc output lies in a linear region, away from \$V_{cc}\$ and \$V_{ee}\$ and add some dc bias to the modulating source \$V_2\$. \$\endgroup\$ Jan 19, 2022 at 6:23
  • 1
    \$\begingroup\$ Why did you make an autogenerated symbol when the device is already available in the database? Just press F2 and type 4625. Even it it hadn't, you're much better off using the [Opamps]/opamp2 symbol and adding the correct .inc or .lib. Anyway, for some reason, I can't get an open loop response, not with 4625 or 4625-1 or 4625-2. That might be a sign that the model has problems. Using UniversalOpamp3b with Aol=31meg GBW=18meg Slew=45meg shows a similar output to the 4625-1 with the same feedback. \$\endgroup\$ Jan 19, 2022 at 12:19
  • \$\begingroup\$ To answer Verbal's concern. The OPAMP's power supply is +-5V, the input offset is set to 0, which is in the linear input region of ADA4625 \$\endgroup\$ Mar 16, 2022 at 7:20
  • \$\begingroup\$ To answer "a concerned citizen"'s concern, the integrated model sometimes differs from the official model downloaded from Analog.com in some features. The downloaded model clarifies that the open-loop frequency response is modeled. \$\endgroup\$ Mar 16, 2022 at 7:23

1 Answer 1


I have already fixed this problem.

By modeling in Mathematica software with a simplified OP-AMP dual-poles math model, I find that my LTspice open-loop simulation circuit is inaccurate because my input signal should firstly be filtered by Ri and Ci, hence producing a new pole Ri-Ci in both the Open-loop response and the Closed-loop response.

$$ f_p=\frac{R_i+R_f}{2\pi R_f R_i(C_i+C_f)}\approx \frac{1}{2\pi R_i C_i} $$

A more dedicated model can illustrate this:

enter image description here In this model, the input stimulus firstly is attenuated by block 'm'. And this model clearly shows the influence of the additional pole Ri-Ci.

Thanks again for all your kind suggestions and help!


Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.