How to design ground pours?

[Fancy Lime]

Hi there,

I am finally shifting to having PCBs professionally made. First try is a rather simple overdrive on a 2-layer board. One layer is poured with ground, the other with Vref. The question I am facing is what to cut out of the pours. At the moment they flow around all other traces and holes, creating lots of loops. Do I want/need to break up all loops to make a proper star grounded plane? How do you Kicad Users out there do it? There is a cutout function but that is rather tedious to use and I have not yet managed to get non-rectangular cutouts.

Thanks,
Andy

[patrick398]

I am by no means an expert but I have made quite a lot of PCBs in kicad all with ground pours. I try to route everything on the front copper layer, using only small traces on the back copper where necessary. If all goes to plan the back copper ground pour is pretty comprehensive. On the rare occasion there are islands I use visa to connect them to the main ground plane.

[ElectricDruid]

I wouldn't try attempting to break up all the 'loops' in a ground plane. Instead, go for the alternative strategy and try and get the most copper connecting it all up as possible. That means not having lots of stuff on your ground plane layer.

I do it pretty much the same as Patrick, but the other way up. I typically have a few power rails and the ground plane on the top, and then route all the tracks on the bottom. Inevitably some stuff finishes up getting "kicked upstairs" to enable me to lay the board out neatly, so the top power/ground layer always finishes up with more breaks and holes in it than I'd like, but it's never been a problem. Occasionally if I'm not convinced there's a low enough impedance between different areas of the ground plane, I'll *add* a nice fat track on the bottom between two convenient component legs or something to make sure there's a simple path for current to flow.

What you're trying to avoid is having different parts of the ground plane at different potentials. As long as it's all connected together with a sufficiently low resistance, that shouldn't be a problem.

[Fancy Lime]

Patrick, Tom,

thanks! My impulse was actually to go the other way: I put most traces on the front and only the necessary ones on the back. Then I filled the front with ground and the back with Vref. The Idea behind that was to separate the signal traces from each other by the ground pour between them. But I guess that should work just as well with the Vref pour, if that has a sufficiently low impedance AC path to ground. I have a 22uF elecrolytic and 100n film cap in parallel shorting Vref to ground so I guess that should be OK. Am I missing something else?

On a related note: one of the next projects will be the *very* high gain fuzz currently on my breadboard. Sort of a "what if they had asked me to design an opamp version of the Big Muff, but better". As of now, I'm using a TL072 for both stages. I am wondering if having the input of the one half as close to the output of the other half as they just are in a DIP package, is asking for trouble at a total gain of 25000. May I want to be using two single opamps instead? Or do I just try to get the layout right and see what happens?

Cheers,
Andy

[bartimaeus]

as others have said, you should route as few traces through the ground plane as possible to keep it as solid as possible. in fact, it's recommended to avoid having a power plane at all in a two layer design, because you'll be risking capacitance and interaction between the top and bottom planes. another option is to avoid planes altogether and instead use a star ground, which should work fine if this is an analog circuit.

for that fuzz, i'd try breadboarding it with a dual vs individual opamps first to see if you can hear a difference. even if that does introduce the complicating factors of a breadboard, seems worth it to avoid having two separate boards made if the dual versions has oscillation problems.

[Fancy Lime]

as others have said, you should route as few traces through the ground plane as possible to keep it as solid as possible. in fact, it's recommended to avoid having a power plane at all in a two layer design, because you'll be risking capacitance and interaction between the top and bottom planes. another option is to avoid planes altogether and instead use a star ground, which should work fine if this is an analog circuit.

I don't quite follow. Why would capacitance be an issue between ground and power planes? They are connected by large capacitors anyway. Capacitance between signal traces and either ground or power planes might be an issue, although a quick back of the envelope calculation tells me that we are talking about fractions of a pF in the absolute worst case scenario I can come up with for the boards I plan to order. Wanting a solid low impedance ground plane makes sense to me though.

for that fuzz, i'd try breadboarding it with a dual vs individual opamps first to see if you can hear a difference. even if that does introduce the complicating factors of a breadboard, seems worth it to avoid having two separate boards made if the dual versions has oscillation problems.

On the breadboard it works fine with a dual. No noise that needs getting rid of, so not much point in trying the single opamp version on the breadboard, imo. Especially since I would first have to order suitable single opamps. However, my personal experience is that things that work fine and without noise or oscillation on the breadboard tend to go haywire once I put them into an actual soldered circuit of whatever kind (strip, vero, pcb, point-to-point...). I understand that that is not the expected behavior and that most people have the bizarre noise problems rather on the breadboard. I might have a rare enchanted breadboard or I may need to have my soldering iron exorcised.

Thanks,
Andy

[Ice-9]

Route as much as possible on a single signal layer and keep the ground plane layer as solid as possible. Vref doesn't need a separate plane and could be routed on the signal layer.

[ElectricDruid]

Vref doesn't need a separate plane and could be routed on the signal layer.

Seconded.

[bartimaeus]

as others have said, you should route as few traces through the ground plane as possible to keep it as solid as possible. in fact, it's recommended to avoid having a power plane at all in a two layer design, because you'll be risking capacitance and interaction between the top and bottom planes. another option is to avoid planes altogether and instead use a star ground, which should work fine if this is an analog circuit.

I don't quite follow. Why would capacitance be an issue between ground and power planes? They are connected by large capacitors anyway. Capacitance between signal traces and either ground or power planes might be an issue, although a quick back of the envelope calculation tells me that we are talking about fractions of a pF in the absolute worst case scenario I can come up with for the boards I plan to order. Wanting a solid low impedance ground plane makes sense to me though.

you're totally right, my mistake! i was just imagining the two parallel copper planes, without considering that with power and ground it can be a good thing. and yeah, with small analog pedals these factors are often pretty minor, perhaps i'm following the rules of thumb a little too closely haha

[phasetrans]

Andy,

This is a very deep topic. There are a few guiding principles, but the correct action depends greatly on a bunch of factors. See, for example Dr. Eric Bogatin's bethesignal.com

And, not exactly for the topic at hand, but maybe the most lucid short discussion on ground planes I've come across over the years:
https://www.analog.com/en/analog-dialogue/articles/reducing-ground-bounce-in-dc-to-dc-converters.html

I think you'll find the principles in that helpful.

Edit: I agree that the concerns are pretty minimal for effects, based on the wide number layout approaches that get to the end, but the article from Analog is a good way to think more deeply about the issues at hand.

[Rob Strand]

You can draw lines or regions which are "keep-outs" to stop automated processes like Fill-regions going where you don't want them.   You can place a keep-out line where you want to split a plane or prevent it from joining in a locate region.  The other way is to place a number of separate Fill-regions.

[PRR]

...with small analog pedals these factors are often pretty minor...

+1