Author Topic: Ground plane AND ground pour?  (Read 2900 times)

0 Members and 1 Guest are viewing this topic.

Offline SoftwareSamurai

  • Regular Contributor
  • *
  • Posts: 170
  • Country: us
Ground plane AND ground pour?
« on: March 18, 2012, 04:03:33 AM »
Let's say I have a common 4 layer board:

1. Signal(s) + components.
2. Full solid copper pour - ground plane.
3. Full solid copper pour - power plane.
4. Signal(s)

Generally speaking, does it help to add a ground pour on the outer layers after signal traces have been drawn out?

Offline w2aew

  • Super Contributor
  • ***
  • Posts: 1041
  • Country: us
  • I usTa cuDnt speL enjinere, noW I aR wuN
    • My YouTube Channel
Re: Ground plane AND ground pour?
« Reply #1 on: March 18, 2012, 04:13:51 AM »
It sure helps alot for debug - giving you easy access to ground to connect your scope probe, DMM, or even for popping on decoupling caps etc. - just in case the circuit needs tweaking.
======================================
YouTube channel: http://www.youtube.com/w2aew

Offline jahonen

  • Frequent Contributor
  • **
  • Posts: 987
  • Country: fi
Re: Ground plane AND ground pour?
« Reply #2 on: March 18, 2012, 04:21:26 AM »
If you do those fills, remember to put a lot of stitching vias into it (I wonder why there isn't a "spray tool" of adjustable density in PCB CAD software to place those vias while taking a care of design rules :P), to tightly connect those fills into main ground plane. Take care that there is no long slivers on the fill, they might be harmful.

Regards,
Janne

Offline SoftwareSamurai

  • Regular Contributor
  • *
  • Posts: 170
  • Country: us
Re: Ground plane AND ground pour?
« Reply #3 on: March 18, 2012, 11:58:53 AM »
I was just wondering if adding ground pours (and additional vias to stitch them to the ground plane) would help with the signal return, and reduce overall ground noise, or possibly reduce unwanted EMI/crosstalk on the board. I haven't read anything yet that says adding ground pours helps, but I'm guessing it couldn't hurt, right?

Offline jerry507

  • Regular Contributor
  • *
  • Posts: 231
Re: Ground plane AND ground pour?
« Reply #4 on: March 18, 2012, 01:09:52 PM »
There may be some advantage to it in very sensitive applications, but honestly, it's not critical. The whole point of a ground plane is to provide a return path of low inductance. When current flows in a trace and you have a ground plane under it, the current will prefer to return directly under the trace. This is because it is the path of lowest inductance. There are some simple experiments with iron shavings that can demonstrate that current will ignore the path of lowest resistance and instead follow the lowest inductance. I'm sure you can find Youtube videos. So no, I'd say that there isn't really a point in pouring ground on the top. In reality, when you have both a power and ground plane internally and you're only using 4 layers, there is no point in pours on the top and bottom. Does it hurt? No. Just doesn't really add a lot.

Offline SoftwareSamurai

  • Regular Contributor
  • *
  • Posts: 170
  • Country: us
Re: Ground plane AND ground pour?
« Reply #5 on: March 18, 2012, 01:26:24 PM »
Thanks Jerry, that does make sense.
The reason I asked is because I did read in a book recently that having a ground pour between two signal lines (not differential lines) helps reduce crosstalk between them. So that lead me into wondering if it, generally speaking, it would just be a good idea to always to a ground pour on the signal (outer) layers.

Offline dfnr2

  • Regular Contributor
  • *
  • Posts: 194
  • Country: us
Re: Ground plane AND ground pour?
« Reply #6 on: March 18, 2012, 06:51:03 PM »
I was just wondering if adding ground pours (and additional vias to stitch them to the ground plane) would help with the signal return, and reduce overall ground noise, or possibly reduce unwanted EMI/crosstalk on the board. I haven't read anything yet that says adding ground pours helps, but I'm guessing it couldn't hurt, right?

Not really, since it's up against a ground or power plane, and there are no signals traveling over or under the pour.  In order for the ground to help, it has to follow the entire length of an overlying or underlying trace.  On a four layer stackup, the adjacent ground or power plane is only about 10 mil or less down.  For a two layer stackup, it's 60 mil down.  So, perhaps for a sensitive or noisy signal, routing a ground plane or trace right along side the signal could significantly reduce the loop size still.

Following your stackup, a ground pour on the bottom may increase capacitance between power and ground, even with smaller area, because of the closer proximity (~10 mil, vs ~40 mil between power and ground planes.) , which is desirable.  It will also add capacitance between ground and your signals, which may be desirable under some circumstances, but will be undesirable for high-speed signals.

