USB Shield. To ground or not to ground?

Question

I have been given a device at work to do some testing on. Basically an IC is becoming obsolete so I need to test a replacement part. Upon redoing the ESD checks, the device failed.

I checked the history of the device, and there were problems passing ESD before. There was a note from the testing facility that as the device was entirely metal (Stainless steel housing) only contact discharge up to 4kV was needed to pass (I am in UK). Apparently it failed a few times untill a capacitor/resistor was added between the USB shield and ground, and a small metal tab was introduced to add better contact between PCB ground and the metal case. This then apparently allowed it to pass.

Move on 5 years and I am redoing the tests. Each time I perform the contact discharge test at +4kV, the device loses its memory (this is a datalogging device) and it needs a factory reset and restart logging to work again. I rechecked some old ones using the previous IC and found that this also fails. It seemed that it was an intermittent problem (some devices passed 3 in 10 tests, others failed all 10 etc) so it seems to me like the pass on the ESD test previously was likely a fluke.

I tried a number of things, I put extra capacitors in parallel with the current one connecting the USB shield to ground (different values, high/low), I changed the resistor to different values (higher/lower resistance) and tried ferrite beads in parallel, and ferrite beads instead of the Resistor/capacitor as I had seen some places recommend, but still it failed. The only way I got it to pass was by grounding the USB shield directly.

Looking online I can't seem to find anywhere that says explicitly whether you should or shouldn't ground the USB shield. This discussion HERE has different views, this HERE also has a discussion on it. THIS link mentions the shield should only be connected to ground at the host, but no device should connect the shield to ground.... THIS document says the shield should be connected to the chassis. Yet, in fig 12 it seems to show the USB shield should be tied to GND plane.

There just seems to be a lot of different views on this so I am a bit unsure what to do next. Grounding the shield allows it to pass ESD, but is this something that should be done? Or should I continue to look for a better solution? If so, what is a good solution?

MORE INFO:

• The PCB is very irregular, and tight on space, making the ground plane near the USB connector very small.
• I am not allowed to change any mechanical design on this. I am just to find a solution which can be easily implemented and does not require a redesign of the PCB or product so those suggestions are pointless to make.
• This is a a work device and as such, I am not allowed to show the schematic, so please do not ask. The USB input circuitry was based on this design:
• The common-mode choke, ferrite and TVS diode protection are all in the design already.
• I am not the original design engineer. They do not work for the company any more so I am unable to find their reasoning for the design choices they made
• The device is USB 2.0
• The unit passes the test at -4kV, it is just the +4kV where it fails

MORE INFO

And more info required in comments will be added here.

• Andy aka: I can show you this much:

  

All I can show of the actual PCB is this:

You can see that the ground plance stops short of the USB socket. The large hole is where the tabs for the USB shield to have a mechanical connection to the PCB. R1 is then connecting the shield to GND, and capacitor C3 is doing the same on the other connection. The shield is connected to ground via the 100k res/100nF cap. There is a metal tab fitted to the PCB which rests on the metal chassis. According to the old ESD report, this was needed or the device failed. As far as I can see, these were the only things added in addition to that example circuit to protect from ESD.

In response to the questions in the comments:

• The failure occurs when doing a contact discharge ESD test on the USB shield (all other areas it is fine, just the USB shield it fails)
• The test occurs while the unit is logging. It is not connected to any device via USB.
• I have tried a 0R link to GND instead of the resistor/capacitor solution, but this still fails. When I add a wire link direct from the USB shield to the chassis (which is connected to PCB GND) then the issue is resolved. I believe this is because of the PCB design. The ground plane near the USB side is very small (about 12mm x 15mm). Yet the chassis is large. This is something I cannot change.
• The location of the Chassis to PCB GND tab is on a sub-PCB, with a 30thou trace to the tab. (yes, I know it sounds strange, but the space constraints were ridiculous and this was not my design!)

Answer 1

Best Practice

Firstly (as a bit of a cop out) personally, in designs I always ground through a 0R resistor so that the decision can be changed. This goes for pretty much any shield (Ethernet, USB etc)

The main problem that can arise is when the shield is grounded at either end, and the two ends don't agree on what 0V is. This can cause damage to either end, by currents flowing where they shouldn't (if the shield path is 0.2ohms, and the voltage difference 1V, that's 5A going where it shouldn't)

You might think why would this ever happen? But think of the situation where a laptop is connected to a piece of mains powered equipment over USB. The laptop could be on battery only (no true earth reference), but the equipment is connected to mains and thus may have a true 0V earth reference.

