2
\$\begingroup\$

I have been trying to simulate the output impedance of ADA4522-1 using LTSpice. I have added a sinusoidal voltage source with 1Vp-p voltage at 1MHz at the output and connected the input to ground just as the picture below:

enter image description here

but the problem is based on the datasheet, the impedance at 1MHz is 4 ohms. But the voltage at the output of the op-amp is 6.26mV, considering the voltage divider between the output impedance of ADA4522-1 and the 1K ohms resistor gives almost 6.26 ohms output impedance. which is not exact. Running the ac simulation based on the picture below also gives an impedance near the value of 6.3 ohms:

ac_sim_outputImp

whereas this curve is in the ADA4522-1 datasheet, page 15, Figure 31:

enter image description here

The question is why can't I get the same results as the datasheet? Is there anything I am doing wrong?

Edit1: the difference between simulation and the datasheet is even bigger in higher frequencies, for example: @ 10Mhz and 100MHz, I get 82.5 and 43.14 ohms respectively while the datasheet output impedance curve says it should be more than 100 ohms and 15(!) ohms.

\$\endgroup\$
0

2 Answers 2

4
\$\begingroup\$

The question is why can't I get the same results as the datasheet? Is there anything I am doing wrong?

There is something you're doing wrong, but it's kind of out the box of what you'd normally think. Other than this slight problem, your test setup is quite good...though you really should do a decade sweep instead of a linear one for the .ac analysis. However, that's not what is causing your issue.

I duplicated your circuit but could not duplicate your results. As shown below, my output impedance plot looks much closer to the one in the datasheet and quite different from yours.

enter image description here

enter image description here


I noticed in the upper left corner of your screenshot, you're using LTspice XVII (i.e. 17.0), which is an older version. I'm also using LTspice XVII (I'm on Windows 7 as well), but I'm using the final update to it which is from January 25, 2023. I took a look at the changelog and noticed this:

11/05/21 ADA4522-1 Model updated to new architecture with accuracy and convergence improvements.

So it looks like you might still have the older model from prior to November 5, 2021. I suggest you do a "Sync Release" on your LTspice XVII install, or install LTspice 17.1 which Analog Devices simply calls "LTspice" now. It still runs on Windows 7 64-bit even though the website says "Windows 10 64-bit and forward".

\$\endgroup\$
1
\$\begingroup\$

It does not seem to me that you are doing something wrong. But you could also say that 6.26 ohms is not so far from 4 ohms (only 3.9dB), especially when the datasheet plot is so steep in the 1 MHz region.

I assume that the spice model of the ADA4522-1 is not very accurate.

\$\endgroup\$

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.