Signal/Shield GND EMC Treatments for USB2.0 Connector Interfaces 2

[SeattleChris]

Hello,

I have a general question about EMC treatments for ground interfaces associated with high speed interfaces. I've seen the cat skinned several different ways for USB2.0 connectors and I'd like to get a better understanding of why these different approaches are taken. It would be nice if I could post a schematic here but I guess words will have to suffice.

For a USB2.0 end-point device, I usually insert a ferrite bead between the USB signal ground and digital ground on the PCB to block bi-directional radiation on that line. For high speed interfaces, education has taught me (perhaps incorrectly) that shield GND should be DC coupled on both ends of the cable. However, I often see AC coupling (0.01uF) in parallel with a 1-M ohm resistor between the local connector shield ground and signal ground on the PCB.

My hypothesis is that this "almost AC-coupled" approach shunts HF noise from the shield quickly while correcting any appreciable DC offsets between shield and signal ground over a longer period of time, but I'm not sure why this is necessary.

Can anyone explain the reason for this approach and perhaps shed some light on theoretical vs. actual needs here? It's easy to overload interfaces with filters, ESD protection, etc. but my focus recently has been on portable high-volume consumer electronics devices where both the BOM and form-factors are very tight. So my target is always the most concise (both necessary and sufficient) approach.

Thank you in advance for your help!

Regards,

Chris

 

[VEBill]

There are tiny USB memory sticks (I think USB 2.0) on the market where the form factor is nothing but the thumb-print sized circuit card that slips into the connector. No metal sleeve, all one thickness. These memory sticks are designed to slip into a pocket in your wallet.

 

[BobbyNewmark]

A lot of EMC features are sheer incompetence that work by coincidence.

Let's think about the case you describe. Most connectors will have at least two wide shield tabs. Connecting those directly to the ground plane would give extremely low impedance, near the theoretical minimum. And it keeps that low impedance out to many gigahertz. It would certainly work well for keeping radio noise out of the signals, as well as keeping the signals from radiating.

But that ground plane is going to have high-frequency noise on it. Possibly a lot if the plane carries high-amplitude high-frequency current spikes (poor power supply decoupling or poor switcher layout), if another connector has poor EMC design, or if some other part of the system is radiating. If the design has those problems, connecting the shield tabs directly to the ground plane would send a lot of RF out the shield, to radiate in the test lab and violate EMC limits.

At which point the boss beats the crap out of our hapless engineer, who panics and tries something, anything, so the factory in China can start cranking out USB gizmos. And low and behold, his brilliant capacitor idea works. Radiated noise is magically reduced.

Because his capacitor is an inductor. That single, little, narrow trace from shield to capacitor, and capacitor to ground, has considerably more inductance than a pair of 0.250 inch wide tabs. At high frequencies, even a few nanohenries will have a noticeable effect. That matters when you're scraping together a few more dB to pass EMI.

The one meg resistor is to keep environmental charge from building up on the shield, creating a voltage that pops the capacitor. The large capacitance (0.01 uF is huge for radio work) is so that stray AC power coupling and ESD won't pop the capacitor, at least not until the customer has forgotten where they bought it.

"For a USB2.0 end-point device, I usually insert a ferrite bead between the USB signal ground and digital ground on the PCB to block bi-directional radiation on that line."

By "USB signal ground" do you mean the ground pin or the shield? Putting a ferrite between the shield and ground would, of course, be madness. (Naturally there are probably folks shipping that madness right now!)

But I'm not so sure about the ground pin. I can't see that it would hurt anything. If anything, I would also put a ferrite on the USB power pin, to keep your noise from getting into the USB data lines, and to keep the crap electronics on the other end from sending their noise into your power supply.

 

[itsmoked]

A star. Thanks.

Keith Cress
Flamin Systems, Inc.-

http://www.flaminsystems.com

 

[SeattleChris]

Ahh... a band-aid in the works... thanks Bobby!

