Design007 Magazine


Issue link:

Contents of this Issue


Page 23 of 87

24 The PCB Design Magazine • October 2017 WHEN DO TRACES BECOME TRANSMISSION LINES? It is important to note the variation in dielectric constant (Er or Dk) that different materials can exhibit. For in- stance, air has an Er = 1, whereas an alu- minum stiffener may have an Er = 10 and then there are barium oxides that go up to 600. Standard FR-4 has an Er = 4 and dielectrics specifically designed to be used for high-speed designs have a very low dielectric constant. For in- stance, Isola Astra-MT77 100GHz ma- terial has an Er = 3. The dielectric con- stant has a direct impact on impedance and the signal propagation through the substrate. That is why the dielectric constant for a specific material should always be obtained from the supplier's specification (or a reliable source) that lists the Er at different frequencies. Please note that datasheets generally list the dielectric constant as Dk. Closed-form equation-based impedance calculators have been around for many years, but unfortunately, they are extremely limited in accuracy. Many examples can be found on the internet and generally their results are just rough estimations but where they all come to - tally unstuck is in the calculation of dual em- bedded (asymmetric) stripline. IPC published impedance equations in the original IPC-D-317 and later in the IPC-2251 standard. The later was based on Brian C. Wadell's book Transmis - sion Line Design Handbook, but even these quite elaborate equations are unable to cope with wide unbalances in surrounding dielectric in the stripline configuration. Since impedance is the key factor that controls the stability of a design, one should never compromise the ac- curacy required, for high-speed design, and the use of a precision field solver is mandatory. I mentioned earlier that a steep rise/fall time may be slowed by loading the signal line with a damping/back-matching resistor close to the source. This also serves to match the impedance of the driver to the transmission line. Unfortu- nately, using mainstream PCB layout software, one really has no idea what the driver imped- ance is, let alone the capability to match the driver to the impedance of the transmission line. Driver impedance is typically low, com- pared to a typical 50 ohm transmission line, but adding a series resistor, of the correct value, solves this issue. The need to terminate a PCB trace is based on several design criteria. The most important being an electrically long trace, when the length exceeds one sixth of the electrical length of the rising edge rate. But even if the trace is short, termination may still be required if the load is capacitive or highly inductive to prevent ring- ing. Series termination is excellent for point- to-point routes, one load per net. It also works well for traces that are electrically short and is used to fanout multiple loads radially from a common source (star routed) without affecting other circuits in the network. Series termina- tion reduces ringing and ground bounce. It is the most common termination used for high- speed design. Revisiting the real-world rise time edge rate (Figure 1), by placing a series terminator (close to the source) the ringing is reduced dramati- cally. This will reduce crosstalk and also knock off the radiation. In Figure 5, the red waveform is the original, ringing signal, and the blue waveform demonstrates the damping effect of a series resistor taking us back to a near ideal waveform. The insert is the projected emissions in the frequency domain. Figure 5: Ringing is reduced dramatically by adding a series terminator (simulated in HyperLynx).

Articles in this issue

Archives of this issue

view archives of Design007 Magazine - PCBD-Oct2017