AC analysis of opamp loop in LTspice

Question

I'm building an electronic DC dummy load and have a problem with stability/oscillations.

This is my circuit:

Vset - controls current, when set to 100mV it makes 500mA at the shunt
Vout1 - Vshunt multiplied by 40 by U1
Vout2 - output from U2, drives mosfet M1
power_in - it is 10V and I added some noise to it

Vout1 and Vout2 oscillate.

power_in:

Vout1:

I'm trying to do AC analysis, so I could make some tweaking.
I understand that loop is not stable if phase shift is 180° and gain higher than 0dB.
I read that I have to break feedback and insert small signal for AC analysis.
This is what I have done:

AC analysis is this:

Is this method correct? I googled for some examples, but I was able to find only simple examples that I was not able to apply to my circuit.
Problem is that result of AC analysis tells that gain is always less than 0dB and phase shift below 180° (well, maybe for higher frequency reaches 180°).

At this point I'm stuck, I appreciate any help or advice how to properly do AC analysis.

UPDATE:
I uploaded source file for LTspice:
https://www.dropbox.com/s/iol9l4zr8wo7j1a/dc_load_heat_test.asc?dl=0

Answer 1

@Chupacabras In your simulation for the loop gain, you set C7 to 100F. This are in Spice 100 femto Farad. But L1 and C7 should have very large values. 1G or 100G is no problem, because it is only a simulation.

The correct expression for the loop gain is V(Vout1)/V(X), where X is the node between (V4,L1,R9).

As LvW already mentioned in the comments, there is no loading problem in this configuration.

Answer 2

The problem is you are mistaking your control input, you still have a closed loop system as shown below, but you need to identify which parts are which.

U1 is H, if you found a transfer function for U1 you could subsitute it in for H

U2 is G and the summing point

\$ \theta_1\$ is your input, which you want to be a DC value, however, if you want to analyze the loop, you need to change your control point.

There are a few ways to identify a control system, one of them is by sweeping the frequency, you want to do this at the control input then look at the output. (or different points in the system)

In your second attempt you were trying to inject the AC analysis after H and before the summing point, which I suppose could be done, but there is a much easier way, and you could use control theory to check the stability. Yes an AC block and injecting AC in your 'sensor loop' can work, but so will an AC analysis of your control input.

Edit: actually I should have been checking Vshunt (in the analisys below , I was checking Vout2). Vshunt is your real output \$ \theta_o\$ but they are pretty close in AC response so I digress...

Source: Electronics tutorials ws: Closed loop system

Here is how I changed your file to do a proper closed loop analysis, I put a new voltage source V4 at the positive terminal of U2 (your control reference point). I also gave it a amplitude of 0.5V and a DC parameter that varied from 1 to 5V.

.step param R list 0.1 0.3 0.6 1 1.5 2 2.5 3 3.5 4 4.5 5
V4 N003 0 {R} AC 0.5

Wait, what if we zoom in, yep, there is a resonance of 3dB at vout1, but 40dB at vout2. that is bad (at the first two runs that correspond to the 0.1 and 0.3 V DC params). All the rest of the runs have no resonance.

What if we move that capacitor... Yep 6db, thats better, not great, might be acceptable. I'll let you sort out the rest.