Call for pcb design tutorials - Learn the basics of PCBs and the information needed to get started designing your first PCB
  1. Blog>
  2. Why Some PCBs Need Edge Plating?

Why Some PCBs Need Edge Plating?

by: Dec 04,2020 1793 Views 0 Comments Posted in Technology

pcb edge plating

Some people may have seen many industrial pcb boards or RF pcb boards with a circle of vias and copper tape around them, and even some RF pcb boards will be metalized around the sides of the board. What is the purpose of the edge plating?

As the system rate of each product increases, not only the timing of high-speed digital signals, signal integrity issues are particularly prominent, but also the electromagnetic interference caused by the system from medium-high-speed digital signals and EMC issues caused by power integrity are also very obvious. The electromagnetic interference generated by high-speed digital signals will not only cause serious mutual interference within the system, but also reduce the anti-interference ability of the system. At the same time, it will also generate strong electromagnetic radiation to the outer space, causing the electromagnetic radiation emission of the system to seriously exceed the EMC limit standards, so that the product cannot pass the EMC standard certification. The radiation on the side of the multilayer pcb board is a relatively common source of electromagnetic radiation.

When the unexpected current reaches the edge of the ground plane and the power plane, edge radiation is generated. These are unexpected currents that may come from grounding and power supply noise caused by insufficient power supply bypass. The cylindrical radiating magnetic field generated by the inductive via will radiate between the various layers of the circuit board and will eventually gather at the edge of the circuit board. The strip line return current carrying high frequency signals is too close to the edge of the circuit board.

The cause of power supply noise usually lies in two aspects:

1. Under the high-speed switching state of the device, the transient alternating current is too large.

2. It is the inductance that exists on the current loop.

From the perspective of manifestation, it can be divided into three categories:

1.Synchronous switching noise (SSN), sometimes called ΔI noise, can also be attributed to this type of ground bounce.

2.Influence of non-ideal power supply impedance.

3.Resonance and edge effects.

In high-speed digital circuits, when the digital integrated circuit is powered on, the internal gate circuit output will undergo a state transition from high to low or from low to high, that is, the transition between "0" and "1". In the process of change, the transistors in the gate circuit will continuously turn on and off. At this time, current will flow from the connected power supply to the entry circuit, or from the gate circuit to the ground plane, so that the current on the power plane or ground plane Produce imbalance, thus produce an instantaneous current △I.

When this current flows through the return path, the existing inductance will cause a drop in AC voltage, which will cause squeaking noise. If there are many output buffers that simultaneously undergo state transitions, this voltage drop will be large enough to cause incomplete power supply. This noise is called Simultaneous Switch Noise (SSN).

The AC noise of the power supply will be between the power layer and the ground layer. The resonant cavity mode of these two planes is used to conduct the AC noise, and it will be radiated into the free space when it reaches the edge of the plane. This will cause the product EMI standard test to fail and fail to reach EMI certification standards.

The figure above is a schematic diagram of Simultaneous Switching Noise (SSN) using the resonant cavity between the power plane and the ground plane to propagate AC noise. Of course, such a resonant cavity not only propagates SSN AC noise, but may also propagate high-speed signal noise if the signal integrity is not done well.

For the noise generated by the vias, the signal lines interconnected on the PCB include the microstrip line on the outer layer of the PCB, the stripline on the inner layer between the two planes, and the electroplated vias for the signal change layer connection (via subdivided into through via, blind vias, buried vias), the microstrip line on the surface and the stripline between two planes can control radiation well through a good reference plane stack structure design.

The via runs through multiple stacks in the vertical direction. When the high-frequency signal transmission line passes through the via hole to change the layer, not only the impedance of the transmission line changes, but the reference plane of the signal return path also changes. When it is relatively low, the effect of the via on the signal transmission can be completely ignored.

