Post History

Connect the shield directly to ground plane
----

Most manufacturers recommend connecting the USB connector case (which is connected to the cable shield) directly to the PCB ground plane.
In theory, when lots of electrons hit the ground plane of an isolated PCB, suddenly changing its voltage relative to planet Earth by thousands of volts, *everything* on that board should be raised or lowered the same amount (through deliberate bypass capacitors or through unintentional parasitic capacitance).
Perhaps some other thing on that board is *not* isolated -- rather than putting more stuff between the shield and the rest of the board, perhaps you could find that other thing and add ferrite beads or resistors to increase its isolation from planet Earth or add capacitors to the GND plane to reduce its isolation from PCB GND or both.

William D. Kimmel and Daryl D. Gerke
say ground the USB shield at both ends,
ideally with the connector shell grounded to the enclosure around its entire perimeter.
They say the common advice to ground the shield at only one end of the cable (single-point ground) only applies when the path length is short relative to a wavelength (1/20 wavelength), such as audio signals.
USB has high-frequency signals that need the shield to be grounded at both ends.
["EMI and USB"](https://web.archive.org/web/20171226003340/http://7ms.com:80/enr/online/2010/02/notebook.shtml)

Intel
says to connect the shield (connector shell) directly the the ground plane, and optionally use a ferrite bead between the USB GND wire and the ground plane.
["Intel EMI Design Guidelines for USB Components"](https://www.ti.com/sc/docs/apps/msp/intrface/usb/emitest.pdf)
p. 9

Silicon Labs
says to connect both the USB shield and USB GND directly to PCB ground for both USB self-powered devices and USB bus powered devices
["AN0046: USB Hardware Design Guidelines"](https://www.silabs.com/documents/public/application-notes/an0046-efm32-usb-hardware-design-guidelines.pdf)
p. 5 and p. 6


["Atmel AT85C51SND3Bx High Speed USB Design Guidelines"](https://www.microchip.com/content/dam/mchp/documents/OTH/ApplicationNotes/ApplicationNotes/doc7633.pdf)
p. 7 and
["Atmel AVR32787: AVR32 AT32UC3A3 High Speed USB Design Guidelines"](http://ww1.microchip.com/downloads/en/Appnotes/doc32122.pdf)
p. 5
doesn't mention the shield or the shell, but the example layouts (such as the one on p. 4) clearly show a wide trace connection between the GND wire (pin 5) and the shell, with lots of vias connecting that GND trace to the GND plane.

I've seen one design guide that contradicts the above advice:

[Atmel AVR1017: XMEGA - USB Hardware Design Recommendations](http://ww1.microchip.com/downloads/en/AppNotes/doc8388.pdf)
p. 7 and 8
recommends putting ESD suppressors between the data lines and the VBus and USB shield (none of the ESD suppressors connected to the GND wire or PCB GND plane),
connecting the GND wire to the PCB GND plane,
and putting an RC filter between the PCB GND plane and the USB shield
(It recommends an RC filter of R = 1 MegaOhm, C = 4.7 nanoFarad). 

Another manufacturer suggests keeping your options open:

FTDI says to place a zero-ohm resistor between USB shield and PCB signal ground, which can later be replaced by a capacitor if necessary.
["AN_146: USB Hardware Design Guidelines for FTDI ICs"](https://www.ftdichip.com/Documents/AppNotes/AN_146_USB_Hardware_Design_Guidelines_for_FTDI_ICs.pdf)
p. 14