Basic Wireless Communication for Microcontrollers
Chapter 4 - Design Project 3: 900MHz Automatic Error-Correcting Data Link
PCB layout for UHF
At UHF frequencies (above 300MHz), stray capacitance and inductance of PCB traces and other wires becomes too high even for relatively short runs. In this project, all of the RF circuitry is contained within the module, so the design task is greatly simplified. Still, we need to talk about UHF layout techniques because we need to supply the connection from the antenna to the unit.
Rather than fighting every step of the way to make PCB runs ultra short, the best philosophy is usually "if you can't beat 'em, join 'em". What I mean by this is that we should treat each PCB run which is longer than about 1/40th of a wavelength as a transmission line. Instead of trying to minimize stray reactances, you utilize them to create a line which, when terminated in its characteristic impedance, will just show that same impedance at the input.
In the first design project, we discussed coaxial and twin-wire transmission lines. At UHF frequencies, transmission lines can also be formed by simply traces on a PCB with a ground plane on the other side. This type of line is called microstripline or microstrip for short. In multilayer boards, an improved form can also be used where both outer layers are ground plane and an inner layer is the signal trace. This is known as simply stripline and is both more predictible (less influenced by outside objects) and less lossy.
Figure 1 - Microstrip illustration and formulas, taken from Linx Technologies document "SC Series Transceiver Module Design Guide" (scmanual.pdf)
Figure 1 shows how microstripline is usually constructed. Each type of PCB material has a certain dielectric constant (or relative permittivity). For common epoxy-fiberglass (FR4), it is about 4.8. The actual effective dielectric constant seen by the line differs from this because the top trace is not surrounded by PCB material, but has PCB on one side and air on the other. The first formula in the figure gives the effective dielectric constant for given microstrip dimensions. Note that this effective dielectric constant should also be used to compute the signal propagation velocity along the line or line length in wavelengths. Finally, the second pair of formulas gives the characteristic impedance (Zo) for microstrip with given dimensions and effective dielectric constant.
In this project, the antenna we will choose (a 1/4 wave vertical above a ground plane) has an approximate input impedance of 36 ohms resistive. The RF module has an output impedance of 50 ohms. The mismatch would be minimal if we simply used either 50 ohm or 36 ohm transmission line. However, since we are designing the microstrip dimensions, it is easy to make a quarter-wave transformer to match the 50 ohm impedance to the 36 ohm impedance. This would require a 1/4 lambda long line with Zo=sqrt(50*36)=42.2 ohms. This is what was done in the actual design, and at 916 MHz, the microstrip paramters were d=.062 inch, w=0.150 inch, l=1.68 inch. I used a simple MATLAB program to compute the epsilon_eff and Zo for given dimensions, and then just tweaked the dimensions until I got Zo=42 ohms. I then used the corresponding epsilon_eff to compute the speed of propagation, and computed the length required for 1/4 wave. You can do this by noting that the signal propagation velocity (in meters per second) is 3x10^8/sqrt(epsilon_eff), and therefore the wavelength, lambda, in meters is 3x10^8/(f*sqrt(epsilon_eff)), where f is the frequency in Hertz.
To actually connect to the output pin of the module and the antenna to the ends of the microstrip, I used very short, somewhat thinner traces.
Additional Notes
Two other important notes: other traces should be kept well clear of the microstrip trace as they can interact with it. As can be seen in the board layout, there are no traces which are close to the line and also parallel to it. Secondly, it is important to ensure that the power supplied to the RF module is well regulated and that there are adequate bypass capacitors near the module. The manufacturer in this case recommends two bypass capacitors, one of about 0.1uF and the other greater than 22uF. In our design, we have a 0.1uF and a 47uF. If the power is noisy, this could distort the outgoing signal, increase the noise on received signals, and cause out-of-band emissions which are illegal.
BACK Table of Contents
NEXT