PDN Impedance Analysis and Modeling: From Schematic to Layout

November 14, 2019 Zachariah Peterson

Traces and components on a PCB for use in PDN impedance analysis

We talk a lot about signal integrity around here, but signal integrity is intimately related to power integrity. This is about more than just reducing switching noise or ripple from your power supply/voltage regulator. This is where the impedance of your PDN in your PCB can rear its ugly head in certain designs, causing components in your board to fail to work as designed due to power problems.

Here’s where it helps to understand some basic models for PDN impedance analysis. If you can build some reasonably accurate models for PDN impedance, you can design proper decoupling networks for your component in order to keep the impedance of your PDN within acceptable limits.

Why Conduct PDN Impedance Analysis?

The high speed and high frequency designers reading this will already know the answer to this question. However, with technological demands mounting, we’ll all be high speed and high frequency designers sooner than we like, so it is important to understand how PDN impedance affects the behavior of signals in your PCB. Unfortunately, we don’t always do the best job of placing this information in one place, so I’ll happily do this here.

In short, your PDN impedance will affect the following aspects of your circuits:

  • Power bus noise. The voltage ripple created due to transient currents in your PCB. Note that, because your PDN impedance is a function of frequency, the voltage ripple caused by a switching will also be a function of frequency. Note that these transients can arise regardless of the level of noise in the output from your voltage regulator.

  • Damping in power bus noise. Any ripple on the power bus could appear as ringing (i.e., an underdamped transient oscillation) in some cases. This is one problem that can occur if your decoupling capacitor is incorrectly sized or if you do not account for your decoupling capacitor’s self-resonance frequency in your decoupling network.

  • Required level of decoupling. In the past, capacitors were insufficient for ensuring decoupling in PCBs with TTL and faster logic families due to their relatively low self-resonance frequencies (~100 MHz). Therefore, designers used interplane capacitance to provide sufficient capacitance to ensure decoupling. Newer capacitors with GHz self-resonance frequencies are available on the market, making them sufficient for providing decoupling in high speed/high frequency PCBs.

  • Current return path. Your return current will follow the path of least resistance (for DC current) or least reactance (for AC current). The impedance in your ground network will vary in space, which depends in part on parasitic coupling between signal traces and the PDN.

  • IR drop. The DC portion of your supply and return current will experience some losses due to the inherent resistance of the conductors that make up your PDN. The image below shows example PDN analysis results, illustrating the return current below a specific signal trace and the DC current in the same ground plane.

  • Timing jitter. Because signals have finite propagation time, the current drawn from decoupling capacitors and the regulator will take some time to reach the switching component. When these signals do reach the component, they can interfere with the output signal, effectively creating some jitter in the rise time for your signal. In general, timing jitter due to power rail noise increases with noise intensity and the length between the regulator and the component. On long power rails, this can cause timing jitter to reach hundreds on the order of nanoseconds, which could desynchronize data and increase bit error rates.

PDN impedance analysis output

Notice the signal trace in this PDN analyzer output

A Simplified Model for PDN Impedance Analysis

You can model the impedance spectrum of your PDN and its transient response directly from your schematic, as long as you account for parasitics in your PDN. In the model below, you’ll notice several circuit elements, but this model only contains two real components. The first is your power supply/regulator, which has some specified output impedance Z(out) and is typically an RL series. The second is the decoupling capacitor, which has an ideal capacitance of Cc1. The remaining circuit elements are parasitics. The Rs and Ls values are intended to model the inherent conductor resistance and parasitic power plane inductance, respectively. The Rp, Lp, and Cp elements account for parasitic coupling between power and ground planes (i.e., interplane capacitance).

PDN impedance analysis model

A simplified model for PDN impedance analysis. Image source: nwengineeringllc.com

Before analyzing this model, you need to determine or estimate the values of the various elements in your model. The decoupling capacitor values are easy; just get them from the datasheet for your desired capacitor. The interplane capacitance is also easy to roughly estimate; just use the dielectric constant for your substrate, the area of your overlapping ground/power planes, and the distance between them in your stackup, and you know the interplane capacitance Cp. The remaining R values can be calculated using your intended trace dimensions. The L values need to be estimated from the approximate loop inductance for each portion of the circuit; these values are generally on the order of pH to a few nH.

Your goal in analyzing this model is two-fold:

  1. Determine the impedance between the + and - terminals on the right side as a function of frequency. This can be done with a simple frequency sweep.

  2. Check that the PDN impedance is less than your target impedance. Note that the target impedance is calculated using the current a switching IC will draw into the PDN and the allowed voltage ripple:

PDN impedance analysis model

Target impedance

  1. Examine the behavior of transients by adding a current source in parallel with the power supply output (put the positive terminal before Z(out)). Set the current source to supply a delta-function impulse with total charge Q shown in the equation below, or to supply a stepped current. This will simulate a burst of current propagating to a switching IC at the right end of the PDN.

PDN impedance analysis model

Impulse magnitude you should use to simulate the transient response in your PDN

  1. Check that the lowest frequency PDN resonance (i.e., peak in the impedance spectrum) is greater than the knee frequency for your switching ICs. The idea is to minimize ripple over the broadest possible frequency band.

Note that point #3 is intended to model the transient response due to downstream switching ICs. If you have 10 ICs that will switch simultaneously and they all draw the same transient current into the PDN, then your impulse magnitude will be a factor 10 larger, and your target impedance needs to be a factor 10 smaller. Once you’ve examined these three points, you can move on to interpreting your results and determine what design steps you can take to suppress power fluctuations in your PDN.

How to Interpret Your PDN Impedance Analysis Results

Regarding points #1 and #2, you want to check that the PDN impedance is less than the target impedance at all frequencies between the clock frequency and the knee frequency (for digital signals) or within the relevant frequency you’ll be using (for analog signals). If this is the case, and you have calculated your impedance based on the case where every IC switches simultaneously, then your PDN will likely work as intended without any resulting signal integrity problems.

Addressing the results from point #3 depends on whether the transient response in your PDN appears as an underdamped oscillation. If the transient response is underdamped, then you need to bring this oscillation into the critically damped or overdamped regime. This requires using a larger decoupling capacitor, or using a capacitor with lower effective series inductance. Your decoupling capacitor should be sized to provide the impulse charge listed above, but you can certainly try to use a larger decoupling capacitor in order to change the conditions for the lowest PDN resonance so that the transient response is overdamped or immeasurably small.

Achieving the goal in point #4 is not always possible, but you should still make an attempt. Even if you can’t meet this design goal, you’ll still be in the clear if the impedance at a PDN resonance is still less than the target impedance and there is only one PDN impedance resonance within your relevant bandwidth. If there are multiple impedance resonance peaks within your relevant bandwidth, then you might be in trouble as the total impedance seen by the transient current is approximately the sum of the peak impedances; it now becomes likely that this total impedance exceeds the target impedance.

In addition to the decoupling capacitor sizing and self-resonance issues mentioned above, the results from point #3 should illustrate why interplane capacitance listed as a requirement for properly decoupling ICs with 1 ns or faster logic (e.g., ECL). Aside from using very large decoupling capacitors with very high self-resonance frequencies (they are now available on the market), placing the ground and power planes on adjacent layers was historically about the only way to provide the required level of decoupling in a PDN. Note that, whether you increase the interplane capacitance or decoupling capacitance by using multiple capacitors (again, see the article linked in the previous paragraph), making this capacitance sufficiently large will bring the transient response into the overdamped regime, effectively eliminating it.

What About the Die and Package?

Hopefully, the astute designer has noticed that the contributions from package and die impedance have not been included in the above analysis as they are built-in to the load in the PDN. These also need to be accounted for in the PDN as they contain capacitive and inductive parasitics.

PDN impedance analysis with component die and package

PDN model with package and die parasitics

With the powerful PCB design and analysis tools in Altium Designer®, you can analyze all aspects of your schematics and layout, and you can help prevent signal integrity problems that arise in complex PCBs. These tools are built on top of a unified rules-driven design engine, allowing you to perform important DRCs throughout the design process. You’ll also have access to a complete set of manufacturing planning and documentation features in a single platform.

Now you can download a free trial of Altium Designer and learn more about the industry’s best layout, simulation, and production planning tools. Talk to an Altium expert today to learn more.

About the Author

Zachariah Peterson


Zachariah Peterson has an extensive technical background in academia and industry. Prior to working in the PCB industry, he taught at Portland State University. He conducted his Physics M.S. research on chemisorptive gas sensors and his Applied Physics Ph.D. research on random laser theory and stability.

His background in scientific research spans topics in nanoparticle lasers, electronic and optoelectronic semiconductor devices, environmental systems, and financial analytics. His work has been published in several peer-reviewed journals and conference proceedings, and he has written hundreds of technical blogs on PCB design for a number of companies.

More Content by Zachariah Peterson
Previous Article
Pulsed Laser Diode Driver Circuit Layout for Lidar
Pulsed Laser Diode Driver Circuit Layout for Lidar

Here’s how your pulsed laser diode driver circuit works and how to place it on your PCB.

Next Article
Length Matching for High-speed Signals: Trombone, Accordion, and Sawtooth Tuning
Length Matching for High-speed Signals: Trombone, Accordion, and Sawtooth Tuning

You can use length matching for high-speed signals with trombone, accordion, and sawtooth tuning.