pcb design - 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.

Answer

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.