When designing a high frequency PCB there are some rules that should be followed in order to get a good working radio/system. Below are some general PCB guidelines. These guidelines should be followed to maximize the performance of the system. It is also recommended to read about PCB guidelines in the reference circuitry page on infocenter.
The RF part of the schematic and layout should be a copy of our reference design. It means that not only the component values, but also the geometry, relative placement of the components with respect to each other, and the lengths of the transmission lines should be the same as in our reference design. The reference design for nRF52832 (altium and pdf) can be downloaded from infocenter.
In Radio Frequencies (RF), things work differently than in "regular" electronics, due to high frequencies (and short wavelengths). One of the resulting effects is that the phase of a signal will vary along the transmissions lines, as opposed to low frequencies where the wavelengths >> 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 loss. The system should be matched to a 50 Ohm reference point by matching each component, eg. chip and antenna to 50 Ohm.
Matching to 50 ohm: The output impedance of the chip is not 50 ohm. Therefore a matching network needs to be inserted between the chip and the reference point. Note: in addition to matching the chip to 50 Ohm, C3 and L1 form a filter that damps some of the 2nd and 3rd harmonics. For this to work, the both the schematic and the layout have to be a copy of the reference layout.
The figure above show parts of the pinout of nRF52. Note that there is only one antenna pin (nRF51 has two). nRF52 has an internal balun which make matching easier to accomplish. Our reference design shows how to match the nRF52 to 50 Ohm. The PCB layout (pad size, lines etc) is a part of the matching, make sure that your design is an exact copy of the reference design*. The matching is done with two components, L1 and C3. These components also form a low pass filter which will suppress harmonics. Note that C3 should be grounded via the VSS pin, see the reference layout. It is necessary to suppress the harmonics to pass the various regulatory standards. The whitepaper "Regulatory and Compliance Standards for RF Device" sums up the most common regulatory standards. If tuning is needed (because the performance, i.e. range, is not as expected) the whitepaper "Tuning the nRF24xx matching network" can be used. Please note that this is written for nRF24LE1, but the principles are the same.
*Exact copy of our reference layout: An exact copy of our reference layout means that both the component values and the distances and the geometries between the components should be copied.
Matching the antenna to 50 ohm: There are basically two types of antenna matching networks; pi-network and a matching network consisting of one shunt component only. The type of antenna decides which matching network to use. If using a PCB antenna, the matching network should consist of one shunt component, and if using a chip antenna, the matching network should be a pi-network. The value(s) of the component(s) in the matching network will have to be found during tuning, by doing measurements using a network analyzer. The reason for this is that the impedance of the antenna depends on its close environment; it means that the measurements on a device should be performed when the device is placed in its final housing, in a similar environment to where it is supposed to be used. It is not possible to calculate the value(s) for the component(s) in the matching network, because there are too many parameters to take into account. The "Antenna tuning" whitepaper explains more about why tune the antenna, and how to do it.
The below figure shows matching between the chip and a PCB antenna.
50 Ohm transmission line: If a transmission line is needed between the chip matching network and the antenna matching network, it is important to use a 50 Ohm transmission line, because it will minimize the loss on that distance. The 50 Ohm transmission line will be a co-planar waveguide, and the width of the line can be calculated using AppCAD.
If the transmission line is not 50 Ohm, there will be loss in the signal between the antenna and the chip. The result is reduced range, the worst case scenario is no range at all.
A co-planar waveguide consists of a transmission line, ground on both sides, and a ground plane below the transmission line.
There are two types of antennas that can be used, a PCB antenna or a chip antenna. Under optimal conditions, the performance of a PCB antenna and a chip antenna will be more or less the same.
PCB antenna: The whitepaper "Quarterwave printed monopole antenna for 2.4GHz" explains how to design a PCB antenna.
Chip antenna: Any 2.4 GHz antenna can be used. In order to obtain good performance, it is important to place the antenna according to its datasheet. The antenna datasheet will also contain information about the bandwidth of the antenna.
A typical design consists of two ground planes; a top ground plane and a bottom ground plane. Both ground planes should preferably be as large and solid as possible. Ground is the reference of the system, the impedance of the antenna should for example be 50 Ohm with respect to ground. The larger the ground planes are, the more it takes to disturb them. The two ground planes should be connected using a lot of via holes. Our reference designs show what the distribution of the via holes may look like.
Crystal: On nRF52 an external 32 MHz crystal is mandatory, and an external 32 kHz crystal is optional. The benefits of including the 32 kHz crystal are discussed here. When choosing a crystal it is important that it is within the specifications. Specifications for 32 MHz clock oscillator is found in table "64 MHz crystal oscillator (HFXO)", for the 32 kHz crystal it is found in "Low frequency crystal oscillator (LFXO)".
Load capacitors: The load capacitors are the capacitors connected to the crystal, C1 and C2 connected to the 32 MHz crystal in our reference design, and C13 and C14 for the 32 kHz crystal.The value of these capacitors can be found using the following formula:
C1 = C2 = 2Cl - C_pcb - C_pin
Cl: Load capacitance of the crystal (found in the crystal datasheet)
C_pcb + C_pin is approximately 4 pF.
Details can be found in the whitepaper "Crystal Oscillator Design Considerations". Please note that this paper is written for older chips (not nRF51/52) and that the input capacitance is ~4pF for nRF52 (not 1pF as stated).
Measuring the frequency of the 32 MHz crystal should be done by measuring the carrier frequency of the radio. If the carrier frequency of the radio is within the specifications, the 32 MHz crystal is also within the specifications. If trying to probe the crystal directly, the frequency of the crystal will drift, because the probe possesses a capacitance, and this will effectively change the total value(s) of the load capacitors.
Please note errata 138.
The reference circuitry page link appears still to be broken.
Please, can you fix this link? Now I see 404:"The whitepaper "Quarterwave printed monopole antenna for 2.4GHz" explains how to design a PCB antenna."
Regarding the 50ohm impedance on transmission line: I downloaded the nRF52840-QIAA Reference Layout 1_0 and opened some of the files in Altium and took a look at the PCB stackup, thickness, track-width and track-separation to coplanar ground, on the part that goes to the (SMA?) connector.
I used two free impedance calculators and had them set to conductor-backed coplanar waveguide. With H=1.51mm, W=0.76mm, S=0.263mm and FR4 (er=4.5), I get for both calculators, Impedance of around 62ohm.
I get that these calculators are based on theoretical equations, but are they in fact approximately 24% off, when calculating the impedance? I guess you have actually measured the impedance to be 50ohm. What are your thoughts on the matter? And what do you recommend if I have different PCB thickness or stackup? What tool to use for approximate design? (I don't have ADS, CST etc.)