General PCB design guidelines for nRF53 series

When designing a PCB with a high-frequency radio onboard certain rules should be followed for optimal radio frequency (RF) performance. This guide will provide some general PCB guidelines that can be used in addition to the PCB guidelines in the nRF5340 Product Specification and the reference design (ALTIUM, GERBER and PDF), that can be downloaded here.

Nordic offers hardware reviews and tuning of the radio matching network and the antenna free of charge. Just create a private ticket on DevZone. 

RF path

The RF part of the schematic and layout should be a direct copy of our reference design. This means that you should copy the component values, the geometry, the relative placement of the components with respect to each other, and the lengths of the transmission lines from our reference design.

Matching network

In RF, things work differently than in "regular" electronics due to the high frequencies and short wavelengths. One of the resulting effects is that the phase of a signal will vary along the transmission lines, as opposed to low frequencies where the wavelengths are much larger than the transmission lines, and this effect can be disregarded. If the system (chip and antenna) is not matched, there will be reflections of the signal in the transmission line, resulting in a loss. The system should be matched to a 50 Ohm reference point by matching each component, e.g. chip and antenna, to 50 ohms.

Matching the radio to 50 ohms

Since the output impedance of the nRF53 chip is not 50 ohms, we need a matching network between the nRF ANT pin and the 50 ohms reference point B.
The matching network matches the output impedance to 50 ohms but also works as a filter that damps the 2^nd and 3^rd harmonics.

Correctly matching the radio will give you the desired output power level and low harmonics at the 50 ohms reference point B.

nRF5340 CSP

Fig. 1

nRF5340 QFN

Fig. 2

Figure 1 and 2 show the ANT pinout of the nRF5340, the radio matching network, the 50 ohms reference point B, a matching network for the antenna, and an antenna.

The matching network for the radio will vary from chip to chip, but the effect of the matching network is the same. Note for the QFN packages, the shunt capacitor closest to the radio should be grounded via the VSS pin closes to the ANT pin. This is to achieve optimal RF performance and is a part of the filtering effect to suppress the harmonics.

This also means that the layout of the RF path should be directly copied from the reference design, as this plays a role in suppressing the harmonics and is necessary to pass the various regulatory standards.

It is difficult to copy the reference layout one to one directly, since differences in substrate, the number of layers, the length of transmission lines etc. can differ. This is why tuning the values of the components is needed to achieve optimal RF performance for each custom design. 

How to tune the radio matching components?

Now we know that the matching components should match the output impedance of the ANT pin to 50 ohms, but also works as a filter to suppress the 2^nd and 3^rd harmonics. This means that when tuning the component values, both the fundamental output power and the harmonics levels must be measured.

The component's values are adjusted until the desired level of the fundamental outpower and harmonics are achieved.

Tuning the matching network is something Nordic can do for you, just create a private DevZone ticket, and ask for radio tuning.

For more information, you can also read the white paper RF performance test guidelines.

Typical mistakes you should try to avoid

Routing directly under the RF path
There cannot be any routing directly under the RF path. You want a solid ground plane under the RF path, working as an RF shield and reference ground for the transmission line. This solid ground should be from the hole center pad of the nRF53, all the way to the antenna clearance. On PCBs with more than two layers; add a keep-out area on the inner layers directly below the RF path (from ANT, pin on the nRF, to the antenna) to reduce stray capacitance.

Not having a 50 ohms coplanar waveguide
It is very important to include ground around the RF path. The 50 ohms transmission line should be a coplanar waveguide. Use a calculation tool to calculate the width, W, of the track and the distance to ground, G, to get a 50 ohms transmission line. This is also essential to be able to perform conducted measurements.

Antenna – 2.4 GHz
Antenna choice is complex and depends on many factors, so spend some time finding an antenna that meets the needs of your specific design.
In Nordics example designs, you can find a monopole and a meander antenna, both printed PCB antennas, that you can copy and add some extra length for tuning.

Monopole quarter wave, printed PCB antenna: This antenna is easy to make and easy to tune, and it only needs one shunt components for impedance matching in addition to the antenna length. Space: About 23 mm long and needs a minimum of 5 mm clearance to the ground plane.
See the white paper on monopole quarter wave antenna. 

