... to connect my Ethernet controller I have to use two signal layers. Let's imagine just as an example having the stack up of option A. As two signal layers, it is better to use the top layer and the inner signal layer, or it is better to use the top layer and the bottom layer?
Signal integrity will be better if both signals are referenced to the same plane. Layer 1 and layer 3 are a better option than layer 1 and layer 6.
... I would have the advantage of having two layers that have the same
ground plane as a reference, but the vias act as stubs.
The advantage that the signal layers 1 and 3 are referenced to the same plane outweigh the stubs caused by vias. For example, there are DDR interfaces laid out in layer 1 and 3, and they have common throughole vias (no blind vias, no back drilling).
Thus - option A.
1 - Signal
2 - GND plane
3 - Signal
4 - Power
5 - GND plane
6 – Signal;
Another approach is to "treat power as signal" and use both layers 3 and 4 for both power and signal, depending on local convenience.
update:
[from a comment ]
Do I have to insert also the power plane as reference or just the ground plane on layer 3 ?
I.e. are the traces on layer 3 microstrip or stripline?
I ask because the width of the traces necessary to have 50ohm is very different in the two cases.
Ideally, you'd use only ground as reference plane(s). Ideally, you wouldn't use both power and ground as a reference planes at the same time, because the will be impedance between power and ground plane. If you chase that ideal, you'd have to add a pair of ground planes to the board, so you'd get an 8-layer board.
I'll make a working assumption that you want to stick with an 6-layer board. There's a compromise - the thicknesses of the dielectric don't have to be equal. If the signal layer is closer to the ground plane than to the power plane, then the ground will act as a reference plane for the most part. If we insert the dielectric thicknesses, then a 6-layer stack-up could look approximately like this:
1 - Signal
0.005" [0.13mm] dielectric
2 - GND plane
0.005" [0.13mm] dielectric // this is the smaller distance between the signal layer and the GND plane
3 - Signal
0.040" [1mm] dielectric // this is the larger distance between the signal layer and the power plane
4 - Power
0.005" [0.13mm] dielectric // same symmetrical thing on the other side of the PCB
5 - GND plane
0.005" [0.13mm] dielectric
6 – Signal
Check with your PCB fab what their default 6-layer stack-up is. If the default is not the stack-up you need, then ask them how much they charge for a non-default stack-up. Then it becomes a question of micro-economics: 6-leyer or 8-layer, prototyping or mass production.