Electronics Design AU
PCB DesignCompliance

What Are PCB Creepage and Clearance Distances, and How Do You Determine Them?

Last updated 7 July 2026 · 7 min read

Direct Answer

Clearance is the shortest distance through air between two conductors at different potentials; creepage is the shortest distance between them measured along the surface of the insulating material separating them. Both exist to prevent a dangerous or damaging electrical breakdown — clearance prevents arcing through air, and creepage prevents a conductive path forming across a contaminated or tracked insulating surface — and both must be verified independently, since a design can satisfy one while violating the other. The required minimum distance for each is not a single fixed number: it's determined by the circuit's working voltage, the pollution degree of the operating environment, and — for creepage specifically — the comparative tracking index (CTI) of the insulating material, looked up in tables published in IPC-2221 (general PCB spacing) or IEC 60664-1 (insulation coordination for equipment, referenced by most electrical safety standards).

Detailed Explanation

Creepage and clearance are named in passing across several pages on this site — mains-adjacent buck converter layouts, PoE isolation barriers, optocoupler and digital isolator selection, and connector voltage ratings all flag that "creepage and clearance must be checked" without explaining what determines the actual required distance. This page covers that directly: the two definitions, the standards that set the numbers, and the factors that actually drive the required spacing on a real PCB.

Clearance: The Through-Air Distance

Clearance is the shortest distance through air between two conductive parts at different electrical potentials — measured as a straight line (or the shortest path around any protrusion), regardless of any solid insulating material that might sit between them. Clearance exists to prevent electrical breakdown of the air itself: at a high enough voltage relative to the distance, air ionises and arcs over, a fundamentally different failure mode from surface tracking.

Clearance requirements depend primarily on:

  • Working voltage — the actual voltage the insulation experiences in normal operation, including any recurring peak, not just the nominal RMS value.
  • Altitude — air is a progressively less effective insulator as atmospheric pressure drops, so clearance requirements increase for equipment intended to operate above roughly 2000 m; most consumer/commercial products designed for typical altitudes use the standard sea-level-referenced table values without correction.
  • Overvoltage category and pollution degree, to a lesser extent than for creepage.

Creepage: The Surface-Tracking Distance

Creepage is the shortest distance between the same two conductive parts, but measured along the surface of the insulating material separating them, following every contour of that surface rather than cutting through it. Creepage exists to prevent a different failure mode: surface tracking, where humidity, contamination, or dust on the insulating surface between two conductors creates a progressively conductive path, which under a sustained voltage can carbonise the surface (particularly for the wrong resin systems) and form a permanent, low-resistance track — an insulation failure that clearance alone cannot prevent, since it doesn't rely on air breakdown.

Because creepage is a surface phenomenon, its required distance depends on more variables than clearance:

  • Working voltage.
  • Pollution degree — how contaminated the operating environment is expected to be (see the FAQ above for the four-level scale).
  • Material Group / Comparative Tracking Index (CTI) — a rating of how resistant the specific insulating material is to forming a conductive track under contamination, from IEC 60112 testing. Material Group I (CTI ≥ 600) is the most track-resistant; Material Group IIIb (CTI 100–175) the least. Standard FR-4 PCB laminate typically falls in Material Group IIIa or IIIb, which is why creepage requirements on a bare PCB surface are often larger than designers expect coming from a components-and-connectors mindset.

Which Standard to Use

IPC-2221 (the base PCB design standard covering electrical spacing, among other topics) publishes minimum clearance and creepage tables directly in terms of voltage and altitude/pollution-adjacent categories, and is the most commonly referenced source for general electronic-equipment PCB spacing in a design-for-manufacture context — see what are PCB design rules (DRC)? for where these checks fit into the broader design-rule-check process.

IEC 60664-1 is the more rigorous insulation-coordination standard, and is the one that most product safety standards (including IEC 62368-1, covering most consumer/ICT/AV equipment, and the electrical safety standards behind Australian RCM marking — see how to get RCM certification in Australia) actually reference and require compliance against. IEC 60664-1's tables are structured around working voltage, pollution degree, material group, and overvoltage category together, giving a more granular (and often more demanding) result than a simplified IPC-2221 lookup.

