Copper Pour for Low Noise Low Interference? or Not? - Page 1
Forum section: electronics / beginners

author: Mechatrommer
author_rank: Super Contributor
timestamp: December 23, 2023, 10:45:45 am
content: i still get my head around this it seems... some writings that i've read stating copper pour is almost always good practice but... most circuits for high speed and low noise i've seen just omitted this advice, WHY? please dont confuse i'm not talking about ground plane which should be there and solid... i'm talking about empty spaces between signal traces on outer layers...here is one example (from random google result) that advice for copper pour..https://zahidmehmood-40074.medium.com/the-importance-of-copper-pour-in-empty-areas-on-pcbs-202d8ba0ceafbut some pictures i can grab from here and there are not using copper pour, this is confusing as to why?...

author: MarkT
author_rank: Frequent Contributor
timestamp: December 23, 2023, 10:50:30 am
content: If its a 4-layer or more PCB, there is commonly a ground plane just under the top layer, so normally there's no need for a groundplane on the top copper.

author: Mechatrommer
author_rank: Super Contributor
timestamp: December 23, 2023, 10:56:06 am
content: Quote from: MarkT on December 23, 2023, 10:50:30 amhow about 2 or more adjacent traces? wouldn't adding copper pour on their sides reduce or improve crosstalk/noise? besides the existing ground plane underneath... esp in tight space where we cant make both traces far apart.

author: eleguy
author_rank: Regular Contributor
timestamp: December 23, 2023, 10:57:06 am
content: In short watch from ~40minutes ->but... copper "pour" can make things better IF you know what you are doing with the stitching for example. Otherwise just dont...And the longer story... Bogatin's book "Signal and Power Integrity - Simplified" is something I can recommend to all to read.

author: MarkT
author_rank: Frequent Contributor
timestamp: December 23, 2023, 11:24:23 am
content: Quote from: Mechatrommer on December 23, 2023, 10:56:06 amWell its a factor, but typically stackups have the ground plane v. close to the top layer to improve shielding like this and allow thinner traces for controlled impedance runs. If space is tight you can't fit a top layer copper pour anyway!

author: Mechatrommer
author_rank: Super Contributor
timestamp: December 23, 2023, 11:48:46 am
content: Quote from: eleguy on December 23, 2023, 10:57:06 amsome of his conclusion is imho questionable. (see attached) dave demo'ed some years ago that paralleling few decoupling capacitors could improve impedance profile. and both videos agree copper pour between traces could improve crosstalk by some percent if properly stitched.Quote from: MarkT on December 23, 2023, 11:24:23 amyou are right, i mean it could improve crosstalk with the other traces few mm away...why i ask this is my recent pcb got 10mVpp 700kHz digital "ghost" cross talk problem amplified by 30x gain opamp. maybe i have mistake somewhere not relating to copper pour, in fact i didnt use any copper pour around it. maybe i run signal trace too close / underneath an insulting smd components (power rail decoupling cap) but i cant be sure since i cant pinpoint the origin of the insulting signal, as if the signal is not coming from my board (daughter board mounted on larger mother pcb). so i run into phobia mode to guard my signal with copper pour and via stitches everywhere, of course routing away from suspicious insulting components etc. but at least the videos linked above could still prove via stitches and copper pour could improve crosstalk/EMI... maybe i should not unlearn yet what i've learnt. just avoid "floating" copper or "end to end only" via termination, heck who's going to do that resonant cavity? when vias are free from fab house today...

author: T3sl4co1l
author_rank: Super Contributor
timestamp: December 23, 2023, 01:06:09 pm
content: Surface pour makes very little difference. Consider the coupling factor between adjacent traces, which is also  the coupling to ground for CPWG (microstrip with ground poured on top). Edge coupling is small, maybe up to 10% at minimum design rules.The small advantage is worthwhile for some applications, or perhaps the overall improvement in ground plane impedance (when well stitched; gives higher isolation, or for low impedance applications e.g. SMPS). But for almost everything (i.e., any generic embedded commercial product), simple inner planes suffices.Tim

author: David Hess
author_rank: Super Contributor
timestamp: December 25, 2023, 12:24:00 am
content: Quote from: Mechatrommer on December 23, 2023, 10:45:45 amIf there is a ground plane, then that provides enough coupling in almost all cases. Adding a pour on the signal layer typically makes things worse unless it is stitched to the ground plane to make a coplanar waveguide, and to what purpose? If you make your impedance targets with a microstrip, then you make them. Coplanar waveguides are used sometimes instead of microstripsFor high impedance high speed circuits, the ground plane is cut away to reduce capacitance. Here adding a fill just adds the capacitance back so there is no reason to use it.In most cases adding an unconnected fill makes things worse, for a broad range of "things".

