Ground rings on PCB's
Ground rings on PCB's
(OP)
I have heard arguments for placing an earth ground trace on PCB's that encircles the main circuit (ground trace around the outside perimeter of board). The argument is that this will shield the circuit from some outside noise as well as contain some radiated noise from reaching the outside world. While I agree that this will provide a LITTLE bit of shielding, I contend that it will cause more harm than good because the ground trace surrounding the electronics is acting as an antenna for radiating noise as well as picking it up. Anyone have any thoughts on this?





RE: Ground rings on PCB's
> Prevents accidental shorts during debug/testing if the edge of the PCB comes in contact with grounded metal objects
> Also provides a ready and known ground for probes, etc. during debug/testing.
> Ensures that high voltages are not exposed on the edges of PCBs. I've personally experienced a 270 Vdc cross layer arcing short because the designer forgot to leave a buffer between the hi-pot trace and the edge of the board
> Contains contaminant induced leakage paths at the edges of the PCB. More prevalent for stuff like low-leakage op-amp inputs, but might be applicable in some instances.
TTFN
RE: Ground rings on PCB's
Where I would see such a feature being helpful would be for basic static protection. Since unwary fingers, or case enclosure gaps tend to contact or be near board edges, this trace would present a first-path for discharge.
RE: Ground rings on PCB's
Comcokid brings up another benefit, ESD protection. However, it will only help with discharges near the edge of the board and not the 'center' area of the board where most buttons, LEDs, etc are located (where most discharges will occur).
I am still not liking a ground trace around the perimeter of a board. I always use a ground plane (even for two layer boards-make plane as large as possible). Attention to layout of traces/parts is way more important than most realize. I have seen some terrible PCB's that could never work properly (EMI). I have never heard of a ground trace around the perimeter, hence this discussion.
Thanks for the posts!
RE: Ground rings on PCB's
I sometimes hear "little loose pieces" of recommendations which - when not presented in their full context - often seem to be difficult to understand. I think that this is one of them.
Ground (or gúard) rings around sensitive pins on opamps is another glass of beer. Knowing that buzzp would never confuse those two things, I hesitate to mention it. But, for someone that might not have heard of them, I think that they should be mentioned.
RE: Ground rings on PCB's
RE: Ground rings on PCB's
EMI reduction? You should be so lucky.
Having lots of test holes in this ground path used to connect to scopes could be a good idea, but it depends how the trace is connected. If it is five inches to the nearest via then it is no different to having a 5 inch ground lead on your scope probe, ie it is pretty useless for HF stuff.
My feeling is that if you need high voltage clearance or guarded traces then do so, but don’t try to solve all problems with a generic "solution".
RE: Ground rings on PCB's
There is no daughter boards (other PCB's) connecting to this 'mother board".
I have recently been helping another company with there design and just found out this is in a metal box (not plastic as previously mentioned) so the benefits of a ground ring (at least the ones I mentioned) are not valid.
Keep in mind that I would have never used a 'ground ring' in this application just questioning the original designers reasoning for having it. Evidentally, he/she must have heard somewhere about using one and simply used one without knowing why.
I am going to recommend it be removed. I see no benefit at all unless some information is still missing from the client.
RE: Ground rings on PCB's
RE: Ground rings on PCB's
RE: Ground rings on PCB's
They are also used to reduce the capacitance seen by a high impedance input, eg on an instrumentation amplifier. The input connections will be screened by rings that are driven by a voltage that is equal and in phase with the signal. No deltaV, no C.
As for the general case of gaining benefit by circling the board with a grounded ring, this is rubbish. You will not reduce RF coupling or even magnetic coupling as the coupling coefficient/mutual inductance will be too low. It might be convenient for attaching test probes but is more likely to be a couduit for EM interference than to reduce it.
RE: Ground rings on PCB's
"Since the discharge is applied to the edge of the modules,
one protective measure to consider is a guarding trace around the perimeter that is clear (say 3/8") of components. This trace should be connected to signal ground through a high resistance. The guard trace should also be connected to chassis ground."
http://www.conformity.com/0203reflections.pdf
RE: Ground rings on PCB's
RE: Ground rings on PCB's
PLL's and high frequency circuits typically have strategically placed grounding planes. Check with manufacturers data books and they go into depth in regards to implications.
A personally leave lots of grounding foil on my proto boards, speeds up etch time and extends bath life.