How to correctly connect a USB shield on a PCB

Question

I have designed a simple PCB on EasyEDA; I am using USB 3.0 as a convenient means of providing power, ground and taking outputs from the magnet sensors (connected to the PCB) which will be routed to the corresponding pins on an Arduino microcontroller.

I would like to know whether I have correctly connected the two pins of the USB shield/shell (through a decoupling 100nF capacitor, through a 330ohm resistor to ground) following the advice of other threads on here.

Image is shown below

Have I done this correctly?

The package size used for the resistors is 0603 and for the capacitors they are 0402 (chosen due to stock on LCSC) Will those package sizes work fine for this use case (because one user mentioned a 0603 package may be ideal due to certain frequencies)?

I have connected them in series, is that correct or do one both or either of them need to be in parallel?

Any other advice, best practices?

Edit:

Thank you guys for your responses. @JYelton I have followed your example (Figure 1) of connecting the PCB to chassis ground. This is shown in the images below:

Image 1: Chassis ground schematic

Image 2: EasyEDA PCB implementation

Can you please check if I have correctly implemented the 'chassis ground' on my PCB. I have done this by exposing the copper trace around the mounting holes where the PCB will be bolted to the aluminium chassis via steel fasteners.

EasyEDA colour guide:

Red - Copper trace covered by silk mask

Pink - Board outline

Yellow - Markings

Purple - Exposed Copper (can be hard to see, labeled on image 2)

Answer 1

A forum post on All About Circuits with sources by user ColinB (some 9 years ago) lists the various options he (and I) have come across:

1. Connect shield directly to GND;
2. Connect shield to GND through resistor/capacitor;
3. Connect shield to GND through ferrite bead;
4. Don't connect shield to GND at all.

There appears to be some disagreement about whether a USB device should have its GND connected to the cable shield, or if this is to be done on the host only.

On devices that I'm involved in designing, I've opted for option 1 (direct to GND) as well as 3 (ferrite bead) at different times. Note that for ESD protection in both cases I've used something like these Littelfuse TVS diode arrays.

According to the USB Implementers Forum, the white paper Managing Connector and Cable Assembly Performance for USB SuperSpeed states:

To minimize the EMI and RFI risk, the connector and cable assembly designers, as well as system implementers must pay attention to receptacle and cable plug shielding design to ensure a low impedance grounding path.

---

Ferrite Bead Option:

I think the ferrite bead is a good method because it acts as a high impedance for high frequency noise but provides a low impedance path to GND for ESD.

The Texas Instruments USB 2.0 Board Design and Layout Guidelines document discusses this:

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.

Silicon Labs also supports this in their USB Hardware Design Guide (AN0046).

---

Resistor/Capacitor Option:

That said, other sources recommend use of parallel capacitor and resistor.

Cypress states in Common USB Development Mistakes:

The most common and simple-to-fix EMI error is mistakenly tying the shield in the USB cable directly to the ground plane of your system. This allows any noise injected into the ground plane to escape any shielding around your device.

They recommend using a 1MΩ resistor and 4.7 nF capacitor in parallel:

Microchip also recommends an RC network but with different values, in the application note AN26.2: Implementation Guidelines for Microchip’s USB 2.0 and USB 3.1 Gen 1 and Gen 2 Hub and Hub-Combo Devices.*1

Microchip has observed positive EMI and ESD behavior on stand-alone designs when connecting the USB cable shield to digital ground with an RC network (330 Ω resistor and a 0.1 µF capacitor in parallel) at each USB connector.

---

Final Thoughts:

There are a few different methods because... it depends. One goal is to suppress noise and prevent your device from radiating EMI. Another is to absorb ESD as users unplug and plug in devices. Yet another is to avoid providing a duplicate current path where one isn't intended (ground loop). You'll have to research the pros and cons of these methods and determine what's best for your application.

---

Edits:

1. Added Microchip RC example from working with the USB2514B hub.

Answer 2

The idea is that shield should not conduct any system ground current, or at least, any AC system ground current.

The connection you show is kind of the opposite of what you want. With the caps as they are, system ground noise is able to make its way onto the shield wire, which will be in common-mode with system ground. This will actually increase EMI. Meanwhile, an ESD upset has a nice AC path to system ground which you helpfully provided with C7 and C8. Neither outcome is very good.

What I've typically done is to connect shield to logic ground via a ferrite bead, then connect shield ground to chassis, or at least, to a chassis plate for a plastic box. This suppresses the system ground AC noise path for EMI, and also blocks an ESD hit to the shield getting to system ground.

Another option is to use a resistor to tie shield to ground. I've seen this done on some USB hubs. This provides some IR drop to outgoing EMI and incoming ESD.

This Intel (via TI) appnote goes into more detail: EMI Design Guidelines for USB Components