Ground Plane on both sides?

[Beo]

Quick question. In eagle, I've designed a two sided board. Almost all my traces are on the bottom, as well as a flooded ground plane that is connecting all ground points. On top I only have a handful of signal traces, and I have no need for a ground plan. However, I don't want to etch all the non-trace copper on the top side, so I have added a flooded plane there as well.

Should I make this top flooded plane a ground plan (and will connect to all ground pads), or should I keep it unconnected to any pins (floating)?

[R.G.]

A few questions come to mind.

First, plus two points for remembering that just because you can do something doesn't imply that it's a good thing to do.

Then the questions:
- Is there any advantage you hope to gain by doing this? If so, what other things would you trade off for it?
- Ground planes introduce extra capacitance between all nodes and ground. Do you have any high impedance points that would be ill-affected by extra capacitive loading?
- Is a ground plane needed at all?

Ground planes tend to work best on very high frequency stuff, RF and up. Individual ground lines tend to work best for low frequencies, power-line and on down to DC. Audio is pretty firmly in the low end, and usually responds best to individual ground lines excepting for the case of very high impedances.

[Beo]

- Is there any advantage you hope to gain by doing this? If so, what other things would you trade off for it?
- Ground planes introduce extra capacitance between all nodes and ground. Do you have any high impedance points that would be ill-affected by extra capacitive loading?
- Is a ground plane needed at all?

Thanks for the reply.

The only advantages I am trying to gain are ease of pcb design using flood to connect my grounds (no manual tracing) and also quicker etch using less etching solution. As a general rule, I use ground planes universally in my pcb designs. I would be curious what examples of circuits you have in mind (having high impedance points) where a ground plane with extra capacitive loading would be detrimental.

In my particular case, this is just a CD4053 CMOS switching circuit with PCB mounted FX SND/RTN neutrik jacks. I don't think a Ground Plan helps or hurts this circuit. I'm using a two sided pcb because I'm making modular units to replace the boards in a dbx PB-48 48 channel patchbay.

[R.G.]

The only advantages I am trying to gain are ease of pcb design using flood to connect my grounds (no manual tracing)

That's a valid thing to want. It does prevent you from then forcing ground currents to go where you want them to go, which is a consideration at lower frequencies.

and also quicker etch using less etching solution.

My experience has been that the etch time is not changed at any given etch solution. It takes just as long for it to go through 1.4 mils of copper if the spaces are 0.01" wide as it does if they're an inch wide, because the action happens on a molecular level.

However, it does make the solution last longer, as there is less copper dissolved.

As a general rule, I use ground planes universally in my pcb designs.

It's fine as long as you get the results you want and know about other methods when you run into problems.

I would be curious what examples of circuits you have in mind (having high impedance points) where a ground plane with extra capacitive loading would be detrimental.

Any circuit involving a FET input and high resistance to ground, which is also driven from a high impedance source. If the source is low impedance, it swamps any capacitive loading at audio. This is not necessarily the case at RF, where the trace inductance and even higher, transmission line effects get into the picture. But in general, any time  you see a FET input, think about what drives that line. High source impedance - like a FET drain or bipolar collector which is not shunted by resistance under 1M or so, or an inductive sensor, like a guitar pickup or worse yet, a piezoelectric pickup - gets easily affected by stray capacitance.

Another issue I've run into is that grounds planes make hacking to fix PCB layout errors ( I can make layout errors faster with a layout system  ) much harder, as well as making unsoldering component leads in the holes difficult. Not a biggie, just something to be aware of. Even thermal reliefs don't necessarily help that too much.

In my particular case, this is just a CD4053 CMOS switching circuit with PCB mounted FX SND/RTN neutrik jacks. I don't think a Ground Plan helps or hurts this circuit.

Will there be guitar or piezo sources driving the inputs?

Ground planes are not always bad or always good. They're a tool, with good, bad, and so-so applications. For grounding in general, one needs to think about what currents flow in the ground, and where they go. Ground planes let them go wherever they want, generally the shortest path around any obstructions, but that may or may not be where you want the currents to go. You're right, it probably won't matter for this one. But it always helps to think.

[Beo]

Ground planes are not always bad or always good. They're a tool, with good, bad, and so-so applications. For grounding in general, one needs to think about what currents flow in the ground, and where they go. Ground planes let them go wherever they want, generally the shortest path around any obstructions, but that may or may not be where you want the currents to go. You're right, it probably won't matter for this one. But it always helps to think.

Even when I use ground planes, I usually try to make sure there is only one path around any component or group of components, such that all current flows in unforked known directions to the pcb ground point. Sometimes this means making multiple ground plan geometric shapes connected at key points, or moving components around to break an unwanted path. That's part of the fun of doing layouts.

Back to my original question... what to do with the top side. I don't need any top side ground points, and I don't want alternate paths for ground current flow anyway, so my top plane should not connect to ground. However, I don't like having a plane of copper not connected to any ground or signal at all (floating), so its best not to have it in the first place. Ergo, etch everything on top except the traces. I'd better go buy more Ferric.

[R.G.]

Back to my original question... what to do with the top side. I don't need any top side ground points, and I don't want alternate paths for ground current flow anyway, so my top plane should not connect to ground. However, I don't like having a plane of copper not connected to any ground or signal at all (floating), so its best not to have it in the first place. Ergo, etch everything on top except the traces. I'd better go buy more Ferric.

I agree. No floating copper areas.

Thomas Organ back in the early to mid 60s did a "minimum etch" style that made the entire copper side be rounded-corner rectangular areas and only about a 0.05" "negative trace" between them. It was sometimes a b143h to work on.

I used to worry about conserving etchant, but I found that my time doing a layout was far more costly than buying more etchant. But I have nothing against it otherwise. Being thrifty for cause is good.

[PRR]

A reasonably short and narrow trace opposite an "unnecessary" ground plane adds very little stray capacitance.

If the trace is not short, it should probably be buffered before it goes anywhere far.

Guitar is an exception. We run it through 10 to 30 feet of cable, 300pFd-1,000pFd capacitance right there. Another inch or three of PCB microstrip doesn't add enough more to matter; less than changing guitar cables. And losing a little bit off the high frequencies must be considered against possible better shielding against line-buzz.