Comments on Signals and plane on the same layer
Parent
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.
Post
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
2 comment threads