RF PCB Filtering and Grounding: Practical Design Rules

RF PCB filtering and grounding address two tightly coupled engineering problems: keeping electromagnetic interference from entering or leaving a circuit through power and control lines, and giving RF return currents a low-impedance, continuous path. At high frequencies, ordinary decoupling and a nominally grounded plane are not enough. Component placement, via arrangement, ground-plane integrity, and the way the board is bonded to its shielding cavity all affect whether the design works. This article covers practical filtering for power, control, and frequency-synthesizer lines; grounding methods; large-area and grouped grounding; RF device grounding; and ground-plane arrangements for double-sided, four-layer, and higher-layer RF boards.

Highlights:

Power and control lines are primary EMI ingress and egress paths. Use EMI absorbers, feedthrough capacitors, surge absorbers, and multi-value decoupling networks at the point of entry.
Cascaded small-signal amplifiers and power amplifier modules need staged supply filtering. Place the smallest high-frequency capacitor closest to the supply pin, and add a 10 pF capacitor when the signal frequency is above 1GHz.
RF grounding depends on short, wide, low-inductance returns: large-area ground, multiple vias per pad, no isolated copper or open stubs, and a complete ground plane bonded tightly to the shielding cavity.

3. Filtering

Power and Control Line Filtering

As electronic systems move to higher frequencies, noise and sharp pulses that once seemed harmless can now threaten equipment operation. Power lines and control lines are the main paths by which electromagnetic interference enters and leaves a circuit. External interference can travel through a power or control line into the circuit and disrupt normal operation. In the same way, interference generated inside the circuit can travel out through those lines and disturb other equipment. Addressing both incoming and outgoing interference paths is an important consideration in EMC design.

Several filtering approaches are commonly used:

Use EMI absorption beads or rings, connector EMI gaskets, and surface-mount (SMT) EMI components to suppress noise and spike interference on signal and power lines. These parts also absorb electrostatic pulses. This type of filter allows only DC or low-frequency signals, typically a few kHz, to pass while strongly attenuating higher-frequency interference, so the equipment can meet applicable Chinese and international standards for electromagnetic compatibility and electrostatic discharge.
For EMI filtering and RF isolation on enclosure entry and exit lines, or on partition plates inside an enclosure, use threaded feedthrough capacitors.
To suppress lightning strikes and surges, use a surge absorber. It has the advantage of fast response. When the pulse current exceeds the component's withstand capability, it automatically opens, so the failure mode is an open circuit.
At the DC power input of an RF PCB, combine three filter capacitors in parallel. In general, their capacitances differ by a factor of 100. Use the advantages of each capacitor to filter the low, medium, and high frequencies on the supply line. A common set is 10 uF, 0.1 uF, and 100 pF.
When the same supply feeds a chain of small-signal cascaded amplifiers, it is recommended to feed the final stage first and then supply the earlier stages in sequence. Each stage should have at least two supply filter capacitors: 0.1 uF and 100 pF. When the signal frequency is above 1GHz, add a 10 pF filter capacitor. The 10 pF capacitor has a high self-resonant frequency and should be placed closest to the supply pin. As shown in Figure 6, power enters the final stage first through C107. C96 and C154 are the final-stage amplifier filter capacitors, with C96 close to the supply-side pin of R108. C94 and C228 are the earlier-stage amplifier filter capacitors, with C94 close to the supply-side pin of R104.

Figure 6 | Power supply and filtering for small-signal cascaded amplifier

Pay attention to decoupling and filtering to prevent different units from interfering through the supply line. During supply routing, keep supply lines isolated from one another.

The power amplifier module supply filtering must include at least three components: 10 uF, 0.1 uF, and 100 pF. They must be close to the relevant pins, and the high-frequency small-value 100 pF capacitor must be closest. When the signal frequency is above 1GHz, add a 10 pF filter capacitor.

