RF PCB Materials, Isolation and Shielding: EMC Design Guide

Mobile communications has grown rapidly over the past decade, and EMC has become a design constraint that must be handled deliberately at every stage: circuit design, test, installation, and operation and maintenance. The problem exists at three levels at once, between systems, between pieces of equipment, and between the devices packed inside a single enclosure. Among the available EMC control techniques, shielding, filtering, and grounding are the three most fundamental interference suppression methods, and all three work toward the same goal: cutting off the path along which interference travels.

RF circuits have characteristics that make RF PCB design diverge from digital PCB design, so the rules cannot simply be carried over. This article examines EMC design for RF boards through five lenses: base material selection, isolation and shielding, filtering, grounding, and routing. The first two are covered here, starting with the laminate decision that sets the electrical baseline for everything that follows, then moving to the physical separation and shielding practices that keep transmit energy out of sensitive receive nodes.

Highlights:

FR-4 is specified at a dielectric constant of 4.25 ± 0.2 measured at 1 GHz. That tolerance is wide enough to shift the distributed capacitance between components and the board, which in turn moves circuit resonant frequencies and filter center frequencies, and its loss is too high for high-power RF stages.
Typical spatial isolation inside an RF PCB is about 50 dB. When the same-frequency gain of a cascaded amplifier chain, or the cascaded out-of-band attenuation, switch isolation, or attenuation inside one cavity, exceeds 30 to 50 dB, a metal shield plate soldered or mounted on the board becomes mandatory.
A shielding cavity needs a via fence of at least two staggered rows of grounded vias spaced closer than λ/20, a solder-mask-free wall footprint, and slot doors taller than 0.5 mm that keep at least 1 mm between the signal trace and the shield body.

1. Base Material Selection

Developers generally have to choose a laminate by weighing circuit characteristics against product cost. The RF laminates available fall into two categories: general-purpose laminates and RF-specific laminates.

General-Purpose Laminates

The standard general-purpose material is FR-4, a flame-retardant copper-clad epoxy glass cloth laminate. Its dielectric constant, measured at 1 GHz, is Er = 4.25 ± 0.2. Two variants of the base laminate are in common use:

Standard laminate: glass transition temperature Tg = 135 °C, low cost, and a mature process.
UV-blocking laminate: Tg = 140 °C, with a UV-blocking function that shields the material from ultraviolet light. Its performance is better than the standard laminate at the same price.

Compared with specialty RF laminates, both variants are electrically unstable and lossy. When the dielectric constant drifts, the distributed capacitance between circuit components and the PCB drifts with it, and that change pulls the resonant frequency of the circuit and the center frequency of filters away from their design values. RF power amplifier circuits are considerably more sensitive to loss. For these reasons, general-purpose laminates are not recommended for high-power circuits.

RF-Specific Laminates

RF-specific laminates are supplied by two vendors, TACONIC and ROGERS. TACONIC offers a well-regarded product line, a complete range of specifications, and moderate pricing. Its materials, with dielectric constant measured at 10 GHz unless noted otherwise, are listed below.

Laminate	Test Frequency	Dielectric Constant
CER-10	10 GHz	10 ± 0.05
RF-35	1.9 GHz	3.5 ± 0.035
TLX-0	10 GHz	2.45 ± 0.04
TLX-9	10 GHz	2.50 ± 0.04
TLX-8	10 GHz	2.55 ± 0.04
TLX-7	10 GHz	2.60 ± 0.04
TLX-6	10 GHz	2.65 ± 0.04
TLC-27	10 GHz	2.75 ± 0.05
TLC-30	10 GHz	3.0 ± 0.05
TLC-32	10 GHz	3.20 ± 0.05

ROGERS materials offer high dielectric constant accuracy, good temperature stability, and low loss, and are therefore frequently used in high-power circuits. Their PCB fabrication and processing flow is the same as that of FR-4, which keeps processing cost low, but the adhesion of copper foil to the substrate is weaker.

