It's reasonable that those changes might be for the low current and the model/components used. I just fear that the simulations might be too diferrent in real life, that would actually suck.
The low current thing is a real effect. For transistors the spice models are quite good and can represent real life. However just like you found with the two JFET models, the spice model for a given part might not be trustworthy unless you verify it - which takes extra effort.
For the zener the low voltage a low currents is a known characteristic of zeners. People have measured the voltage on the MXR pedals over the years and it does come out around 4.8V.
There's no zener model in spice and zener models are the least trustworthy. Many won't show enough drop in voltage at low currents.
If you take your simulation you have a solid Vbias. Physically that's not realistic but it's often a good strategy. To make the simulation better you would use the human knowledge that the zener voltage is 4.8V and not the 5.1V on the label. The simulation would represent reality quite well and you don't have to deal with the messy problem of having an exact zener model with a 10k resistor to 9V, which is going to give you 4.8V anyway!
In general you have to have a good level of mistrust in spice. The models are rarely good. Different models from different manufacturers vary. I've got about 5 models for LM741 opamps and only one or two are even close to reality. For AC simulations, I don't even use real models I use something like LTspice's model "opamp"; IIRC the supplied model had a bug. For .TRANS you need on opamp model with PSU rails.
So, as I mentined before, I was just testing the voltages on the input, and as a standar I was actually using 1Volt so you're right. It gives a bettwr result. It's just it shouldn't be different response fpr diferrent input voltages, I guess. Why would I have more gain on higher voltages?
The key thing is it doesn't plot gain. It plots dBV, which is defined as
dbV = 20*log10( V / 1V) = 20*log10(V)
It is simply a conversion of volts to dB without any consideration of the input source level.
For gain you need,
dB gain = 20*log10(Vout/Vin).
So the two only agree when Vin is 1V.
You can actually plot expressions in LTspice and other Spice versions, so if you wanted you could plot the AC analysis expression,
Vout/Vin
and then plot would show dB gain = 20*log10(Vout/Vin).
In some versions of spice the variable expressions are already in dB and to get gain you can type something like Vout - Vin, which is actually dB(Vout) - dB(Vin).
I did 1V and got +- 5dB of gain in the end of the chain. And thanks for the insight on the working of the simulations. That could help me a ton. I actually had problems one time with amplitude response (on 3 different softwares I couldn't do it with an class AB amplifier if I'm not mistaken, and my colleagues too).
Unfortunately with spice sims it only takes one thing to go wrong and it all falls in a heap; like not plugging in the power on your breadboard. Small differences between packages can confuse things. I often start with simple dumb circuits where you already know the answer, then run a lot of sims and play with the waveform plotter. No doubt you will find some things which don't make sense. Good to keep notes.
Anyway, with a voltage divider I must be able to have 0 gain on the output, right? Or do you recommend me trying only when I test it physically?
I'm not sure what you are asking here.
