Signals and plane on the same layer
Hi, I’m working on a PCB layout, which is only about the second board I’ve ever designed. I’d appreciate some help with the following issue:
This board has two layers:
-
The top layer is used for signals and power planes.
-
The bottom layer (shown in the images) is intended to be a ground
plane.
I’ve tried to minimize the number of traces on the ground layer, but in some cases, routing constraints leave no choice.
My question is:
When placing traces on this ground plane, is it better to:
- Keep them as tightly packed as possible, grouping them into a concentrated "island" within the ground pour (Image 1)?
- Space them out slightly, allowing the ground pour to flow between them, thereby increasing the overall ground area surrounding the traces (Image 2)?
Maybe these images don't demonstrate the issue very well, but I’d love to hear your insights on the best approach anyway.
3 answers
You are accessing this answer with a direct link, so it's being shown above all other answers regardless of its score. You can return to the normal view.
When placing traces on this ground plane, is it better to
- Keep them as tightly packed as possible, grouping them into a concentrated "island" within the ground pour (Image 1)?
- Space them out slightly, allowing the ground pour to flow between them, thereby increasing the overall ground area surrounding the traces (Image 2)?
Definitely #2, but that's not what your second image shows. Lots of little islands in a ground plane aren't as much a problem as a large island. Think of a ground plane metric as the largest linear dimension of any island, not the number of islands, with smaller being better.
Your bottom image has the same problem as your top image. The only difference is that you didn't flow the ground plane into all the little dead ends. Dead ends don't help a ground plane much anyway, and in pathological cases act like little antennas that can resonate and actually make things worse.
What you should be doing is first minimizing the length of traces interrupting the ground plane. Set the cost of routing in a polygon high. That may require a few more vias, but that's one of the costs of trying to have a ground plane in a two-layer board.
Once you only have short "jumpers" in the ground layer, then you have to unclump them. Again, you want to minimize the maximum dimension of any island, not the number of islands. Manually move things around so that the ground plane flows around all the little jumpers.
Here is an example of a ground plane on a two-layer board:
Note how most of the "jumpers" have ground plane flowing around them. Unfortunately some of the traces directly under the microcontroller at left-center are longer than I'd like and abut other jumpers to make larger islands. Hopefully you can still see the overall philosophy.
1 comment thread
My answer from another place: -
It's best to use a 4 layer board looking at the tracks you have on your ground-plane side.
But, if you are really insistent on using only two layers (why?) then do whatever you can to minimize the track lengths on the ground side. I would say from experience in answering this type of question on this site that you have almost certainly (a probability thing) not minimized the track lengths on the ground side so, please do so.
Work on the top layer tracks and do what you can. If necessary go from top to bottom then back to top then, back to bottom and then back to top to keep the ground-plane as uncluttered as possible.
If you are going to group tracks, keep the group small and leave a good amount of ground plane between adjacent track-groups.
Based on very little information and you just starting PCB layouts, you may be overthinking this problem or rightly concerned. There are a lot of fundamentals you might already know about how to make a capacitor and inductor using just a PCB trace and ground plane.
Generally, ground planes are for products where high-speed or high-frequency signals exist. I highly recommend you look inside some Japanese products like an old DVD player or look online for some teardowns that include PCB designs. Here all the high-speed signals are properly taken care of and everything else has no ground plane and might even use a single-sided board with jumpers.
So you many have over-designed it to not. We cannot assume where you have high speed signals.
See my related answer here https://electrical.codidact.com/posts/293375
There is also a great tool called Saturn PCB Design Tool I recommend
0 comment threads
2 comment threads