Laminate	Test Frequency	Dielectric Constant
RO4350	10 GHz	3.48 ± 0.05
RO4003	10 GHz	3.38 ± 0.05

2. Isolation and Shielding

2.1 Isolation

Isolation in this context also includes simply opening up physical distance. When the input and output ends of a circuit are laid out inside the same shielding cavity, two basic approaches keep them apart.

The first is the in-line layout shown in Figure 1, where AT is an attenuator and A1 and A2 are amplifiers. The two stages sit in a straight line, with the attenuator between them, so that the output of the chain faces away from its input.

Figure 1 | In-line layout

Space constraints sometimes make an in-line layout impossible inside a single cavity, in which case an L-shaped layout is used, as shown in Figure 2. Here again AT is an attenuator and A1 and A2 are amplifiers. Within one shielding cavity, Z-shaped, U-shaped, and crossed layouts must not be used, because each of them folds the output back toward the input and creates a coupling path that the cavity wall cannot interrupt.

Figure 2 | L-shaped layout

Component Placement

Component placement inside the cavity determines whether the isolation designed into the circuit survives in hardware. The following points apply.

Pay attention to the signal flow path and to the interaction between components.
Inductive components must be protected against mutual inductance; place adjacent inductors perpendicular to one another.
Insert an attenuator at the receiver input. The attenuation an attenuator applies to an n-th order product is n times the attenuation it applies to the wanted signal. A 3 dB attenuator, for example, will reduce the third-order intermodulation product by 9 dB, while the attenuation of the wanted signal remains 3 dB. The layout of a three-resistor attenuator is shown in Figure 3(a).
The layout of the bias inductor for a low-power amplifier is shown in Figure 3(b).

Figure 3(a) covers the attenuator layout and 3(b) the bias inductor layout, together forming the placement examples used in RF front-end design.

Sensitive Circuits and Strong Radiators

RF signals radiate through air, so the coupling between an output and an input depends on how far apart they are placed. The greater the physical separation and the lower the operating frequency, the smaller the parasitic coupling between input and output and the greater the isolation. Typical spatial isolation on an RF PCB is about 50 dB. Certain sensitive circuits and strongly radiating circuits therefore need shielding measures. The circuits listed below should be shielded, but where shielding is difficult, for example because of space or cost constraints, it may be omitted provided the decision is confirmed experimentally. The list is as follows.

Receiver front end: a sensitive circuit. The signal level is very small, so shielding is required.
RF unit and IF unit: both must be shielded. In the receive path, the intermediate-frequency signal produces significant interference in the RF signal; conversely, in the transmit path, the RF signal radiates interference into the IF signal.
Oscillator circuit: a strong radiation source. The local oscillator source must be shielded separately, because its relatively high level creates substantial radiated interference in other units.
Power amplifier and antenna feed circuit: a strong radiation source. The signal is strong, so shielding is required.
Digital signal processing circuit: a strong radiation source. The steep rising and falling edges of high-speed digital signals interfere with the analog RF signals.
Cascaded amplifier circuit: the total gain may exceed the spatial isolation from the output back to the input, which satisfies one of the conditions for oscillation and can make the circuit self-oscillate. If the same-frequency gain inside the cavity exceeds 30 to 50 dB, a metal shield plate must be soldered or mounted on the PCB to increase isolation. In practice, the decision to add a shield plate is made by weighing frequency, power, and gain together.
Cascaded filter, switch, and attenuator circuits: inside one shielding cavity, the out-of-band attenuation of the cascaded filter circuit, the isolation of the cascaded switch circuit, and the attenuation of the cascaded attenuator circuit must remain below 30 to 50 dB. If the value exceeds this, a metal shield plate must be soldered or mounted on the PCB to increase isolation. As above, the actual decision weighs frequency, power, and gain.
Transmit and receive units: when these are interleaved on the same board, they must be shielded.
Mixed digital and analog circuits: clock lines must be isolated with a copper ground pour or shielded.

