# What are good practices for traces on the "mains" side of a relay?

I'm trying to switch a reasonably sized load (800W at 120VAC), so let's call it 7A using a PCB interfaced to a microcontroller.

Obviously I need to make sure that the relay I'm using can support this load, and I can use the circuit calculator to figure out the trace width for a given thickness.

For example, this PCB has a relay with thick external traces (86 mil) and a two-layer signal plane (the dashed line area). However, I'm not crazy about the separation at the terminals themselves. My goal is reliability and longevity.

I guess it's a broad question, but I'm very new at this, and would love for some guidance on "best practices" for high(er) voltage traces like this.

Thanks, Chris

• In the absence of any specific requirement, regulatory or otherwise, keep any 110V line power at least 5 mm away from any isolated parts of the circuit. Solder mask doesn't count, only real distance. Feb 7, 2013 at 16:35
• Hi Olin, Thanks for the comment. Can you clarify "solder mask doesn't count, only real distance?" Feb 9, 2013 at 3:57
• Solder mask is a insulator, and you might be tempted to not require as much spacing due to there being this insulating layer over the wires. However, you can't count on that. Solder mask can easily have small cracks, so for purposes of voltage isolation you have analyze as if the traces are open on top. Using the PC board itself as the insulator is legitimate in some cases. This depends in part on which layers the traces are on, but may also require derating the creapage distance. Feb 9, 2013 at 14:53

what you're interested in is creepage and clearance distances. Creepage basically is the separation distance of copper traces. Clearance on the other hand is the air gap separation of leads/conductive surfaces.

Typically, most standards are based on conditions being pollution degree 2 and overvoltage category II. It is important to note that as working voltage, pollution degree, overvoltage category, and altitude increase, the creepage and clearance distances also increase. The altitude is particularly important when testing to EN 61010.

Using the data from table IV, if we choose a working voltage of 125VAC, pollution degree 2, and material group IIIa or IIIb ther is a minimum of 1.5mm creepage required.

Clearance is calculated using the peak voltage, for 120VAC that's ~170Vdc. this table has the appropriate air-gap clearance requirements. Assuming peak voltage of 210Vdc, that means we will need at least a 2mm clearance.

Personally I like having a comfortable safety margin, so at the minimum I would probably go with 3mm creepage and 4mm clearance, with more being better.

There are a few other circuit protection devices you can add to your system to prevent spikes such as Metal Oxide Varistors (MOVs), Transient voltage suppression diodes, circuit breakers/fuses, etc.

Another route you can take is adding a physical barrier between devices, either by filling with an appropriately rated dielectric material (known as potting) or using a physical non-conductive shield.

This article has some other good high-voltage PCB design suggestions. Granted, they are generally catering for operations in KV's, but it does get you thinking about some of the potential problems and possible solutions when dealing with higher power PCB circuits.

• That's great, thank for the references & insights. Feb 9, 2013 at 3:58