Power polygon and matching ground
For power polygon that primarily carry DC, how critical is it that it is located above a ground plane?
If it is important, how crucial is it that the polygon completely overlaps the ground plane beneath it?
Additionally, if overlap is important, how significant is it that the ground plane remains continuous and is not split by traces?
2 answers
If it is important, how crucial is it that the polygon completely overlaps the ground plane beneath it?
A power polygon can hang off the side a of a power plane. Complete overlap isn't crucial.
[...] how significant is it that the ground plane remains continuous and is not split by traces?
Keep the ground plane as intact as possible. Splitting ground plane by traces leads to increased parasitic inductance of all the signals which have to run across the split. Don't "Swiss cheese" the ground plane and run signals over voids. It's more importnat for signals than for power.
For power polygon that primarily carry DC, how critical is it that it is located above a ground plane?
Why is this even a question? : )
How many layers are you planning to have? These days there are too few reasons to do a 2-layer board instead of 4-layer. With a 4-layer board you'll have ground plane everywhere.
When a power polygon overlaps the ground plane on the adjacent layer, you get the benefit or power plane capacitance. The capacitance value is small on the order of hundreds of pF per square inch. But the benefit of power plane capacitance is that it comes with very low equivalent series inductance (ESL).
As a general rule, the lower the speeds (rise times) of your signals, the less important power plane capacitance becomes for power integrity.
As a general [philosophical] rule "Treat power as signal."
1 comment thread
For power polygon that primarily carry DC, how critical is it that it is located above a ground plane?
Practically not at all.
Power planes are overrated. Think about what problem you are really trying to solve. If you have high power currents, then you need to use wide and/or thick traces. In some cases, you might even add wires to carry some of the current. I've seen boards where the solder mask was deliberately left off a long power trace so that a wire could be soldered over it in production. I don't recommend that unless it's either a one-off, or you have access to very cheap labor.
In some exceptionally high frequency cases, having a power plane can be useful to get a high-quality distributed capacitance with the ground plane. In such cases, you put the power and ground planes on the two most closely-spaced layers.
In most ordinary cases (no exceptionally high currents or high frequencies), power planes are silly. A good ground plane with small and few interruptions is much more important. If you properly bypass the power at each point of use with a 100 nF to 1 µF SMD ceramic cap, then the power leads can have some impedance at high frequencies. The high frequency impedance is then made low at each point of use by the bypass caps.
Usually, with a good ground plane and proper power bypassing, you don't need power planes.
0 comment threads
1 comment thread