Shielding Materials and Methods

The shielding materials in common use are all highly conductive: copper plate, copper foil, aluminum plate, aluminum foil, steel plate, metal plating, and conductive coatings. Electrostatic shielding is used mainly to prevent the influence of electrostatic fields, and two essentials apply, a complete shield body and good grounding. Electromagnetic shielding is used mainly to prevent the influence of alternating electric fields, alternating magnetic fields, or alternating electromagnetic fields. It requires a shield with good conductive continuity, the shield must be connected to the same ground reference plane as the circuit, and the shield ground on the PCB must be placed as close as possible to the ground of the circuit being shielded.

Sensitive circuits and strongly radiating circuits need a shielding cavity soldered onto the PCB, and the PCB must be designed with a via shielding wall, meaning grounded vias placed on the board at the locations that will sit tight against the cavity wall. The requirements are as follows.

Use at least two rows of vias.
Stagger the two rows of vias relative to each other.
Within a single row, the via spacing must be less than λ/20.
No solder mask is permitted on the areas of the PCB that are soldered to the shielding cavity wall.
Where an RF signal trace passes through the shielding wall on the top layer, a slot door must be opened in the wall at the corresponding position. The door height must be greater than 0.5 mm, and the door width must guarantee that the distance between the signal trace and the shield body after assembly is greater than 1 mm, as shown in Figure 4.

Figure 4 | Slot door in the shielding wall

Shielded Cavity Dimensions

Every RF PCB is mounted inside a shielded cavity. At RF, the cavity is not an ideal enclosure; it behaves as a three-dimensional resonator with many resonant frequencies. These resonances depend on the mechanical dimensions of the cavity and also on the layer structure and dielectric materials of the PCB. In RF PCB design, the lowest resonant frequency is the critical parameter. When the operating frequency approaches this lowest resonance, part of the energy is absorbed and attenuated peaks appear, disrupting normal circuit operation. The cavity dimensions must therefore be selected so that its resonant frequencies do not fall within the operating band of the microstrip circuit.

The lowest resonant frequency of the shielded cavity shown in Figure 5 is obtained from the cavity resonance expression. The calculation uses the following geometric and material parameters:

F_min: lowest resonant frequency of the shielded cavity, MHz.
L, a, h: length, width, and thickness of the single-sided or double-sided PCB, mm.
L, a, b: internal length, width, and height of the shielded cavity, mm, with L > a > b.
C: propagation velocity of electromagnetic waves in free space, 3 × 10¹¹ mm/s.
ε_r: relative permittivity of the PCB substrate.

Figure 5 | Schematic of the inner wall dimensions of the shielding cavity

The resonance expression also includes a correction factor related to the h/b ratio and the relative permittivity ε_r, which accounts for dielectric loading of the cavity by the PCB. The quantities b and h require particular attention. When the PCB inside the cavity is a multilayer board, the second layer is usually a ground plane and is at the same potential as the cavity. In that case, h is the dielectric thickness from the top layer of the PCB to the second layer, and b is the height from the second layer of the PCB to the inner top surface of the cavity. This distinction matters because the effective cavity height above the ground plane is reduced by the PCB dielectric and copper layers.

Dimension a is critical and must satisfy a < λ/2, where λ is the wavelength in air at the upper frequency of the operating band. If this condition is not met, waveguide-type propagation can occur inside the enclosure. When oppositely traveling waves form positive feedback, the in-band gain flatness deteriorates and peaks appear at certain frequencies. If the feedback is too strong, self-oscillation can also occur. The λ/2 limit is therefore a geometric constraint on the cavity cross-section: the cavity must remain below the size at which a propagating waveguide mode can be supported.

All RF PCBs must be installed in a shielded cavity, and the cavity dimensions must be chosen so that the lowest resonant frequency is well above the operating frequency, preferably by a factor of 10 or more. The cavity height is generally at least 15 to 20 times the thickness of the first dielectric layer, which also ensures that taller components can fit inside. For a fixed cavity base area, increasing the length-to-width ratio raises the lowest resonant frequency. In other words, a square shielded cavity should be avoided.

Related Reading: