I’m currently working on my first 4-layer PCB design, and my stack-up is as follows:
Signal traces + ground fill
Ground plane, no traces
5V plane, no traces
Signal traces + ground fill
While the board incorporates a few different voltages, aside from the 5V connected to most parts, they are generated and utilized in localized areas. I’m considering utilizing the bottom copper to define multiple power planes around where they are used and created. Additionally, they could serve as thermal dissipators.
However, I’m unsure if this approach is recommended or if it might cause any interference. My circuit doesn’t involve high-frequency components except for a few using 10 MHz signals. Any guidance or insights on this matter would be appreciated.
It’s common practice to use multiple layers for power planes on PCBs. You can even allocate the top layer for localized power planes if needed. With careful planning, layer 3 could also accommodate localized power planes if heat-sinking isn’t necessary. Maintain the integrity of the 0 volts ground plane as much as possible, although experienced designers may deviate from this rule based on their expertise.
I typically opt for a signal/ground/-15V/+15V stack-up for op-amps. This configuration frees up a significant amount of space on the top layer for routing signals without interference from the dual power supplies.
Keep in mind that the +5V plane on Layer 3 may experience some coupling with the small power pours on Layer 4 due to the capacitive effect between parallel layers. If your +5V line tends to be noisy, it’s advisable to place the copper pour with the low-noise voltage reference on top of the ground plane. However, if you’re not dealing with low-noise requirements, there shouldn’t be any issues.
Building on what others have mentioned, a key advantage of utilizing additional ground or power planes—even if they are partial in your 4-layer PCB design is the significant reduction in the effective impedance of those planes. This can improve the overall stability of your design, especially in scenarios where localized power distribution or noise reduction is crucial.
To maximize this benefit, ensure there are sufficient stitching vias connecting the primary ground plane on Layer 2 to any additional ground pours or partial planes on other layers. The same principle applies to power planes: doubling up multiple power planes across layers and stitching them effectively with vias can halve their impedance, improving power delivery and noise performance.
If your design budget allows for buried vias, you can achieve these connections without consuming routing space on the outer layers. However, this approach is most relevant in high-density designs where board real estate is extremely constrained. For less complex layouts, stitching vias on the outer layers can still provide significant benefits without the need for more advanced manufacturing processes.
Your proposed stack-up appears to work well for a 4-layer PCB design. However, it’s important to consider the coupling between the 5V plane in Layer 3 and the ground plane in Layer 4. The 5V plane will rely entirely on the Layer 4 ground plane for its return path.
If you decide to pour multiple localized power planes (non-5V) in Layer 4, ensure that you do not cut off the 5V return path. Interrupting this return path could increase loop inductance and potentially degrade signal integrity or create EMI issues. Careful placement of the additional power pours, along with sufficient stitching vias, will help maintain reliable operation.