What's the purpose of the ground plane?

Go To Last Post
40 posts / 0 new
Author
Message
#1
  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Hi Freaks,

I guess it's a pretty basic question and I tried to understand it by reading http://en.wikipedia.org/wiki/Gro... but I still don't really get it.

The "allowing the designer to ground anything without having to run multiple tracks" part is clear but the others are not so much.

I observed that various PCBs have, but others don't have a ground plane. Also, how usual it is to have a ground plane on one side and a power plane on the other side? What are the benefits? Is it supposed to lessen electrical noise? In what applications is it preferred?

I guess it's a lot of questions but I'm really interested about the answers.

Thanks in advance!

Laci

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Quote:

I observed that various PCBs have, but others don't have a ground plane.

Some PCBs have more than two layers, the additional ones being internal, and one of them might be a ground plane.

As of January 15, 2018, Site fix-up work has begun! Now do your part and report any bugs or deficiencies here

No guarantees, but if we don't report problems they won't get much of  a chance to be fixed! Details/discussions at link given just above.

 

"Some questions have no answers."[C Baird] "There comes a point where the spoon-feeding has to stop and the independent thinking has to start." [C Lawson] "There are always ways to disagree, without being disagreeable."[E Weddington] "Words represent concepts. Use the wrong words, communicate the wrong concept." [J Morin] "Persistence only goes so far if you set yourself up for failure." [Kartman]

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Google pcb ground plane design

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Well, that wikipedia article looks like a very good summary of how I'd like to explain ground planes, to be honest.

The theory can be however advanced you wish - it's explainable using electrical fields and how these cause potential shifts (what's popularly known as "voltage difference") - or if it's the other way around... That requires some serious studies in advanced math, so I won't go in to it. I'll give you an easier example though:

What happens is a current flows from a power source (let's say it's at 5V), through the Vcc traces on the board, does some "work" in an IC, and returns in the Gnd traces to the power source. Roughly.
Now, these traces are not ideal (they're not superconductors), so they have a resistance. It's low, but it's there. If you're using small traces, say it's 0.1 Ohms. The IC draws 100 mA of current, which causes a voltage drop across the traces of 10 mV (U = R * I), which means that the Vcc input to the IC is at 4.99V, and the ground is at 0.01V, relative to the power supply's ground. Not that bad? Well, possibly it is, especially the ground not being at 0V.
Imagine if it's an AD converter with high resolution. Say 16 bits across the 5V spectrum - that gives that the LSB is "worth" roughly 76 µV. Now, the input to the AD converter doesn't draw much current (certainly shouldn't draw more than a few dozen µA), so the voltage drop along that trace is much smaller. Let's ignore it for now.
What this in effect means is that any voltage that's applied to the AD input that is below 0.01V won't be registered (the AD can't measure anything below its ground reference potential), effectively invalidating what should be the lowest 131 values (if I did my math right), and causing an offset for every value above this of 131. In audio, that's a problem.

Adding in a ground plane should lower the return resistance significantly, alleviating this problem. It makes the ground that's seen across the PCB closer to the power source's ground, which is all together a good thing.

Ground planes do other things too, such as noise shielding (both in and out), and usually make manufacturers happier - they have to get rid of less copper, which means a more stable board for you.

Edit: As Guillem Planisi and others have pointed out further on in the discussion, one of the largest problems that can be alleviated with a ground plane is not the DC voltage dips I described, but rather intermittent voltage changes caused by switching currents, mainly from CMOS-based chips (which is most all of today's µC's). However, I felt it easier to explain using a static DC case with resistances, something most people should be familiar with, rather than the intermittent and complex nature of spikes. You can calculate these as well, but it quickly gets very, very complicated. What you need to do to take care of these problems is still a good ground plane, but here decoupling caps become a major factor too. That's another discussion for another time.

Last Edited: Tue. Aug 31, 2010 - 11:00 AM
  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Thanks, a very useful information

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Yes, I also say thanks for TrainzStoffe for the detailed explanation.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

One last question: Is it considered a good practice to put the ground plane to one side and put the power plane to the other side?

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

You mean copper pour, presumably, rather than planes. It won't do any harm, but there isn't much point to it.

Leon Heller G1HSM

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

I didn't mean for the planes to occupy the whole sides, of course. That wouldn't make much sense.

Wouldn't putting the power plane to one side make routing VCC tracks easier?

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

It might help, in the same way that it often helps with ground connections. I just thought of a possible problem - it might be difficult to avoid unwanted circulating currents which might be bad from an EMC point of view. With tracks you know where they are, but predicting them with copper areas is rather difficult.

