Designing a 6 Layer Stackup for Enhanced EMC
Designing a multilayer board is like putting together a great sandwich. The right arrangement of components can be satisfying in both cases. You won’t have to worry about signal integrity in your BLT, but you will have to design your PCB layer stack to keep your signals clean.
6 layer PCBs are an economical and popular stackup for a variety of applications with high net count and small size. Larger boards might work fine with a 4-layer stackup, where signal layers can be sacrificed to ensure isolation between each side of the board. With the right 6-layer stackup, you can suppress EMI between different layers and accommodate fine-pitch components with high net count. However, there are cases where it makes more sense to use a 4-layer or 8-layer stackup, and it helps to understand the function of plane layers in the board to make this judgement.
How Many Power, Ground, and Signal Planes Do I Need?
The answer to this question is extremely important and really depends on the application for your board. If you are routing a dense board with limited space, you’ll want to opt for one power, one ground, and four signal planes. If you need to significantly reduce susceptibility to EMI, you should opt for more ground and fewer signal layers. The arrangement of ground planes will have a significant shielding effect in your PCB without the need for an inelegant solution like shielding cans.
If you will be mixing digital and analog signals, mixing high and low frequency signals, or a combination of all of these, you can still make some creative use of a 6-layer PCB stackup. At some point, you might need to opt for a larger board or more layers in your stack (or both!). There are many signal/plane layer of combinations for 6 layer PCB stackups, but a few common ones will be shown below.
With this in mind, let’s jump dive into a few 6-layer PCB stackups:
Signal Layer/Power/2 Signal Layers/Ground/Signal Layer
This 6-layer PCB stackup that is a popular entry-level option that provides shielding for low speed traces from higher speed traces while providing tight coupling to solid planes. You can route signals with lower frequency/slower switching speeds or through an interior layer as long as they are orthogonal. I would route higher speed digital or higher frequency analog signals on the outer layers in order to shield them from each other and the lower speed/frequency traces on the inner layers.
On this, I would not mix analog and digital in the inner layers unless you can separate them into different regions of the board. However, in that type of situation where you need separation between digital and analog sections, you can probably make due on a 4-layer stackup with internal planes and some creative layout/routing. With an 8-layer board, you can have 2 plane layers around the core that provide shielding for the 2 internal signal layers.
The main problem with this is the lack of interplane capacitance between the power and ground plane layers. Because these plane layers are separated, more decaps will be needed to compensate, or the planes need to be made larger. For this reason, these boards should probably not be used with very high speed digital signaling as decoupling can get difficult.
Signal Layer/Ground/Power/Ground/Signal Layer/Ground
This is a good asymmetric stackup for boards that need to mix high speed and low speed signals while providing high shielding for an internal layer. The interior signal layer will be shielded from the surface signal layer as it is encased between two ground planes. It is also useful for suppressing EMI from interfering with the interior signal layer as the solid conductors provide effective shielding. The power and ground planes will likely be closely spaced to provide effective decoupling for high speed digital and RF devices. It is a good idea to place grounded vias between the alternating ground/power/ground plane layers around the outline of the board in order to suppress radiated EMI from the board edge.
The main problem with this stackup is that it only allows easy component placement on the top layer unless you start cutting out ground from the bottom layer to make room for components. This is an expensive proposition for fab as it requires a lot of drilling to place vias to the internal signal layer. It highlights the advantages of a 4-layer or 8-layer PCB stackup. With an 8-layer stackup, you can create a similar arrangement of adjacent power/ground in the internal layers while also accommodating internal routing and components/routing on the bottom layer.
Ground/Signal Layer/Power/Ground/Signal Layer/Ground
If your board will be deployed in an electrically noisy environment, or if it will be placed near a board that emits strong radiation, this stackup provides excellent EMI suppression. It also provides high isolation between the signal layers. The downside is that there are only two signal layers, so board space for routing signals will be limited. That being said, placing the signal layers between stacked conductors is a good choice from an EMC standpoint.
You can also place mounting pads on the surface layers for components, and nearby grounded pour on the surface layer provides additional shielding. If designed to the right tolerances, you’ll be able to easily route signals and power to your components with vias. Again, this can be expensive from a fabrication standpoint as more drilling and plating will be needed to produce the board.
This layer stack provides another not-so-obvious benefit: better thermal management. If you will be working with high currents, the conductors on each side of a signal layer can absorb heat and transport it to the board edge, where it can be dissipated with passive or active cooling. You won't have the same level of heat dissipation as you would with a metal-core board or a ceramic, but you've got the advantages of multiple planes for shielding to aid EMI suppression.
A Note on Routing Between Multiple Layers
We often talk about routing vias through multiple layers, but doing this can create a discontinuity in the return path that increases the loop area for the circuit. In this case, the parasitic capacitance for the board will provide some discharge that induces a return current near the signal via. Unfortunately, the capacitance is usually too small to provide a low reliable impedance return path. For this reason, the return path will appear in the nearest decoupling capacitor, which might be far from the signal via.
One option is to place a decoupling capacitor in parallel with the signal via to provide the return path. A possibly better option is to place a grounded via running alongside the signal via as long as the two reference planes are at the same potential. This keeps a return path with low inductance and without breaking the coupling to the reference planes.
Integrated circuits should contain a nearby bypass capacitor that connects directly to the same reference plane as the signal vias/traces. This helps reduce fluctuations in the supply voltage, provides a charge reservoir that combats ground bounce, and provides a path for the induced return current for signals that transition between layers.
Your PCB design package should include the tools you need to design your stackup entirely from scratch. With Altium , you’ll have full control over your layer arrangement, material constants, and dimensions. You’ll even be able to use the layer stack manager to create rigid-flex and multi-board systems with ease. All these design tools integrate directly with your schematic design, layout, and deliverable generation tools in a single program.
Download a free trial of Altium to see how the powerful tools give you full control over your board. You’ll also have access to the best design features the industry demands in a single program. Talk to an Altium expert today to learn more.
Trade In Your Outdated PCB Design Tool & Unlock 45% OFF Altium today!