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?

  • \$\begingroup\$ A chassis ground on typical USB devices is fairly uncommon and certainly not required. Think plastic thumb drives, web cams, etc. Are you possibly confusing signal ground (which is required to route controlled impedance traces) with an Earth ground ? \$\endgroup\$ Dec 25, 2022 at 5:14
  • \$\begingroup\$ No @jemalloc has a point, because the host should provide a shield ground. Not the plugged in device. I would also go for the cap/resistor combo connection to ‘GND’. \$\endgroup\$
    – RemyHx
    Dec 25, 2022 at 6:06
  • \$\begingroup\$ @RemyHx Cap/resistor in series or in parallel? The last article I read on this -- Example 1 on acmesystems.it/pcb_usb -- just had a 1 nF/3kV cap (no resistor) connecting "shield ground" (i.e., chassis ground) to signal ground. I interpreted this as an anti-ESD measure. What would be the purpose of the resistor? Thanks. \$\endgroup\$
    – jemalloc
    Dec 25, 2022 at 7:17
  • \$\begingroup\$ @tobalt Are GND / Chassis always shorted at the host? That depends on the pcb designer.. As I understand here the host is designed by jemalloc and he has a question about how and if to connect GND/Chassis... I red somewhere: if you ask 6 engineers how to make this connection, you get 12 answers... The antenna thing could also be reversed, from the used device. My thought was to at least provide a way to equalise potential differences, but to be honest I'm not sure about the solution. As is the internet. Principally shield should be a faraday cage. It's not now. \$\endgroup\$
    – RemyHx
    Dec 25, 2022 at 9:30
  • \$\begingroup\$ @RemyHx you are right about this being the host. I didn't read well. In this case, if you ask me 😉, I would just short the shield to the GND plane \$\endgroup\$
    – tobalt
    Dec 25, 2022 at 10:13

2 Answers 2


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).

  • \$\begingroup\$ "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." Thank you! I was wondering about that. \$\endgroup\$
    – jemalloc
    Dec 25, 2022 at 7:40

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)

enter image description here

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.

  • \$\begingroup\$ The ferrite on VBUS is serving as a low-pass filter for high frequency EMI on that line. Is it roughly equivalent in purpose and function to the LC low-pass filter in the schematic under the words "Example 1" on this page? acmesystems.it/pcb_usb Any advantage to the ferrite over the LC low pass filter (or vice versa)? \$\endgroup\$
    – jemalloc
    Dec 25, 2022 at 7:39
  • \$\begingroup\$ IMO it's not worth to consider individual conductors in a cable (e.g. shield) and prevent common-mode noise from them. It is common-mode. Decoupling one conductor with a bead is futile as the wires in the cable are all capacitively coupled. So this bead is bypassed by the other conductors. A common-mode bead on the cable is what inhibits cable noise. \$\endgroup\$
    – tobalt
    Dec 25, 2022 at 10:21
  • \$\begingroup\$ @jemalloc,Compared with general inductors, ferrite beads have a high resistance component R and a low Q value. These characteristics can be utilized in noise elimination \$\endgroup\$
    – Confused
    Dec 25, 2022 at 11:08
  • 1
    \$\begingroup\$ Unfortunately, TI misreads the USB standard, and doesn't understand EMI. Any impedance between circuit (signal) ground and shield, explicitly permits external interference to enter, and unbalanced signals (namely J/K states) to radiate. This arrangement makes things strictly worse when there is no metal chassis to provide the necessary shielding. \$\endgroup\$ Dec 25, 2022 at 12:13
  • \$\begingroup\$ This approach may be acceptable when internal noise is low enough amplitude not to violate CMR, and when there is enough noise that isolating circuit ground from chassis ground is otherwise desirable (to reduce the noise current I suppose). Desktop PCs may be such an example. \$\endgroup\$ Dec 25, 2022 at 12:14

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.