opinions on copper pours on PCBs

[geekEE]

I wanted to get input on the advantages and disadvantages of using copper pours to fill in all unused spaces of outer layers of PCBs with ground in cases where plane layers already exist. It seems to me that there is the possibility of providing additional shielding if there are internal signal layers, but that this may be offset by the fact that it is chopped up into so many small pieces. It also seems that, unless you're really careful about putting ground vias in the appropriate places, it's easy to end up with pieces of copper that are connected to ground at one end only, which would allow them to act as antennas for any noise in the ground plane.

I suppose the other advantages copper pours may have is some additional heatsinking or using less etchant when fabricating.

I tried looking for any info on copper pours that actually had testing or simulations done, but didn't find anything. The info that I've found has been more anecdotal. If anyone knows of any books or white papers or other sources that would be helpful, let me know.

I don't have any particular issues with copper pours right now. I am just interested in the reasons that people use them.

Glenn

 

[treez]

I was always under the impression that the more "ground pours" you do the better. Though really there should not be that much space for this ground pouring as really PCBs should be made as small as possible, and any eg power traces should be as wide and short as possible and so not leave large aeas where you could pour some ground into.

I never heard about that problem with traces connected to ground in just one place radiating noise from the ground plane. I would have thought the prescence of the ground would conveniently capacitively couple noise away from adjacent traces away to ground.

 

[Comcokid]

If used properly, designed properly, and executed properly, additional ground pours can help in shielding and noise. It always involves attention to the details of the PCb as a whole.

Sometimes ground pours are done to reduce the possibility of PCB warping during reflow by balancing the amount of continuous copper on each side of the board.

But, adding pours to a poor PCB layout may achieve nothing.

Remember - patch antennas, at first glance, resemble a ground plane or ground pour.

 

[geekEE]

I must say that I have not typically used ground pours in the past and have not had any EMC issues (I haven't done any significant RF design, so I expect that would have significantly different design rules). I pay a lot of attention to rise-times and to return paths for current. But, I would always like to know if I can do things better. Here are a couple of scenarios.

1. If there's a four-layer board (signal-plane-plane-signal) that passes all EMC tests with no copper pour on the outer layers, will adding grounded copper pours show any reduction in radiation? Will it stay about the same? Can it make it worse?

2. If there's a six-layer board (signal-signal-plane-plane-signal-signal) that passes all EMC tests with no copper pour on the outer layers, how will the addition of grounded copper pours affect the tests?

Glenn

 

[itsmoked]

Probably reduce them in both cases.. But you'd likely need to retest. It would be imprudent to just add them summarily.

I never bother with pours unless at a glance the board appears to have acres of wasteland, as it were. Most of my boards are so specialized or dense that pours would be folly. Often they're 4 layer and would have planes anyway.

Keith Cress
kcress -

http://www.flaminsystems.com

 

[geekEE]

treez, here's one article that briefly mentions copper pours that are grounded at one point.

http://electronicdesign.com/Articles/ArticleID/5944/5944.html

However, I don't know if this only becomes a problem if the chunk of copper is long. i.e. Is there some length below which it becomes such an inefficient antenna that a single ground via would be acceptable?

Keith, I agree that retesting would be wise. I guess I'm just trying to figure out cases where it makes sense to do the ground pour in the first place. It can be a considerable amount of work to do the pour, put a bunch of ground vias in the appropriate places, and make sure that there are no isolated or single-via areas of copper.

Glenn

 

[MikeHalloran]

If the process used is 'subtractive', e.g. copper is removed from a solid sheet by selective etching, then the ground pour produces less acid waste to account for and treat.

Additionally, if the copper is thick, the full perimeter heat sink makes desoldering in repair and service operations more difficult, or more skill-intensive, and may interfere with soldering at first assembly. I've seen more than a few power supply boards with full copper pours that were actually etched all the way around the vias, except for a few radial spokes of copper.



Mike Halloran
Pembroke Pines, FL, USA

 

[itsmoked]

Mike those are called, 'thermals', short for 'thermal reliefs'. They are often needed to prevent assembly disasters. e.g. "Where's my 575 watt Weller?"

Keith Cress
kcress -

http://www.flaminsystems.com

 

[MikeHalloran]

Wellers are for pansies.

My first task at my first for-pay job ever was replacing a loudspeaker at the top of a telephone pole, using a Bernz-O-Matic to do the soldering.

Not a Bernz-O-Matic torch with soldering tip; just the torch.



Mike Halloran
Pembroke Pines, FL, USA

 

[MacGyverS2000]

Comco pretty much summed up everything I was going to say, so I won't try to add anything more.


Mike, thermal reliefs should be added as a matter of habit in PCB designs. Imagine something as simple as no reliefs on a part, but it will not be reworked, just IR soldered. That part will have a significantly reduced life as the heat retained in the remaining copper will continue to transfer to that component long after the IR oven has cooled down, killing off the original heat ramp spec.

I used a Weller from the time I first grabbed my father's off of the shelf at the age of 8 until just a year ago, when I switched to a Metcal. The Weller did it's job quite reliably, but I found myself trying to work around problem components (such as large components with no thermal relief pads!). Now that I've spent some time with the Metcal, I'll never voluntarily go back... inductive heating is the way to go! Even beefy 10W components are no match for the smallest of tips.

Dan - Owner

http://www.Hi-TecDesigns.com

 

[Noway2]

I have used copper pours on TWO layer boards to effectively achieve power and ground planes. While the planes on the two layer will be full of holes, and won't have the constant impedance properties of a higher layer layout, you can still achieve a lower impedance on your ground (and power) nets than you can with serpentine traces.

Remember, the high frequency return currents will follow the path of least impedance, which at their frequencies is almost certainly the path of least inductance. To get low inductance at high frequencies on a PCB you need a wide, flat surface and one full of holes is better than a set of serpentine traces.

You need to also remember that the high frequencies / high speed signals have nothig to do with logic clock speed. Rather it is the rise and fall times of the devices that are doing the switching that is important.

I had a two layer board desgin that suffered terribly from EMI problems. I redesigned the board using 'finger traces' off a wide trunk for the power and a copper pour on the top side of the board for a ground plane. I also switched from through hole to SMT components because of the flatter - wider tabs over long thin pins (lower inductance). Cleared the EMI problems right up and never had another failure in the 3 years I remained at that company.

The website sigcon.com has a lot of information on this subject if your interested.

 

[geekEE]

Thanks Noway2. I checked that site, which belongs to Howard Johnson, and found some info that directly related to what I was looking for.

http://sigcon.com/Pubs/edn/GroundFill.htm

I had looked at Johnson's first book, but didn't think of checking his website. His advice is to use copper pours on 2-layer boards, but not on boards that have power planes already. However, his advice is from a signal integrity point of view, and not with respect to heat or manufacturability.

By the way, I also have high praise for the Metcal soldering irons. When I'm soldering 0402 components under a microscope, a Weller tip looks as big as a club. And I suspect a Bernz-o-matic torch might be a little bit of a problem as well.

Glenn

 

[MacGyverS2000]

Nah, the Bernz-O-Matics are just fine for 0402 chips... you just need to make sure the gas pressure is set low enough that the flame won't blow the chip off of the board or melt your optics ;-)

Dan - Owner

http://www.Hi-TecDesigns.com