I made a SWeq element so that it would be possible to analyze the noise of several different circuits simultaneously. Noises of all analyzed circuits are obtained on one diagram, which is convenient.

I was doing almost the same thing. Distortion in my case! How accurate are SPICE's distortion and noise calculations? I'll be waiting until the end of the lockdown before I can go see my colleague who has a Audio Precision analyser.

 

Some skill is necessary. It also depends on the accuracy of the models. Sometimes it is necessary to take into account the parasitic elements of the assembly. Not all models are accurate enough. This is especially true for noise calculations. For example look at factory models of transistors:
.model LSK170C NJF(Beta=27.85m Betatce=-0.5 Vto=0.80 Vtotc=-2.5m Lambda=12.24m Is=24.52f N=1 Rd=12 Rs=6 Cgd=42.2p Cgs=42.3p Fc=0.5 M=610m Pb=0.92 Kf=0 Af=1 Mfg=Linear_Systems)
my model:
.MODEL LSK170C_n NJF BETA=0.0278541 VTO=-0.800434 LAMBDA=0.0122435 IS=2.45217E-14 N=1 RD=12 RS=5.8 CGD=4.22E-11 CGS=4.23E-11 PB=0.9265487 MJ=0.6098477 FC=0.5 KF=4e-18 AF=1 isr=1p nr=2 Alpha=1u Vk=100

Also field-effect transistors have a large error margin at low currents. In reality, there is not only a quadratic dependence of current at nominal values, but also an exponential dependence at small currents. I came across two articles about this effect a long time ago (the articles were in Russian and investigated the KP303A transistor). Here is an example of how I investigated this: