I am implementing the General Feedback Theorem (Prof. Middlebrook, 2006) in LTSpice, using the example given in the Spice folder.

I used it to calculate the loop gain in a simple voltage follower configuration, to be sure that everything is working correctly (schematic below).

I plotted, as can be seen, the loop gain as:

T= 1/(1/(D)-1)

Which, for this configuration, should be just the gain of the amplifier, since the loop gain is T=A*B, where "A" is the amplification of the main block (in this case the op.amp) and "B" is the feedback factor (in this case 1).

However, as you can see, the result looks incorrect, since we have a loop gain of about -6dB also at almost DC. The closed loop gain, H(), looks correct, being 0dB constant until the poles of the op.amp makes it decrease.

Any idea where I have made mistakes? Thanks a lot!

LTSpice model and loop gain T

  • \$\begingroup\$ I'd recommend looking at this site: sites.google.com/site/frankwiedmann/loopgain \$\endgroup\$
    – Victor S
    Jul 24 '18 at 7:43
  • \$\begingroup\$ I already did this (the same note is appended with the model re-arranged by Frank Wiedmann), but it's only the theorethical basis used for the model. Here is stated that, as i knew, the terms "return ratio (T)" is the same as "loop gain". \$\endgroup\$ Jul 24 '18 at 8:09
  • \$\begingroup\$ I originally pointed out that site because I am not very familiar with that approach but I had seen it before on that site - the approach shown in this video is what I typically do: training.ti.com/ti-precision-labs-op-amps-stability-3?cu=14685 \$\endgroup\$
    – Victor S
    Jul 24 '18 at 8:14
  • \$\begingroup\$ I will look at the video, but usually the companies use these example with other methods (approximated) such as putting the big capacitor and inductor in the loop, or anyway other approximated methods (not this GFT implementation). Thanks anyway! \$\endgroup\$ Jul 24 '18 at 8:18
  • \$\begingroup\$ Allessandro...what is your task? To proove Middlebrooks GENERAL theorem or just simply find the loop gain of the circuit? In the last case, the simplified theorem using only one single ac source would be sufficient. \$\endgroup\$
    – LvW
    Jul 24 '18 at 8:35

It seems that in LTspice the .step param list command has changed.

So use the list parameter in increasing order: .step param z list -1 0 1

and change the sign in the expressions for Iz and Vz.

GFT.asc in the example folder of LTspice should work too.

And see the yahoo LTspice user forum.

Simulation with changed schematic.

  • \$\begingroup\$ Was going to post this, you were faster. :-) Here's the quote from the Changelog.txt: 05/16/18 The first .step dimension is now reordered to be increasing. \$\endgroup\$ Jul 25 '18 at 6:54
  • \$\begingroup\$ Yes, came to this conclusion on the yahoo group this morning :) Solved, thanks all! \$\endgroup\$ Jul 25 '18 at 7:46

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

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