- pcb007 Magazine
Getting to Know Your Designer
In this issue, we examine how fabs work with their design customers, educating them on the critical elements of fabrication needed to be successful, as well as the many tradeoffs involved. How well do you really know your customer? What makes for a closer, more synchronized working relationship?
In this issue, the biggest names in PCB manufacturing share their economic outlook for the upcoming year and beyond. As you will see, they were all bullish on our industry, but there was some apprehension as well. No one wants to get burned by another the supply chain disruption.
- Events||| MENU
- pcb007 Magazine
Estimated reading time: 7 minutes
By Barry Olney
< Back To Columns
Beyond Design: Standing Waves in Multilayer PCB Plane Cavities
Plane cavities in multilayer PCBs are essentially unterminated radial transmission lines. They form a transmission line that propagates electromagnetic (EM) energy within a plane cavity emanating from a feed point within the plane and outward in all directions. Like all transmission lines, it will reflect if not terminated. This creates standing waves—ringing. The bigger the mismatch, the bigger the standing waves, and the more the impedance will be location-dependent. As frequency and edge rates continue to increase, the impact of intrinsic electrical characteristics becomes more pronounced. AC switching currents in the power/ground planes can be very large. Under these circumstances, a plane pair acts more like a radial transmission line rather than a distributed planar capacitor.
A parallel plate capacitor (or a planar pair) has two conductors separated by a dielectric layer. Most of the electromagnetic energy in the structure is concentrated directly between the plates. However, some of the energy radiates into the area outside the plates. The electric field lines associated with this effect are called fringing fields (Figure 1).
When displacement current flows through the impedance of a cavity between two planes, it generates voltage. Although quite small (typically in the order of 5 mV), the accumulated noise from simultaneous switching devices can become significant. This voltage, emanating from the vicinity of the signal via, injects a propagating wave into the cavity, which can excite the cavity resonances or any other parallel structure (for instance, between copper pours and planes). Other signal vias also passing through this cavity can pick up this transient voltage as crosstalk. When the wave meets the PCB edge, the two reference planes form a slot antenna that will radiate noise with the potential to generate electromagnetic interference (EMI) to nearby equipment.
The more switching signals that pass through the cavity, the more noise is induced into other signals. It impacts vias all over the cavity, not just the ones in proximity to the aggressor signal vias. This cavity noise propagates as standing waves spreading across the entire plane pair. This is the primary mechanism by which high-frequency noise is injected into cavities: by signals transitioning through cavities, using each plane successively as the signal return path.
Cavity resonance also affects the power/signal return layers at the edges of the PCB. Edge effects can be particularly problematic since it is the board edges that are in such proximity to the chassis and, hence, the radiation fields can induce currents into the chassis frame.
When the cavity has open-end boundary conditions, resonances arise when a multiple of half wavelengths can fit between the ends of the cavity. If the clock or data harmonics overlap with the cavity resonant frequencies, there is the potential for long-range coupling between any signals that run through the cavity. This is one reason why all return planes should be GND layers, so that stitching vias between GND planes can be placed adjacent to each signal via transition to minimize the possibility of exciting the cavity resonance. Figure 2 shows a standing wave produced by the superposition of two harmonic waves of equal amplitude, frequency, and wavelength moving in opposite directions.
A region under a large BGA densely populated with vias also appears as a discontinuity due to the large array of anti-pads eating a hole in the plane. A discontinuity reflects propagating energy because it represents a mismatch with the characteristic impedance of the transmission line.
The edges of the board cause the greatest amount of reflection since an edge is a totally abrupt open circuit surrounding the board. Reflected energy is accompanied by phase reversals in its components, and combined reflections from the open circuit at the edge of the board can cause a phenomenon known as voltage doubling, creating a standing wave. The standing wave appears to be vibrating vertically without traveling horizontally.
There are various approaches to reducing radiation edge effects from the PCB. In many cases, energy can be reflected, possibly creating additional internal cavity resonance effects and coupling to internal vias, and resulting in increased radiation. When plane pairs resonate, their emissions come from the fringing fields at the board edges. With ground/power plane pairs, edge-fired emissions can be reduced by reducing the plane separation and lowering the AC impedance. Alternatively, make the power planes slightly smaller (~200 mil) than the GND plane. This modifies the pattern of the fringing fields, pulling them back from the edge, and may help reduce emissions to some extent.