Sometimes, on a four layer board, if I'm not routing many traces on the bottom, I'll use pours on the bottom plane for power, and then make both internal planes ground planes, tightly stitched.  This gives tighter loop areas for top and bottom traces.  In that case, I'll make sure to place a ground-stitch via right next to any vias where a signal trace switches from top to bottom layer or vice versa.  If you are using the more common sig-gnd-pwr-sig stackup, then put a capacitor somewhere close to the signal vias, to stitch the gnd and 5V planes at high frequencies, providing a high-frequency signal return path that follows the signal from GND to PWR planes.

Dave

Offline SoftwareSamurai

  • Regular Contributor
  • *
  • Posts: 170
  • Country: us
Re: Ground plane AND ground pour?
« Reply #7 on: March 19, 2012, 12:31:29 AM »
Sometimes, on a four layer board, if I'm not routing many traces on the bottom, I'll use pours on the bottom plane for power, and then make both internal planes ground planes, tightly stitched.
By that you mean you add a uniform grid array of internal uVias to stitch the two internal ground planes together?

In that case, I'll make sure to place a ground-stitch via right next to any vias where a signal trace switches from top to bottom layer or vice versa.
Ah, interesting idea. I think I've seen that technique described somewhere but I didn't fully understand the reasoning until now. Is there a recommended minimum spacing distance between the vias, or is "as close as can be manufactured" the best in this case?

If you are using the more common sig-gnd-pwr-sig stackup, then put a capacitor somewhere close to the signal vias, to stitch the gnd and 5V planes at high frequencies, providing a high-frequency signal return path that follows the signal from GND to PWR planes.
I see. Would it be overkill to put such a power dcap next to every signal via?

Offline Neilm

  • Frequent Contributor
  • **
  • Posts: 893
  • Country: gb
Re: Ground plane AND ground pour?
« Reply #8 on: March 19, 2012, 05:26:22 AM »
I was just wondering if adding ground pours (and additional vias to stitch them to the ground plane) would help with the signal return, and reduce overall ground noise, or possibly reduce unwanted EMI/crosstalk on the board. I haven't read anything yet that says adding ground pours helps, but I'm guessing it couldn't hurt, right?

If you are not careful the gap between the copper pour and the track could end up as a slot antenna that could present problems.

Neil
Two things are infinite: the universe and human stupidity; and I'm not sure about the the universe. - Albert Einstein

Offline jerry507

  • Regular Contributor
  • *
  • Posts: 231
Re: Ground plane AND ground pour?
« Reply #9 on: March 19, 2012, 06:07:03 AM »
Thanks Jerry, that does make sense.
The reason I asked is because I did read in a book recently that having a ground pour between two signal lines (not differential lines) helps reduce crosstalk between them. So that lead me into wondering if it, generally speaking, it would just be a good idea to always to a ground pour on the signal (outer) layers.

Such things are called something like guard pours, guard track, pretty much guard *. I've rarely seen situations that require these, and they are usually cases where you've got a very small signal right next to a higher power AC signal. Think like the current sense signal running very close to motor drive signals. Crosstalk shouldn't be a big issue unless you've got signals with very fast risetimes AND your traces are very close. In many cases, physical separation is more than enough to solve these problems but YMMV.

Offline Neilm

  • Frequent Contributor
  • **
  • Posts: 893
  • Country: gb
Re: Ground plane AND ground pour?
« Reply #10 on: March 19, 2012, 09:18:33 AM »

Such things are called something like guard pours, guard track, pretty much guard *. I've rarely seen situations that require these, and they are usually cases where you've got a very small signal right next to a higher power AC signal. Think like the current sense signal running very close to motor drive signals. Crosstalk shouldn't be a big issue unless you've got signals with very fast risetimes AND your traces are very close. In many cases, physical separation is more than enough to solve these problems but YMMV.

In my experience, guard tracks are used whenever leakage across the PCB could be an issue. For instance, if you are measuring a signal that is only a few nano Amps, then even a 5V track nearby could cause a significant offset.

Neil
Two things are infinite: the universe and human stupidity; and I'm not sure about the the universe. - Albert Einstein

Offline dfnr2

  • Regular Contributor
  • *
  • Posts: 194
  • Country: us
Re: Ground plane AND ground pour?
« Reply #11 on: March 20, 2012, 05:33:54 AM »
Sometimes, on a four layer board, if I'm not routing many traces on the bottom, I'll use pours on the bottom plane for power, and then make both internal planes ground planes, tightly stitched.
By that you mean you add a uniform grid array of internal uVias to stitch the two internal ground planes together?
You have the idea, except that they don't need to be internal or micro, and don't really need to be uniformly spaced, as long as they're a close as reasonalble (1/4 inch average spacing, or density of 16 or more per inch, where signals are passing by).

