Hi.
I have a 4 layer design for 5V operation with minimal current (max of 1.5A). Layer 2 is ground and layer 3 is +5v. Should I also flood fill the top and bottom layers (layers 1 & 4) with ground as well around the traces? Or perhaps might it be better to flood the top with another ground and the bottom with another +5v? Or just leave the top & bottom laters alone with just their normal traces and no flood fill?
Thanks,
Kevin
In general, filling with copper flood is a good thing. So long as you have the one good solid ground layer on 2 (and unless you are likely to have a lot of heat) you are probably not likely to notice much difference from the extra fill. Maybe someone else has info to the contrary. I am keeping in mind that this is a 5V design. Make sure that none of your copper fill is floating.
I have the opposite problem at the moment. I have a 2 layer design where I am using jumpers (some at funny angles) just to get my power and signals around without breaking up ground too much on my bottom layer. This one would be much easier with 4 layers.
Thanks Bob. I have three ground pours and one +5v pour and I am wondering if there might be a benefit to instead, having two ground pours and two +5v pours. Like for example doing it this way will create even more capacitance between power and ground sort of like a huge capacitor. I already have that with the +5v sandwiched between two grounds. It also might not really make much of a difference either way.
My background is switching power conversion. Layout can be critical for this. Within a low voltage “hot loop” you want to minimize inductance with short connections and close proximity to a ground plane. This does increase pcb capacitance but this pcb capacitance is likely to be less than a few hundred pF; much less than a 10 nF (small value) bypass capacitor. So aside from spreading heat as I mentioned, placement of ground planes can be important to minimize stray inductance and crosstalk. With low voltage circuits, those are much more likely to be caused by stray inductance than by stray capacitance.
In a typical 4 layer board stackup, the center dielectric is much thicker than the outer two dielectric layers. So given that ground is layer 2 (of 4) it is best to put as many as possible of your high frequency signals on the top layer. I only had a quick glance at it but I think this page discusses noise cancellation via “image currents”:
In a high frequency voltage converter, I can see a few volts difference in voltage spikes and ringing (due to layout inductance) in a board which is really good versus one which is not so great. But so many designs are just not that critical.
I generally wouldn’t put large areas of +5V on an outside layer, as it makes grounding the PCB harder and increases the chance for short circuits. It’s okay to fill some areas with +5V if you have lots of components there that need it and where it would be easier to route than many small tracks, but I would avoid for example areas near mounting holes or the board edge, where scratches can easily happen.
Usually you’d put signal lines (and components) on layer 1 (top side), ground on layer 2, 5V (or whatever main voltage you use) on layer 3 and a ground fill with additional signal lines (if needed) on layer 4 (the bottom side). There is usually no need for another 5V fill on the bottom side as you can already connect all the vias to layer 3. If using multiple different voltages it could make sense to fill some areas on the bottom layer with it, but generally I would probably prefer an island on layer 3.
Thanks Jonathan! Right now I have layer 1: signal plus various miscellaneous ground fills. Layer 2: all ground. Layer 3: all +5v. Layer 4: signal plus miscellaneous ground fills.
I think that’ll work nicely. Yes?
That sounds fine and pretty standard, yes. Of course if your board has very high frequencies or very high current or if you need special shielding because of RF or crystals, you might need some special layout, but for a generic micro controller board, it’s probably a good approach.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.