How should I route USB Connector shield on PCB? Should it be connected to GND plane right where USB is placed, or should the shield be isolated from GND, or should it be connected to ground through ESD protection chip, high resistance resistor or fuse?
PS. Should I put the shield connections on schematic, or just route it on PCB?
For the shield to be effective, it requires as low impedance connection as possible to your shield ground. I think those recommending resistors, or not connecting it to ground at all, or strictly talking about your digital logic ground, and assuming you have a separate shield ground. If you have a metal enclosure, this will be your shield ground. At some point, your digital ground must connect to your shield ground. For EMI reasons, this single point should be close to your I/O area. This means it's best to place your USB connector with any other I/O connectors around one section of the board and locate your shield to logic ground point at that location. There are some exceptions to the single point, rule, if you have a solid metal enclosure without any apertures, for example, multiple connection points can be helpful. In any case, at shield to circuit ground connection, some may recommend using a resistor or capacitor (or both) but rarely is there a reasonable reason to do this. You want a low inductance connection between the two to provide a path for common mode noise. Why divert noise though parasitic capacitance (e.g. radiate it out into the environment)? The only reason usually given for such tactics is to prevent ground loops, but you're talking about USB, ground loops most likely won't be an issue for most USB applications. Granted, such tactics will prevent ground loops, but they will also rend your shielding all but ineffective.
Herny Ott discusses this in his book, "Electromagnetic Compatibility Engineering". You need to look at it from the bigger picture. IE, what is the shield doing?
For low frequency signals, the shield is used to protect the signal being transfered. You want to avoid power line/AM/FM radio signals to couple into your signal because it will interfere with normal operations. Therefore you must not tie the GND on both ends. Ground loops will cause small noises to couple into your signal, therefore the ground loop must be broken. This does not mean that you leave the shield hanging. You should tie the shield of the cable, to your enclosure, and if needed (as in the case of coax), you can tie the ground of your circuit to this same point. You want to use single point grounding as much as possible for low frequency for the above reasons.
However, for high frequency signals, the opposite is true. They are usually digital signals at very high frequencies. Even if some noise did get coupled, the digital nature of the electronics as well as filtering should easily maintain normal operations. You want to reduce the emissions of the data signals, NOT protect it from radiation. For this reason, the lowest impedance path should be connected to shield at BOTH ends. Yes, there will be ground loops, and noise will get coupled in, but it won't matter. In the case of high frequency, multipoint ground is prefered.
Check to see if the manufacturer of your USB chip specs out what you should use. I'm pretty sure Cypress recommends a 1M resistor and 4.7nf cap connecting the shield to ground. The two shield holes should be connected with a very large trace (I believe they suggested 100 mils?)
Possibly conflicting guidelines:
The receptacle shell shall be connected to the PCB ground plane.
[But connected through what?]
Cypress Guide to a Successful EZ-USB®FX2LP™ Hardware Design (formerly High-speed USB PCB Layout Recommendations):
- Connect the SHIELD connection to GND through a resistor. This helps isolate it and reduces EMI and RFI emissions. Keep this resistor close to the USB connector. Some experimentation may be necessary to obtain the correct value.
- Provide a plane for the USB shield on the signal layer adjacent to the VCC plane that is no larger than the USB header.
Intel EMI Design Guidelines for USB Components:
The principal challenge of full speed device EMI compliance is preventing high frequency energy from coupling to the shield.
Full speed devices use a shielded cable which requires that the connector shell be tied to the ground plane. It is important to note that a ground plane does not behave like an equipotential surface at high frequencies. The location of the connector shell’s termination to the Gnd plane is critical. The connection needs to be made to the quietest area of the ground plane to prevent noise from the ground plane from coupling to the shield...
etc.
Google for "USB guidelines"
I based a project on a design spec calling for a 33k resistor connecting the USB shield to the ground plane. It was a project for ham radio, so conveniently my circuit board was placed in proximity to a sensitive EMI detector!
In my case I had to remove the 33k resistor and short the USB shield directly to the ground plane of my PCB to clear up the EMI.
The danger of directly connecting your shield to ground is that if two devices have "grounds" at different potentials and there is significant DC current capability from those sources, this connection could serve as a fuse between the two power systems.
Remember that a capacitor is nearly a dead short at its resonant frequency and generally conducts at a fairly broad band around that frequency, so a capacitor between the shield ground and the system ground is often the needed compromise.
I design automotive databus communications and some standards require that only one device connects the shield directly to ground and the rest of the devices must do this through a series RC. An automotive databus is significantly lower speed than USB 2.0, but the risks should be similar. USB 3.0 might be difficult to correctly maintain without solid shield connections, though. That (5 to 10GHz) is out of the scope of my current design experience.
The shield shouldn't be grounded. It is grounded at the host end, of course.
I have designed several boards and always used FTDI chip (FT245R). The datasheet clearly indicates the shield must be connected to GND. The same GND of chip which is the Ground of PCB!
Not olny the EMI is the problem. You have to know that any time you connect the cable to the connector you get an ESD discharge puls. This is dangerous for the electronics. So I would never connect the usb shild direct to ground.
Well, since it appears we need another answer, I'll put in my vote for grounding it through an ESD protection chip, like the USBLC6. It's worked well for me on several projects - No apparent destruction of components through ESD, and no issues with data integrity. I feel that it would be at least a little suspicious if STmicroelectronics manufactures such a chip, and is aware that a resistor, capacitor, or short to ground would be just as good.
I don't know if this success is because it's the right thing to do, or just dumb luck. Given the wide variety of responses, I'd be tempted to say that no one does.
At work, we tie Ethernet jacks straight to ground. AFAIK, this is the same as the issue at hand, even though the Ethernet cable carries no ground signal. It seems to work, and was decided by someone with more experience than myself.
I use a resistor between 10K and 50K. IIRC I saw a value of 33K in an FTDI application note.
I would put all connections on the schematic.
I think ESD protection chip and thicker tracks with more than 100 mil between shield and ground would be a good choice.
Also more stitching around the shield provides a Faraday cage to the noise.
See EMI and USB which recommends grounding both ends to prevent EMI transmissions at the frequencies used for USB data transmission.