Practical rule: for any product that must pass formal safety certification, design to the specific safety standard's referenced insulation-coordination requirements (typically IEC 60664-1, via whatever product safety standard applies) rather than relying on IPC-2221 alone — IPC-2221 is a reasonable general PCB-design reference but is not always what a certification test house will check the product against.

Where This Matters Most in Practice

  • Isolation barriers. Any design with a galvanic isolation boundary — an isolated flyback supply's primary-to-secondary gap, an optocoupler or digital isolator's data path, a PoE PD's isolation transformer secondary — must maintain creepage and clearance across that boundary independently of the isolator component's own isolation voltage rating; see optocoupler vs digital isolator and Power over Ethernet (PoE) for embedded devices for where this specifically applies.
  • Mains-adjacent and high-voltage sections. Any PCB section carrying mains voltage, or a DC bus above roughly 30–60 V, needs creepage/clearance checked against the actual working voltage present, not just the nominal supply rating — see how should you lay out a buck converter PCB? for where this interacts with a switching regulator's layout.
  • Connector selection. A connector's voltage rating alone doesn't guarantee adequate creepage/clearance for the application's actual pollution degree and working voltage — see how do you select the right connector for a PCB design? for the connector-specific version of this same requirement.

Design Considerations

  • Determine working voltage correctly before looking up spacing. Working voltage for spacing purposes includes recurring peak voltage, not just steady-state RMS — a switching regulator's ringing voltage spike, if it recurs on every switching cycle, is part of the working voltage the insulation must withstand, not a transient to be ignored.
  • Confirm pollution degree honestly for the product's actual operating environment, not the most favourable assumption. A conformally-coated, fully sealed enclosure genuinely qualifies for a lower pollution degree; an enclosure with any vent, seam, or connector opening exposed to a normal indoor environment should be assessed at Pollution Degree 2, not 1.
  • Use PCB slots to extend creepage where board space is tight, but remember a slot only helps creepage — it does nothing for clearance, since clearance is a straight-line through-air measurement that a solid board material doesn't interrupt in the first place.
  • Check both distances independently, not just the larger of the two. Because clearance and creepage depend on different variables, a layout can pass one and fail the other — verify each against its own applicable table rather than assuming the more conservative-looking number covers both requirements.

Common Mistakes

  • Using the connector or component's voltage rating as the PCB spacing requirement. A connector or isolator's own voltage/isolation rating describes that component; the PCB copper spacing on the board around and beyond it is a separate requirement that must independently satisfy the applicable creepage/clearance table for the actual working voltage and pollution degree.
  • Assuming standard FR-4 has a high CTI. Off-the-shelf FR-4 PCB laminate commonly falls in Material Group IIIa or IIIb (CTI well below the highest-rated materials), which increases the required creepage distance compared to what a components-only mindset would assume — check the actual laminate's CTI rating if creepage margin is tight.
  • Designing to IPC-2221 alone for a product that requires formal safety certification. IPC-2221 is a useful general PCB design reference, but the certification test house will check against the specific product safety standard's insulation-coordination requirements (usually derived from IEC 60664-1) — design to that standard from the start rather than discovering a shortfall at formal testing.
  • Forgetting altitude derating on a product intended for high-altitude deployment. Clearance requirements increase above roughly 2000 m because air is a less effective insulator at lower pressure — a design validated only against sea-level clearance tables can fail on equipment deployed at altitude even though nothing else about the design changed.

Zeus Design's PCB design team applies the correct creepage, clearance, and isolation-coordination requirements — sized to the product's actual working voltage, pollution degree, and applicable safety standard — as part of complete electronics product design.

