Finding or displaying the shortest path through a ground plane to power supply ground

I have designed a 2-layer P.C.B. with a ground plane on both sides of the board.
There are many areas of the ground plane that are separated from one another
by traces. I have made 100’s of modifications to the traces on the board to get
the ground plane to be electrically connected to all the /GND pads on the P.C.B.

Now I am wondering about what path through the ground plane the current will be
returning on. I surmise that some pads will have a long spaghetti like route to get
from a /GND pad to the power supply ground.

Question 1: What problems will I incur with a ground plane strategy like this?
Question 2: Is this the correct way to use the ground plane?
Question 3: Should vias be used to stitch the top and bottom ground planes?

And the real reason for this post:

Question 4: Is there a way to display what path through the ground plane the
current will take. ( I am assuming I could click on a /GND pad and then click
on the /GND pad that exits the board to the power supply , and see a track
drawn on the screen showing the shortest route through the ground plane. )

Ok, thanks for listening.

The questions surrounding GND planes are abundant this week. This is at least the third.

Watch this video from Rick Hartley (from altium). It’s 2 hours 19 minutes, and worth all of it.

First goal is to have a single undisturbed GND plane. Often this is not possible on a two layer PCB. First compromise is to allow “dog bones” / “hop unders” to make it possible to finish routing of nets that are crossing each other. The denser a PCB becomes, the more compromises you have to make. The costs are higher EMI and signal integrity degradation. The PCB will still “work”, but it may become difficult to pass EMC regulations (for commercial projects).

GND plane is so important (in high speed digital designs) that on a 4 layer PCB, both inner layers are often used as GND layers. (This reduces distance between a signal line and it’s GND return from 1.6mm, to 0.2mm or less.

In (“low speed”) analog designs, considerations for PCB design are… different.

You should do everything you can to have at one side full continuous GND plane.
If it is not possible you should really consider using 4 layer board.

You can use vias for example like I have done it in this PCB:

All vias you see there are GND.

The way current will take through GND plane depends on this current frequency.
Imagine you have full GND at bottom and at top you have a track that runs along the short sides of a right triangle. If the state change is propagated through this track than this signal return current DC content will go back through the GND plane the shortest way (along the hypotenuse). The higher frequency part of this slope the more closer to going just under the track it will select. You should use continuous GND plane to ensure the best return current path for each signal and each its frequency contents.
You can read much more about it in pdfs linked here (hope they are still valid):

The above comments are pretty much true, but it also depends a lot on the circuit (references to “high speed”…I would strike the word “digital” because high speed analog is no less critical.)

I have a 2 layer board which I built a few years ago. It centers around a SEPIC converter which runs at 200 KHz or so. This could be a problem but it runs OK. I built it for myself and have attached the project file. I have no objection to anyone copying it but I would be amazed if anyone did.

One point is to understand where a good ground plane is important and where it is less so.

Another point: Instead of chopping and jumpering my ground plane, I chopped and jumpered the slower signals where I needed to do so.

Digipot SEPIC (519.8 KB)