In that case, I'll make sure to place a ground-stitch via right next to any vias where a signal trace switches from top to bottom layer or vice versa.
Ah, interesting idea. I think I've seen that technique described somewhere but I didn't fully understand the reasoning until now. Is there a recommended minimum spacing distance between the vias, or is "as close as can be manufactured" the best in this case?

I get the impression you do understand the reasoning by now.  The purpose is that the ground return path has a way to jump from one ground plane to the next as close as possible to the signal line, keeping loop area small.  You would want to make the via as close as possible without stressing manufacturing capability, but taking care that you don't choke off the copper connections on the signal via, depending on your via-connection style.  Your DRC will warn you if you are too close, if it's set up properly.
If you are using the more common sig-gnd-pwr-sig stackup, then put a capacitor somewhere close to the signal vias, to stitch the gnd and 5V planes at high frequencies, providing a high-frequency signal return path that follows the signal from GND to PWR planes.
I see. Would it be overkill to put such a power dcap next to every signal via?
That really depends on your application.  For High-end, high reliability, high frequency, high markup applications where you not only really want to pass compliance testing the first time, but also want to be as robust as possible, I'd say it's probably not overkill.  For high-volume, low margin consumer apps, especially on high-density boards where you have lots of bypassing anyway, the already installed bypass caps may provide a small enough path divergence that you will be fine for low frequency signals. The issue there will be more of immunity than of radiation.  If you have adequate filtering or chokes on your low frequency signals, use the slowest spec part that will suit your application (e.g., 74LSxx instead of 74ACTxx; 4 MHz uP instead of 20 MHz), you probably won't have any issues.  But it's good to know about the technique, in case you do have any issues at compliance testing.

If you're making hobby boards or kits, and don't have to worry about compliance, then you can do just focus on the high-frequency or sensitive signals.  In my case, for hobby boards, I'll use 2 layers if everything fits, and do all the tricks I can throw in for free, and worry about high-frequency signals as special cases.  For commercial boards where robustness and reliability are a concern, and price is not, I start with 4 layers as a minimum, and either use the 2-ground layer technique if there's room, or the stackup you listed if there's not, and worry about the immunity of the low-frequency lines as well, put the i/o sections on their own chassis-connected planes, and route all the wires in from those sections via chokes.

Offline dfnr2

  • Regular Contributor
  • *
  • Posts: 194
  • Country: us
Re: Ground plane AND ground pour?
« Reply #12 on: March 20, 2012, 05:42:49 AM »
Thanks Jerry, that does make sense.
The reason I asked is because I did read in a book recently that having a ground pour between two signal lines (not differential lines) helps reduce crosstalk between them. So that lead me into wondering if it, generally speaking, it would just be a good idea to always to a ground pour on the signal (outer) layers.

Such things are called something like guard pours, guard track, pretty much guard *. I've rarely seen situations that require these, and they are usually cases where you've got a very small signal right next to a higher power AC signal. Think like the current sense signal running very close to motor drive signals. Crosstalk shouldn't be a big issue unless you've got signals with very fast risetimes AND your traces are very close. In many cases, physical separation is more than enough to solve these problems but YMMV.
There are some places where it does make sense, and is free, so it's good practice.  For example, for a uP crystal circuit over 4 MHz or so, it's free and easy to place a guard ring.  Also, very low signals, and high precision signals if there are nearby high-frequency traces.

Dave

Offline SoftwareSamurai

  • Regular Contributor
  • *
  • Posts: 170
  • Country: us
Re: Ground plane AND ground pour?
« Reply #13 on: March 20, 2012, 10:47:26 AM »
In that case, I'll make sure to place a ground-stitch via right next to any vias where a signal trace switches from top to bottom layer or vice versa.
Ah, interesting idea. I think I've seen that technique described somewhere but I didn't fully understand the reasoning until now. Is there a recommended minimum spacing distance between the vias, or is "as close as can be manufactured" the best in this case?

I get the impression you do understand the reasoning by now.  The purpose is that the ground return path has a way to jump from one ground plane to the next as close as possible to the signal line, keeping loop area small.  You would want to make the via as close as possible without stressing manufacturing capability, but taking care that you don't choke off the copper connections on the signal via, depending on your via-connection style.  Your DRC will warn you if you are too close, if it's set up properly.
Right, must maintain DRC distance. Got that.

Can you comment on adding, say, two ground vias next to a signal via? I've seen that pattern in some boards where the signal via appears to have two ground vias next to it, forming roughly a 90 degree angle between gnd-sig-gnd vias. Usually the signal trace goes directly away from the two ground vias (not between them). Would that be more for specialized, very high frequency, very small signal propagation? (Talking GHz and above I imagine.)


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf