What Is Altium's PDN Analyzer and When Should You Use It?

Detailed Explanation

Schematic-level simulation and design-rule checks confirm that a power net is connected correctly, but they don't know anything about how wide the actual copper is, how many vias connect a plane to a component pad, or how far a load sits from its regulator on the finished board. PDN Analyzer fills that gap by working from the completed PCB layout itself: it extracts the actual shapes of every power and ground plane, trace, and via along a defined power net, and builds a resistive mesh model of that copper.

Given the current each load component draws and the voltage each source (VRM, battery input, or regulator output) supplies, the tool solves that resistive network to report two things across the board:

• IR drop: how much the voltage sags between the source and each load, due purely to the resistance of the copper it travels through. A rail that leaves the regulator at a clean 3.3V can arrive at a component several centimetres away measurably lower once real copper resistance, via count, and current draw are accounted for.
• Current density: where current concentrates in the copper. A plane with a narrow neck, an isolated island connected by too few vias, or a trace segment carrying more current than its width comfortably supports shows up as a hotspot, even if the DRC and connectivity checks pass cleanly.

Because the analysis depends on physical geometry, running it earlier than a substantially complete layout doesn't give a meaningful result. It's most useful once plane shapes, via stitching, and component placement for the power section are settled, but before the board is released for fabrication.

Setting Up an Analysis

A typical PDN Analyzer setup involves three inputs: identifying the source (the regulator or connector supplying the rail, with its nominal output voltage), identifying every sink (each load component on that net, with its expected current draw), and defining the tolerance band the rail needs to stay within at each load. Sink current values should come from the actual component datasheets and the board's real operating condition (worst-case load, not typical), since the analysis is only as accurate as the current figures fed into it.

The tool then produces a colour-coded overlay directly on the board view: green for copper within acceptable voltage-drop and current-density limits, shading toward red as either measure approaches or exceeds the defined threshold. This makes it straightforward to spot a specific via cluster, plane pinch point, or long thin trace run that needs more copper, more vias, or a repositioned component, without manually calculating resistance by hand across an irregular plane shape.

A Worked Example

Consider a board with a 1.0V FPGA core rail supplied by a point-of-load regulator, feeding an FPGA that draws up to 4A under worst-case load. The regulator sits roughly 60mm from the FPGA on a 2oz copper plane, connected through a cluster of six 0.3mm vias where the plane transitions between layers near a connector cutout.

Copper resistance, not the regulator's own tolerance, is what PDN Analyzer is checking here: even a well-regulated 1.0V ±3% output (a 30mV budget) can lose a meaningful fraction of that margin to plane and via resistance over 60mm at 4A if the plane is narrower than it looks on screen, or if the via cluster is the effective bottleneck rather than the plane area either side of it. Running the analysis with the regulator as the source and the FPGA as a 4A sink shows exactly how much of that 30mV budget the copper itself consumes, and highlights whether the via cluster near the cutout is the limiting factor rather than the plane's overall width. If the result eats too much of the tolerance budget, the fix is usually widening the plane where the cutout forces a pinch, adding vias to the transition cluster, or moving the regulator closer, not changing the regulator's own specified tolerance.

PDN Analyzer vs AC PDN Impedance Analysis

PDN Analyzer addresses a DC problem: does the copper carry the required current without an unacceptable voltage drop or a thermal hotspot. It does not address the separate, frequency-domain question of whether the power delivery network's impedance stays low enough across the frequencies a load actually demands current at during fast switching events, which is the problem decoupling capacitor placement and target-impedance design solve. A rail can pass PDN Analyzer's DC check completely and still ring or sag transiently if the decoupling network is poorly chosen or placed. Treat the two as complementary checks on the same power delivery system, not substitutes for each other: DC copper sizing and via count from PDN Analyzer, and decoupling capacitor selection and placement for the AC transient response.

When It's Worth Running

PDN Analyzer earns its setup time on boards where a load has a tight voltage tolerance, a high current draw, or both. A modern FPGA or high-performance MCU core rail with a ±3% or tighter tolerance and several amps of load current, a motor driver's power stage, or a busbar-style high-current distribution plane are the boards where a few tenths of a volt of unaccounted IR drop, or an underspecified via cluster running hot, actually matters. A lightly loaded 3.3V logic rail feeding a handful of low-current ICs rarely needs this level of scrutiny; standard plane and trace sizing practice and current-capacity trace width guidance are usually sufficient there.

Design Considerations

• Feed the analysis real worst-case currents, not nominal ones. Using a component's typical operating current instead of its peak or worst-case datasheet figure produces an overly optimistic result that won't hold up in the field.
• Via count and size limit current just as much as plane area. A wide plane connected to a load through a single small via can still show a hotspot at that via, because the bottleneck is the via's cross-sectional copper, not the plane it feeds from.
• Re-run the analysis after any late-stage layout change that touches the power section, such as component repositioning, a plane split, or a stack-up change. A result generated before those changes no longer reflects the board.
• This tool checks copper sizing, not thermal management of the components themselves. A component drawing more current than its package can dissipate needs heatsink or thermal design work in addition to a clean PDN Analyzer result.
• Zeus Design's PCB design team runs power-delivery validation, including IR-drop and current-density analysis, as a standard part of high-current and multi-rail board layouts. Learn more about our circuit board design services.

Common Mistakes

• Running the analysis on an early or partial layout, before plane shapes and via stitching are finalised, and treating the result as final.
• Using default or estimated sink currents instead of datasheet worst-case figures, which understates real voltage drop.
• Treating a clean PDN Analyzer result as proof the power delivery network is fully validated, when it has not checked AC impedance, decoupling capacitor placement, or transient response at all.
• Ignoring a flagged hotspot because the board "has always worked that way" on a previous revision, without accounting for a higher-current component substitution or a changed operating condition.