Transmission line impedance matching is critical in any PCB layout. Before we even get into the reasons you should match transmission lines, I want to mention one point that I've mentioned on a number of technical blogs:
Every trace in a modern PCB should be treated as a transmission line.
Now that we have this out of the way, we can start to understand why impedance matching is important in a transmission line. Modern digital and analog systems require impedance control and impedance matching due to the preponderance of components with fast rise time (less than a few ns) and low supply voltage, as well as analog components that are running at ever higher frequencies. Once you get above WiFi frequencies and below 1 ns rise time, your board is likely to fail if interconnects are not designed properly. One important aspect of interconnect design is your stackup, and the other is impedance control. If you can get both of these areas correct, then your system has a much higher chance of meeting important performance standards.
Impedance matching is a simple concept: you design a transmission line so that the driver, transmission line, and receiver all have the same impedance value. In modern PCBs, you won't need to worry about parasitic losses that arise from DC resistance in the trace or the substrate conductance, so your impedance will be a real number (resistive). There are a number of methods for impedance matching different components; this typically involves compensating the capacitive or inductive nature of the component with a matching network. These networks can be easily simulated using a basic circuit simulator (e.g., SPICE).
There are three reasons why impedance matching is important in a transmission line:
Your goal in transmission line design is to ensure that the 5 V signal (or whatever the signal level is) you send down a transmission line is read as 5 V at the receiver. However, even if you impedance match your transmission lines, there are still some signal integrity problems that can arise, especially in today's PCBs. Newer devices are running with lower power requirements, a variety of communication protocols, higher interconnect density, exotic materials, higher data rates, and faster rise times/frequencies. While we can't cover absolutely everything here, I'll bring up one important misconception about transmission line behavior that is mistakenly related to impedance matching.
If you frequent PCB design blogs, you'll probably notice that many designers refer to a phenomenon known as "ringing," which technically describes the transient ripple produced in a transmission line when a digital driver switches. These days, COTS components have fast rise times (less than 10 ns) that will easily trigger strong transient ringing in your transmission line if your lines are not sized properly. Many designers state that transmission lines should be impedance matched to the source and driver because removing reflections prevents transient ringing. Nothing could be more incorrect. The transient response in a transmission line is not caused by signal reflection, it is caused by a sudden change in the signal level in any circuit, regardless of impedance matching.
In reality, the transient response (ringing, see Fig. 1) in your transmission line has nothing to do with reflections. Even if your transmission line is impedance matched, ringing will still occur and can be very strong because it is related to parasitics in your transmission line. You can read more about the specifics of transmission line ringing in a previous blog post. You can also read one of my blog posts on Altium's PCB Design Blog. As a designer, your challenge is to size the trace such that the desired characteristic impedance is maintained while the inductance is decreased to the point where critical damping is reached.
Fig. 1: Typical transient oscillation (ringing) in a transmission line. This response occurs when the driver switches between ON and OFF states, regardless of impedance matching.
When many designers refer to ringing, they are really referring to a stair-step response in the voltage and current when a transmission line is driven with a digital driver. This particular phenomenon is related to impedance matching and results specifically from reflection at when the source and receiver have an impedance mismatch with the transmission line. When only the source is mismatched, there will be a reflection back towards the driver, and the voltage seen at the receiver may be lower than the value required for latching/switching. When only the receiver is mismatched, we effectively have the same phenomenon.
The stair-step response that many designers mistakenly call ringing results when the source and receiver are mismatched from the transmission line. When this is the case, a signal will reflect back-and-forth between the mismatched end. Depending on the exact mismatch at each end, the signal can experience a phase-shift as it traverses the transmission line. Each time there is a reflection, there is a slight signal level change, which brings about a new transient response on the line. The important point to remember here is that the transient response occurs when the signal level changes very quickly, regardless of whether it is caused by a reflection or switching in the driver. This leads to the type of behavior shown in Fig. 2, where the voltage seen at the receiver slowly rises to full scale after repeated reflections.
Fig. 2: Stair-step response in a completely mismatched transmission line. This response occurs due to repeated reflections at each end of the transmission line. Notice the transient ringing that is superimposed on top of the stair-step response. This occurs due to the level change that occurs at each reflection. In the top graph, the load resistance is greater than the transmission line's characteristic impedance, and vice versa in the bottom graph. Read more about this in my recent article on Cadence's PCB Design Blog.
You can read more about transient ringing in a perfectly impedance matched transmission line in an article from Bogdan Adamczyk in In Compliance Magazine.
When both ends of a transmission line are mismatched and the line is driven with an analog signal, the forward and backward travelling waves can form standing waves if the line is driven at specific frequencies. Some signalling standards actually exploit this behavior to properly drive a downstream component (e.g., antennas). When driven with a high power pulse, such as in radio-over-fiber, transmitting antenna, or RF power electronics applications, a standing wave on a completely mismatched line can actually damage a trace with low copper weight.
Note that I've largely been referring to single-ended traces, but the discussion here applies equally to differential pairs. The difference is that termination in most signalling standards is specified in terms of the differential impedance. As an example, in LVDS, the differential pair is typically terminated at the receiver with a parallel resistor. Contrast this with a single-ended transmission line with a low-impedance driver; this arrangement requires placing a series resistor at the driver such that the driver's impedance matches the transmission line's characteristic impedance, which should also be matched to the receiver. Be sure to check your component datasheets and signalling standard when designing and matching a transmission line.
In an upcoming set of articles, I'll get into the stackup and impedance matching network design issues. For now, my hope is that readers gain a better understanding of why impedance matching is important in a transmission line. 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.