Take the 2-minute tour ×
Electrical Engineering Stack Exchange is a question and answer site for electronics and electrical engineering professionals, students, and enthusiasts. It's 100% free, no registration required.

I've seen many 2-layer PCBs that have a ground pour on both the top and bottom layers, I was wondering why do that ? and wouldn't it be better to use the top layer for power and signals and the bottom layer for ground to simplify the routing and also taking advantage of the capacitance between the planes ?

share|improve this question
    
This isn't so much an answer, but I'd propose that the reason most people do it is simply because they think it's good, that it would otherwise be wasted space, etc. You can free connections to ground assuming there is at least one via connecting to your bottom ground plane or if the top layer can hit the pad for a through-hole pin that happens to be ground. .. or as Olin said... religion takes a foothold. :) –  Toby Lawrence Sep 23 '12 at 15:14
    
yes, I couldn't think of a good reason for that either, if it was a power plane well then maybe the capacitance, but what good is a couple of ground layers ? especially that the top one is most likely to be chopped up badly, with all the components on top, so I thought I'd ask :) –  mux Sep 23 '12 at 15:24
2  
One good reason for planes on both sides is to keep the amount of copper on each side of the PCB about equal. If one side has much more copper than the other then the PCB will be more prone to warping. This is one reason why multilayer PCB's are often symmetrical on their layer stackup. The exact risk of warping is not clear to me however, but I have had PCB companies comment when I haven't done it quite right. –  user3624 Sep 23 '12 at 16:05
    
In addition to what David said, tour board shop likes to have a maximum amount of copper on every layer, because it minimizes the rate of using up etchant. If your volumes are not extremely high, though, it doesn't really make sense for you as the designer to worry about this. –  The Photon Sep 23 '12 at 22:57
add comment

2 Answers

up vote 7 down vote accepted

Good layout and grounding seems to be poorly understood out there so religion finds a foothold. You are right, there is really very little reason to use both the top and bottom of a two layer board for ground.

What I usually do for two layer boards is to put as much of the interconnects as possible on the top layer. This is where the pins of the parts are already anyway, so is the logical layer to use to connect them. Unfortunately you usually can't route everything on a single layer. Paying attention and thinking carefully about part placement will help with this, but in the general case it is not possible to route everything in one plane. I then use the bottom plane for short "jumpers" only when needed to make the routing work. The bottom plane is otherwise ground.

The trick is to keep these jumpers on the bottom layer short and not abutting each other. The metric of how good a ground plane is left over is the maximum linear dimension of a hole, not the number of holes. A bunch of short 200 mil traces scattered about won't keep the ground plane from doing its job. However, the same number of 200 mil traces clumped together to make one island a inch accross is a much bigger disruption. Basically, you want the ground to flow around all the little disruptions.

Set the auto router cost for the bottom layer high and don't penalize it much for vias. This will automatically put most of the interconnects on the top layer. Unfortunately, the auto-router algorithms I have seen can't seem to be tweaked for not clumping the jumpers. In Eagle, for example, there is the hugging parameter. Even if you turn this off, you still get clumped jumpers. Let the auto router do the grunt work, then you clean things up afterwards. Sometimes you can spot a case where a little re-arrangement can eliminate a jumper altogether. Most of your time, however, will be spent moving the jumpers apart to not make large islands.

As for power planes, that's mostly silly religion. Route the power just like any other signal, although in this case you have to consider the voltage drop due to the trace resistance, since power traces presumably handle significant current. Fortunately even 1 oz copper traces on a PCB are quite low resistance. You can make the power traces 20 mil or whatever instead of 8 mils for signal traces. In any case, the point is that the DC resistance matters but it is usually not much of a issue unless you have a high current design.

The AC impedance isn't all that relevant, which the religious folks don't seem to get. This is because the power feed is locally bypassed to the ground plane at each point of use. If you have a good ground plane, you don't need separate power planes for most ordinary designs, just good bypassing at each power lead of each part. The bypass cap connects directly between the power and ground pins, then there is a via right at the ground pin to connect to the ground plane on the bottom layer.

