I have a DB25 I/O connector, thru-hole. The pins connect to an SMT MCU, which I want to protect from ESD, specifically IEC 61000-4-2. I want to use SMT Zener diodes to protect the pins.
I am considering various layouts. I imagine the optimal layout would have the diodes between the DB25 and the MCU. In this way, an ESD event can be shunted to ground before it gets to the MCU
MCU <-> Diodes <-> DB25
However, I would like to take advantage of the thru-holes in the DB25 to simplify routing and reduce the number of vias that I would need. However, in doing so, the diodes will end up on the "other side" of the DB25.
MCU <-> DB25 <-> Diodes
Is this a bad idea? I'm slightly concerned about whether a sufficiently fast ESD strike could "split up" and reach the MCU before the diodes begin fully conducting.
If this is the case, would it be mitigated if the MCU <-> DB25 traces were run on bottom-layer, while DB25 <-> Diodes traces were on the top layer? Would the added vias between the MCU and DB25 encourage the ESD current to go through the diode instead?
Best Answer
ESD is difficult to deal with, and solutions are more black magic than science. That being said, what you want is for the impedance to ground to be smaller than the impedance to the chip you're protecting. There are several ways to do this, and the most practical solution will probably involve several of these things at once.
Placement and routing of traces is a good start. As you noted, MCU <-> Diodes <-> DB25 is probably the best, although MCU <-> DB25 <-> Diodes can work. To make it work, the traces to the diodes should be thick and short. The traces to the MCU should be long-ish and thin. But, IMHO, just doing this is not enough for a commercial product.
Put some sort of of resistor or ferrite bead between the DB25/Diodes and the MCU. I prefer resistors for this because their impedance is more predictable at high frequencies, but a bead could work too. A resistor of around 10 to 50 ohms is good, depending on the nature of the signals you're running. This resistor/bead will increase the impedance to the MCU, guiding the ESD to ground through a different way.
Put a capacitor in parallel with the diodes. A value of 3 nF is ideal for ESD protection. But depending on your signal you might have to use a smaller or larger one., or none at all. The largest you can get away with will also reduce your EMI problems. The basic function of the cap is to quickly absorb the ESD shock and re-emit it more slowly and with a smaller voltage. If the cap is large enough then the diode is not required. This cap also forms an RC filter with #2 above and prevents EMI from going in or out of the box.
Connect the shield of the DB25 to chassis ground, and make sure your chassis make a good shield.
Recently I had an issue with a USB device that would crash whenever an ESD zap happened within 8 feet of the box. In the end I had to connect the USB shell to Chassis, add 33 ohm resistors to the USB data lines, add caps, and diodes. Until I did all that I still experienced failures. If I left off one of those, any one, it would fail. Now it runs solid, even with 1 inch long sparks right to the chassis.