2
\$\begingroup\$

I have a 2 PCB layer. Bottom and Top layer are used for signals and power and the remaining area is copper ground.

I read about EMI etc and I decided to go to 4 layers for reduced EMI.

I realized now that actually it does not make any big difference since I read that the Top and Bottom can be used and the inner ones will be ground planes. So I cannot technically use more layers to separate high speed signals with analog and digital signals and power line etc.

Do I miss something?

Also, why isn't enough the copper ground and they suggest to have plane layers in between bottom and top? Should those layers in between, be copper ground or not?

\$\endgroup\$
3
  • 1
    \$\begingroup\$ A. on 2-layer PCBs, you typically reserve the bottom layer for ground (or other return paths), and don't use both sides for signal and power. I hope you designed with current return paths in mind! B. You say "I realized it make a big difference": that's wrong, but you don't say how you come to that conclusion, so we'll have a hard time explaining what you're missing! \$\endgroup\$ May 5 at 14:40
  • \$\begingroup\$ Isn't the copper ground area enough instead of a complete layer ground plane? Like for example top layer has some lines and the rest ground plane.. isn't that enough? \$\endgroup\$
    – Kris
    May 5 at 14:48
  • 1
    \$\begingroup\$ The number of layers is usually driven by the number and complexity of the connections. The speed (frequency) of the signals is also a factor. For a 2 layer board, normally you would start out with 1 layer being continuous ground, and use the other layer for all of your connections. If you can make all your connections on one layer, this is perfectly fine, and can yield a good result. If you cannot make all the connections (some crossovers needed), you can make small incursions onto the ground layer or switch to a 4 layer stackup. \$\endgroup\$
    – Troutdog
    May 5 at 16:10
5
\$\begingroup\$

A four layer board allows you to

  • Provide a complete power plane, reducing the inductance of the connections between the power source and its loads

  • Reduce the separation between the power plane and ground plane, reducing the loop area, and thus the generated magnetic fields, associated with power and return currents.

  • Reduce the separation between the signal layer and the return plane, again reducing the loop area for each signal path, and reducing its magnetic field emissions.

Whether you actually design your board to take advantage of these possibilities is up to you. If you know what you are doing, and depending on the complexity of the design, you might very well be able to achieve low EMI from a 2-layer board. If you aren't careful you could also easily produce high EMI from a 4-layer board.

\$\endgroup\$
11
  • \$\begingroup\$ Do we need a complete layer as ground plane or copper area on top or bottom layer is enough? Also layer stack has to be symmetrical right? So in 4 layers PCB the 2 inner ones have to be ground.. right? \$\endgroup\$
    – Kris
    May 5 at 15:08
  • \$\begingroup\$ @Kris Usually 4 layer PCBs use one internal plane for power, one for ground, but having two grounds will improve signal integrity and reduce EMI if you can route them. Ground layers should be unbroken all high speed and high power traces to be effective. Just copper playing the unused space on a signal layer does very little. \$\endgroup\$ May 5 at 15:20
  • \$\begingroup\$ "having two grounds will improve signal integrity and reduce EMI if you can route them" I'm not sure that is good advice for someone who is just becoming aware of return currents and loops. Having 2 grounds can easily make things much worse, and confuse, or at least have unintended consequences, in your pcb design and your cad software. Also, food-for-thought, what's the difference between a ground plane and a power plane? \$\endgroup\$ May 5 at 17:30
  • \$\begingroup\$ @Kris, as I said in my answer, " If you know what you are doing, and depending on the complexity of the design, you might very well be able to achieve low EMI from a 2-layer board." \$\endgroup\$
    – The Photon
    May 5 at 17:53
  • \$\begingroup\$ @ChrisKnudsen You could reference a power plane too, but for a beginner I think getting that right is more likely to be problematic then having a dedicated ground for both signal layers. Hence if you don't need a power plane, I would make it a dedicated ground. \$\endgroup\$ May 5 at 18:03
4
\$\begingroup\$

The typical 2-layer stackup that I'm used to working with is all the wires going one way (i.e., right and left) on one layer, and the other (i.e. up and down) on the other layer. Then try to make sure that there's a big web of ground wires -- I usually fill top & bottom with a ground pour, and put in lots of vias. I'm not sure how well it actually works, but I tell myself its clever, and so far all has been well.

The 4-layer stackup I've seen is signal traces on top & bottom, with ground and power in the middle. Unless you're working with super-high frequencies, a well-bypassed (i.e., lots of caps) power layer will "look" like ground -- but critical signals should be routed against the "real" ground layers.

If you haven't figured it out already, different boards have different requirements, and different designers are used to different things. If you understand the implications, then you can make informed choices about how to do the board stackup -- if not, just guess.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.