PCB Unconnected Copper Pour - Bad Idea?

GroupDIY Audio Forum

Help Support GroupDIY Audio Forum:

This site may earn a commission from merchant affiliate links, including eBay, Amazon, and others.

john12ax7

Well-known member
Joined
Oct 15, 2010
Messages
2,463
Location
California, US
Suppose a 2 layer pcb,  bottom copper pour is gnd plane.  What to do with the top copper pour?  Connect to gnd also or leave floating?

For RF circuits it's generally a terrible idea to leave copper unconnected.  But I've never directly measured it for audio.
 
ruffrecords said:
No electronic reason then?

Cheers

Ian

Top copper pour helps with RF circuit performance. Top and bottom planes get stitched together with a lot of vias.

But with audio I'm not sure.  It should improve EMI, but could also accidently create unwelcome additional ground return paths.
 
Generally I would ground it, but I am apprehensive about giving broad sweeping advice...

JR

PS: For TMI back in the day Hartley would ask PCB designers to leave as much copper as possible to save etchant...  Hartley might be even cheaper than me.  8)
 
Boards can easily warp if you have a lot of copper on only one side. Just ground it. Or, if you have a part that needs to dissipate power, create a grid of vias to make both planes into a heat sink.

Besides, it's already there to start with. It would just take the board house more time and energy to remove it.
 
Some points on this -
It's never a great idea to have floating conductors in any circuit. The signal being processed may not be 'rf' but basically any circuit functions in an environment where it may be subject to rfi. Having more low impedance copper (generally a ground plane) may* helps with this. A floating copper plane is definitely a bad thing - may give rise to all sorts of unpredictable behaviour wrt rfi.

* I say "may" because I can only remember reading one technical report on having both Ground Plane and 'Top Copper Pour'.
This was on an avionics application IIRC so critical to viability. Result was basically that a very marginal improvement could be achieved IF the 'stitching' of the top copper to the ground plane was optimised. But in general there was no measurable improvement and performance could be impaired if the 'stitching' was implemented in some ways. Not as simple as more vias the better as the vias themselves disrupt the ground plane. Also consider that via geometry alters the inductive impedance of the via itself - basically smaller via gives higher inductance - see online calculators.

Since standard pcb fabrication is a subtractive process it does make sense to not remove copper unnecessarily for reasons that have been stated.
Take account of any high impedance nodes - probably don't want to increase 'stray' capacitance to 'Ground' there.

In general I'd say have a top copper pour and stitch it to the Ground plane layer in what looks like a common sense way.
wrt 'Ground Loops' - I wouldn't worry - the 'loop areas' should be so small such as not to be an issue.
An interesting way to think about a solid ground plane is an infinite number of ground loops with infinitesimally small loop areas  ???
 
I would not connect it to shield ground, that will introduce any crap at Pin 1 further into the box.

Nor would I leave it floating, because of the capacitive coupling potential.

I pretty much agree with Newmarket and Squarewave, although I've never really agonized
over minimizing the etch process for board cost control.
 
Just want to add to what's been said. Copper pour has two main purposes in audio:
  • Reducing ground path resistance; however, this can result in mixing "grounds" that shouldn't be mixed. Hence the necessity of creating islands.
  • Providing electrostatic guard, such as to eliminate cross-talk
The rest is marginal. It's true that some PCB fabs offered premiums for minimum etching; I haven't seen it in ages.
 
Dan Kennedy said:
I would not connect it to shield ground, that will introduce any crap at Pin 1 further into the box.

Nor would I leave it floating, because of the capacitive coupling potential.

I pretty much agree with Newmarket and Squarewave, although I've never really agonized
over minimizing the etch process for board cost control.
Of course we need to inspect where the current flows. You do not want to corrupt a Ov clean signal node, but low Z ground sewer makes a good catch all.  Treat audio signals differentially and flush the noise currents harmlessly into a robust ground.

A large ground pour is like an antenna or single plate of a capacitor... It can be used for benefit or not....

JR
 
I've definitely seem a few pro audio products that don't follow the recommendations in this thread,  which got me thinking as to how much of an issue it really is.

But it seems  there is consensus that the prudent thing to do is ground it.
 
john12ax7 said:
I've definitely seem a few pro audio products that don't follow the recommendations in this thread,  which got me thinking as to how much of an issue it really is.