So the solution is to connect at only one end, but have some agreement on which end.

Generally, a USB host will be expected to provide the power and the device is quite often entirely bus powered and has no connections to anything else in the outside world (think USB memory stick, WiFi dongle etc). In general, the USB host should connect the shield to ground (and earth, if possible). This is why the host side is typically expected to tie the shield to ground or earth.

The fact that there are so many conflicting comments from people and different experiences shows clearly that it is far from safe to assume this is always adhered to, so as I mentioned firstly - add the option to change it easily.

In This Situation

After discussing this in a chat, the proposed solution is different. Since this is a question about ESD, it's messy and complicated and involves many aspects of the design (electrical, mechanical, system). The chat is available for all to see, but there important bits:

• This datalogger has no other connections, apart from the USB connection to a PC/laptop
• The datalogger has a metal chassis, that is bonded to the PCB board ground.
• When the USB shield is not directly connected to PCB board ground (for example connected by R||C or HiZ), the datalogger fails (loses memory contents).
• In the ESD test, the USB cable is not attached (or is floating at the other end).
• The OP is not the design author, and has very limited scope for making design changes to solve this problem.

I surmise the problem is most likely PCB layout related. The ESD surge is taking a path from the shield, past sensitive electronics and finally reaching the chassis. By directly connected the shield to the chassis with a wire, ESD surge path reaches the chassis without going near the PCB so avoids the problem.

In this situation, as the datalogger has no other connections to any other devices; the potential issues (pun intended) cannot occur. So I would suggest connecting the shield to the chassis. Either by a wire, or a more production friendly approach is an ESD gasket around the connector which is a spongey conductive material that gives a connection without manual soldering and doesn't permeantly attach the chassis to the board.

In a more ideal world, I would respin the board so the chassis is isolated from the PCB board ground and the chassis is connected to the shield. That means that its not possible for ESD surges to reach the sensitive electronics at all. Except if you poke the datapins on the USB connector for fun - in which case, ESD diodes on the datalines that give a path to chassis ground, not PCB board ground.

Answer 2

Good shielding simply means good shield continuity. The PC board usually doesn't even figure in any of it - for shield continuity, you should mentally replace the board with an insulator. For purpose of analysis, replace the board with a piece of bare FR4, no copper, just holes and epoxy used to fasten the connectors. The shielding between all shielded cables and the enclosure must still be continuous when you do that.

This implies that there must be direct electrical connection between the metal of the connector (each and every connector!) and the metal enclosure, and there must be direct connection between the cable shield and the metal of the plug going into the connector, and such connection must be done in 360-degree fashion to surround the apertures being protected. You're quite literally working to cover all the holes/gaps as well as you can. The fact that signal lines run through those apertures is secondary :)

In the cable plugs it the shield must be captured in a cage that extends to form the plug shield itself, and then the plug and the connector must interoperate to provide multiple contact points around the circumference to keep this 360-degree requirement carried throughout.

Any sort of a pigtail in the shield connection introduces so much impedance that it is an instant qualification failure. If you use any high-frequency signaling cables that have any visible shield pigtails in them - junk them, and use good stuff instead. This will fail EMC, and has good potential to fail your customers in their applications even if it somehow squeezes through. There are HDMI cables sold by reputable dealers (I'm not talking about Walmart) that have pigtails in them. It's on you to actually qualify the cable for your application, including the disassembly (butchery) of any overmolded plugs to inspect their construction. If you don't do that, you'll eventually pay for it in failed tests or "mysterious" customer complaints, and any savings you may have amassed over the years of ignoring this basic good engineering practice will vaporize in an instant.

In the device receptacles, 360-degree shielding continuity is often assured using EMI spring tabs or using cast-metal connectors that can be fastened directly to the enclosure while assuring good, 360-degree contact all around the plug's outer shield.

No matter what you do, external shielding is not the PCB's job, so any such analysis should begin by forgetting that the PCB even is there. Nothing you do on the PCB itself can even remotely match the performance of a continuous external shield. As you have learned, the hard way.

