Printed Circuit Boards - 4 layer

[thylantyr]

If you were to layout a 4 layer circuit
board (using CAD software)
for a high powered amplifier
design, what would be a good layer stackup?

Method #1
Layer 1 = signal
Layer 2 = split plane, + rail and gnd
Layer 3 = split plane, - rail and gnd
Layer 4 = signal

Method #2
Layer 1 = signal
Layer 2 = split plane, + rail and - rail
Layer 3 = ground
Layer 4 = signal

Method #3
Layer 1 = signal
Layer 2 = signal
Layer 3 = ground
Layer 4 = split plane, +rail, -rail

Method #4
Layer 1 = signal
Layer 2 = ground plane
Layer 3 = + rail plane
Layer 4 = -rail rail plane
** only 1 signal layer - yikes.

Method #5
Layer 1 = signal
Layer 2 = + rail plane
Layer 3 = ground plane
Layer 4 = -rail rail plane
** only 1 signal layer - yikes.

etc.

 

[Petter]

My limited understanding of the field is that the following is quite flexible:

Top: Routing + external plane (plane made out of non-used sections, often hooked up to ground or appropriate power plane
middle a: Appropriate power for that section + minimal routing
middle b: Appropriate ground for that section, sometimes + minimal routing
Bot: Routing + external plane

Petter

 

[hifiZen]

I think Petter's got it just about right. I always put signal traces on the outer layers, so you can follow them when debugging! It is also sometimes necessary to cut traces and whatnot while prototyping, plus if you're using any SMD componentry the traces can connect directly to the pads without vias - an important space-saving concern with fine lead pitch SMD devices. These few points become increasingly important the more complex the design is.

Unused area on the signal layers is often filled with polygon islands attached to ground, sometimes with multiple vais. These little islands serve well as grounding points for SMD components, and work nicely as launching points for guard traces. If the board is going to have a solder mask, you'll want to consider creating some carefully placed patches of exposed copper on these grounded fills, so that you can later use them as points to meter on, or solder test leads to. I just pepper them around the board, and put them in convenient places close to pins I think I may need to scope or make modifications to.

I like my ground plane next to the top layer, as the top layer is generally the most important signal layer, having the most traces and the most components. It makes sense to me to have the ground plane as electrostatic sheilding between the majority of your signal traces and the power layer below.

Power generally doesn't require a plane, just some fatter traces, so your various supplies should easily be able to share a layer. Of course, you don't have to confine power traces to this layer - there will inevitably be cases where you'll need to want to run the odd trace on a signal layer, but do try to avoid running any traces in the ground plane layer.

So, my choice for final stack-up would be:

Layer 1 = signal
Layer 2 = ground
Layer 3 = power routing
Layer 4 = signal

 

[thylantyr]

The issue where signal is on one layer and ground is on
the next layer....

At work we use $20k software to check crosstalk
after the pcb is designed. According to this software
and the people who designed it, to minimize crosstalk
between signal layers, ie layer 1 = signal, layer 2 = signal,
all you need is a plane in between, a large area of copper to dampend the magnetic fields on traces, which neither has to be
grounded nor connected to a power supply. So, what
they are telling us is......

Layer 1 = signal
Layer 2 = ground plane

is the same as

Layer 1 = signal
Layer 2 = power plane

is the same as

Layer 1 = signal
Layer 2 = floating plane.

But as you say, it's common to see signal then ground plane,
which is what I would do.

Ripleys beleive it or not ?