The high frequency power loop current of a part should go out the power pin, thru the bypass cap, and back in to the ground pin without ever running accross the ground plane. This means you don't use a separate via for the ground side of the bypass cap. Connect it directly to the ground pin on the top side, then connect that net to the ground plane with a via at a single point. This technique will help a lot with RF emissions and cleanliness in general.

share|improve this answer
    
This is a great answer, thank you sir, so, if I understand correctly, especially from the last paragraph, I shouldn't use a pour on the top layer at all, correct ? it is useless ? also, should I use short jumpers on the bottom layer, even if it means that some signals won't take the most direct route ? –  mux Sep 23 '12 at 15:00
    
@mux: Yes for most cases. Exceptions are special high speed signals, signals that must be impedance controlled, signals that must be delay-matched, etc. However, you don't generally find these on a 2 layer board. These usually imply other expenses such that going to 4 or more layers is a minor additional cost. –  Olin Lathrop Sep 23 '12 at 15:33
    
@OlinLathrop I really don't get it. Yes, the decoupling caps give a very low impedance path, already. Let's say we neglect all the inductances of all the traces. Then we only left with sudden current demands by the (let's say) IC. OK, decoupling cap will give that. But, how and thru where that decoupling cap will recharge, for the next sudden current demand? Will it have time to recharge? I am really confused. –  abdullah kahraman Sep 23 '12 at 16:19
    
@OlinLathrop I'm a little confused about your last paragraph. The bypass cap has its GND pin going directly into the GND pin of the IC. Then I've always taken the GND pin of the cap and drawn another trace going the other direction (typically away from the IC) which connects through a via to the GND plane on the bottom. Is that what you mean by connect that net to the ground plane with a via at a single point? It should be on the other side of the cap from the IC correct? –  NickHalden Sep 23 '12 at 17:15
1  
@abdullahkahraman: That's where having multiple caps can come in, a small one that can handle the higher frequencies of the spikes and a larger one that can handle the lower frequencies . Being nearby the larger one can also recharge the small one faster than it could be by the voltage supply. –  Nemo157 Sep 27 '12 at 21:37
show 4 more comments

Having a power plane on the top and ground at the bottom would hardly give any capacitance.

\$ C = k \cdot \epsilon_0 \cdot A / d \$

where k is relative permittivity, about 4.5 for FR4, \$\epsilon_0\$ is permittivity of empty space, 8.85 pF/m, \$A\$ is area in square meter, and \$d\$ is distance also in meter. A Eurocard size PCB is 160 mm \$\times\$ 100 mm, at 1.6 mm thickness that's

\$ C = 4.5 \cdot 8.85 pF/m \cdot 0.016 m^2 / 0.0016 m = 400 pF \$

Decoupling capacitors will give you a lot more. Also, properly decoupled it doesn't matter whether you use ground or power for the copper pours; for HF they should be the same. Usually ground is chosen because that net will have the most connections, and it will be easier to connect the different isolated copper pours at the top to the copper pour at the other side.

share|improve this answer
1  
Yes, but that 400 pF can be pretty significant at the highest frequencies that need to be decoupled -- e.g., 4 ohms impedance at 100 MHz -- and this capacitance has the least amount of series resistance and inductance associated with it. Very important in very high-speed designs, but if you're doing that kind of work, then you're probably using more than two layers and less spacing between the planes. –  Dave Tweed Sep 23 '12 at 14:11
    
@Dave - agreed, but the 400 pF is for a PCB consisting of just the copper pours. Routing though it will significantly decrease the area, and the connections between islands will have their inductance too. For HF I would go for a 4-layer and use the inner layers for ground and power planes. Distance will be lower = higher capacitance and there won't be that much cuts though them. –  stevenvh Sep 23 '12 at 14:25
    
so the capacitance is insignificant, at least for a 2-layer PCB, so other than having many ground connections, there's really no good reason for using a ground pour on the top layer ? correct ? –  mux Sep 23 '12 at 15:15
    
@mux - Not really: you want to cut as little as possible through the bottom layer ground plane, which means all the routing on the top layer will leave too little of the ground plane there. OTOH, placing a copper pour there won't hurt, and if it's also ground you can connect isolated islands through vias. If the top copper pour is Vcc connecting the islands may be more difficult, and may make less sense. But Dave doesn't completely agree, I'm afraid :-). –  stevenvh Sep 23 '12 at 15:22
    
@DaveTweed Keep in mind that the 400 pF number that Stevenvh mentions is for the entire 160x100mm PCB. I would hope that the high frequency return paths for any given signal does not actually "go through" the entire PCB and so you can't really benefit from the entire 400 pF. –  user3624 Sep 23 '12 at 16:12
show 4 more comments

Your Answer

 
discard

By posting your answer, you agree to the privacy policy and terms of service.

Not the answer you're looking for? Browse other questions tagged or ask your own question.