This also points to a common misunderstanding: mechanical and electrical design are both an integral part of the design-for-EMC - and thus an integral part of the overall design process, for EMC is not some "bolt on" but really fundamental, and are truly inseparable from each other. Whenever you design anything electrical, there's no separate "case" it's put into. The enclosure is part of the electrical design process, and its properties are just as important as those of the components on the board itself.

There are quite often retrofit situations like what you face where the inadequacy of the original design process is unveiled, and you should never assume that the device you got has really "worked well" or "passed the tests", for you can't know how close it was to failing, and sometimes the tolerance stackups end up working to one's atrocious advantage. Why is the advantage atrocious? Because it's a lie, a lie that is known to have wasted thousands of engineering hours and millions of dollars. You "pass" the tests whereas you really have a marginal device that may never pass those same tests again once it goes into production. Therein is the lie. Your prototype had an atrocious advantage. Once. It's gone now. Forgetaboutit. You get presented by management with "this device that always worked well and passed the tests" and you have to "make it pass again". Unh-unh, dear managers. You can't win an argument with nature. Poor engineering will always come to bite you back in the rear end, no ifs, no buts. It's never "keep the case the same". If the case was the source of the problem to begin with, you can't use your will to convince nature that, retroactively, let's not talk about the case anymore. If the enclosure is the problem, you have to accept it and solve it - usually by modifying the case, choosing better connectors, etc.

Answer 3

You need to examine the high-current path across your design, and the design must provide a separate shield net to avoid the ESD discharge to go over signal ground, which will create "ground bounce" and disrupt functionality. This is not an easy matter. By making a simple solid connect between signal ground and shield, you might run into EMI issues and fail EMI certifications. For more details, you might want to review this topic on how to balance two contradictory requirements for USB shields.

Answer 4

Considering what you have told us about the device:

• Battery powered
• Not normally connected to USB
• Does not have connections to external sensors or devices during measurements
• Does not have any accessible metal parts apart from chassis and USB
  shield.

Just connect the chassis to USB shield and be done with it.

Previous answer pointed out issues with loop currents (two different GND paths in circuit to mains) but since you have floating battery-powered device, this is a non-issue.

If you want to experiment, you may try removing resistor/capacitor between the shield and the GND. Also you may want to use smaller NP0 C0G ESD capacitor, 100nF capacitor has X7R dielectric which is not well suited to this kind of task.

The GND-to-Shield connection is apparently rather weak and not near the USB connector. So shorting shield to GND makes the transient travel through your PCB until it hits the chassis tab.

I think the problem here is that the original designer put USB shield under the signal traces. Zapping the ESD gun makes the shield "jump" which couples capacitively with the traces and components nearby. Now signal and VBUS traces are crowbarred to GND so they're protected. However, these traces then go to have CMC and ferrite while the GND is directly coupled - So probably these suppress the transient in those wires while the GND transient continues unabated.

NB this is just speculation.

Answer 5

By the description and the basic schematics provided. It looks like they are using the wrong TVS circuit. Because the +/- data is balance transmission line, and the TVS circuit in the schematic is for unbalanced transmission lines. Shield is little of importance compared to this circuit and how well it operates to protect, and only really needs to be grounded at one end for its basic function of the circuit. Here is a good application guide from ON semiconductor for future reference. https://www.onsemi.com/pub/Collateral/AND8231-D.PDF

Answer 6

I have two solutions:

Solution A
Replace C3 with the largest capacitor possible (micro, not nano farads).
If this does not work, then

Solution B
1) Remove the resistor and capacitor that were added (R1 & C3),
2) disconnect ground from this connector,
3) solder a wire from the shield tab (R1 C3 node) to this connector ground and the other end solder it to the PCB ground tab of the opposite connector.

The net result of these instructions, is to isolate the PCB ground plane from the USB shield. This way, when the USB shield is zapped, the ESD will bypass the PSB and go to ground.

Answer 7

If I look at your circuit correctly and also look at the https://www.onsemi.com/pub/Collateral/AND8231-D.PDF I see that you have used a device (Diode Array Plus TVS) used for Use with single−ended data line and the USB protocol is supposed to be a differential protocol.

The link informs that you should use Schottky Diode Array or Diode Array instead, which are meant for Differential data lines.