1
\$\begingroup\$

I saw a PCB with something like this. A trace that connects the four holes on the corners. I assume that they do it to prevent some kind of noise. I am not sure if the connect that trace to GND

Also, for the shield of an USB, I saw some schematics that connect the shield to the GND using a ferrite.

So, this layout, a trace on the border, connected to the shield of the USB cable, and connected to GND through a ferrite.. it is a good or a bad idea?

enter image description here

\$\endgroup\$
11
  • 1
    \$\begingroup\$ Looks like a loop antenna to me. What are the mounting holes connected to? \$\endgroup\$ – The Photon Jun 3 '15 at 15:45
  • \$\begingroup\$ @Javier What is (or will be) the purpose of this instrument? \$\endgroup\$ – Nick Alexeev Jun 3 '15 at 16:39
  • \$\begingroup\$ I would guess that the trace is outlining a ground polygon. I know Eagle works that way before clicking the "ratsnest" button to fill in the pour. \$\endgroup\$ – DerStrom8 Jun 3 '15 at 16:57
  • \$\begingroup\$ "Something like this" doesn't sound confident. Why is the inductor shorted out? Without knowing what the PCB in the picture does then nobody can say if it's good practise. \$\endgroup\$ – Andy aka Jun 3 '15 at 17:04
  • 1
    \$\begingroup\$ @JavierLoureiro without a circuit diagram, nobody can tell what it's meant to do. If you can't tell what it's meant to do you can't decide if the layout is appropriate or not. Simple - edit the question to give facts. \$\endgroup\$ – Andy aka Jun 3 '15 at 20:17
1
\$\begingroup\$

Starting with what's probably here:

It's possible that the trace between holes is a guard ring for the entire board, meant to be a barrier between the stuff on the board and the stuff around the board. But that all depends on what the screws are connected to. Get it wrong, and it becomes an antenna, like The Photon said. I've never seen it like your example, but it's done quite commonly between sensitive analog stuff and the rest of a board.

More sensible to me would be a ground pour connected to the screws, but you said it's a trace, so we can drop that possibility.

The ferrite to ground is likely a ground loop breaker or something like that, where you want your circuit to be ground-referenced, but a direct connection picks up noise. * It's effectively a "soft" lowpass filter: close to zero ohms at DC (wire resistance) up to a wide peak of few hundred ohms at a few MHz.

As the bead's impedance goes up with frequency, we have another problem: the stray capacitance between the ring and the circuit reduces impedance with frequency. Depending on how close things are to the ring (capacitance follows area/distance^2), this can take over from the bead so you end up with noise anyway.

* I have a laptop that made what sounded like hard drive noises on both the headphone output and a USB sound card, but only when plugged into power. It turned out to be a ground loop problem picking up noise from its own power supply. A USB isolator fixed it. So ground loop symptoms aren't limited to AC power hum.


As for good practice:

Possibly yes to use the ferrite, but probably not for a whole-board guard ring. It might be redeemed by connecting the ring to ground AFTER the bead, but only if you have traces for ground instead of a pour.

\$\endgroup\$
3
  • \$\begingroup\$ So, "Is this pcb layout good practice?" \$\endgroup\$ – Andy aka Jun 3 '15 at 17:06
  • \$\begingroup\$ It is a single trace, not a ground pour. Thank you, that is the idea of my question, to see the "bad things" that can happen with the guard ring. So, the antena will pick up noise, amplify it, and send it back to the rest of the pcb? the ferrite wont filter that noise? \$\endgroup\$ – Javier Loureiro Jun 3 '15 at 17:40
  • 1
    \$\begingroup\$ If it's an intentional antenna, that's not the way to do it because it's connected to ground instead of an input or output of something, so we'll assume that it's an unintentional antenna. The bead is basically a short at DC and a few hundred ohms at a few MHz, so that path will be filtered to that extent. But it's not the only path. The most likely path that I can see at a few MHz or higher is capacitive between the antenna and the circuit, acting in parallel with the bead. Small guard rings for analog are connected directly to ground, not through a bead, so any capacitance there is shorted. \$\endgroup\$ – AaronD Jun 3 '15 at 18:22
1
\$\begingroup\$

Personally I do not believe it to be good practice. My opinions only come from personal experience and unorganized research. I have not found an authoritative explanation as most authors take the matter for granted.

My understanding of the theory is that any ESD from the connector or otherwise will travel through the chassis ground ring to the chassis connections and earth ground. The ESD is supposed to see this path as low impedance compared to the single point of entry at the ferrite or inductor that protects digital ground. I have no problem with this theory like that.

However, in your layout, the ground ring is very small which as others have mentioned, appears a non-zero impedance. So if you do want to use this grounding topology, then I would widen the chassis ground loop trace.

The above theory has limitations though. What happens when I want more connectors than just USB? Look at a PC or laptop motherboard with many peripherals. For each of these you would need to a clear path to chassis ground for any ESD. Some designers decide to add ferrites at each of these entry points to maintain that high impedance but keep the same DC ground needed for operation.

Also consider what happens if I connect an off board device such as a hard drive or touch screen. Now I have to make sure that the peripheral is using my ESD protection architecture. If for example the touch screen uses a unified ground theory, then any ESD coming through the touch screen will find its way to my motherboard's digital ground. Couple that with the fact that my motherboard has high impedance ferrites blocking the exits to chassis/earth ground and now my components have to soak up all the excess energy from the ESD event.

This is why I do not believe that this isolated ground theory (also known as star ground) is scalable. It's ok for small sections like an analog critical area, but is difficult to maintain through a large system.

The alternative is a unified ground theory. Treat all grounds where possible the same. To reduce the impedance between different parts of ground, try using planes (voltage and ground), thick copper, many vias and generous mounting holes. If done right, there should be no useful ground loops. Combined with sufficient board capacitance (the right kind too), power rails and signals should be able to float right over the ESD event. The majority of ESD should find it's way straight to earth. Or in essence, we are applying localized single ground theory.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.