I’m designing a mixed-signal PCB with components on both sides featuring MCUs, ADCs, DACs, and various analog opamp circuits. The power requirements include +/-15V for the opamps, 3.3V for digital components, and a few reference voltage rails (1.5V and 3V).
Could someone suggest an optimal layer breakdown for a 4-layer PCB? My initial plan is to dedicate one inner layer to the ground. For the second inner layer, I’m considering filling it with a 3.3V plane for the digital section, while leaving it unfilled for the analog section to accommodate power traces (+/-15V and 1.5/3V ref). Is this good approach?
Both inner layers should be ground. Outer layers are mixed signal/power. Here’s why.
Whenever you have changes occur in any one of your nets – power or signal, it radiates energy outwards. When that energy encounters copper, it generates a displacement current (noise.) The effect is greatest the closer the other copper is. So if you have signals on layer 4, power on layer 3, ground on layer 2, signals on layer 1, whenever there is a change in a net on layer 4, it’s not going to send the displacement current back on layer 2 (Gnd). It’s going to create the displacement current on the closest copper – in this case layer 3.
Displacement currents don’t form on layers marked “ground” – they form on the nearst bit of continuous copper. Every signal needs a return – yes – in the form of uninterrupted copper return path on an immediately adjacent layer.
Normally, I’d be inclined to go S-G-P-S for most designs, but the idea of going S-G-G-S and spreading out your power might be appropriate when you have ADC’ s, DAC’s, and small signal, high gain op-amps to squeeze as low a noise floor as possible. Much of the differences would be related to routing and placement. The old “If you MUST place this connector here, then…” so the final decision is always case-by-case.