# Why route air gaps for voltage isolation on PCBs?

Learning about PCB design for power supplies, I frequently see boards with routed gaps to separate low and high voltage sections of the layout.

Why go to the trouble of routing an air gap when etching the copper away should create the same level of isolation? Is the breakdown voltage of air much higher than FR4?

I assume that such gaps are used to avoid situations where copper may not be etched away perfectly.

• Air is a lot cheaper than FR4. – Marquis of Lorne Jun 27 '13 at 12:47
• @EJP The potential cost is in routing out the tabs as opposed to leaving existing FR4 material there. – JYelton Jun 27 '13 at 15:34

High voltage PCB design

High Voltage PCB design for arc prevention

A few reasons why:

1. When arc-over occurs, it could cause carbonization (a.k.a. "burning") on the PCB surface. This could result in a permanent short. This is also irreversible damage, where-as arc-over in air isn't (unless something else goes wrong). This would be especially bad if a single high-voltage spike created a permanent short, then any "low-level" voltage source would still have a low impedance path available.
2. You have the option of installing a high-dielectric strength shield (something much better than FR4/soldermask, and better than air).
3. Dust/dirt can accumulate on a board surface, reducing dielectric strength. Not as much of a problem (though still could be a problem) if that surface just isn't there.
4. In the second link, they did some experiments where humidity had a drastic effect on the breakdown voltage of the soldermask, and a smaller (though potentially still significant) effect on a slot. Their best result was from removing soldermask and cutting a slot (no significant performance hit).
5. Any inadvertent creepage mistakes will be removed by the router, though really this should be caught in the design stage, especially with modern CAD. The PCB might not work right if tracks has unexpected open circuits, and making a high-current track smaller could cause other issues :P
6. Required air clearance seems to be smaller than surface required surface creepage distance.

A quick look at some creepage/clearance tables :

clearance table III

creepage table IV

seems to confirm that creepage distance > clearance distance, especially with higher pollution degrees.

Pollution degree is a measure of how the environment could affect your PCB. See: Design for Dust.

Description of various polution degrees (table 1):

1. No pollution or only dry, nonconductive pollution, which has no influence on safety. You can achieve pollution degree 1 through encapsulation or the use of hermetically sealed components or through conformal coating of PCBs.
2. Nonconductive pollution where occasional temporary condensation can occur. This is the most common environment and generally is required for products used in homes, offices, and laboratories.
3. Conductive pollution or dry nonconductive pollution, which could become conductive due to expected condensation. This generally applies to industrial environments. You can use ingress protection (IP) enclosures to achieve pollution degree 3.
4. Pollution that generates persistent conductivity, such as by rain, snow, or conductive dust. This category applies to outdoor environments and is not applicable when the product standard specifies indoor use.
• Thanks for a great, detailed answer. Can you explain what "pollution" means in this context? – JYelton Jun 27 '13 at 15:35
• The second link is excellent because it shows actual designs and the point at which they fail. Much thanks. – JYelton Jun 27 '13 at 15:44
• updated to include explanation of pollution in context with PCB design. – helloworld922 Jun 27 '13 at 15:50
• Would give you more upvotes if I could. My searches on the subject were not effective because I kept trying to search for "air gaps on PCBs" instead of "high voltage PCB design." – JYelton Jun 27 '13 at 15:53
• The second link is now dead. – Bort May 20 '16 at 17:15

An air gap has a much higher breakdown level than non-coppered surfaces on a circuit board. There are two mechanisms at play - physical air-gap (clearance) and what is called "tracking" on PCB surfaces (creepage).

Creepage Distance. Creepage is the shortest path between two conductive parts (or between a conductive part and the bounding surface of the equipment) measured along the surface of the insulation. A proper and adequate creepage distance protects against tracking, a process that produces a partially conducting path of localized deterioration on the surface of an insulating material as a result of the electric discharges on or close to an insulation surface. The degree of tracking required depends on two major factors: the comparative tracking index (CTI) of the material and the degree of pollution in the environment.

and,

Clearance Distance. Clearance is the shortest distance between two conductive parts (or between a conductive part and the bounding surface of the equipment) measured through air. Clearance distance helps prevent dielectric breakdown between electrodes caused by the ionization of air. The dielectric breakdown level is further influenced by relative humidity, temperature, and degree of pollution in the environment.

As a practical example of air gap over PCB distance I once designed a high-voltage PSU (50kV dc). The output stages were diode triplers (unimportant for this example) but the PCB mounting the diodes and capacitors that took 6kV and turned it into 50kV had to have big holes around the components thus the "creapage" across the circuit board could not make a direct straight line across the PCB surface, rather it had to weave around the slots and holes and this gave it significantly higher breakdown voltage capabilities.

There is a similar question on stack exchange here that has tables of voltages and gaps for creapage and clearance.