Ground plane, power plane, signal ground vs. power ground?

[Taylor]

While doing the Gristleizer PCB, I discovered the joy of a ground plane. Instead of having to route all my grounds to the ground ring around the board, I can ground any pad right where it is. Really cuts down on trace clutter.

However, I'm a little uncertain about a couple of things.

1) Is it bad to treat all grounds equally? In other words, some people make the distinction between power and signal ground, or "sewer" ground and signal ground, etc. In the context of effects, when is it ok to just connect all grounds to the ground plane, and when is this bad? In cases where I shouldn't do this (I'm thinking circuits with clock signals) how exactly should I handle the separation of grounds?

2) Can I do the same thing with power? In other words, if I have a ground plane on copper layer 1 (on a double-sided PCB), could I make a power plane on layer 2? This would make routing so much simpler, but something tells me this would be bad. I can imagine I may be creating a capacitor by having two flat layers of copper separated by fiberglass, although it would probably be negligible compared to the intentional ripple filtering. Would this create extraneous noise or crosstalk, or anything?

[R.G.]

I've alluded to what I'm about to say, if not said it directly, several times.

At low frequencies, it's probably best to route the traces from a source to a load and back from the load separately.This gives you detailed control of where the currents go, and where the currents are flowing, not where the voltages are, is what matters in many high gain low frequency (i.e. DC to ultrasonic!) circuits. Sometimes it is critical to know where the return current for a particular part of your circuit flows. An example is the return wire from a speaker needing to go on it's own, separate path from speaker to the power supply. At high frequencies (probably 100kHz, if the signal has lots of harmonics) on up, ground planes rule. Above a few MHz, you need to consider every signal trace to be an RF transmission line.

Of course, most pedals are too small to take advantage of the differences. And most layout "artists" are not advanced enough, nor do they have the layout tools to make a ground plane automagically. So for pedals, it's largely a moot question. And so to your questions.

1) Is it bad to treat all grounds equally? In other words, some people make the distinction between power and signal ground, or "sewer" ground and signal ground, etc. In the context of effects, when is it ok to just connect all grounds to the ground plane, and when is this bad? In cases where I shouldn't do this (I'm thinking circuits with clock signals) how exactly should I handle the separation of grounds?

Bad? Depends. The name of the game, as I said above, is knowing where the current flows. At low frequencies, the current will flow where the resistance is lowest, and so if you could see charge carriers, most of them would try to follow the straightest path (which is the lowest resistance path) across a copper plane. But, being charge carriers, they push each other away, and cause a voltage by flowing. This forces the carriers around them to spread out. So the carrier density is highest in a straight line between source and return, but spreads. And if there are any voids in the ground plane, then the carriers bunch up in the gaps. Gaps in planes are serious business at high frequencies, indeed.

As frequency and current increases, the inductance of the path matters more than resistance. Inductance can get bigger than resistive impedance quickly.

Of course, you need special equipment to sense this kind of thing happening. Like a differential input probe with high impedance FET inputs and high gain. Um... wait! That's kinda what the input to many effects looks like! oooohhhh.

This is another case where the devil is in the details. I use ground planes a lot for stuff that beginners don't have to try to make with press-n-peel, because you're definitely not getting a ground plane on a single sided board. But if you can afford the price and design time for ground planes, sure, use them. But know where your high impedance paths are for both current sensing reasons and for the capacitive loading effects. And worry about where high currents go. 

2) Can I do the same thing with power? In other words, if I have a ground plane on copper layer 1 (on a double-sided PCB), could I make a power plane on layer 2? This would make routing so much simpler, but something tells me this would be bad. I can imagine I may be creating a capacitor by having two flat layers of copper separated by fiberglass, although it would probably be negligible compared to the intentional ripple filtering. Would this create extraneous noise or crosstalk, or anything?

A three- or more-layer board, with power on one plane and ground on the other? Pure goodness for high frequency logic circuits. This gets you to the lowest inductance, highest capacitance and lowest characteristic impedance power distribution setup you can get. Unfortunately, it's kind of wasted for audio unless you have a really critical application where it's worth the money to do any and everything you can do to get the last ounce of goodness squeezed in.

Copper layers tend to cost about the same as another board. A double sided board is about twice as expensive as a double sided board where the volume lets the maker set up a single sided batch on his line. They're the same price where you're forced by economics to buy your single layer boards from a maker who only does double sided and makes single sided by etching away the second side. But a three layer board will cost 50% more and a four layer will cost about twice what a double sided board does.

