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?
Eng-Tips is the largest engineering community on the Internet
Intelligent Work Forums for Engineering Professionals
Ground rings on PCB's
- Thread starter buzzp
- Start date
Not sure about EM specifically, but there may be other reasons for ground rings at the edges.
> 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
> 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
If your board has a fairly good ground plane, such a trace would be unnecessary. If the board had any fast digital or RF, you should have a good ground plane or your going to have radiation problems regardless of the extra trace.
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.
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.
- Thread starter
- #4
This board will be in a plastic enclosure. While I agree with IR's statements, I believe the cons (antenna) far out weigh any pros. This will be in an industrial environment (very noisy).
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!
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!
Skogsgurra
Electrical
There might be still onother reason for those perimeter ground traces. ABB, for instance, uses such a trace together with spring contacts along the card guides to ensure a low impedance wide area connection between card ground plane and chassis ground (metal card cage and metal guides). It is being used in the Prism protective relay system, among others. A ground plane is, of course, a better choice.
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.
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.
Sounds like an old wives tale to me. Most of the reasons given by IRStuff require the trace to have the solder resist removed round the whole guard track; is that being done?
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".
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".
- Thread starter
- #8
The concern is about picking up noise in the air.
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.
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.
I have never used a "ground ring" except in the context of a ground grid on double-sided PCB's. A "ground ring" alone, as suspected by buzzp, is a jim-dandy loop antenna that both emits and receives external RFI noise. If buzzp keeps it for other reasons mentioned by the group, it should be tied to the ground plane at short intervals.
I agree with geezer. Even though there could be some reasons or special conditions, I have never seen it used during the last 30 years for anything other than helping to make a good connection to earth ground. It will not help any EMI problem although it probably will not hurt.
Ground rings are commonly used to screen very high impedance points from surface leakage across the board. They dont help with conducted leakage through a contaminated board though.
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.
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.
A ground ring is also used to meet NEBS EMC Compliance, GR-78-CORE. A requirement for RBOC equipment.
"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."
"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."
DetlefHerbst
Computer
I have seen the ground ring on boards on the past. They failed EMI miserably. They are a good antenna though. If you use the ground ring, break the connection so it doesn't go all around the board(maybe 3 sides). I have used these ground rings as a chassis ground and connected them to logic ground through a 1M ohm resistor (per O1VIPER's post). The ring is a good place to connect the shields of connectors and to make contact with the chassis. By doing this, you do not have an antenna, and it is easier to pass the regulatory agencies.
automatic2
Industrial
have you ever heard your hard drive through your audio output. It would be a lot worse if it wasn't for grounding planes. Not so bad these days with micro traces, but earlier units required substantial grounding planes to quiet the voice coil drive/control loops.
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.
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.
- Status
Similar threads
