Platform forum

ESD Protection

JohnsonMiller , 08-28-2016, 12:45 AM
Hi Guys,

Checking your sample board, I do see some ESD protection diodes, I got questions:
1- As a general rule, where we need to add ESD protection devices?
2- There are some interface IC (RS485, CAN , etc) which has build-in ESD protection, however I have seen design using this devices and also adding external ESD protection devices, I was wondering why? Example is TCAN337.
3- Does it make sense to have ESD test on board without enclouser?
robertferanec , 08-28-2016, 09:12 AM
1) Place ESD protection as close as possible to the connector. Use direct short connection between the connector pins and ESD pins (no VIAs).
Note: Do not give much space for the "ESD spark" discharge on the way to your ESD protection circuit. If an ESD pulse can discharge on the way to your ESD protection circuit, it is not going to protect. If you use an ESD gun and there is bad ESD protection, you can sometimes very nicely see the sparks getting between tracks on your PCB (or in the worse case it discharge inside the chip and if without protection, it can damage it).

2) Place these chips close to the connector. It may not be necessary add external ESD in case the chip has it, but some environments may require higher ESD protection than it is provided inside the chip. Also some chips (including CAN transceivers) have pin to pin compatible replacements and some of the replacements may not have the internal protection. That could also be a reason why you may want to use it.

3) Depends, but it is not a bad idea to do ESD for a bare board too. For example, if someone places the board inside a plastic box, enclosure is not really going to help with ESD.
JohnsonMiller , 08-29-2016, 11:05 AM
Thank you Robert for clean explanation, regarding (1), and along with physical location main question is electrical location, what type of IO or interface require ESD protection? My early suggestion is any net that human touch or ESD spark is probable, do you agree?
robertferanec , 08-29-2016, 12:59 PM
Yes, anything people can touch, but maybe there are more precise definitions when they do the official certification.
JohnsonMiller , 08-30-2016, 03:19 AM
Should we include Ethernet RJ45 with/without isolation transformer in the list? Reason for this question is that I have not seen ESD protection on the Ethernet related nets?
robertferanec , 08-30-2016, 07:38 PM
Some connectors are designed the way, that ESD spark will always discharge to the shield (if properly grounded), because the pins are very deep hidden or you can not normally directly touch them. Also, Ethernet is transformer isolated, there is no really reason to add ESD protection (you should not cross the transformer isolation voltage) - there is no reason why ESD should discharge to the Ethernet isolated pins. They are not connected to ground, they are basically "hanging in air" and if you touch them, maybe they can carry the potential, but I do not think you will see ESD spark there ... but that is my opinion
JohnsonMiller , 09-02-2016, 02:24 AM

Or in other words, you are saying we should connect shield of RJ45 connector to ground? I have checked some reference designs, figure is a sample.
They are assigning a separate net to shield (1), then connecting it to GND via some passive components, CAP or FerriteBead in some cases!(2) Also there is a cutout in top/bottom and internal layers. Cutout or void, make sense not allowing discharge to internal nodes and probably impedance tune.
Another interesting or let's say strange feature of this design, on each side of T1 you can see the ESD diodes, while T2 just the PHY side has those diodes, and very strangely placed on backside and connected using via! (4)

I have also question, it is the way that they treat crystals (5), there is cutout in nearby plane?

robertferanec , 09-02-2016, 10:06 AM
Properly grounded does not necessarily mean connect it directly to the board GND.

As I mentioned in another forum about mounting holes, this is very similar:
"I normally connect them to GND, but this depends on the type of board you are designing, what kind of enclosure you have and how it is going to be mounted in your system. Capacitors will prevent DC voltage flow e.g. if you have two boards connected together via an interface and they are grounded far away of each other (e.g. plugged in to MAINs in different rooms), but still makes a connection for high frequency signals e.g. in some cases it can help to filter noise or still be able handle some ESD discharge."

You may want to read also about guard ring:

The other things you noticed, such cutout around crystal, ESD on the ethernet or VIAs on the ethernet tracks - I would not do that. But you never know what are the reason of engineer who was doing the design.
Use our interactive Discord forum to reply or ask new questions.
Discord invite
Discord forum link (after invitation)

Didn't find what you were looking for?