8.2.2 Step 2: Physical Placement

A critical step in designing an optimized PDN is that proper care must be taken to making sure that the initial floor planning of the PCB layout is done with good power integrity design guidelines in mind. The following points are important for optimizing a PCB’s PDN:

• Minimizing the physical distance between power sources and key high load components is the first step toward optimization. Placing source and load components on the same side of the PCB is desirable. This will minimize via inductance impact for high current loads and steps
• External trace routing between components must be as wide as possible. The wider the traces, the lower the DC resistance and consequently the lower the static IR drop.
• Whenever possible for the internal layers (routing and plane), wide traces and copper area fills are preferred for PDN layout. The routing of power nets in plane provide for more interplane capacitance and improved high frequency performance of the PDN.
• Whenever possible, use a via to component pin/pad ratio of 1:1 or better (i.e. especially decoupling capacitors, power inductors and current sensing resistors). Do not share vias among multiple capacitors for connecting power supply and ground planes.
• Placement of vias must be as close as possible or even within a component’s solder pad if the PCB technology you are using provides this capability.
• To avoid any "ampacity” issue – maximum current-carrying capacity of each transitional via should be evaluated to determine the appropriate number of vias required to connect components.

Adding vias to bring the "via-to-pad” ratio to 1:1 will improve PDN performance.

• For noise sensitive power supplies (i.e. Phase Lock-Loops, analog signals like audio and video), a Gnd shield can be used to isolate coplanar supplies that may have high step currents or high frequency switching transitions from coupling into low-noise supplies.

Figure 8-2 Coplanar Shielding of Power Net Using Ground Guard-band