After extensively researching the topic why it’s a bad idea to separate ground or power in mixed analog and digital circuits. I’ve decided to implement a 4-layer PCB design with full GND and VCC planes inside, and the signal routing outside.
However, I’m still uncertain about the necessity and effectiveness of including a VCC plane. While some sources suggest that having separate GND and VCC planes, with a dielectric in between, can act as a decoupling capacitor, others argue for using two ground planes and routing power like another signal, with appropriate width.
In my specific scenario, routing the entire power net may pose some challenges but is not entirely impossible. Therefore, I’m seeking advice on the advantages and disadvantages of including a VCC plane in my design.
It’s true that the ground plane and power plane essentially form a parallel plate capacitor. Depending on size and spacing, you might expect something like 20 pF per square inch. Supposing you have a 6” by 6” PCB, that would be 720 pF. That’s a value quite close to the nominal decoupling cap, plus, it’s everywhere (assuming complete planes). Both the ground plane and power plane will form a shield for suppressing EMI. They will also give the lowest possible impedance to the power and ground nets.
For a four layer stackup that leaves you 2 layers for routing. I’ve always found this stackup works well for most designs, so I would recommend it.
For some circuits that may be fine although maybe not so much for others. Using a VCC layer for return path might be ok if all signals reference that VCC, but many designs have multiple VCC values and referencing the wrong one can create issues. Inner layer capacitance is only something you can rely on if the GND and VCC layers are close to each other (like in the less than 6 mil range where thinner is better for plane capacitance). The concern with 4 layer boards are most are 62mils thick which means the dielectic between the two inner layers might be in the 40mil range if you do not specify what you want and resulting plane capacitance is likely be nearly nonexistent.
In some cases, you might be better off with both inner layers as GND and pouring VCC on the outside layers with the components and routing.
It all comes down to what the circuits need and can live with. This is a subject where multiple opinions exist and some methods work better for certain circumstances.
If you circuit includes high data rate signals and you need to move these signals from top layer to the bottom layer then the option propose by Timothy is the best option: Ground in the inner layers and Vcc and signals in the top and bottom. Doing like this the return path is much cleaner and free of resonances.
Vcc and GND has to be as closer as possible because the capacitance between both planes increase and the loop inductance decrease. If Vcc is located on the top, the distance between top and 2nd layer will be always smaller as the distance between 2nd and 3rd layer.
We choose to designate the 0V net as a plane initially because many components require connection to this node, and numerous return currents flow through it. Routing all these connections with individual traces can be complex and messy. By assigning this node to Layer 2 (L2) as a plane, it simplifies the routing for the rest of the design.
If you have multiple components that need to connect to the same power node and anticipate numerous signal return currents through this node, using a plane is a practical choice. However, achieving tight coupling to the ground plane, which is essential for high frequencies, is challenging with a standard 4-layer stackup. This consideration often requires a 6-layer board or a custom 4-layer stackup.
Here are reasons why power planes may not be suitable for regular 4-layer boards:
In standard stackups, the power plane may not be tightly coupled to ground, impacting high-frequency performance.
High-frequency currents are typically kept local, so the power net mainly carries low frequencies, making routing feasible.
For mixed-signal boards, different power nodes are often specific to certain areas, reducing the need for a continuous plane across the entire board.
The decision to forego a power plane in a 4-layer board is fairly simple: it allows you to use that layer for other critical routing. Trying to route power without a plane can be challenging as it tends to spread everywhere across the board.
The main purpose of having two ground planes in a 4-layer board would typically be for shielding, especially if they are positioned on the outer layers.
Consider whether your circuit truly requires shielding due to noise sensitivity or capacitive plane coupling for high-frequency signals. Assess whether the signal density and power routing demand a third signal layer, which is likely unnecessary for most designs. In such cases, prioritize ease of routing over unnecessary complexity.
In a typical 4-layer PCB stack-up, the decoupling capacitance the power plane provides is quite low, ranging from about 10-30pF/in^2. This level of decoupling is more beneficial for high-frequency signals in the 100MHz+ range, which may be fine for many designs operating at lower frequencies.
However, maintaining a continuous ground plane is crucial to a good PCB design. This helps minimize inductance and resistance on the ground plane, which is essential to signal integrity.
The power plane doesn’t necessarily need to cover the entire layer and can consist of traces or polygon pours carrying different power planes. RF designs require careful consideration of power plane design to prevent unintentional radiation.
The ground and power plane design is less critical for designs that don’t involve signals above 50MHz. A continuous ground plane is essential for these signals if transmission lines are used, although decoupling capacitors can also be used as an alternative solution.
In most 4-layer designs, I typically place the ground and power layers in the middle. The main signal layer is placed adjacent to the ground layer on the top, while the bottom layer is also used for signals, particularly for slower signals.