It's nice, but you're well into diminishing returns for something that has no particular advantage except easy routing. Of course, if you can afford a Rolls Royce, great! 

[Taylor]

I may be (probably am) using the wrong terminology; what I'm talking about is a copper flood I guess, where the ground fills up all the spaces where there are no pads or traces, and then to route a pad to the ground, you just make little lines from the pad across the little void ring around the pad, or use the tool in your CAD program that does this for you.

So I'm talking double sided board here, where traces are on both sides, but the ground and/or positive rail fills in all the spaces without traes or pads, leaving empty space between the traces and ground pour.

Thanks for that detailed reply!

[R.G.]

Ok, the price issues don't apply if it's built on double sided copper board.

A copper flood puts whatever signal you flooded with everywhere. That's good for running ground around. That can be bad for the reasons I cited: if it increases capacitance to ground for a very high input impedance point like a JFET input, you can lose treble, although that's not going to be a huge issue with bias resistors under 1M; and you can lose control of where your ground currents run. This last is probably not a big deal unless you have either high impedances or big current users... like LEDs... which put steps of current into your ground path, which you may not have thought about since "it's a ground plane".

Probably it's fine in the vast majority of cases. I'm just used to thinking about the "edge" cases as a matter of course.

[Processaurus]

The copper flood for ground looks like a good idea if the layout software has it (I guess it could be made just as an automatic groundplane on a busy layer).  I see that on older boss PCB's, both the hand drawn ones and the other single sided boards after.  You gaining lower resistance from the fat parts even if it bottlenecks.

You might know this already, but even without a groundplane/flood type traces, it's good to make the power and ground traces wide, for low resistance.  30mils is good.

If you do use a ground plane, a solder mask is a good idea, or increase the standard clearance from the plane to traces (to maybe 15, or 20 mils), I recently got in a bad situation with the bare bones type PCB (no soldermask or silkscreen1) where the groundplane was 6 mils away, and I had to drill some stuff out, and little copper bits would short to the groundplane, and I had to watch every solder joint on the groundplane side.  A couple of times it didn't work and scrubbing the bottom with a toothbrush made it work, nightmare.

[Cliff Schecht]

R.G. is spot on as always. Ground planes are great for many things but only if you understand what you are doing and why you are using a ground plane. The most important point that RG made really can't be reiterated enough, know what currents are going where. This is important in digital and mixed signal cases where controlling the coupling of signals from trace to trace is key (including traces running alongside grounds). Ground planes can be used to greatly reduce the impedance of ground runs (resistance decreases as surface area increases).

Certain types of signal AND ground runs are notorious for coupling unwanted noise into a system. As we've all experineced, LFO bleedthrough happens because the relatively fast rise times of any modern part (being op amp or transistor based) can easily be in the low uS to high nS range. These types of signals can bleed through a ground that is too close to a trace and couple into other parts of a circuit, especially if the ground trace itself is too long or too thin (both contributing to excessive resistance). Also, as RG said, LED's can be a big source of noise in any ground, be it a ground plane or a trace, because they have a lot of return currents that must be handled properly.

PAiA (I promise this isn't an advertisement ) uses a special grounding scheme that separates high current grounds from important signal grounds. Keeping these two types of signals separate really helps to keep down on the ground noise. The big trick with these schema is to only have the power and signal grounds touch at one place, the input voltage filtering caps. This is the lowest impedance ground point (or should be) and is where ground currents get swamped out by the voltage smoothing caps. I use a modified grounding scheme that is much like the old PAiA way (meaning John Simonton's way) but takes advantage of dual layer boards. All of the important signals, from front panel to op amp inputs, etc. are connected through a ground plane set at a minimum of 20 mils from any trace. Any high current or otherwise noisy ground/return path, be it LED or digital switching, gets a separate ground that is carefully routed on the board (usually just avoiding important signal paths). The only point at which any "noisy" ground touches a signal ground is back at the power supply. This has worked wonderfully and is the same schema I use on all of my personal projects whenever feasible.

[Cliff Schecht]

Also worth mentioning: Eagle has a fantastic ground pouring system. You can set the layer, exact shape, clearance and thermals (just a few of the options) with very few clicks and every pour is rock solid.