Learn how to stack-up a board's trace, power, and return layers to minimize interference.
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:
- Every signal and power trace (or plane) on a PC board should be considered a transmission line.
- 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)
One stack-up I frequently see is this six-layer design (Figure 1). This probably worked well enough in the 1990s through early 2000s, but with today's much faster and mixed signal technologies, it's 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.
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 a several ideas for PC board stack-ups that comply with the transmission line aspects of digital signal propagation.
Four-layer board: Design 1
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 board: Design 2
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).
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)
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.
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].
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].
- Schmitt, Ron, Electromagnetics Explained - A Handbook for Wireless/RF, EMC, and High Speed Electronics, Newnes, 2002.
- Bogatin, Eric, Signal Integrity - Simplified (3rd edition), Prentice Hall, 2018.
- Beeker, Daniel, Effective PCB Design: Techniques To Improve Performance.
- Hartley, Rick, Control of Noise, EMI and Signal Integrity in PC Boards (2-day seminar), Rick Hartley Enterprises.
- Morrison, Ralph, Digital Circuit Boards: Mach 1 GHz, Wiley, 2012.
- Morrison, Ralph, Fast Circuit Boards: Energy Management, Wiley, 2017.
—Kenneth Wyatt is president and principal consultant of Wyatt Technical Services.
- Design PCBs for EMI, part 1: How signals move
- PCB’s top ground plane and its effect on a microstrip line’s characteristic impedance
- 7 Tips for overcoming PCB EMI issues
- Manage EMI in PCB design: EMI sources and solutions
- Return path discontinuities and EMI: Understand the relationship
- Designing Ethernet links for EMI compliance
- RFI: keeping noise out of your designs
- Eliminating EMI protection components