PCB Ground Pours - WHY?

[MoltenVoltage]

Being a programmer and not an EE, I am wondering why it is better to use a ground pour on the bottom layer of a PCB as opposed to simply ground traces.  I am thinking about digital circuits in particular.

I know it is common practice, but from my perspective it seems that the more ground there is running right alongside every other trace, the more chance of coupling and noise bleeding into the ground.

What am I missing?

Also, is there any reason to use a ground pour on the top layer as well?

Thanks!

[jefe]

I know one advantage to ground pours is that less etching = saving money. Your etching solution lasts longer.

[jkokura]

I know one advantage to ground pours is that less etching = saving money. Your etching solution lasts longer.

I think that's why many of the DIY solutions work. It's also much, much easier when doing a layout in Eagle to connect the grounds in that way. It instantly removes many, many air wires and helps me do my layouts much quicker with effiecient use of space.

That's why I do it. I haven't noticed any noise as of yet, but I'm also doing small layouts for things like buffers and fuzzes! I've only done overdrives and smaller.

Jacob

[amptramp]

Ground pours provide some shielding and also some heat removal.

I have worked on spacecraft where the boards were foamed after manufacture so there was no radiative or convective heat transfer - everything depended on conduction through leads and if you have a ground pour, you can get rid of a lot of heat.  The ground pour should be broken up in the vicinity of leads so it will not take an excessive amount of heat to solder and many people use a checkerboard or some other pattern of etching to avoid warpage due to retained stress in the unetched portion.

[Paul Marossy]

Ground pours provide some shielding and also some heat removal.

I have worked on spacecraft where the boards were foamed after manufacture so there was no radiative or convective heat transfer - everything depended on conduction through leads and if you have a ground pour, you can get rid of a lot of heat.  The ground pour should be broken up in the vicinity of leads so it will not take an excessive amount of heat to solder and many people use a checkerboard or some other pattern of etching to avoid warpage due to retained stress in the unetched portion.

Huh, interesting.

[Hides-His-Eyes]

It helps to keep the potential of the ground consistent. It's an easy way to approximate a star ground without trying to route every ground to the offboard individually.

[R.G.]

Ground pours, like every other technical item, have their place and are not universally applicable.

At DC, the best operation of the circuit is usually with what amounts to a star grounding system, every ground return going from the load back to the power supply return. At RF, ground planes are far superior because of the field effects of the fast signals.

=> There is a continuum of the transition from star ground to planes as the frequencies of the signals involved rises.<=

At audio - which is DC as far as most signal frequencies are concerned for ground plane/traces - the best results are usually obtained by star grounding. This is because what we call "ground" is at least three different function: voltage reference, shielding, and what I call "sewer ground" for returning used electricity to the power supply. I've typed this stuff repeatedly here, so save me some typing and search for "sewer ground" for more explanation.

Ground planes can cause problems with signal loss at treble in proportion to the impedance driving a trace. The higher the drive impedance, the worse the treble loss, even at audio. Same issue as long cables loading down treble from a guitar. There is no substitute for knowing the electrical characteristics of what moves through a PCB trace, what drives it and what loads it. This is one reason computers still don't give good analog layout - the nature of the signal, sources, and loads is so highly variable.

Inappropriate ground pours is another of the hallmarks of a PCB neophyte.

[MoltenVoltage]

Thanks for the replies.

From what RG has said, it makes more sense to put a ground pour under the digital parts of the circuit (because of the higher frequencies involved), but use ground traces for the analog portions.  Then, to the extent possible, all those grounds should be in a straight line to the power supply.

I assume (and have read) that you also want to keep the analog and digital grounds as physically isolated as possible - like on separate sides of the PCB with the power connection in the center.

The other question was whether it makes any sense to have a second ground pour on the top layer as well.  Any thoughts?

[R.G.]

Analog planes, digital planes, and split planes are not simple subjects. Multiple planes become a large, low quality capacitor, and unless other things are right, you can induce noise where you've piously tried to exclude it.

For effects purposes, use a ground plane for digital edges, use them for analog where you have a particular purpose in mind more to the point than "keep things quiet".

Effects being the trivial examples of almost everything that they are, you'll probably get away with things that would rise up and bite you in other places - at least until the situation arises that you can't get away with it.

[MoltenVoltage]

I actually have your book PCB Layout for Musical Effects (from SB), and I just picked it up again and noticed there is no discussion of ground pours and none of the examples contain ground pours or ground planes.  Based on what you have said, I assume this was by design since the book doesn't address digital circuits.

I also assume that when you say "Multiple planes become a large, low quality capacitor, and unless other things are right, you can induce noise where you've piously tried to exclude it" means that a ground plane on the top and bottom of the PCB in the digital sections is likely to create more problems than it solves.

Thanks again.

[Processaurus]

"Multiple planes become a large, low quality capacitor, and unless other things are right, you can induce noise where you've piously tried to exclude it" means that a ground plane on the top and bottom of the PCB in the digital sections is likely to create more problems than it solves.

You use planes for power and ground, which are always decoupled through big capacitors anyway, what would the harm be in adding a little capacitor in parallel?

On commercial digital pedals (the examples I've poked around are the whammy pedal and line 6 pedals) I've noticed they keep a separate ground plane for the analog and digital sections, and star ground those planes at a single point.  The goal being to herd the little spikes the digital section is producing on the ground rail away from being upstream of any of the sensitive parts of the analog section, and have both of them meet back at the power supply.

Here's the bottom of a DL4, that's the analog section on top, and the digital section on the bottom.  Not sure why they made the two planes meet where they did, rather than up by the PSU input...

[Processaurus]

Here's a Digitech pedal, same deal, that's the analog section on top, and digital on the bottom, they look like they hooked the planes up back at the PSU back in the upper right corner:

[R.G.]

Things get odd as frequencies go up. There are no more resistors, capacitors and inductors - all components are combinations of these as the frequencies change. One can no longer think of a conductor as a short circuit, or even resistive. So any two plates of metal form a capacitor, even if they're connected together one point, and there is inductance trying to keep any signal changes apart even on the same plane. The signals take time to get from where they are on one plate around the connection and to the place on the other plate. Meanwhile, they can cause mischief locally by coupling between plates before the signal can run over ...there... to the connection and around to where the current is flowing.

The way to do multiple planes correctly is to ensure that all current demands on one plane are satisfied on that plane for all frequencies larger than the one where the field effects don't cause problems in that particular physical setup of planes and conductors. That is, there isn't a general answer. You have to know the signals, current demands, frequencies, and physical setup. The results depend on the shapes of the things involved.

I left this out of the PCB book because it's way beyond what most neophytes need to worry about, and because audio is thankfully below most of this. The issue I'm sure you're running into is that you're messing with multi-MHz controllers and want to keep things quiet. Rather than worrying about planes, put a ground plane under your digital stuff and keep all signal lines as short as you can possibly get them. Short and direct is always good practice in circuit layout, but especially with fast signals. Do your audio ground separate from the digital ground **entirely** and then connect them at one and only one point, so that no currents can flow across one ground to get to the other power domain. The one and only one point is selected so that any signals that have to communicate between the two domains flow on the single connection, and you can force these to be slow ones by selecting what happens on each side of the divide between power domains.

There is a large amount of stuff that goes into layout at high frequencies and with fast logic edges.