TVS diode for the CP2102N USB-to-UART bridge

[Nikos A.]

Hi I want to include ESD protection for the CP2102N USB-to-UART bridge. The datasheet (page 7) recommends the SP0503BAHTG TVS diode array. This diode has a max. positive clamping voltage of 8.5V, while the maximum rating of the bridge is 5.8V. If the diode clamps at 8.5V, won't destroy the chip?

https://eu.mouser.com/datasheet/2/368/cp2102n_datasheet-1634912.pdf
https://eu.mouser.com/datasheet/2/240/Littelfuse_TVS_Diode_Array_SP05_Datasheet_pdf-777043.pdf

[T3sl4co1l]

The chip is probably already rated for 1kV or so ESD, but you don't know what clamping voltage it experiences during that pulse.  The question is, will making a current divider with an external TVS, sink enough current to make e.g. 15kV contact discharge look like 1kV to the chip?

The answer is much improved with a series resistor between TVS and IC.  Typically one can afford a couple 10 ohms here.

Which, curiously, the transmitter impedance is rated 28-44 ohms, while 45 is needed for USB; evidently you should add 9 ohms, but they omit this (out of laziness / not worthwhile?).

Probably it's still fine with the "traditional" 22 ohms in series as well, though I would expect somewhat reduced maximum range in rare cases (i.e. when a random unit happens to have max. output resistance: it's a manufacturing distribution).  You might never notice this.

Direct ESD strike is also unlikely, as USB is fully shielded and the shield is generally struck preferentially over the pins.  Especially for mini/micro/USB-C.  (I would still prefer a TVS, myself.)

Tim

[Nikos A.]

Which, curiously, the transmitter impedance is rated 28-44 ohms, while 45 is needed for USB; evidently you should add 9 ohms, but they omit this (out of laziness / not worthwhile?).

Probably it's still fine with the "traditional" 22 ohms in series as well, though I would expect somewhat reduced maximum range in rare cases (i.e. when a random unit happens to have max. output resistance: it's a manufacturing distribution).  You might never notice this.

Thank you for the tip, I didn't notice that. I will include the 9ohm termination resistor since 36ohms is the typical value of the transceiver.

So it's safe to proceed with the TVS suggested in the datasheet right?

[T3sl4co1l]

Yes.

Or, round it to 10 ohms as the next common value.

Tim

[tooki]

Hi I want to include ESD protection for the CP2102N USB-to-UART bridge. The datasheet (page 7) recommends the SP0503BAHTG TVS diode array. This diode has a max. positive clamping voltage of 8.5V, while the maximum rating of the bridge is 5.8V. If the diode clamps at 8.5V, won't destroy the chip?

https://eu.mouser.com/datasheet/2/368/cp2102n_datasheet-1634912.pdf
https://eu.mouser.com/datasheet/2/240/Littelfuse_TVS_Diode_Array_SP05_Datasheet_pdf-777043.pdf

We don’t know much about the reaction times of each. It’s entirely possible the IC can handle 8.5V for some very short amount of time. (So while a sustained 8.5V would damage it, a very brief pulse — as happens in an ESD event — of 8.5V wouldn’t.)

Just be sure to lay out your USB data lines carefully, using 90 ohm impedance-controlled differential traces. I’ve seen a CP2102N board fail completely because of poor USB data line layout. I found it easiest to put the TVS array on the opposite side of the board so it could sit directly beneath the USB traces without affecting their placement.

[Nikos A.]

We don’t know much about the reaction times of each. It’s entirely possible the IC can handle 8.5V for some very short amount of time. (So while a sustained 8.5V would damage it, a very brief pulse — as happens in an ESD event — of 8.5V wouldn’t.)

Just be sure to lay out your USB data lines carefully, using 90 ohm impedance-controlled differential traces. I’ve seen a CP2102N board fail completely because of poor USB data line layout. I found it easiest to put the TVS array on the opposite side of the board so it could sit directly beneath the USB traces without affecting their placement.

