PCB layer stackup


Is this a good layer stackup for an 8layer PCB with components only on the top layer?

1.) Top (Mount/Low speed signal) 2.) 3.3V 3.) GND1 4.) Signal horizontal 5.) Signal Vertical 6.) GND2 7.) Mix Voltage 8.) Bottom (Low speed signals)

This is for a high speed digital board (Xscale PXA270 and USB 2.0 high speed etc)

It seems a bit cautious to me, but I used to having to squeeze circuits onto 2 layers..

cheers, Jamie

Reply to
Jamie Morken
Loading thread data ...

This is a way I would do it :-) Signal layers are not adjacent to each other this way

1.) T> Hi,
Reply to


The stackup does depend upon a number of things and there is no stackup that works best for all cases.

If your signals have rising edges faster than 200 ps then, for long runs, it is nice to be able to keep them on an inside layer because of dispersion. But, that means a discontinuity due to the vias used for the layer change, unless, there is no layer change because the signal is launched by through hole (or press fit) connectors (and that has its own issues). Pick your poison there.

If you have the luxury of surface mount launches to surface mount landings on the same layer then keep your routes on the outside layers, if possible (few discontinuities and hence, few reflections).

For longer rising edges, like 10 us (and longer), then for short runs you won't have much of a problem no matter where your routes are unless you are really careless.

Many people tend to devote whole layers to voltages even if the connections are few. If I had a choice between a whole other ground pour and having to route a few extra signals for power on my signal layers I would take the ground layer. Yes, a DC voltage is AC ground but nothing is as much like a gound as is ground.

Also, in your stackup, you have two signal layers close to each other. Yes, they are orthogonal and that does make a difference. However, two rules have to be followed and they are difficult to follow to the letter. 1) The signals need to be completely orthogonal and this is next to impossible to do on a dense route. 2) The layers need to be far apart so as to look like two microstrip layers. Otherwise, crosstalk will be induced. In an analog system, crosstalk could be a disaster. In a digital system, this could add jitter, which has the effect of closing the signal eye.

I hope this helps.

Tom Cipollone

Reply to

Do you need two grounds? The L4 and L5 trace impedances could get awfully low. I like

1 parts and as many signals as possible (keeps vias down)

2 sigs

3 power, mixed pours

4 ground

5 sigs

6 sigs

If that won't work, add another power plane,

1 parts and as many signals as possible (keeps vias down)

2 sigs

3 power, mixed pours or solid Vcc

4 ground

5 power, mixed pours

6 sigs, slow and high current maybe

7 sigs

8 sigs

Signals on adjacent planes should be mainly orthogonal to reduce crosstalk. Even here, the L2 impedances can be awkward. Keep the 3/4 and 4/5 dielectric as thin as possible.

I can't imagine how people manage 16-layer boards.


Reply to
John Larkin

ElectronDepot website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.