author: Mechatrommer
author_rank: Super Contributor
timestamp: December 25, 2023, 05:51:55 pm
content: Quote from: David Hess on December 25, 2023, 12:24:00 amlets just assume for the topic's sake thats nobody is doing this idea. it also mentioned in the videos linked earlier... thinking about it, the pro (ground connectedsignal layer pour) maybe:1) save echant cost in fab house in exchange to higher drill bit cost for stitching vias.2) if nasty EMI from outside exist, outer layer pour may absorb it first and somewhat shield traces next to them?3) my pcb will be mechanically stronger4) lower gnd plane impedance due to more path for current to get back to the source. and its cooler too.5) lower impedance (thicker gnd) will absorb more smps current spikes, crosstalk / EMI..6) in case i want to add experiment or circuit on my prototype board, i can cut and mask scratch islands on the pour to attach my add-on circuit/components.for whatever reason to do it, i mean why not?

author: uer166
author_rank: Super Contributor
timestamp: December 26, 2023, 10:22:05 am
content: Quote from: Mechatrommer on December 25, 2023, 05:51:55 pmNone of these provide any tangible improvement except maybe point #6, but if adding the pour makes you feel better, then why not.. Btw, copper does not "absorb" EMI, unlike say lossy ferrite.

author: Smokey
author_rank: Super Contributor
timestamp: December 26, 2023, 10:45:55 am
content: Based on my extensive youtube research... I'm pretty sure the main issue with unnecessary pours is resonances. You are creating a cavity between the pour and the plane that will have some resonant frequency. If you are careful to terminate the pour correctly (every 1/10th the shortest wavelength) then it not only probably won't cause problems, but it's the lowest noise option. But if you don't terminate it correctly it will cause resonance issues.So there is a slight upside if you get it right and a huge downside if you get it wrong, and you have to intentionally not get it wrong. That's the impression I get at least.

author: tszaboo
author_rank: Super Contributor
timestamp: December 26, 2023, 11:02:44 am
content: Top and bottom layer pour enhances the PCB thermally. It enables me to use CPW instead of microstrip. It increases the capacitance between the power plane and ground, which is good for high frequency. And it's free. I do it just because the first reason by default, it's a safety thing in my designs.

author: radiolistener
author_rank: Super Contributor
timestamp: December 26, 2023, 11:28:35 am
content: Quote from: Mechatrommer on December 25, 2023, 05:51:55 pmIf there is EMI, it's better to shield it with proper metal enclosure. Layers on PCB is a bad shield due to capacitive coupling.If you put metal surface close to very high frequency circuit it can lead to ringing issues, so using unnecessary metal surfaces in sensitive circuit which works with very high frequency is a bad idea. Especially if it don't use many vias to the ground layer. Such structure can work like waveguide or resonator and it leads to a bad results...It might also be a bad idea to cover the transmission lines with varnish or paint, because it's properties is not stable and it can affect transmission line impedance in random way. This is why transmission lines often are not covered with mask and are not covered with solder and you can see raw copper wires on PCB.

author: David Hess
author_rank: Super Contributor
timestamp: December 26, 2023, 03:01:13 pm
content: Quote from: Mechatrommer on December 25, 2023, 05:51:55 pmQuote from: Smokey on December 26, 2023, 10:45:55 amThere are all kinds of mechanical reasons to leave the fill, including to prevent the board from warping.In my experience the problem is that an unconnected fill increases capacitive coupling to adjacent circuits and the environment. In the later case, it acts as a big capacitor plate and couples to adjacent circuits.If the fill is connected to ground, then it acts as a shield, but then it increases capacitance to ground which may or may not be a problem as I described above.QuoteSmall isolated pads do not create as much coupling; all of the capacitors are essentially in series. And this type of fill is often found on circuit boards to reduce etching and increase mechanical strength.

author: Terry Bites
author_rank: Super Contributor
timestamp: January 12, 2024, 04:29:36 pm
content: Just chucking in a groundplane may or may not help. Component placement and routing will scupper any benefits if you don't consider them carefully.