Designing an RF PCB stackup for high frequencies

Designing Your RF PCB Stackup

By ZM Peterson • Dec 5, 2019

RF PCBs are not often seen by the everyday designer, unless they are designing a board that includes WiFi/Bluetooth/LoRaWAN or other wireless communications capabilities. As these boards involve the use of analog signals and require precise oscillations in voltage and current to run properly, signal integrity is an extremely important aspect of RF PCB design.

With the rollout of 5G, broader use of IoT devices, applications like car/UAV radar, and other areas, many more designers will need to become familiar with some important points of RF PCB design. Engineering an RF PCB stackup is vital to ensuring high frequency analog signals will not be corrupted due to crosstalk and EMI. If you’re planning to develop a new product with mixed signal or high frequency analog functions, I’ve compiled some important points on RF PCB stackup design that can help you design successfully.

The Goals of RF PCB Stackup Design

Any stackup should be designed to ensure signal and power integrity, but this is quite critical in RF design due to the requirements for clean analog signals (see the section on signal integrity below). The three most important points to consider in RF PCB stackup design are:

  • Isolation. The primary goal in RF PCB stackup design is to ensure isolation between critical circuit blocks. As many RF systems are really mixed signal systems, isolation is critical for ensuring RF regions at different frequencies do not interfere with each other, and for ensuring analog signals do not interfere with digital signals. This is as much a layout problem as it is a stackup design problem.
  • Decoupling. This is something of a generic term. In terms of an RF PCB stackup, this refers to sufficient decoupling between power and ground planes in order to ensure power integrity.
  • Layer arrangement. At minimum, you should use a 4-layer PCB stackup with internal power and ground planes. Power and ground planes can be placed in two adjacent internal layers, which provides decoupling and power integrity. Components can then be placed on a surface layer adjacent to the ground plane.

In addition to the three points mentioned above, you should consider your design decisions in the following two areas:

Decoupling and Power Integrity

I’ve discussed the importance of stackup design in terms of power integrity in previous articles, but the same ideas apply to RF PCBs. The power integrity effects in an analog PCB are slightly different compared to a digital PCB, but the end goal of PDN design for an RF PCB is the same: ensure the power seen by your components does not fluctuate for any reason. This hinges on designing the right RF PCB stackup and providing decoupling in your PDN.

Placing your stackup and using properly-sized decoupling capacitors will ensure your board has the necessary level of decoupling to bring your PDN impedance down to a low value. In contrast to working with all-digital systems, you only need to worry about the target impedance at a narrow range of frequencies or at specific frequencies, rather than worrying about a broad bandwidth.

Decoupling capacitor self-resonance frequencies

Decoupling capacitor self-resonance frequency examples. Your component manufacturer should be able to provide similar curves for your capacitors.

Any capacitors you use should have sufficiently high self-resonance frequency; some example capacitor insertion loss curves are shown above, and the self-resonance frequency is clearly visible. Decoupling will help ensure the PDN impedance is low enough to prevent PDN ripple. When you suppress ripple in your PDN, you then prevent jitter from propagating to the output of any RF oscillator you use for frequency synthesis.

Your RF PCB Stackup and Signal Integrity

In terms of signal integrity, analog components are highly susceptible to noise. It is not that these components necessarily generate more noise than digital components. Instead, noise that is induced in an analog interconnect, whether it is from external radiated EMI or conducted EMI from another area of your board, will propagate into the input of a purely analog receiver component. This noise will then be passed through to the output of the component and will affect the operation of all downstream signals.

Why are analog components and signals so sensitive to noise? The reason is that analog components are generally run in the linear regime, whereas digital components are run at saturation. In digital components, the voltage simply needs to be above or below a certain threshold in order to be registered as a 1 or 0, respectively. Any variation in the signal level within a digital component’s noise margin will have no effect. This means noise on a digital signal has to be much larger to cause errors compared to an analog signal. With an analog signal, any noise seen at the input of an analog component generally produces some proportional change in the output signal level. This is why noise in analog circuits is so critical.

Johnson noise, pink noise, and shot noise are much less important in an RF PCB than crosstalk. A digital signal at only a few volts can induce strong capacitive and inductive crosstalk in an analog signal during switching, but the reverse is not always the case. Analog signals generally need to be at a much higher signal level in order to generate crosstalk in a low-level digital signal. If you design your stackup and layout correctly, you can isolate mixed signal boards and ensure high frequency analog signals, low frequency analog signals, and digital signals do not interfere with each other. This should underscore the importance of isolation in these systems.

RF PCB stackup with shielding

An example RF PCB with strong isolation.

Your Stackup and Layout

With your stackup being so critical to passing EMI checks, you should start by considering the number of layers you need, and then determine how to arrange them so that you prevent EMI problems. Low layer count boards are most likely going to be unacceptable in an RF PCB. At minimum, you will need to use a higher layer count board in order to provide sufficient room for power, ground, and signal layers.

2-layer and 4-layer Stackups

With 2-layer boards, you simply won’t have enough space. In order to provide sufficient decoupling, which becomes more important at successively higher frequencies, you need to use large power and ground planes to bring your PDN impedance to a low level. This leaves no room for signal routing. Routing signals and power on the same layer above a ground plane may have been fine with kHz frequencies, but this type of board 2-layer will fail when run at GHz frequencies.

4-layer stackups are technically fine as long as layers are arranged properly, and as long as you route all signals and components on a single layer. You would need to place adjacent power and ground layers on one side of the core, and signal and ground layers on the other side of the core; this is the only way to provide decoupling and ensure signals have low loop inductance. If you need two signal layers, you are better off working with a 6-layer stackup as this is the only way to provide multiple layers with sufficient shielding, decoupling, and low loop inductance.

6 or More Layers

A basic 6-layer stackup is shown in the image below. This stackup provides routing on the outer surface layers, and the plane layers will provide shielding between signal layers. In addition, the power and ground planes are placed adjacent on the same side of the core. This provides significant decoupling and high interplane capacitance. The ground planes should also be linked with stitching vias to provide a consistent reference potential throughout the board.

 

6-layer RF PCB stackup

Basic 6-layer RF PCB stackup in Altium Designer.

 

This should be the starting point for thinking about an RF PCB stackup. Folks like Rick Hartley recommend going for at least an 8-layer stackup, and I tend to agree when more signals need to be routed. You can also check out the 10-layer stackup I’ve created in this article for more guidance.

Routing and Shielding

For signal traces on the surface layer, one common practice is to use ground copper pour and via fences shield different sections of the board. The grounded copper pour and vias provide image charge that strongly opposes any EMI radiated from a nearby board section. The via fences need to be precisely designed, although a good approximation for the case where the pour region is much larger than the diameter and spacing between vias is to set the spacing equal to half the wavelength (in air) of the signal to be shielded. There are several basic simulation tools and calculators online that can be used for via fence/via gridding design on the surface layer.

Using coplanar waveguides or substrate integrated waveguides is a great routing strategy as these routing topologies provide excellent isolation. While these structures can be rather large compared to microstrip traces, these structures provide high levels of isolation and are already used in many microwave/mmWave devices.

Copper pour shielding in an RF PCB stackup

Ground pour used for RF shielding. Different functional blocks can be separated with this design strategy.

 

We’re only scratching the surface of RF PCB design; take a look at some other recent articles on our blog. If you're looking for a knowledgable firm that offers cutting-edge PCB design services and digital marketing services for innovative electronics companies, contact NWES for a consultation.

 


Subscribe to our updates

* indicates required



Ready to work with NWES?
Contact us for a free consultation.

Contact Us Today