Inductors and capacitors are pretty much the same thing when we get to GHz, huh. They could have gotten away cheaper though by using an inductor. Parasitic capacitance between the windings would discharge through L and solve the environmental charge issue (without the resistor) when the USB cable is unplugged. The inductor itself probably would have snubbed the radiation issue. There, I just saved them $0.002 on the BOM! :O)

With regard to my statement about the ferrite bead, I was talking about the USB signal ground pin on the connector. So USB connector pin to FB to ground plane on my PCB.

Good call on the power line. I will add a FB there as well.

Thanks so much for the helpful response.

-Chris

 

[BobbyNewmark]

I'm glad to have helped.

"Inductors and capacitors are pretty much the same thing when we get to GHz, huh."

At lower frequencies, too. All components, including resistors, have a self-resonant frequency where their impedance is minimum. Even at audio frequencies, you can get surprised by the inductance of roll-of-foil capacitors and spiral-conductor resistors. It's also not hard to find inductors that are too capacitive to be used in switching power supplies.

"They could have gotten away cheaper though by using an inductor."

Indeed! Perhaps even as a trace on the circuit board, which you'd think these made-in-China folks would simply adore.

I once saw an antenna lightning protector for a cell-phone base station that was just a (controlled-width) spiral of copper connected to the ground plane. And it wasn't some sort of nickel and dime thing either. It perfectly filled the gap between the big gas discharge protectors and the tiny protection diodes.

 

[Noway2]

I have a follow up question....

Bobby, you say, "Putting a ferrite between the shield and ground would, of course, be madness. (Naturally there are probably folks shipping that madness right now!)"

I am working on a product right now that has two shield tabs on it and am wondering what would be the best way to connect them. The manufacturer says that they are part of the device heat sinking and should be connected to at least one square inch of copper. This part isn't a problem, but I am wondering if and how that SHOULD be tied and if so, to WHAT?

If I understand your first post correctly, if there are other devices in the system that are radiating, then connecting the shield directly to ground would make a nice radio, which should be avoided.

If a ferrite is, "madness" then is a small capacitor in parallel with a large resistor the correct approach or is there something better?

 

[VEBill]

The Golden Rule of EMC: Control of EMI is the opposite of a good antenna.

 

[BobbyNewmark]

Noway2 asks "The manufacturer says that they are part of the device heat sinking and should be connected to at least one square inch of copper. This part isn't a problem, but I am wondering if and how that SHOULD be tied and if so, to WHAT?"

It depends on the device. The datasheet usually has a diagram of what they want on the PCB.

If the tabs are electrically active, then they must be connected to the specified signal. If they have no internal connection (float), it may be useful to ground them, to keep noise from being capacitively coupled into unexpected places.

If they are connected to a signal that has a plane under the device, you might want to put several vias between the plane and the tabs. The vias will conduct a lot of heat to the plane, reducing the temperature rise. You can even use vias without thermal reliefs. Be warned that lots of vias and/or lack of thermal reliefs can make the device very hard to solder by hand.

"If I understand your first post correctly, if there are other devices in the system that are radiating, then connecting the shield directly to ground would make a nice radio, which should be avoided."

Yes.

"If a ferrite is, 'madness' then is a small capacitor in parallel with a large resistor the correct approach or is there something better?"

It depends on the application.

If you want the shield to actually shield as much as possible, then there is no choice: the shield goes straight to the ground plane, with short traces and several vias per tab if it is surface mount. Period. Anything else will turn your connector into a loop antenna. This would be appropriate for a Hi-Speed USB interface, which runs at microwave frequencies.

But some applications don't need that. For example, a sensitive microphone input might already have excellent bidirectional RF filters. Worrying about the connector would be like putting 14K gold plating on a bar of pure gold. In that case you could get away with a ferrite in the ground path, which might help you fix a radiated emission problem caused by another part of the board.

 

[Noway2]

Thank you for your reply.

In this case, the data sheets and integration guides provide no clue as to what the shield tabs expect, electrically. I have passed this question back to the manufacturer of the device, which is an embedded ethernet controller, from Lantronix.

Ve1bll, I am acutely aware of that golden rule. It has been foremost in my mind the whole time I have been working on this project. I am by no means an expert on the subject, but I do make an effort to learn as much as I can about it - both the art and the science.