Shared ground path vs shared supply path

Understand the physics, and then you don't need these silly and often misleading "guidelines". Such myths may have started with a kernel of truth, but the limitations and conditions under which they apply are usually forgotten to the point that the result is too often wrong. Mostly, they are crutches for the incompetent.

Whatever current flows thru the ground return path causes an offset voltage. Usually ground is your 0 V reference, so differences in this reference between parts of a circuit causes the parts to "see" the same voltage differently. This leads to several considerations:

1. How much does it matter? In a purely digital circuit, even a few 100 mv of difference in the apparent voltage level of a signal probably won't cause harm. In a sensitive analog front end, a few µV could matter.
2. Thicker ground conductors reduce the offset. Since the offset is caused by the current thru the ground return path times the path's impedance, reducing that impedance reduces the ground offset. On a PCB, this means using wider ground tracks, or the ultimate, a ground plane.
3. Frequency matters. Note that the ground offset is the ground current times the ground path impedance, not just resistance. A reasonable copper trace on a PCB might have 10 mΩ impedance at DC (resistance), but it could easily be much more than that at 100 MHz. This is especially true if the trace is not straight. Even straight wires have some inductance, but any curves increase the inductance.
4. Current loop area matters at high frequency. When current goes out one path and back on another, there will be some overall area of the current loop. That not only increases the inductance of the loop, but can act like an antenna. Parts of the high frequency energy in the loop is radiated into space. This may make your circuit non-compliant with emission regulations, like part 15 of the FCC rules here in the US. Also, all antennas are reciprocal between emission and reception. If your circuit can radiate, then it can also pick up similar radiation from the environment, which increases noise and could cause erroneous operation.
5. Return path geometry matters at high frequency. At high frequencies where the outgoing and return conductors of a signal (which can include a power feed) form a transmission line with the dielectric of the PCB, the return current "wants to" follow the outgoing current geometry. In the case where the return path is a ground plane, the return current flows on the plane underneath the outgoing trace, not a straight path as it does at DC. This is actually useful since it minimizes the loop area all by itself.

So what do do on a typical PCB? If you have to ask here, use enough layers that you can dedicate one as a ground plane. That gives you the lowest possible impedance, and minimizes loop area at high frequencies on its own.

Unless you are doing something complex or very space-constrained, four layers should be enough to dedicate one as the ground plane. Nowadays, the additional cost to go from 2 to 4 layers is relatively small. Considering the extra engineering time to create a good layout with 2 layers and then the lower noise immunity and higher radiation, 2 layers is more expensive unless it's a very high volume product. You're not ready for one of those yet.

I have designed many industrial PCBs with 4 layers. Usually layer 2 is the ground plane. Most of the connections to the parts are on layer 1. You therefore try to route the interconnects on layer 1. The ground plane is then immediately beneath that, and acts as a shield between the signals on layer 1 and those on layers 3 and 4. Try to use layer 4 for signals next, then layer 3 only when you need to. That leaves most of the signals on the outer layers where you can manually make changes to prototypes more easily.

Note that none of this says anything about "separate" return paths.

Don't forget to properly bypass the power supply feeds at every point of use. The ideal power supply has 0 impedance. The traces from the power supply to the places the power is used always have some impedance. The DC resistance is usually good enough to not cause an unacceptable voltage drop, so the real problem is at high frequencies. A bypass cap to ground at each point of use locally decreases the power supply impedance.

You may be tempted to connect all ground leads of all parts to the ground plane with vias, but don't do that for the bypass caps. The ground pin of a chip should be connected to the ground plane as directly as possible, but the loop from the power pin to the bypass cap and back to the ground pin should be off the ground plane. The nasty high frequency currents generated by the chip run thru that loop. By keeping them off the ground plane, you avoid the ground plane from becoming a center-fed patch antenna. The bypass caps still does it's job either way, since its effect is only meant to be local anyway.

Regarding the bypass caps, I've actually seen recommendations to connect them to the ground and power planes ... This would seem to be in conflict with what you've said here

Again, follow the physics. I've explained the reason behind my recommendation. Find why others come to different conclusions, then make up your own mind.

posted 22 days ago

CC BY-SA 4.0

21d ago

Olin Lathrop‭

8419 reputation 18 349 999 480