4 layers: top = signal, 2 = gnd, 3 = signal, bottom = power. Good idea?

[Webo]

Hello everybody

I'm asking myself - and would like to ask you - why in the usual case people do not choose the bottom layer of a 4 layer pcb for a power plane, but rather the third layer.

I see the following advantage in using the proposed layer order: Both signal layers are close to the ground plane, which lets one avoid the discontinuity of the return current path (which must in the usual case "jump" from ground plane to power plane or vice versa) when placing a via for routing.

Should I nevertheless use the "traditional" layer order, i.e. top = signal, 2 = gnd, 3 = power, bottom = signal?

 

[mho_logos]

One reason to use the traditional stack-up is that it is more symmetrical, thus better prevents warping of the PCB.

 

[qieda]

Hi,

the traditional setup is more symetric, which to my feeling is a better solution.

Here some (maybe weak) arguments, which comes into my mind.

normally the distances between the layers are not equal
the distance between top <-> 2 is equal to the distance between 3 <-> bottom but 2 <->3 is different.
So the two sigal planes behave different.

Also if you place one layer on top and the other inside the layer which is inside has a reference in the ground plane and in the power plane which is different to the layer on top.

In the traditional setup power and gnd are opposite to each other and form some kind of decoupling.

For high speed signals If you jump between the layers with a via you will get a stub in your setup, which my distort the signal.

If you want to rework your PCB (due to some bugs) I think it is better to have both signal layers outside.

If you place parts on bottom your power plane will have lots of holes.



Maybe you can separate your design to have critical signals near to the gnd plane and less critical signals on the other signal plane.


regards

 

[qieda]

Hi,

I found this on the web
PCB Stack-Up - Part 2

your stackup is not discussed there.
but there also a stackup were the power is routed in the signal layer is discussed
means

top = signal/power
lay2 = gnd
lay3 = gnd
bottome = signal/power

maybe this fits better to your project

regards

 

[YanivS]

You need the two external layer to be signal layers because you usually need to solder the components to them. If the 3rd layer is the signal layer then you will need a lot of VIA's for all the pads. In addition having the signal layer an external layer, gives you the ability to make some changes on the board after production, in case that the PCB has some faults in it.

 

[venu.gongal]

The Traditonal stackup is Signal, gnd, power, signal/gnd.... The advantage u have large decoupling capacitor for power, double sided pcb, less interference for power supply.