Why Should ESD Protection Devices Be Placed Close to Interfaces? An Analysis of PCB Layout and Discharge Paths

Ideally, ESD protection devices should be placed between the connector and the chip being protected, and as close to the interface as PCB routing permits. There is no universal, fixed distance in millimeters that applies to every PCB. The key objective is to ensure that static electricity entering from the interface encounters the protection device first and is discharged via a short, direct path, rather than traveling along a long trace deeper into the board.

When conducting a post-mortem analysis of an ESD issue, I typically examine two things first: the placement of the TVS diode and the return path for its ground connection. Even if the component part number specified in the schematic is correct, if the protection device is placed too far away on the PCB or the ground trace takes a circuitous route, the transient voltage experienced by the chip may still exceed expectations.

Why Even a Short Trace Cannot Be Overlooked

PCB traces, pads, and vias all possess parasitic inductance. Electrostatic discharge (ESD) currents change rapidly, causing a transient voltage component to be superimposed along the discharge path; this can be understood through the following relationship:

V = L × di/dt

Here, L represents the parasitic inductance of the discharge path, and di/dt is the rate of change of the current. The longer the trace between the interface and the TVS, the more convoluted the TVS grounding path, and the more vias included in the series path, the greater the concern regarding the additional voltage generated by this segment.

Consequently, the voltage experienced by the chip is not merely the clamping voltage specified in the TVS datasheet. Factors such as the package, pads, traces, vias, ground planes, and component placement all play a role in the actual circuit loop. Component selection completes only half the job; the other half depends on the PCB design.

Route the signal through the protection node first.

The routing sequence should follow this path:

External connector → ESD or TVS protection device → Protected chip

The discharge path is:

Ground terminal of the protection device → Ground copper on the same layer → Nearby ground via → Inner-layer ground plane or the system-designated discharge ground

Ideally, the trace should run directly from the connector to the protection device's pad, and then from the pad to the chip. Avoid routing the main line toward the chip first and then branching off a long segment to connect to the TVS. Such a branch is commonly known as a "stub"; when an electrostatic discharge reaches the junction, it will not automatically divert toward the TVS, meaning the main line could still carry the transient pulse to the downstream circuitry.

Also, minimize layer changes between the connector and the TVS. If vias are unavoidable, place them after the protection node—that is, on the side closer to the chip. This ensures that the parasitic effects of the vias remain within the protected zone, rather than being part of the path the ESD travels before reaching the TVS.

You cannot simply pick any random GND point for the TVS.

The TVS grounding pin should be connected directly to the nearby copper ground—ensuring a short loop with minimal bends—and tied into the ground plane in the immediate vicinity. If the ground trace is long and thin, or if it routes to a distant point before connecting to ground, loop inductance will increase; in such cases, the actual clamping performance of the TVS cannot be determined solely by the device's specifications.

If a product incorporates chassis ground, shielding ground, and digital ground, first confirm the system-level grounding scheme before deciding where to connect the TVS return path. Do not bridge different ground networks simply for the sake of routing convenience. The handling of interface shielding shells and the return paths for signal line TVS devices often involve distinct current paths; these must be evaluated holistically within the context of the system's overall structure.

Another area easily overlooked is the unprotected trace section between the connector and the TVS. Reset lines, clock lines, and high-impedance nodes should not pass through this area, nor should they run alongside it for any significant distance. If board space is extremely limited, at least ensure the reference ground plane remains continuous, and pay close attention to potential coupling issues during the prototype stage.

High-speed interfaces must also account for signal integrity.

Placing a TVS diode close to the interface does not mean high-speed traces can be arbitrarily interrupted. For differential pairs, the component pinout must be checked, and the routing paths and pad structures of both lines should be kept symmetrical as much as possible; factors such as device junction capacitance, package parasitics, and branch lengths must also be evaluated. Once the layout is complete, ESD protection and signal quality must be verified separately; one cannot substitute for the other.

How to conduct checks during a PCB design review

1. Are the protection devices actually located between the connector and the chip?

2. Do the interface signals pass through the protection device pads before entering the board?

3. Are there any excessively long stubs between the main signal lines and the TVS?

4. Are there any layer-transition vias between the connector and the TVS that could be relocated to the protected side?

5. Is the path from the TVS ground pin to the ground copper, ground vias, and ground plane sufficiently short and direct?

6. Does the discharge path cross any slots in the ground plane, and are there reset lines, clock lines, or other sensitive signals near the unprotected area?

7. Were signal integrity checks and system-level ESD testing scheduled prior to finalizing the layout?

Frequently Asked Questions

What is the appropriate distance (in millimeters) between an ESD device and the interface?

There is no universal figure. Placement is influenced by factors such as the package, PCB stack-up, impedance control, connector structure, and available assembly space. The criterion is not a specific measurement on a ruler, but rather whether the path from the interface to the protection node is sufficiently short and the discharge loop is direct.

Is it acceptable to place the TVS diode next to the interface chip?

This is only feasible if the chip is located immediately adjacent to the connector. If the chip is far from the interface, placing the TVS diode next to the chip leaves a long stretch of unprotected trace, creating a risk that electrostatic discharge (ESD) could enter the PCB interior before reaching the TVS diode.

Is a single via sufficient for the TVS grounding pin?

You cannot judge based on quantity alone; factors such as via diameter, layer stack-up, ground plane location, the distance from the pad to the via, and the return path structure must also be considered. The goal is to minimize the inductance of the entire grounding path, and the specific number of vias should be determined through board design reviews and actual measurements.

Is system-level ESD testing still required after the schematic and simulations have passed?

Yes, it is. Real-world products involve enclosures, connectors, cables, shielding, and grounding contacts—factors that are difficult to fully capture in a schematic. If issues arise during system-level testing, you should trace the path segment by segment, starting from the current entry point and following the return path.

During design reviews, do not limit the discussion to whether the correct TVS model was selected. It is usually much clearer to map out the entire path—from the point where static electricity enters the interface, through the protection device, and back to the discharge ground—to identify unprotected traces or locations where parasitic inductance has been introduced.