Leon Heller G1HSM

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Although this probably falls into the TMI realm, another reason for both power planes and ground planes is that in circuits everything is a transmission line. Ideally, your power delivery should have the lowest transmission line impedance possible. In more pragmatic terms, from the component to the voltage source you want to minimize series R, series L and maximize parallel C. The use of planes does all of those things.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Thanks for the valuable insights, guys! The explanation of tomwwolf is encouraging but the possible problem that leon_heller mentions is discouraging. I'm not really sure whether it's a good idea to use a power plane.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Well as an additional note, by making either the power or ground a plane (convention prefers ground), you reduce the series R and L for that side of power distribution. The the parallel C can be cheated through the use of high quality ceramics close to the devices. I am fond of the 0.1uf ceramics all over the place.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

I have had good experience avoiding Vcc planes. It is desirable to have some impedance to decouple the various loads, and let the very close bypass capacitor supply the peak current. This minimizes loop area. Having copper pours over large areas can act as antenna and couple or radiate noise. I learned this working with very experienced EMC engineers that spent their careers evaluating products in an EMC lab.

It all starts with a mental vision.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Thanks KitCarlson! I think I won't use a power plane then.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

"Dare to be naïve." - Buckminster Fuller

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Quote:
everything is a transmission line

Not up to a certain frequency, you don't have to regard a trace that carries a signal with 10us rise/fall times as being a transmission line.

I once read in a (internal) Philips appnote that solid VCC planes can create horrendous resonances all over the place.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Layout rules get trickier as freq goes up. Double sided boards with plate thru holes work up to about 33mhz, then the pulses start bouncing off the vias, which are a little bump in the road. The higher the freq, the less Rs, Ls and Cs look like ideal components. Somewhere up there, every component has some R, some L and some C. I think minimizing the ground impedance is the main reason almost EVERY rf board I've seen has a big ground plane.

Imagecraft compiler user

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

How about putting one ground plane for the top side and one for the bottom side? Are two sides better than one side?

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

If you read the Amatuer Radio Relay League handbook, it describes always using a ground plane when using multiple antennas to get directional aiming, and dimensions of ground plane must have something to do with wavelength.

Imagecraft compiler user

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

We can go on talking in general terms, but what might be good for one application might be bad for another. What sort of circuitry are we talking about? 1GHz CPU and ddr400 ram? Or a 8MHz AVR? What is the expected environment and required compliance?

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Kartman: It's 16Mhz AVR. Nothing specific, I'm curious about it in general.

Currently I'm rather interested whether it makes sense to use two ground planes.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

It does when you use a six layer PCB.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

a few years back when i was working on some L-Band RF boards we were doing 8 layer boards, and that had ground plane cladding on both external layers - but that board was about 20x of a 2 layer board. Which is why most commercial boards are 2 layers. I was working at a defense contractor at the time.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

I can see your reasoning regarding multi-layer boards, guys, but regarding 2 layer boards I guess two ground planes cannot hurt since the manufacturer has to remove less copper. I'd be interested how usual this practice is, though.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Are the manufacturers using a subtractive method for copper?

I thought they normally used additive, while subtractive was a hobby thing...

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

krazatchu wrote:
Are the manufacturers using a subtractive method for copper?

I thought they normally used additive, while subtractive was a hobby thing...

Maybe we are confusing terms. By subtractive, most people understand the removal of copper from an inital complete layer of copper by etching, or milling, thus producing circuit defined tracks of copper. I have never heard of any manufacturer laying down copper traces on the insulating substrate ... except for printing conductive inks. Happy to be educated.

Cheers,

Ross

Ross McKenzie ValuSoft Melbourne Australia

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

He means the photographic process. That can be negative (exposed = copper removed) or positive (e.g. exposed = copper).

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

jayjay1974 wrote:
He means the photographic process. That can be negative (exposed = copper removed) or positive (e.g. exposed = copper).
Really? OK I stand corrected.

Cheers,

Ross

Ross McKenzie ValuSoft Melbourne Australia

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Pouring ground on both bottom and top won't hurt, and it's (apparently) preferable from an EMC view, rather than pouring power on one side. Having power pour will create a nice little C through the board to the ground plane, but then again, it won't matter until you're way, way up there in frequency, and by then we're most likely talking 4-layer boards anyway, where it'll come naturally.

With a 16 MHz AVR, you don't need to worry at all. Anything you do will most likely work just fine for prototype or hobby work. EMC compliance will require some thought. But I've seen horrible boards with ground and power on thin traces, and a copper pour from one of the signal layers, and the circuit still worked without issue.

And re: additive/subtractive vs. negative/positive: It's ambiguous, isn't it? I had the same reaction as Ross did. :)

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

TrainzStoffe: Yeah, I think it's a good practice to pour ground on both sides even if the low-frequency doesn't justify it.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

I hate ground pours all over the board, it makes following the traces more difficult and I don't like the look. I even more hate it when there are big gaps that could easily have been avoided by rerouting a single trace :) On on the other hand I like it when traces are laid out as big planes.

