What is this peak in this JFET amplifier (JFET preamp + feedback opamp)?

[Verdefluox]

So, I'm trying to learn about JFET preamplifiers, mainly thanks to their low noise characteristics. Here I tried to test a simple JFET preamp with (hopefully) standard components, mostly taken from appnotes. I added a low pass filter in the feedback, since the frequencies I'm interested in are much lower.
As I tried to add a real opamp (in this case, a general NE5534, tried also with a JFET, more modern opamp - LT1792) I noticed this ugly spike at very high frequency (>10 MHz) in AC analysis, well beyond the operating range of the opamp. I'm wondering what this is due to, because I didn't find any info about it and I can't understand where it comes from. Is this some simulation artifact or should I worry about that in general?

[TimFox]

The 5534 is not unity-gain stable, unless you add a suitable compensation capacitor to pins 5 and 8.
With the capacitor across the feedback resistor on the 5534, the feedback factor will get close to unity at high frequencies, and the phase shift will cause the peak you see.
Go to the datasheet and determine an appropriate value for the additional capacitor.
Also, the low-resistance feedback network is good for noise purposes, but is a rather heavy load for the 5534, which usually runs into at least 600 ohms load.
Although simulation might not require bypass capacitors on the power rails, it would not hurt to add them.

[Kleinstein]

The circuit is missing the compensation for the JFET stage. This usually requires some local feedback around the OP-amp.
The problem with not being unity gain stable comes on top with the NE5534.  As the JFETs already provide about a 10 fold gain, it would need more capacitance at the NE5534 to make them at least somewhat stable - it would need to be stable with the external gain of 10 and this more like 10 x lower BW than unity stable.

[Gerhard_dk4xp]

This peaking is an indication of a tendency to oscillate.
The real fun starts when you have a inductive signal source.
If you measure into the input, you'll see a capacitance in
series with a resistance. The resistance may be negative over
a range of frequencies. With the right inductance You'll get
an oscillator.

I have seen this behavior in virtually all FET + Opamp amplifiers,
even in designs by the GODs, for example Art Of Electronics ed. 3
It gets worse when the op amp is slow, as soon as you close the loop.

I got a stable design (single ended) with a TI current feedback opamp
but it had such bad 1/f noise that the FET stage was pointless.

You can see the effect when you measure S11 on the VNA.
When the trajectory leaves the unit circle, then there comes more
energy out of the measured port than the VNA sends into it.
That could never happen on a passive device.

At Marker1 in the Smith chart, the negative resistance is 144 Ohms.
That would require an even larger gate/base stopper for stability,
which does not go well with low voltage noise.

(The 2 pictures are not necessarilly the same device.
Must sort my pics. )

The closest thing to stability I have accomplished is single ended
FET -> cascode -> follower -> feedback to source.
I have only simulated it, not yet built. It eats too much current,
bad for the 18650 batteries.

[Verdefluox]

The 5534 is not unity-gain stable, unless you add a suitable compensation capacitor to pins 5 and 8.
With the capacitor across the feedback resistor on the 5534, the feedback factor will get close to unity at high frequencies, and the phase shift will cause the peak you see.
Go to the datasheet and determine an appropriate value for the additional capacitor.

This actually solved the problem, thanks! According to the datasheet and to various sources online, 22 pF should be sufficient for more or less most purpose, so if I'm not wrong now it should be unity gain stable. Here I deliberately increased it in order to tame the peak a bit more, at least accordingly to what I obtained in the simulation. The file for the NE5534 is taken directly from TI website, and the modification for the compensation pins is as follows:
https://e2e.ti.com/support/tools/simulation-hardware-system-design-tools-group/sim-hw-system-design/f/simulation-hardware-system-design-tools-forum/721377/tina-spice-ne5534-how-to-add-the-external-compensation-cap-to-a-5534-in-tina-spice
Since it's meant for low noise, however, I noticed that in a noise analysis I'm getting the same peak, this time unresolved. I swear I don't understand why. Shouldn't the whole circuit, with compensation in place act as a low pass for everything and avoid this?
In the while I searched also for an alternative (possibly Analog Devices, for now just for the sake of having a somewhat more accurate simulation), and I found the LT1792 (should be unity gain stable if I read correctly), which has similar behaviour in AC analysis and a likeable one in noise too. Why does this happen?