PCB Design for RF Boards
- Jack Christensen
RF transmission lines are traces that carry radio frequency signals between components. When designing them, follow design choices that enable power delivery with minimal loss.
When designing two-layer RF boards, it is recommended that you use the top layer of the board for all the PCB components and traces, and leave the bottom layer as a solid ground plane.
If designing a complex RF board, it is recommended that you use a four-layer board layout to allow for simpler routing and a full ground plane. Use the following stack-up for four-layer PCBs:
Top Layer - RF Traces and Components, Antennas, Decoupling Capacitors, and Other Signals
Layer 2 - Ground Plane
Layer 3 - Power Plane
Bottom Layer - Non-RF Components and Signals
To keep the RF traces isolated, fill the unused area of the RF trace layer with a ground pour, make the layer below it a ground plane, and connect the two layers with a via fence (more on this later). This is referred to as a “Grounded CoPlanar Waveguide” and is seen in Figure 2.
If the ground plane MUST have traces going through it, ensure that no traces cross the path of the RF trace on the above layer.
Avoid split ground pours to ensure that no current loops are formed in the return path.
The width of RF traces should be such that its characteristic impedance is 50 Ω. Use this calculator to find the required width.
RF traces should maintain this width and keep a constant gap between it and the ground pour to keep a constant characteristic impedance
Avoid bends in an RF trace. If it is unavoidable, make a curved bend instead of a sharp one to ensure uniform trace width. If a right-angled turn is required, mitering can be done to the dimensions as shown in Figure 3.
Recommended dimensions for mitering in 90-degree RF traces
Keep the RF traces as short as possible. The longer the trace length, the more the traces and the substrate below attenuate the RF signal.
Avoid adding test points to and branching RF traces. Doing such affects impedance matching. This is why you should also follow reference designs exactly, as even small alterations can impact impedance matching.
Do not place other traces close to and parallel to RF traces. This causes mutual coupling of signals between traces.
RF traces should be fenced in on either side by vias that connect the ground pours of the trace layer and ground plane. These are called “via fences”. Via fences should also go along the perimeter of the PCB if possible
The vias in these fences should be spaced apart at a maximum distance of λ/20, where λ is the wavelength of the highest significant frequency going through the trace. This wavelength can be calculated with the signal frequency and the dielectric constant of the PCB material through this equation.
An overview of via fencing
Additionally, if extra RF isolation is required and the size of the ground plane surrounding the RF trace permits, you can fill the empty area of the plane with spaced-out vias. This is called “via stitching”. The spacing between these vias should be no more than λ/8, with λ being calculated through the equation given in the previous bullet.