Thank you for your input tooki, I will use a surface mount USB connector, and my plan is to route on a two-layer PCB through a 90ohms differential coplanar. It will give me a manageable trace width and gap. Also I calculated the trace length to be at least 1/6 of the critical length.

[T3sl4co1l]

If you can place connector, TVS and UART adjacent (trace length a couple cm total), impedance and differential won't really matter.

What is board thickness?  Those trace widths are suspiciously small for 2-layer.  Make sure dielectric height (height to plane) is correct.

Tim

[Nikos A.]

I set up a standard 1.6mm PCB thickness with 1.5mm FR-4

[voltsandjolts]

It's only USB Full Speed which is 12MHz, forget about impedance control and just do sensible routing on a double sided board made of 'whatever'.

[tooki]

Since the OP has the ability to do impedance controlled traces, and clearly knows how to do it, there’s no reason not to! No, it’s not essential, but why not eliminate every source of uncertainty that easily can be?

[voltsandjolts]

The OP seems to think "controlled impedance because USB". As a learning exercise, sure, but its not needed here.
Part of being an engineer is knowing where to spend the time (=money), for hobbyists its not a consideration.

[Njk]

The real problem with BAHTQ is the capacitance (30 pF). It's very old TVS type. No idea why it is still referenced. It was suitable for USB1.1, but for 2.0 you need something better (2-3 pF or less), to avoid certification problem because of D+/D- timings degradation. Better options are available (TI TPD1E1B04, Tech Public ESD5V0B03-323, etc.)

[voltsandjolts]

That's for USB2 HS 480Mbps, this is just USB2 FS 12Mbps, as seen in USB 1.1

[Njk]

Yes, it still uses FS. Did not noticed that in the spec

[tooki]

The OP seems to think "controlled impedance because USB".

USB data lines are 90 ohm differential, it’s part of the standard. So yes, one should aim for that.

[voltsandjolts]

At 12Mhz, total waste of time. At 480Mhz, absolutely yes.

[tooki]

Just because it’s not absolutely critical doesn’t make it a waste of time. It’s still a good idea to stick to what the standard says!!

As I said: I’ve seen a CP2102N board fail entirely because of bad USB layout. Admittedly it was really bad, but still.

Again: since OP has the ability and knowledge to do it, they should. It takes little effort and reduces the risk of it not working.

[voltsandjolts]

it’s not absolutely critical

For the few cm of tracks from connector to mcu, it's not critical in any way, shape or form, there is huge margin at 12MHz.
In fact, I'd be interested to see that pcb layout where you say it caused problems, that's quite an achievement!
Seperate DP/DM around different sides of a high power DCDC converter maybe?!

[tooki]

it’s not absolutely critical

For the few cm of tracks from connector to mcu, it's not critical in any way, shape or form, there is huge margin at 12MHz.
In fact, I'd be interested to see that pcb layout where you say it caused problems, that's quite an achievement!
Seperate DP/DM around different sides of a high power DCDC converter maybe?!

I don’t have the design files unfortunately, but I do have a few of the nonfunctional boards I could beep out tomorrow.

They were basically the ESP32 Devkit C reference layout, modified to not use 0402 components. (So what’s on it is the ESP32 module, the CP2102N, a 1117 LDO, the two programming transistors, a few diodes, the power LED, and passives.) For reasons unbeknownst to me, the kid doing it didn’t just scoot around the few things that were in the way, but tore up all existing traces and then did them all anew. I remember one of the USB data lines taking a weird stroll around one way, while the other was more direct. His boards simply wouldn’t enumerate. Windows would sometimes make the “new device” sound, but then it would be followed by some error message.

I then took my own shot at the same task (modifying the layout to larger passive footprints), plus extending the USB a few mm to a pin header in lieu of a micro-B port, and it worked flawlessly. I then fully integrated the CP2102N and ESP32 module into the main PCB. It also works perfectly. (I did use impedance control in Altium for the USB data lines on the fully integrated board.)