8.2.4 Step 4: Frequency Analysis

Delivering low noise voltage sources are very important to allowing a system to operate at the lowest possible Operational Performance Point (OPP) for any one Use Case. An OPP is a combination of the supply voltage level and clocking rate for key internal processor domains. A SCH and PCB designed to provide low noise voltage supplies will then enable the processor to enter optimal OPPs for each Use Case that in turn will minimize power dissipation and junction temperatures on-die. Therefore, it is a good engineering practice to perform a Frequency Analysis over the key power domains.

Frequency analysis and design methodology results in a PDN design that minimizes transient noise voltages at the processor’s input power balls. This allows the processor’s internal transistors to operate near the minimum specified operating supply voltage levels. To accomplish this one must evaluate how a voltage supply will change due to impedance variations over frequency. This analysis will focus on the decoupling capacitor network (VDD_xxx and VSS/Gnd rails) at the load. Sufficient capacitance with a distribution of self-resonant points will provide for an overall lower impedance vs frequency response for each power domain.

Decoupling components that are distant from their load’s input power are susceptible to encountering spreading loop inductance from the PCB design. Early analysis of each key power domain’s frequency response helps to determine basic decoupling capacitor placement, optimal footprint, layer assignment, and types needed for minimizing supply voltage noise/fluctuations due to switching and load current transients.

• Decoupling capacitors must be carefully placed in order to minimize loop inductance impact on supply voltage transients. A real capacitor has characteristics not only of capacitance but also inductance and resistance.

Figure 8-6 shows the parasitic model of a real capacitor. A real capacitor must be treated as an RLC circuit with effective series resistance (ESR) and effective series inductance (ESL).

Figure 8-6 Characteristics of a Real Capacitor With ESL and ESR

The magnitude of the impedance of this series model is given as:

Figure 8-7 Series Model Impedance Equation

Figure 8-8 shows the resonant frequency response of a typical capacitor with a self-resonant frequency of 55 MHz. The impedance of the capacitor is a combination of its series resistance and reactive capacitance and inductance as shown in the equation above.

Figure 8-8 Typical Impedance Profile of a Capacitor

Because a capacitor has series inductance and resistance that impacts its effectiveness, it is important that the following recommendations are adopted in placing capacitors on the PDN.

Wherever possible, mount the capacitor with the geometry that minimizes the mounting inductance and resistance. This was shown earlier in Figure 8-1. The capacitor mounting inductance and resistance values include the inductance and resistance of the pads, trace, and vias. Whenever possible, use footprints that have the lowest inductance configuration as shown in Figure 8-9

The length of a trace used to connect a capacitor has a big impact on parasitic inductance and resistance of the mounting. This trace must be as short and as wide as possible. wherever possible, minimize distance to supply and Gnd vias by locating vias nearby or within the capacitor’s solder pad landing. Further improvements can be made to the mounting by placing vias to the side of capacitor lands or doubling the number of vias as shown in Figure 8-9. If the PCB manufacturing processes allow it and if cost-effective, via-in-pad (VIP) geometries are strongly recommended.

In addition to mounting inductance and resistance associated with placing a capacitor on the PCB, the effectiveness of a decoupling capacitor also depends on the spreading inductance and resistance that the capacitor sees with respect to the load. The spreading inductance and resistance is strongly dependent on the layer assignment in the PCB stack-up. Therefore, try to minimize X, Y and Z dimensions where the Z is due to PCB thickness (as shown in Figure 8-9).

From left (highest inductance) to right (lowest inductance) the capacitor footprint types shown in Figure 8-9 are known as:

• 2-via, Skinny End Exit (2vSEE)
• 2-via, Wide End Exit (2vWEE)
• 2-via, Wide Side Exit (2vWSE)
• 4-via, Wide Side Exit (4vWSE)
• 2-via, In-Pad (2vIP)

Figure 8-9 Capacitor Placement Geometry for Improved Mounting Inductance

Decoupling Capacitor (Dcap) Strategy:

1. Use lowest inductance footprint and trace connection scheme possible for given PCB technology and layout area in order to minimize Dcap loop inductance to power pin as much as possible (see Figure 8-9).
2. Place Dcaps on "same-side” as component within their power plane outline to minimize "decoupling loop inductance”. Target distance to power pin should be less than ~500mils depending upon PCB layout characteristics (plane's layer assignment and solid nature). Use PI modeling CAD tool to verify minimum inductance for top vs bottom-side placement.
3. Place Dcaps on "opposite-side” as component within their power plane outline if "same-side” is not feasible or if distance to power pin is greater than ~500mils for top-side location. Use PI modeling CAD tool to verify minimum inductance for top vs bottom-side placement.
4. Use minimum 10mil trace width for all voltage and gnd planes connections (i.e. Dcap pads, component power pins, etc.).
5. Place all voltage and gnd plane vias "as close as possible” to point of use (i.e. Dcap pads, component power pins, etc.).
6. Use a "Power/Gnd pad/pin to via” ratio of 1:1 whenever possible. Do not exceed 2:1 ratio for small number of vias within restricted PCB areas (i.e. underneath BGA components).

Frequency analysis for the CORE power domain (vdd) has yielded the Impedance vs Frequency responses shown in Section 8.3.8.2, vdd Example Analysis.