But it seems  there is consensus that the prudent thing to do is ground it.

I have not seen any convincing evidence that it is worth having.

Cheers

Ian
 
ruffrecords said:
I have not seen any convincing evidence that it is worth having.

Cheers

Ian
Maybe when you deal with a very dense PCB containing several signals that may or may not be mixed, such as a single PCB mixer, you'll see the evidence.
Anyway, the subject is not about copper pour: yes or no, it is about floating or not, and I can't imagine a case where a floating pour gives any advantage over non-floating.
 
please pardon my english, i'm still learning electronics but i have some related questions about ground planes and copper pours.

It seems like a good idea to ground the copper pours to prevent them acting like antenas and coupling noise to the signal. ( what i understood).


I etch at home and always leave copper pours and ground planes as much as i can for convenience in etching, but also shielding and minimising loop area and ground impedance,  in hopes of low noise.

It seems to work well so far with my homebrew prototypes. (low freq audio only).


But i have a related question,  i'm curious,  in what cases having ground pours and ground planes everywhere would be negative for audio?  no digital or rf.


About mixing returns signals,  would not the ground reduced impedance minimize the negative effects?

And in the case of high impedance nodes on a board,  would the extra capacitance to ground affect audio?  I mean it should act like a lowpass filter no? but could it affect the audio band?  Should i, as precaution try to identify high impedance nodes and leave spaces without ground pours around theses traces and dedicate a return path?

I hope my question was clearly expressed, many thanks for all the knowledge you guys are sharing.

John
 
diggy fresh said:
please pardon my english, i'm still learning electronics but i have some related questions about ground planes and copper pours.

It seems like a good idea to ground the copper pours to prevent them acting like antenas and coupling noise to the signal. ( what i understood).
While not very common, careless connection of multiple parallel ground paths could inadvertently create a loop that looks like a one turn transformer winding in the presence of strong magnetic fields (like inside a large power amplifier). This loop can develop a voltage across it, just like a winding. 
I etch at home and always leave copper pours and ground planes as much as i can for convenience in etching, but also shielding and minimising loop area and ground impedance,  in hopes of low noise.

It seems to work well so far with my homebrew prototypes. (low freq audio only).


But i have a related question,  i'm curious,  in what cases having ground pours and ground planes everywhere would be negative for audio?  no digital or rf.
For shielding as long as those shield noise currents get harmlessly dumped, the more the better.  For brute force low impedance grounds lower is better, but power rails need to be low Z too.
About mixing returns signals,  would not the ground reduced impedance minimize the negative effects?
maybe
And in the case of high impedance nodes on a board,  would the extra capacitance to ground affect audio?  I mean it should act like a lowpass filter no? but could it affect the audio band?  Should i, as precaution try to identify high impedance nodes and leave spaces without ground pours around theses traces and dedicate a return path?
The capacitance is relatively small (picoFarads), but for very high impedance it all matters.  I am generally more worried about added capacitance from an op amp - input to ground that can add lag to the NF signal and diminish stability.
I hope my question was clearly expressed, many thanks for all the knowledge you guys are sharing.

John
Better than many... I didn't have to search any of your words....  8)

JR
 
diggy fresh said:
But i have a related question,  i'm curious,  in what cases having ground pours and ground planes everywhere would be negative for audio?  no digital or rf.
It's difficult to think of a scenario were it would have a negative effect. Abbey road d enfer's example (which I assume is trying to demonstrate some kind of loop that might have currents induced around it) is not particularly realistic since all of the ground leads would stitch together the two planes and break up the loop making it (them) insignificant. And the drawing is not representative of how the parts would be laid out. It would have to be all surface mount spread out over a large area with no vias. And something would have to be throwing some serious current around. I think it would challenging to deliberately design a board that exhibited negative effects from a ground plane loop like that.

diggy fresh said:
And in the case of high impedance nodes on a board,  would the extra capacitance to ground affect audio?  I mean it should act like a lowpass filter no?
Almost certainly "no". The capacitance would depend on the surface area shared by the high impedance net and the ground plane. That "surface" area would only be the edges of where the nets are in close proximity. And the gap in between would have to be very narrow. If the high impedance trace was really long, it would increase the "surface" area but that would make noise a much larger problem long before capacitance ever showed up. The transistor junction(s) of whatever the high impedance net was connected to would completely swamp any capacitance to ground.
 
Back
Top