Issue link: https://iconnect007.uberflip.com/i/396835
28 The PCB Design Magazine • October 2014 As signal rise times increase, consideration should be given to the propagation time and reflections of a routed trace. If the propaga- tion time and reflection from source to load are longer than the edge transition time, an electrically long trace will exist. If the trans- mission line is short, reflections still occur but will be overwhelmed by the rising or falling edge and may not pose a problem. But even if the trace is short, termination may still be required if the load is capacitive or highly in- ductive to prevent ringing. Note that series terminators are the most effective for high- speed design. For a driver signal with a 1ns rise time, since the speed of a signal in FR-4 is approximately 6in/ns (150mm/ns), then an un-terminated trace can only be 6 x 1/6 = 1.0 inches (25mm) before reflections occur and termination is re- quired. Rule of Thumb: All drivers, whose trace length (in inches) is equal to or greater than the rise time (in ns), must have provision for termi- nation. In order to terminate a transmission line, one first needs to know the impedance of the driver and the transmission line. So how do we find this information? First of all an accurate field solver, such as the ICD Stackup Planner is required to determine the impedance of the PCB traces. Then, the source impedance must be extracted from the IBIS model. Subtracting the source impedance from the trace characteristic impedance gives the required series terminator value. Further details on how to find the source impedance in the IBIS model can be found in a previous column Beyond Design: Impedance Matching: Terminations. Differential pairs are frequently used in high-speed design to provide noise immunity on serial interconnects. A differential pair is two complementary transmission lines that transfer equal and opposite signals down their length. These lengths should be kept equal and they should be coupled evenly along the signals length where possible. Symmetry is the key to successfully deploying differential signals in high-speed designs. Maintaining the equal and opposite amplitude and timing relationship is the principle concept. Many people believe that since the two halves of the pair carry equal and opposite signals, that good ground connection is not required as the return current flows in the op- posite signal. However, the return current ac- tually flows in the reference plane below each trace. Figure 4, illustrates the return current of a microstrip pair flowing directly below each trace—just as is the case for a single ended transmission line. The only reason the pair of traces need to be coupled, is to reject common external noise. If a differential pair can be routed closely coupled along the entire length, then consid- er using tight coupling. Otherwise, if the pair need to separate around an obstacle (a via for instance) then coupling the pair by twice the trace width is more effective. The reason being that a tightly coupled pair will increase imped- ance by 25% if separated while a more loosely couple pair will only vary by about 4% imped- ance. This provides more stable impedance along the trace length. The rule of thumb: Gap = 2x trace width. Next month's column will continue to dis- cuss signal integrity, in particular the effects of crosstalk, timing and skew on signal integrity so stay tuned. Points to Remember • Advances in lithography enables IC man- ufacturers to ship smaller and smaller dies on chips. • In order to reduce power consumption, IC manufacturers have moved to lower core volt- ages and higher operating frequencies, which of course mean faster edge rates. • Faster edge rates mean reflections and sig- nal quality problems. SIGNAL INTEGRITY, PART 1 OF 3 continues Figure 4: return current of a microstrip differential pair. (courtesy of ansoft) beyond design