How to correctly connect a USB shield on a PCB
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:


Connect shield directly to GND;
Connect shield to GND through resistor/capacitor;
Connect shield to GND through ferrite bead;
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:


Added Microchip RC example from working with the USB2514B hub.