I'm working with two chips on a board, a dsPIC33F and a PIC24F as well as a serial EEPROM (24FC1025.)
I've seen these little ESD protection devices in 0603 packages:
http://uk.farnell.com/panasonic/ezaeg3a50av/esd-suppressor-0603-15v-0-1pf/dp/1292692RL
For MCUs like I'm using, is this necessary? The boards may be constantly handled and the external interfaces (I2C, UART) may be exposed to ESD.
Would the internal diodes protect the chip anyway and make these pointless?
You can certainly use such devices. They are usually a poor choice for anything that has lower power usage requirements as they have high leakage current.
You also have to be careful of the clamping voltage, ESD of ~200V can damage a micro-controller, the device you linked is specced at 500V max. Make sure whatever your trying to protect is actually be protected to the extent it needs.
For digital lines also pay attention to the capacitance of these device/package, they can screw up your signal integrity.
What I usually do if the input is likely to get hit with ESD, like an input that is often connected in the field is use a 2 pronged approach.
First Use a ESD device, or diodes closer to the circuit to protect, which type I would use depends on the signal/circuit in question. This is to protect against lower spikes, say 8kV. More and more you see this type of protection inside devices, especially boundary devices like RS232 drives and line drivers.
Second, when you build the PCB use spark gaps, which is really nothing more than putting 2 pads on the surface of the PCB, 1 being the signal, the other being a good ground and spacing them very close to each other, like 6 thou apart. This will protect against higher voltage hits, like 25kV. Pretty simple concept, the high voltage jumps the gap and goes straight to ground. Just be careful how you place these, as close to the connector as possible with the best possible ground connection.
Also pay attention to the manufacturing process your using, you don't want solder to accidental bridge the gap.
Gaps can be tough to do on digital traces and avoid changing the impedance, usually requires tweaking the signal termination after the prototype run.
There is some argument over the proper shape of the pad, some use half moons, some use pointed triangles with the tips near each other and some use square pads. I've always used square pads, the more area that is close to the other pad the more repeated strikes the gap will survive. The trade off is that the square pads will take the most effort to ensure there is no solder bridging. Best answer is to get your CM to not apply solder to these pads at all, but that can require special effort on their part.
I put similar parts on the signals that leave the board, such as UART, Ethernet, digital I/O. For intra-board signals, don't worry about it.
About the internal diodes: There's a limit of what the diode will take. The internal diodes will be OK with normal handling. The external diodes will protect against larger "shag carpet in the dead of winter" static shocks.