Meander, printed PCB antenna: This antenna type requires a smaller area than the monopole antenna, but it needs a pi-network for impedance matching in addition to the antenna length.
See the design files for Nordic’s nRF52840 dongle, to see the meander antenna.

Other printed PCB antennas: There are multiple other options for printed PCB antennas; you can design your own or find them online. If you copy/reuse a printed PCB antenna, make sure you also copy the distance to the ground plane and add a suitable matching network for the antenna.

Off-the-shelf chip antennas: There are numerous chip antennas to choose from, and the antenna vendors can also help with the decision-making of choosing the right antenna for your design or provide an easy antenna selection guide. Pay attention to the recommended mounting for the antenna when choosing an antenna and make sure to follow the reference design, and ask the antenna vendor for review in addition to the review from Nordic on DevZone.

Power supply
To prevent noise from one source from affecting the others on the same PCB, we recommend using start routing. This means each supplied device will have its own track from the power supply. The center of the star network should be placed close to the power supply.

Normal or high voltage mode: VDD pins must be connected externally for both alternatives.
In addition to using star routing, a good ground plane is essential for reducing the risk of power noise.

Ground planes

The reference design from Nordic consists of four ground planes: A top layer, inner layer one, inner layer two, and a bottom layer. All ground planes should preferably be as large and solid as possible, and having four ground planes instead of one gives more room and freedom for routing and component placement.

Ground is the system's reference, as it is for the 50 ohms transmission line, and it is also the return path for noise. The larger the ground planes are, the more difficult it is to disturb them.

The ground planes should be connected by using via holes. Pay attention to the number of vias in the center pad of the nRF53, this should be copied from the reference design.
In general, add a via to ground near every ground pad of a component, add vias on the side of the RF path, and larger ground areas, add a via at least every 5 mm. Try to avoid small ground islands (local ground areas). When they occur, add multiple vias to ground to ensure proper ground of the components connected to this ground.

Decoupling capacitors

In Nordic’s reference designs, there are decoupling capacitors on the VDD (power supply) and DEC pins. These must be placed close with short tracks to their respective VDD/DEC pin.

The crystal oscillators

On the nRR53, an external 32 MHz crystal is mandatory, and an external 32.768 kHz crystal is optional. It’s important to choose a crystal that follows the specifications given in the product specification. See HFXO for 32 MHz and LFXO for 32.768 kHz.

External and internal load capacitors

The load capacitors, Ccap, are connected to the crystal, and when designing with nRF53, you can choose to use external or internal load capacitors.

The values of Ccap, internal and external, are given by the formula:

Ccap = 2*CL – C_pcb – C_pin

CL is the load capacitance of the crystal in use and can be found in the datasheet of the crystal.

C_pcb + C_pin is approximately 4 pF for the HFXO pins and approximately 5 pF for the LFXO pins. 

See more information on using the internal capacitors in the product specification. 

Frequency accuracy

For the 32 MHz crystal, the values for the load capacitors should be adjusted/altered if the frequency accuracy is not satisfactory, it must be below 40 ppm.

Measuring the frequency accuracy should be done by measuring the carrier frequency of an unmodulated carrier transmitted by the radio. If the carrier is measured above the center frequency, then increase the values of the load capacitors. If the carrier is measured below the center frequency, then decrease the values of the load capacitors.

This adjustment of the load capacitors is something Nordic can do for you during the radio/antenna tuning process.

Component placement

When designing a PCB with a radio onboard, consider the entire PCB as an RF PCB. Noise on the board can result in noise on the radio, causing problems during regulatory certifications.

When starting to design an RF PCB, begin by placing the antenna and antenna clearance area. The antenna should be placed as open as possible, giving it space to resonate. 

When the antenna is placed, you can move on to the rest of the RF part of the design, RF path, matching networks, and the nRF53. Make sure to have room for all the required components in the reference design provided by Nordic.

Place the rest of the components.

Routing tracks: Use one layer for tracks first and move on to the other layers when needed. One layer should preferably be mostly solid ground.