This mainly falls under rules of thumb, does not mean the best solution in all cases, just the least likely to cause issues.
1. They say not to share Via's and equally to use multiple vias to reduce the inductance of that given decoupling capacitor, in reality it only gets important when your dealing with either fast edges, low noise or high current signals. as these are when that inductance can cause issues for the single via per capacitor, and crosstalk via the return path for low noise signals.
Fast Edges - As the frequency increases away from DC, more and more of the return signal (your ground current for most things) starts following the path of least impedance instead of the path of least resistance, this path generally follows the signal trace as close as possible, and how it could be described is having the smallest loop area, so for each decoupling capacitor you ideally want it so the current can hop adjacent to your signal or under it in as short a distance as possible. more distance = more inductance = larger loop area ~ poorer decoupling
Low noise - Most people like to think of a via to a ground plane as a perfect 0 ohms, in reality it has resistance and inductance, so lets say you have a nice high resolution ADC with a few uV / bit, well the internal reference voltage and other parts shift up and down in voltage with that devices Ground pin, lets say you share a via to ground with something else, say a little status LED, or something that takes gulps of a few mA of current. the voltage across that via to the ground plane can cause your ADC to jump up and down in reading,
High current - Any time the current changes, inductance is a problem, Equally at a certain point heat dissipation is an issue. so sprinkling lots of vias around something you expect to take large gulps of current e.g. a GSM modem, (can draw spikes of 1.2A) helps improve the decoupling to that device
Inductance adds like resistance, you have 2 vias in series you have double the inductance, you have 2 vias in parallel you have half the inductance.
Actual rule of thumb to follow
- Pay attention to the return path of a signal, e.g. where its ground current has to flow to keep close to the signal, the smaller this loop the better, this is why they recommend a ground plane via where a high speed signal changes layers. beside it is just as good as below it
- Keep decoupling capacitors close to the device pins, and dont forget the length of the ground path, Usually its better to keep the ground trace to the chip on the same layer where possible,
- For decoupling capacitors, the current to your device should flow through the decoupling capacitor pads, this way the capacitor filters down any current spikes from your device.