Correct way to connect to GND and Power planes

[Piotr]

@johannespfister

I personally would switch between 5V and GND planes on the stack. meaning: Top: Use GND plane between the signal tracks, inner top: 5V plane without signal tracks or only very few signal tracks, inner bottom: GND plane

Continuing to nitpick or split hairs (both terms from Google translator and not sure if mean what I wanted)…
Gnd at top has many big and long holes in it so it is not good return path for most of tracks. As all signals are related to GND then in my opinion at 4 layer PCB the first layer under the layer with ICs on it (here it is top layer) have to be GND. No exceptions.
For many years I was designing only 2 layer boards always with bottom being full GND.
It was possible because:

• I frequently use 0603 47 ohm resistors at digital signal lines close to the source - in my opinion they reduce supply current pulses as changing state signal need only to reload its own output capacitance and reloading tracks and inputs of another ICs capacitance is little delayed. These resistors help me to untangle the connections,
• I used microcontrollers in TQFP cases. At top I went with VCC under it and then propagated VCC starry going out through all corners and through all VCC pins,
• I had nothiong against using some 0Rs to have my GND continuous.

I linked it few times but once more - here is PCB made according to these rules:

Approaching PCB track routing for a newbie

Positioning for me is the main work in designing PCB. If each element is where it is needed than routing is simple. Till now all my PCBs are 2 layers and all of them have GND plane taking 100% of bottom layer. So except GND I design my PCBs as 1 layer. I use microcontrollers in QFP packages without thermal pad at bottom. This allows me to go with VCC under the microcontroller and go out through all corners and all VCC pins. That way GND and VCC don’t disturb my signal connections. At all digi…

So when I moved to 4 layers the continuous GND laying under all signal tracks was my priority so if elements are at top then it is In1.
I was reading many times that In2 is typically used for VCC and other supply and was thinking that I will do it that way. But someone here at forum (year or two ago) said that he uses both inner layers for GND and I said: bingo - it will be the solution I will use. Thanks to it you need not to place blocking capacitor whenever you go with track from top to bottom (to allow return current to jump from VCC to GND or opposite). Via connecting both GND planes near the track jumping layers is replacement for this capacitor.
I am writing ‘will’ as till now I have designed only few 4 layer PCBs and all of them had In2 empty. Even the PCB manufacturer asked our contract manufacturer and he asked me if it is not a mistake, but it was as I wanted it (I needed as little GND as possible there but I had to use 4 layers because of QFN package that didn’t allow me for the trick with VCC under it.
Next I will take @paulvdh example to show how I would do it.