I've recently get an answer from TI and they said me that all CAPs of VR should be connected to VR power/ground domain.
Two things:
1. Likely, they* are not grounding experts, themselves. They are merely parroting the safest information that they have: put the caps as close to the regulator as possible.
2. The underlying purpose, is to minimize possible stray inductance between the regulator and the nearest capacitors.
The reason underlying that purpose, is the regulator needs to be in an environment where the impedance is low, stable, and resistive or capacitive (depending on type).
The amounts of capacitance and resistance allowed or required, [necessarily] dictate the maximum inductance that can be allowed between those components.
If an LDO requires an ESR of 0.5 ohm and a capacitance of 2.2uF, the RC time constant is 1.1us. The L/R time constant must be shorter than this, in order for the supply to have a predominantly RC-like impedance. (Otherwise, the L would dominate, and the supply would exhibit ringing; possibly, the regulator itself would become an oscillator.) This means Lstray << 0.55uH. Which is a pretty considerable amount of inductance (about a meter of hookup wire), but how far smaller than this amount it must be, depends on the LDO's internal circuitry. If the factor is 1/10th, then the limit is 10cm, which is typical of most HDOs (classics like the LM7805). Fast LDOs will be even more critical, so that a few cm is the limit.
Returning the capacitors to a distant ground would obviously violate this, but in a particularly sneaky way, because the inductance is between grounds: so that, what you thought was "ground" (in the absolute sense), is actually being skewed by the currents flowing between these two branches of ground. And as a result, neither regulator (nor most other loads in the circuit) are truly seeing the "ground" you should hope to provide.
*The TI forums are made up of customers and FAEs. I've met plenty of FAEs; most are generalists, and few are expert at any particular subject. They're almost universally bad at EMC, and matters such as grounding.
To be clear: you absolutely can make a circuit worse by adding too many bypass caps. But the chances of this happening at random, are very small. The chance of a circuit being worse by using too few bypass caps, is very high. This is the only reason why datasheets, appnotes and FAEs recommend bypass caps, and lots of them. It does not arise from a nuanced understanding of power distribution network (PDN) dynamics.
After all, they don't know your particular circuit, or how you're going to route it, so it is impossible for them to evaluate your PDN, for you. That is your responsibility (or mine, if you hire a consultant like myself to do this analysis and provide you that assurance of quality!).
I've found that in electronics there's a lot of discordances about ground topic. This remember me also that I've read some papers about how to ground correctly capacitors or connect local ground planes to main ground plane; a lot of people advice to use a single via each plane but in most of professional boards you can find 4-5-6 vias connecting same plane to main plane. Who is right?
You're asking the wrong question.
You should be asking to quantify a via.
Making a sweeping generalization that "four is better than one" is ridiculous.
A single 0.3mm via, through 1.6mm PCB, with typical 0.5-1oz copper plating thickness, has about 3nH inductance and a minuscule amount of resistance (< 1mohm). It is capable of handling 2-3A without getting dangerously hot.
If this is sufficient for a given location, then you only need one. More will have no effect.
If it is insufficient, as might be the case for a high current switching converter (where nH and uohms matter), you will need to use more.
The most frequent application of many vias, is thermal. A tight array of vias will almost triple the thermal conductivity of the PCB. If filled with solder, double that again. (You should use relatively large vias, if you expect them to fill with solder. I recommend 0.5mm i.d..) Applied to a DPAK type power device, the power dissipation can be increased from a limit of 1W (no copper pours or vias) to over 10W (with large copper pours, solder-filled thermal vias, and thermal pads and heatsinking on both sides).
Tim