ESD protection question

[pix3l]

Hi all,

I'm working on a board where there are some signals being fed through the board, going from 1 connector to another connector, and I'm not quite sure whether I'm being too precautios with ESD protection. I've attached a drawing to show the idea: the signal has ESD protection next to both connectors and I'm not sure whether one of them is abundant.

Any advice?

Cheers,
Sander

[Gibson486]

Better safe than sorry....For me, any point that leaves the board at least gets steering diodes. 

[rs20]

The standard advice is to put the steering diodes as close to the connector as possible. But when one wants to go to the extreme and spend extra money deploying extra silicon on the board in the name of this rule, we really need to take a step back and re-evaluate because now we're using extra resources and have to ask why.

Moving the steering diodes close to the connector means they're further away from the DBP (device being protected), those traces leading between the steering diodes and the DBP are longer and have higher impedance, and therefore the ESD discharge sees the steering diodes as more preferable path to travel. This is why the rule is to put it close to the connector. But what you realise is that it's actually nothing to do with the connector, it's really about putting the steering diodes as far away from the DBP as possible (under the very specific condition that the steering diodes are sitting on the traces between the DBP and the connector of course, as opposed to be off on a side branch*.)  Steering diodes work on a USB thumb drive where the DBP, steering diodes and connector are within millimeters of each other, so one would be a fool to suggest that having the steering diodes 20mm away from the DBP would be ineffective just because the connectors are another 50mm away. What are you saying, that the ESD is magical and starts gaining destructive power as soon as it realises that it's passed through a connector? Of course not!

In this case, it's quite clear that you can place a single set of steering diodes above the junction Tee point. This is evidently equivalent to your board having a single connector there, and the pass-through facility being provided by an external three-headed cable. Both perfectly fine solutions from an ESD standpoint.

BTW, if you really want to have super duper bulletproof ESD protection, you'd be adding series resistance inline on the signal traces between the steering diodes and the DBP. I'm not saying for a second that this is warranted or anything but overkill for your application; but it is cheaper and vastly more effective than adding a second set of steering diodes.

(I may be wrong about all this, but I'm curious to find out why if so.)


* You can see why "put it close to the connector" has a nice ring to it, even if it's overly reductive and fails in cases like the OP's.

[pix3l]

Hi both,

Thanks a lot for your answers. This is very helpful.

So if I understand correctly you say that having one TVS should be enough and it could be placed on the vertical line just after the T junction in my drawing?

What I'm wondering is whether I should be worried about creepage distance on the board in the case of using one ESD suppressor. Or is the creepage on a board much less than the 1kV/mm through air?

Cheers,
Sander

[T3sl4co1l]

If you can afford the extra routing space, and wish to save on protection components, then routing the connector-to-connector traces around the board perimeter, and teeing off that trace, with one ESD protector, then the MCU, will be acceptable.

What is not acceptable is having the ESD protection on a stub, or having the connection routed across the MCU area with only one protector (same idea, there's an unprotected stub between protector and MCU).  In that case, you would need two protectors as shown.

Tim