Guidelines for routing PCB traces and placing components are necessary when trying to maintain signal integrity, avoiding noise pick-up, and lower EMI. Although an endless number of precautions seems to be taken, this section provides only a few main recommendations as layout guidance.

1. Keep signal traces 3 times the trace-to-ground height, (d = 3h), apart to reduce crosstalk down to 10%. Because the return current density under a signal trace diminishes via a 1/ [1+(d/h)²] function, its density at a point d > 3h, is sufficiently small to avoid causing significant crosstalk in an adjacent trace.
   Figure 4-9 Separate Traces to Minimize Crosstalk
2. Use 45° bends (chamfered corners), instead of right-angle (90°) bends. Right-angle bends increase the effective trace width, and thus the trace impedance. This creates additional impedance mismatch, which may lead to higher reflections.
   Figure 4-10 Use 45° Bends Instead of 90° Bends
3. For permanent operation in noisy environments, connect the Enable inputs of an isolator through a via to the appropriate reference plane, that is, High-Enable inputs to the V_CC plane and Low-Enable inputs to the ground plane.
4. When routing traces next to a via or between an array of vias, ensure that the via clearance section does not interrupt the path of the return current on the ground plane below. If a via clearance section lies in the return path, the return current finds a path of least inductance around it. By doing so, it may cross below other signal traces, thus generating cross-talk and increase EMI.
   Figure 4-11 Avoiding Via Clearance Sections
5. Avoid changing layers with signal traces as this causes the inductance of the signal path to increase.
6. If, however, signal trace routing over different layers is unavoidable, accompany each signal trace via with a return-trace via. In this case, use the smallest via size possible to keep the increase in inductance at a minimum.
7. Use solid power and ground planes for impedance control and minimum power noise.
8. Use short trace lengths between isolator and surrounding circuits to avoid noise pick-up. Digital isolators are usually accompanied by isolated dc-to-dc converters, providing supply power across the isolation barrier. Because single-ended transmission signaling is sensitive to noise pick-up, the switching frequencies of close-by dc-to-dc converters can be easily picked up by long signal traces.
9. Place bulk capacitors, (i.e., 10 μF), close to power sources, such as voltage regulators or where the power is supplied to the PCB.
10. Place smaller 0.1-μF or 0.01-μF bypass capacitors at the device by connecting the power-side of the capacitor directly to the supply terminal of the device and through two vias to the V_cc plane, and the ground-side of the capacitor through two vias to the ground plane.
    Figure 4-12 Connect Bypass Capacitor Directly to V_CC Terminal