Does USB 2.0 high speed host require a chassis ground?

Question

I'm trying to design a microcontroller-based board in which the MCU will function as a USB 2.0 High Speed (480 Mbit/s) host for connected USB HS devices. I have been researching circuit design for USB HS, including issues like matching trace lengths, spec-compliant differential impedance, ESD protection, etc. One issue that comes up in some references (such as this answer: Ground and earth layers on PCB) is the need for separate digital and chassis grounds.

I am just designing a bare prototype PCB with no enclosure to ground to. After a few revisions of the PCB, I may want to 3D print a plastic enclosure to make it look nice, but even then there would be no true earth ground available to me. Does this lack of a chassis/earth ground mean that USB 2.0 HS speeds are not attainable in this circuit? How bad might the performance degradation be if I get everything else right?

For clarity:

• My board is powered by a 9V (unregulated) wall wart connected through a DC barrel jack on the PCB, with, possibly, a 9V battery backup in case the cord comes unplugged. From this I plan to create regulated 5V and 3.3V rails. The wall wort is two pronged, so there is no earth ground available even from it. I am just a hobbyist and do not want to touch mains voltages, so building an entire PSU (i.e., A/C transformer + rectifier) is something I'd prefer not to do.

• The closest I could come to a chassis ground that I can think of is to call the USB shield the chassis ground and treat it as such, i.e., connect it through a 1nF/3kV capacitor to the signal ground plane in the PCB. But is this a good enough "chassis" to be worth doing or do I need an entire separate chassis ground layer in the PCB stack to accomplish anything?

Answer 1

Chassis and signal return serve different purposes. Using one as the other requires some considerations and definitely layout provisions.

But do you even need a chassis node? It's mainly an ESD fast-track and EMI shield in your application. Both of these functions are nice to have, but can be lived without as commenters have noted. As you lack mains voltage, you don't need the protective Earth function for Class I equipment.

• Prevent EMI with good layout. Your biggest concern will be the long cables anyway, and it doesn't matter for EMI if there is Earth Ground or any other potential and the other end of thise cables. You must make sure, not to develop large common-mode currents over those cables. Certainly possible without a chassis, e.g. with common-mode chokes.

• ESD can be nasty, so you have to design stuff in a way that the ESD strikes rugged structures, e.g. your GND plane, instead of susceptible parts like MCU.

Also note that none of the classical tasks of a chassis are achieved by an on-board chassis plane in the stackup. That is just a wasted layer.

As you are designing the host, this still leaves the question about how to connect the shield. This should be connected to the host chassis, so you have to assign something as your chassis node. In your case, I would derive the Chassis just plainly from your ground plane with a short (or 0 Ω resistor).

Answer 2

The below is take from TI application note(USB 2.0 Board Design and Layout Guidelines).

This is also a very good reference.(How to correctly connect a USB shield on a PCB)

Place a ferrite in series with the cable shield pins near the USB connector socket to keep EMI from getting onto the cable shield. The ferrite bead between the cable shield and ground may be valued between 10 Ω and 50 Ω at 100 MHz; it should be resistive to approximately 1 GHz. To keep EMI from getting onto the cable bus power wire (a very large antenna) a ferrite may be placed in series with cable bus power, VBUS, near the USB connector pin 1. The ferrite bead between connector pin 1 and bus power may be valued between 47 Ω and approximately 1000 Ω at 100 MHz. It should continue being resistive out to approximately 1 GHz, as shown in Figure above.