It's important to stitch copper islands to ground, and the last thing you want is a big plane of copper connected to ground with only one via. This will make an excellent antenna. Both in and out.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

jayjay1974: I've just checked the PCBs of a number of consumer electronics devices and they all have copper traces. I don't know whether it's ground, power or netral but they're everywhere. I wonder 1) what they are (ground vs power vs neutral) in most of the cases and 2) whether they're laid down because economical or EMC reasons.

Regarding connecting the copper islands, it's an interesting issue which I haven't think about. Should they be connected in a matrix wherever possible? If so, how much space should be placed between rows / columns?

Also, what about neutral planes / copper pours?

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

"Dare to be naïve." - Buckminster Fuller

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

It's not just the frequency you're working at. It's the edges that matter, and these can be as sharp at 1kHz as 100MHz. If you are - say - using an address latch for external memory, it latches on the rising edge of ALE and with a fast latch this can put a large, rapid transient current in the ground pin of the latch. What happens next is dependent not so much on the DC resistance of the ground trace, as its inductance. With quite a modest inductance, in the nanohenries, and a fast transient in the nanoseconds, you may see a bounce of several volts, enough to upset the internal logic of the latch, or indeed to other chips that share the ground path. Generally this will be an intermittent problem, dependent on the data pattern, and very difficult to trouble-shoot. Using a ground plane with wide, multiple paths to the ground pin reduces the inductance by orders of magnitude and makes such problems go away. It's less important to plane the Vcc because signal levels are generally referenced to ground, so sudden dips in Vcc are less catastrophic, but nevertheless it's good practice to "net" the Vcc and provide multiple paths so that no devices are hanging on the end of a long slender trace.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Just as a side note, the return current on the GND line that TrainzStoffe had pointed out has another big issue: CMOS digital circuitry. Those little IC's don't have a high consumption on the DC side, but they tend to consume huge amounts of current each time they switch state. That generates lots of current spikes on the power lines, that can generate 'ground bouncing' unless they are under control. Exactly as Peret had explained.

The usual and easier way to do that is using lots of decoupling caps as close to the supply as possible, and prioritizing the GND line to reduce impedance. Xilinx has some good app notes regarding this issue with the quite difficult to bypass FPGA's.

Regarding power and gnd planes, I tend to flood all my 2-sided boards with GND only, leaving VCC or other power planes for 4 layer boards, where I use the internal layers as a solid (or moated, depending on the circuit topology) GND plane, and the other one as power distribution, as solid as possible, in order to have maximum parasitic capacitance. Then I flood the other outer layers with the opposite kind of plane than the closest one. Using this technique I never had problems with EMC.

Guillem.
"Common sense is the least common of the senses" Anonymous.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Naturally, the spiky CMOS current draw will pose the largest problem for the ground plane on PCB's, however I felt it more complicated to explain. With simple resistance and voltage drop you have easy to follow calculations - with switching currents there's nothing tangiable that people have approached before. In retrospect I should've added a notice about this to my post - I'll go back and edit it.

@peret - You're of course correct, it's the edge frequency content that's important, not the switching frequency itself. The two are usually somewhat correlated though. If you have 100 MHz-compatible rise and fall times (at 100 MHz, one period is 10 ns, which means the edge times should be on the order of a single ns) on circuits running much slower, it's usually a good idea to somehow slow down the edges. There are multiple ways to do this - lowering the line drive strength if possible, adding in series resistance on the line, parallell resistance, series inductance, or parallell capacitance. They'll all do the job, each with their pros and cons.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Most FPGAs, and some MCUs and other assorted ICs, have programmable output driver strength (sometimes in multiple steps, sometimes just normal and reduced/'Low EMI mode').

It's nice to see on a scope how ringing after edges becomes less and less as you decrease driver strength. To a point that the circuit does not work any more and you need to increase it again. This way you can select the most appropriate and optimal strength.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Only problem with watching on a scope is that you're putting a load on the line, which may or may not be significant... I.e. it'll work when the scope's there, but once you remove it?
There's no real way around it, but you just have to be aware of it.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Hi,

mondalaci wrote:
How about putting one ground plane for the top side and one for the bottom side? Are two sides better than one side?

This is what I do.

I consider the bottom ground pour to be my "main ground pour" and I do everything I can not to cut it with traces. If I have to I do, but I make every effort to leave the bottom as nearly continuous as possible.

I run my VCC traces on the top using a heavier track (40 or 50 mils) and then run all my other traces on top if possible. If I have to run one on the bottom, I make it as short as possible and so that it cuts the ground pour as little as possible, even if it means a longer trace or extra via's.

I finally do a ground pour on top which fills the areas it can get to with ground as well. Having two ground pours means less copper is removed from the board. Better heat transfer, stronger, less copper to etch away for the pcb manufacturer, and more grounding.

Good luck,

Alan