PCB 2 Layers Design

[avaldezc92]

Hi I'm new 

I found this forum very useful in this past weeks, I have a question about the power planes in 2 layers pcbs.

Why or what is the advantage of having two ground planes in a 2 layer pcb? because I've seen a lot of boards with this design.

Greetings from México.

-Angel

[Neilm]

I would have thought these was not a plane, but a copper pour. Good for copper balancing to stop the PCB warping and as you are not removing (wasting) the copper, it cuts down the wast produced and could be cheaper to produce in high volume. I would not have thought it would do anything for signal integrity if it is only a 2 layer board.

[Precipice]

Flood filling top & bottom with ground, and stitching them together wherever possible with vias, makes for as good a ground as you can get, on a 2 layer board. Where a track breaks the plane on one layer, you try to make sure there's a plane on the other layer, and vias to join them all together.
Good grounding is (more or less) layout rule 1 (and is the rule most thoroughly violated by breadboard designs).

Manufacturing is very, very secondary to ground integrity, in my book, but yeah, keeping copper balanced is a good thing - but on a 2 layer board, it's irrelevant.

[alimirjamali]

In addition to the mentioned points, large area of copper (on outside PCB layers) connected together with multiple vias could improve thermal properties of PCB and act as a heat sink.

[tszaboo]

I would still advice, that route the GND like the other signals, even with more care, and add the pour and vias as the last step. It is too easy to make a narrow path on the GND on two layer.

[Precipice]

Absolutely! Hoping that a last-minute ground flood-fill will be good enough is doomed - big fat tracks, in a mesh, joining everything. Other tracks can hop under / over on vias, they're rarely as important as ground being (mostly) the same everywhere.
At the very end, stiffen up the ground as much as possible with floodfills and stitching vias. Heck, even on 8-layer boards, I'll flood & stitch ground on the signal layers. There are some times when more ground is bad, but they're pretty few and far between.

[zapta]

I would still advice, that route the GND like the other signals, even with more care, and add the pour and vias as the last step. It is too easy to make a narrow path on the GND on two layer.

Especially with Eagle auto router. Otherwise you risk getting having the 'collapsed polygons' problem. The pre routed ground guaranteed connectivity and the pour is a free bonus.

[akis]

Less copper to remove. Helps greatly with HF designs. If you are lucky/ careful you will not need to route the GND net but the flood fill will take care of it, all on the bottom layer so no need to solder on top at all.

[alank2]

I always put a ground pour on both the top and bottom, the bottom is what I consider the ground.  I route as many traces as possible on the top and usually I only have to put some traces on the bottom.  The traces on the bottom are chosen purposefully to cut the bottom pour as little as possible by minimizing them at the expense of more top signals.  Multiple traces on the bottom are put next to each other so they don't cut the bottom pour twice, but once.  In the end there will be lots of cut off areas on the top where the pour will have holes, just use a ground via to link it to the bottom pour to minimize the copper difference between the top and bottom.

[avaldezc92]

If im using SMD components (Most part) should I place a VIA for each ground and then make the pour and  then VIA stitching or just make the pour and then place VIA stiching?

[Dago]

Copper balance. If there is too little copper on the top layer compared to the bottom then the board can become warped (and any good factory will complain about poor copper balance).

[Precipice]

Copper balance. If there is too little copper on the top layer compared to the bottom then the board can become warped (and any good factory will complain about poor copper balance).

It has to be really, really bad, and on a 2 layer board, if it's on 1,6mm prepreg, I don't think it _can_ be that bad. Heck, 1-layer PCBs tend to be made by etching away the second side of a 2-layer board, until you get to some volume, just because it's easier to stock.

Sure, on a thin prepreg in a multilayer stackup, you need to behave - no solid plane one side, sparse tracks the other, but OP is asking about 2 layer, where you can get away with pretty much anything. Still flood it with ground and stitch it together, though. It's one of those things that's cheap, easy, and good.

[Dago]

Copper balance. If there is too little copper on the top layer compared to the bottom then the board can become warped (and any good factory will complain about poor copper balance).

It has to be really, really bad, and on a 2 layer board, if it's on 1,6mm prepreg, I don't think it _can_ be that bad. Heck, 1-layer PCBs tend to be made by etching away the second side of a 2-layer board, until you get to some volume, just because it's easier to stock.

Sure, on a thin prepreg in a multilayer stackup, you need to behave - no solid plane one side, sparse tracks the other, but OP is asking about 2 layer, where you can get away with pretty much anything. Still flood it with ground and stitch it together, though. It's one of those things that's cheap, easy, and good.

I don't know what the specific "rules" are but I've had a factory complain about a ~100x80mm board or or so with 2-layers and 1.6mm board where the bottom was ground and there was no fill on top and quite few tracks.

[DerekG]

I've had a factory complain about a ~100x80mm board or or so with 2-layers and 1.6mm board where the bottom was ground and there was no fill on top and quite few tracks.

The factory is complaining because they don't want to etch away any more copper than they really have to.

Etching away more copper uses more etchant & results in more copper in solution. Copper is a heavy metal & most health departments insist on it being removed before any waste solutions are disposed of.

This all costs money.

[alank2]

Is there any reason one would want a board with only tracks present and an excessive amount of copper etched away?  If the traces are separated, why would it be necessary or beneficial?

[DerekG]

Is there any reason one would want a board with only tracks present and an excessive amount of copper etched away?  If the traces are separated, why would it be necessary or beneficial?

Leaving much of the unused copper on the board involves an extra step in the design process - placing a polygon plane with appropriate clearances on each signal layer.

Some designers are unsure about how to do this

[DavidMenting]

Is there any reason one would want a board with only tracks present and an excessive amount of copper etched away?  If the traces are separated, why would it be necessary or beneficial?

Laziness, as DerekG said could be one reason, but dealing with clearance for high voltage signals might be another.

Isn't the copper recovered from the etchant? Coppers seems like a too valuable resource to waste.

[DerekG]

Isn't the copper recovered from the etchant?

Yes, but this costs money. Also, 100% of the copper is not removed, often only about 99.6% - then it becomes uneconomic.