Design PCBs for EMI, part 2: Basic stack-up

Kenneth Wyatt -March 20, 2019

Part 1 of this series described how digital signals propagate through PC boards [Refs. 1, 2, 5, 6]. In part 2, we look at specific board designs to achieve low EMI. The biggest issue I see in my clients’ board designs is poor layer stack-up.

Reiterating the two fundamental rules from part 1 and realizing digital signals and power (transients) are electromagnetic waves moving in the dielectric layer, we see there are two very important principles when it comes to PC board design:

  1. Every signal and power trace (or plane) on a PC board should be considered a transmission line.
  2. Digital signal propagation in transmission lines is really the movement of electromagnetic fields in the space between the copper trace and GRP.

To construct a transmission line, you need two adjacent pieces of metal that capture or contain the field. For example, a microstrip over an adjacent ground return plane (GRP) or a stripline adjacent to a GRP, or a power trace (or plane) adjacent to a GRP. For example, locating multiple signal layers between power and ground reference planes will lead to real EMI issues for fast signals. Observing these two rules will dictate the layer stack-up.

In other words, every signal or power trace (routed power) must have an adjacent GRP and all power planes should have an adjacent GRP. Multiple GRPs should be tied together with a matrix of stitching vias. In this article, we’ll examine several stack-up designs.

Typical six-layer design (Altium) Design PCBs for EMI, part 2: Basic stack-up

One stack-up I frequently see is this six-layer design (Figure 1). This probably worked well enough in the 1990s through the early 2000s, but with today’s much faster and mixed-signal technologies, it’s a recipe for EMI disaster. There are two issues with this: the bottom two signal layers are referenced to the power plane and the power and ground return planes are non-adjacent and too far apart.

6 layer board stackup
Figure 1. A very common, but poor, EMI stack-up design (6-layer example). Signal layers 4 and 6 are referenced to power, while the GRP and power planes are non-adjacent with two signal layers in between. This will couple power transients on those two signal layers.

With few exceptions (some DDR RAM power and signals, for example) currents want to return to their sources, which are referenced to the GRP. Referencing these signals to the power plane is very EMI-risky, because there is no clearly defined return path, except through plane-to-plane capacitance, which in this case is relatively small. In addition, these gaps in the return path result in field leakage into other areas of the board’s dielectric layers. That, in turn, leads to cross-coupling and radiated EMI.

The second issue occurs when we have the power and GRP separated by two signal layers. Any power network transients will cross-couple within the dielectric layers, coupling to any signal traces on layers 3 and 4 along the way. You also lose any plane-to-plane capacitance benefit if these planes are separated by more than 3-4 mils.

The following are several ideas for PC board stack-ups that comply with the transmission line aspects of digital signal propagation.

Four-layer board: Design PCBs for EMI, part 2: Basic stack-up 

A good four-layer board stack-up for improved EMI (Figure 2). Instead of a power plane, we use either routed or poured power, along with signals on layers 2 and 3. Thus, each signal/power trace is adjacent to a GRP. Also, it’s easy to run vias between all layers, so long as the two GRPs are connected together with a matrix of stitching vias. If you run a row of stitching vias along the perimeter (say, every 5mm) you form a Faraday cage.

four layer PCB stackup
Figure 2. This good four-layer board stack-up for improved EMI keeps the signals and routed power near the ground reference planes.

Four-layer board: Design PCBs for EMI, part 2: Basic stack-up
If, on the other hand, you’d prefer to have access to the signal and routed/poured power traces, you may simply reverse the layer pairs, such that the two GRP layers are in the middle and the two signal layers are positioned at the top and bottom, with routed power and sufficient decoupling caps, rather than a power plane (Figure 3).

four layer PCB stackup
Figure 3. This good four-layer board stack-up for improved EMI places the ground reference planes inside the board.

For both four-layer designs, you want to run a pattern of stitching vias connecting the two GRPs about 1cm apart, maximum.

Eight-layer board (Altium) Design PCBs for EMI, part 2: Basic stack-up

Both the four- and eight-layer board designs (Figure 4) follow the two fundamental rules that preserve good transmission line design. In addition, for the eight-layer design, the power and GRP planes are now 4 mils apart, providing fairly good plane-to-plane capacitance. Closer would even be better. For example, a spacing of 1 mil to 3 mils is ideal for minimizing EMI. All GRPs should be stitched together with a 1 cm pattern of vias.

8 layer PCB stackup
Figure 4. A good EMI stack-up design (8-layer example). All signal layers are referenced to an adjacent GRP, while power is also referenced to an adjacent GRP.

Of course, there are many more iterations on creating proper transmission line pairs between signal and GRP or power and GRP.

What about two-layer boards?
Simple, just run signals and routed power on layer 1 and use a GRP on layer 2. Well, that may have worked in yesterday’s technology. in today’s technology, we often need to use at least two layers to run signals. The answer is to run “triplets” with a ground return trace between two signal traces (Figure 5). This was an idea from Daniel Beeker, Senior Applications Engineer with NXP Semiconductor [Ref 5].

two-layer PCB design for minimizing EMI
Figure 5. An example of routed triplets for signals, as well as attempting to preserve the transmission line principles for routed power. Courtesy: Daniel Beeker, NXP Semiconductor

Here, we see an attempt to preserve the transmission line properties for the routed power. The example also shows analog signal traces with a ground return trace between them—a routed “triplet.” Because the electromagnetic field is captured adequately between each signal trace and the return trace, there is little field leakage.

If you’d like to learn much more about designing for EMI compliance in your PC boards, I’d also recommend Rick Hartley as an excellent source with his 2-day seminar (Reference 6). Finally, I have to thank Ralph Morrison, Dan Beeker, and Rick Hartley, who really taught me about fast signals in circuit boards [Refs 3, 4, 5, 6].
Part 3 of this series will address partitioning of circuit sections, routing of high-speed traces, and a few other layout practices to help reduce EMI.
Please contact us for more detail.