Edge plating, as the name suggests, is the process of plating the edges around the PCB. This is an elegant (but expensive) solution to prevent emissions from extremely high-speed SerDes signals on terabit routers, etc., but is an overkill for a typical high-speed design.
Another way to mitigate this problem is to create a via fence, stitched to ground around the perimeter of the PCB. If the spacing between the stitching vias is less than or equal to 1/12th of a wavelength, the via fencing will appear as a short circuit, causing the propagating wave to be reflected back to the source rather than being launched from the PCB edge. Unfortunately, most of the above techniques create reflections and possibly exasperate the issue.
Parallel planes in multilayer PCBs exhibit multiple resonances, which increase the impedance and the EM radiation. A typical FR-4 laminate of 4-mil thickness produces a characteristic impedance of about 3 to 5? for adjacent planes. The larger the plane area, the lower the impedance.
The best solution to dampen the plane resonance is to terminate the transmission line with an impedance-matching resistive element along the board edges. But in practice, this means approximating a continuous structure with resistors spaced around the perimeter. Obviously, multiple low-value resistors cannot be placed directly between the power supply and ground as it would needlessly dissipate a huge amount of DC power. To prevent this, they should be AC coupled with a ceramic capacitor of sufficient capacitance to allow the resulting impedance to appear predominately resistive at and above the lowest frequency of interest. A 10nF, X7R ceramic capacitor is a typical value. The addition of loss to dampen modal resonances is more important than the exact termination value and distribution. Notice how the 20-series RC terminations of 3R5? and 10nF (blue) dampen the plane resonance, pushing the effective PDN impedance (Zpdn) down below the resonance, above 200MHz (Figure 3b).
A standing wave can be generated at switching locations within the interior of the PCB. Therefore, there may be hot spots within that cavity that would benefit from the placement of an additional AC-coupled load at or near the source.
Reflections occur in a transmission line only when there is a discontinuity. If the edge of the board is terminated in the characteristic impedance of the radial transmission line, then the EM energy will be absorbed and there will be no reflections. This will not eliminate the initial transient but does, however, prevent it from being compounded. Termination elements inhibit standing waves from developing between the planes and protect peripheral signals and electronics from radiation.
- Plane cavities in multilayer PCBs are essentially unterminated radial transmission lines that will reflect if not terminated.
- The energy that radiates from the edges of the plane pair is called a fringing field.
- When displacement current flows through the impedance of a cavity between two planes it generates voltage.
- Signal vias passing through a plane cavity can pick up the transient voltage as crosstalk.
- A standing wave is produced by the superposition of two harmonic waves of equal amplitude, frequency, and wavelength moving in opposite directions.
- Standing waves impact vias all over the cavity, not just the ones in proximity to the aggressor signal vias.
- All return planes should be GND layers, so that stitching vias between GND planes can be placed adjacent to each signal via transition to minimize the possibility of exciting the cavity resonance.
- A region under a large BGA densely populated with vias also appears as a discontinuity due to the large array of anti-pads eating a hole in the plane.
- The edges of the board cause the greatest amount of reflection since an edge is a totally abrupt open circuit surrounding the board.
- The standing wave appears to be vibrating vertically without traveling horizontally.
- Parallel planes in multilayer PCBs exhibit multiple resonances, which increase the impedance and the EM radiation.
- The best solution to dampen the plane resonance is to terminate the transmission line with an impedance-matching resistive element, along the board edges.
- Beyond Design by Barry Olney: “Dampening Plane Resonance with Termination,” “Plane Cavity Resonance,” “Fringing Fields.”
- Signal and Power Integrity—Simplified, 3rd ed., by Eric Bogatin.
- “Optimized Power Delivery Performance Using Plane Terminations,” by Istvan Novak, Samtec. Published in 2020 IEEE 24th Workshop on Signal and Power Integrity (SPI).
- US5708400A—AC coupled termination of a printed circuit board power plane in its characteristic impedance, Google Patents, Terrel Morris, Hewlett-Packard.
This column originally appeared in the July 2023 issue of Design007 Magazine.
More Columns from Beyond DesignBeyond Design: Embedded Capacitance Material
Beyond Design: Return Path Optimization
Beyond Design: Just a Matter of Time
Beyond Design: Design Success with IPC Standards
Beyond Design: Integrating AI Into PCB Design Flow
Beyond Design: Balancing Trade-offs for Optimal PCB Design
Beyond Design: Select Dielectric Material With Precision
Beyond Design: Containing Electromagnetic Fields in Wireless PCB Design