However, when the signal frequency rises to the radio frequency or microwave frequency band, the current return path changes due to the change of the reference plane of the via. The TEM wave generated by the via will propagate laterally between the resonant cavity formed by the two planes, and finally radiate out into the free space through the edge of the pcb, causing the EMI index to exceed the standard.

It is known that for high-frequency and high-speed pcb boards, edge radiation problems will occur on the sides of the pcb boards, so how to protect them?

There are three elements that cause EMC problems: electromagnetic interference source, coupling path and sensitive equipment.

We can't control sensitive equipment. And we can add a metal shielded equipment enclosure or something to cut off the coupling path. Here, we will focus on how to remove interference sources.

First of all, we must optimize the key signal traces on the PCB to avoid EMI problems. There are more than vias for changing layers. We can put ground vias around the key signal vias to provide additional return paths for the key signal vias. 

For reducing PCB edge radiation, there is a 20H rule mentioned before. The 20H rule was first proposed by W. Michael King in 1980 and elaborated by Mark. I. Montrose in his works. It is often listed as an important EMI design rule. H refers to the thickness of the board, that is, the power plane is reduced by a distance of 20H from the ground plane.

In order to reduce the effect of edge radiation, the power plane should be retracted compared to the adjacent ground plane, and the effect of shrinking the power plane by 10H is not obvious. When the power plane is retracted by 20H, 70% of the marginal flux boundary is absorbed; when the power plane is retracted by 100H, 98% of the marginal flux boundary can be absorbed; therefore, the retracted power layer can effectively suppress the marginal effect caused by Radiation.

We believe that the 20H rule is no longer suitable for the current high-frequency and high-speed PCB design. The previous printed circuit board area was large, and the resonant frequency of the planar antenna caused by indentation was not obvious; Nowadays, due to the small PCB board surface, the radiation intensity of the retracted power layer design changes significantly with different resonant points of the retracted power layer size, resulting in higher radiation energy at high frequencies.

The use of indentation by 20H cannot completely solve the decrease in radiation. Although the frequency below 430MHz is improved, and 40H improves the frequency below 590MHz, the reduction in area makes the resonance frequency higher, and the radiation suppression for higher resonance frequency bands, which is not helpful.

Then, to remove the interference source of the side radiation of the pcb board, a shielding structure must be used to process the edges, thereby reflecting the noise back into the inner space, which will increase the voltage noise on these layers, but the edge radiation will also be reduced. The low-cost implementation method is to punch a circle of ground vias around the PCB board with a 1/20 wavelength hole pitch to form a ground via shield to prevent external radiation of TME waves.

As for the microwave circuit board, the wavelength is further reduced, and because the current PCB board production process cannot make the distance between the holes and the holes small, at this time, the method of punching shielding vias around the pcb board with a pitch of 1/20 wavelength has no obvious function for the microwave board. So it is necessary to adopt the method of edge plating. Enclose the edge of the entire pcb board with metal, so that the microwave signal cannot be radiated from the edge of the pcb board.

For some sensitive circuits of radio frequency and microwave pcb boards, as well as circuits with strong radiation sources, you can design a solder shielding cavity on the pcb board. The pcb should be designed with a "through hole shielding wall", that is to add a grounded via on the PCB board and the part close to the shielding cavity wall. In this way, a relatively isolated area is formed.

The design requirements for via-hole shielding walls are as follows:

  • There are more than two rows of vias;
  • The two rows of vias are staggered;
  • The pitch of vias in the same row should be less than λ/20;
  • No solder mask is allowed at the place where the grounded PCB copper foil is crimped with the shielding cavity wall.


PCBWay provide service including PCB Prototype & Batch Production, PCB Assembly (SMT), PCB Design and Electronics Modules Selling. We are committed to meeting the needs of global makers from different industries in terms of quality, delivery, cost-effectiveness and any other demanding requests in electronics.

 Click to Get Your Instant Quotation 

  • Comments(0)
You can only upload 1 files in total. Each file cannot exceed 2MB. Supports JPG, JPEG, GIF, PNG, BMP
    View More
    Back to top