Are there any guides on how to do top layer ground ‘islands’ on a 2 layer board (gnd plane on bottom)? Is it a manual process or are there ways of selecting zones to fill?
Presumably this is where to start by selecting the outline of the PCB and filling, but how to select remaining islands, for that matter which ones?
You just need to add a via (called a stitching via) in the middle of each unfilled area to connect to the ground plane on the other layer
Creating all those loose “fingers” is not a good idea. It just creates more antenna’s that can both pickup and transmit noise. The minimum you should do in such a case is to stitch corners together, but if you have a bit of bad luck you can even create oscillators by combinations of the inherent length of copper and the capacitance between the GND planes (Such oscillators work somewhere in the GHz range.
To avoid trouble a single but GOOD GND plane is preferable.
I see you already found my tinkering in the other thread. I’m not a professional PCB designer and I did not want to put too much effort in it, but I do think that design is mostly OK.
If you’re interested in this part of PCB design then do a bit of research into the direction of EMC. Watch youtube video’s, read books, that sort of thing.
Good books about EMC are expensive and boring, but there are some quite good youtube video’s and I’ve watched a few of them, (Even those which are > 1hour long).
In very short:
Usually a badly designed PCB also “works” Especially when it has relatively low speed microcontrollers (Made with “old” technology, all those uC’s which can not have clock frequencies > 20MHz). It’s mostly bad from an EMC viewpoint. Even if you have no intention of meeting EMC requirements (needed if you want to sell products), Having some knowledge about the basics of EMC and how it relates to PCB design will improve your PCB’s without very much effort (or costs).
That board is looking mostly fine. Obviously not on a professional level, but good for a beginner (and I’m no expert either).
What you want to do is simply to add lots of stitching vias. Like every finger or cul-de-sac of your ground planes should be either eliminated by moving the tracks closer together (assuming interference between the signals isn’t a problem) or at least connect them to the ground plane on B.Cu. It’s also a good idea to add GND vias next o vias of other signals.
Here’s a very rough example where I would draw vias (green circles) and where I’d remove fingers (blue lines):
However you might want to repeat the gap of your B.Cu GND plane on the front plane.
Vias are usually free in manufacturing. There’ nothing wrong in adding hundreds on them. Generally, the more both ground planes are connected, the better. Where I have drawn a green point you could even add multiple vias if there’s enough space (like in the corners for example).
I can see how the bottom finger can be eliminated by moving the track beneath it upwards. But the upper finger cannot be since it is fixed as part of the connector footprint - how can that finger be ‘eliminated’?
Draw a rule area there and set it to keep out copper fills.
Then press B to update the fills.
See once more a PCB I showed you in your other thread. There all vias are GND and most of them are to connect top GND islands with bottom GND. I add these vias manually.
Jonathan
If I convert this to a 4 layer board with Gnd and Vcc layers
@Jonathan_Haas I recommended to add the cutout because up to 3A is flowing from the power connector in the west to the motor connector in the South -East and I wanted to keep that current though the GND plane away U3. A better solution would be to close that gap and move U3 (+ surrounding parts) further away from that current in the GND plane, but I was under the impression that was considered as “too much work” at that time.
The cutout is sensible (or at least shouldn’t hurt). If the front layer is filled, the cutout could be mirrored there.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.