Frequently Asked Questions

Do clearance and creepage need to satisfy the same distance requirement?
No — they are two independent requirements measured differently, and the required minimum distance for each is usually different at the same working voltage. Clearance depends only on working voltage and, for higher voltages, altitude (air is a less effective insulator at higher altitude, so clearance requirements increase above 2000 m in most standards). Creepage depends on working voltage, pollution degree, and the insulating material's comparative tracking index (CTI) — a lower-CTI material (more prone to surface tracking, such as many standard FR-4 laminates) requires more creepage distance than a high-CTI material at the same voltage and pollution degree. In most practical PCB designs, the required creepage distance is equal to or larger than the required clearance distance at the same working voltage, because creepage has more variables working against it — but both must be checked independently against their own table, not assumed to be equal.
What is pollution degree, and which one applies to a typical electronic product?
Pollution degree describes the environment the insulation actually operates in, on a 1–4 scale defined in IEC 60664-1: Pollution Degree 1 (no pollution, or only dry, non-conductive pollution — e.g. inside a sealed, conformally-coated enclosure), Pollution Degree 2 (normal indoor environment where only occasional, temporary condensation-driven conductivity occurs — the default assumption for most consumer and commercial electronics in a housing), Pollution Degree 3 (conductive pollution is expected, or dry non-conductive pollution that can become conductive from condensation — typical of unsealed industrial or outdoor equipment), and Pollution Degree 4 (continuous conductivity from rain, snow, or similar — rare for enclosed products). Most commercial and consumer electronics in a normal indoor enclosure are designed to Pollution Degree 2; industrial equipment in an unsealed or harsher environment is often designed to Pollution Degree 3, which requires meaningfully larger creepage distances at the same working voltage and material.
How do I extend creepage distance on a PCB without making the board bigger?
The standard technique is a PCB slot or cutout: routing a physical gap through the board material directly between the two conductors, which forces the surface-tracking path to detour down one wall of the slot, across its base, and back up the other wall — increasing the effective creepage path length within the same board footprint. This is the standard construction used across an isolation barrier on isolated power supplies and digital/analog isolators (see how isolator manufacturers specify a recommended slot in their evaluation board layouts). A slot does not help clearance, since clearance is measured as the shortest through-air distance regardless of any solid material in between — only a genuine increase in the straight-line air gap, or a solid insulating barrier rated for the working voltage, satisfies clearance.

References

Related Questions

What Is a PCB Stack-Up, and How Do You Design One?

A PCB stack-up is the arrangement of copper and dielectric layers in a board. Here's how layer count and plane assignment shape a stack-up design.

What Are PCB Design Rules (DRC), and Why Do They Matter?

PCB design rules define the manufacturability and electrical constraints a layout must meet. DRC is the automated check that verifies them before fabrication.

How Do You Get RCM Certification for a New Electronic Product in Australia?

How to get RCM marking in Australia: standards selection, NATA lab testing, Declaration of Conformity, and ACMA registration — explained step by step.

Optocoupler vs Digital Isolator: How Do You Choose?

Optocouplers suit low-speed, AC, and triac circuits. Digital isolators win for UART/SPI isolation and high-noise switching environments. How to choose.

How Do You Design Power over Ethernet (PoE) into an Embedded Product?

Design Power over Ethernet (PoE) into an embedded product: PD controller ICs, IEEE 802.3af/at/bt classification, isolation, and the DC-DC stage that follows.

How Do You Select the Right Connector for a PCB Design?

Select a PCB connector by current rating, pitch, mating cycles, contact plating, keying, and environmental sealing — the trade-offs that matter in production.

Related Forum Discussions

Using a certified ESP32 module — why does the complete product still need CISPR 32 testing for RCM?

We're building a commercial IoT product around an ESP32-WROOM-32E. Did a bit of research and found the module in the ACMA compliance labelli

Is a double-sided PCB enough for a simple ESP32 sensor board, or should I go multi-layer?

Building a little battery-powered sensor board around an ESP32 module (the kind with the PCB antenna already built into the module, not desi

Decoupling caps placed right next to the IC but still seeing power rail noise

Fast digital board, MCU running a few hundred MHz core clock plus a couple of high-speed peripherals. Put 100 nF caps right next to every po

Best 4-layer stack-up for a board with both analog and digital circuitry?

Spinning up a board with an STM32 doing the digital side and a precision analog front end (instrumentation amp into an ADC) reading a low-le