Filtering Data, Clock, and Enable Lines in Frequency Synthesizers

In RF PCBs, the data, clock, and enable lines of a frequency synthesizer are critical signal lines. RF PCBs routing must follow digital PCB design rules and also meet the following requirements:

Add isolation measures to ensure that no other signals are present on the data, clock, and enable lines. Lines that enter the PCB from outside the shielded cavity must pass through feedthrough capacitors mounted on the shield wall. A simpler method is to add an RC low-pass filter on these lines, as shown in Figure 7. The resistor and capacitor values must still guarantee correct programming timing.
Do not route the data, clock, and enable lines on the surface layer beneath digital frequency synthesizer chips, crystals, crystal oscillators, transformers, optocouplers, power modules, and similar devices.
Avoid crossing these lines with analog signal lines on the same layer or on adjacent layers.

Figure 7 | Add RC low-pass filters on data, clock, and enable lines

4. Grounding

Grounding Categories

An ideal ground plane is a physical body at zero potential. Any interference signal level passing through it produces no voltage drop. A real ground plane, however, can develop a potential difference of a few microvolts or more between two grounding points.

A designer should consider and analyze the ground potential distribution to find low-level points on the ground plane and use them as the grounding point for sensitive circuits or equipment.

Common grounding methods include floating, single-point, multipoint, and hybrid grounding.

Floating ground isolates a circuit or equipment from the common ground or from a common conductor that may cause circulating currents. To eliminate the effect of static charge accumulation, connect a high-value bleeder resistor between the equipment and earth.
At low frequencies, when the ground-line length is less than λ/20 of the operating wavelength, single-point grounding is generally used.
When the ground-line length is greater than 0.15λ, multipoint grounding is used.
For circuits operating over a wide frequency range, consider hybrid grounding.
For RF circuit grounding, ground lines should be as short as possible or large-area grounding should be used.

Large-Area Grounding

To reduce ground-plane impedance and achieve effective grounding, follow these rules:

RF PCB grounding requires large-area grounding.
In microstrip printed circuits, the bottom surface is the ground plane; a complete ground plane must be ensured.
Because of the skin effect, the ground plane should be gold- or silver-plated with good conductivity to reduce ground-line impedance.
Use fastening screws to bond the board tightly to the shielding cavity.

Grouped Local Grounding

Divide the entire circuit into N groups according to circuit structure and current magnitude. Each group grounds locally to form a return loop. Adjust the orientation of filter capacitors within each group to reduce the ground loop.

Ground lines should be short and straight. Crossing and overlap are prohibited. This reduces interference caused by common ground impedance.

RF Device Grounding

When surface-mount RF devices and filter capacitors require grounding, reduce device ground inductance by following these requirements:

Each pad should have at least two thermal-relief spokes connected to the ground copper; if the process allows, use full-contact grounding.
Use at least two plated vias for local grounding next to the device pin.
Increase via diameter and parallel several vias.
Some components have a grounded metal shell on the bottom. Add ground vias within the component's projection area, and leave no solder mask in the surface-layer projection area.

Grounding Precautions

Within process capability, shorten the distance between the pad edge and the via pad edge.
Within process capability, a large ground pad must directly cover at least six ground vias.
When a ground line must travel a certain distance, shorten it. It must not exceed λ/20, to prevent antenna effects that cause signal radiation.
Except for special applications, do not leave isolated copper. Copper areas must have ground vias.
Do not leave open-ended stubs on ground copper. Add a ground via at the open end.
For RF cable shields at the input and output, the solder point on the PCB should be on the ground copper around the end of the trace. The solder point must have no fewer than six vias to ground to ensure RF ground continuity.
For microstrip circuit terminations, the diameter of a single ground via must be larger than the microstrip line width, or use a large number of densely arranged small vias in a row for grounding.

Ground Plane Distribution

In a double-sided RF PCB, the top layer is the signal layer and the bottom is the ground plane. If there are no non-ground vias, leave the entire bottom surface free of solder mask and press the board tightly against the bottom of the shielding cavity to further reduce ground impedance.

In a four-layer RF PCB, the top layer is the signal layer, the second and fourth layers are ground planes, and the third layer carries power and control lines. In special cases, some RF signal lines may be routed on the third layer, but vias affect the signal, and test results show that stripline flatness is poorer. Every layer should have large-area copper.

As equipment becomes more complex and compact, RF PCBs with more layers have appeared, such as six and eight layers, and RF PCBs made with HDI (high-density interconnect) processes are also possible.

Related Reading: