Hello,
So basically the question. Should I fill the unused space on a 4 layer PCB with outer layers being the signal layers? Should I scatter some GND vias in these fills? If so where?
Thanks!
Yes. It doesnât cost any extra, it is very little effort, and it can only help. Both with high-frequency signal integrity, and with making sure all chips have a solid ground. There is nothing worse than having to debug a chip acting weird because its ground bounces up to where you lose Vil margins. (To quote Opus the penguin: Yes there are things that are worse, like being eaten by a walrus.)
While you are at it: Also make all Vcc traces wider, or connect them to hand-made planes. And put your decoupling caps really close to the chips. On my most recent 2-layer board, I made all ground and power traces at least 20 mil wide, and for the main arteries I try to find room for 40 mil (1mm) traces.
Where should the ground vias go? Wherever there is a solid ground (or Vcc) trace nearby. See above, make those traces wider, and vias are easy to place.
One thing that annoys me a little about KiCad: Sometimes, you end up with an âislandâ on a layer that could be ground filled, but doesnât have a ground trace or pin nearby. To get it filled, you need to manually add a via. Sometimes the only place that extra via can go is in the middle of nowhere, connecting to another fill. No problem, I put the via there. But then the next DRC check complains that the via isnât connected to anything (duh, the DRC is right!). Supposedly there is a way to mark a via as âexempt from connection checkâ, but I havenât found it. So for now I just manually add a ground trace.
1 Like
Depending on your design, if you want to avoid issues with a fragmented power plane and bad routing due to 100s of vias connecting all your seperate ground islands on the outer layers to not build fancy little antennas you can use the âCopper Thiefâ plugin from the plugin manager to fill the empty areas with unconnected patterns to prevent you PCB from bending due to a lack of copper. But as often with electronics, it depends greatly on your design, what performance you want to achieve and what tools you have at hand. And if you ask 5 people you will get most likely 7 different opinions, especially without seeing your layout 
2 Likes
yes you can fill ground pour to have better return path and in terms of solder conductivity it will be helpful
In my opinion it will make return path better in such a small extent that it canât be the argument for pouring.
Return current traveling along internal layer will not âlikeâ to go through vias to ground islands at outer layers to then went back to this internal layer through another via. Not âlikeâ means impedance through vias and island at outer layer is much higher than through continuos internal layer.
You can pour with GND external layers but based on another argument than return current path, I think.
2 Likes
It will improve the return path only if you really know, what you are doing. The ground impedance is for alternating currents the relevant factor, not only the ohmic resistance, and you ground current might take paths you did not foresee. With good decoupling and a single ground plane you will get most likely more predictable results than with two additional fragmented ground planes and a very fragmented power plane due to the many necessary vias.
You can do this, it probably wonât do any harm but if you already have an internal GND plane (of course without any slots and being the first plane below the component side), in my opinion it will hardly improve anything. But, Spaceboy, if you develop for aerospace you simply might want to save the extra weight
Hehe, the name and my application was not meant to be related. But this is a Cubesat OBC, for your information
Okay so the fragmented GND planes might wreak havoc? Can you please tell me what exactly are these cases?
Well, I gather from Rick Harlteyâs PCB Optimization video that copper thieves are a bad idea because they might actually as antennas. The better option he suggested is a ground pour.
Also my PCB is for a cubesat OBC and I read from the reddit post by the creator (I think )of the Copper Thief plugin that copper thieves are bad for vacuum applications.
I guess the other argument was to prevent warping. But not sure of warping is a problem these days
Fragmented ground planes:
- currents take the path of least impedance starting at as low as 500Hz
- current might take a impedance shortcut through some fragmented ground pieces
â the size of the loop area increases and therefore emissions increase
â if you insert a high frequency current into a copper area you have a patch antenna
â irregular shapes might be resonant on different frequencies and therefore can act as an antenna over a wide frequency range
Fragmented power plane:
- to minimize the effects of radiating ground islands these should be connected to the inner ground layer with d< lambda/20
â your ground plane will get (possibly) very fragmented
â current path and return path diverge around the vias increasing your loop area and therefore emissions
Copper Thieves
- the dimensions and radiation patterns of each thieving element are known and so the resonant frequencies can be calculated
- HF-current must be coupled into the elements which decreases with distance and smaller dimensions which is also somewhat predictable
- you can choose the frequencies to be far away from signal frequencies or harmonics on your board
But if your application is a cube sat you will do EMC measurements anyway just give it a try which method works for your specific application best.
And warping is still an issue, this 1mm PCB warped for example ca 1mm upwards (kind of hard to see in the image) due to bad copper dispersion:
1 Like
I have heard about warping in times when I didnât even considered more than 2 layer boards. May be if boards have internal layers practically 100% filled with copper what is going on external layers donât matter (I donât know).
My private argument for making a GND filled zone on top (assuming SMD elements are at top) layer is to provide a path for surge current pulses (that I assume 25A) back from SMB 600W transil to terminal block without need of going this current through vias.
I see. My board uses the PC104 and also has some additional through hole pads. Expected current is maybe like ~200mA. Havenât estimated the current yet though. Just a guess
âPie-In-the-Skyâ and because your User-Name is Spaceboy⌠and reading the above Postâs brings back a 40yr old experience, Forgive me⌠Iâm amusing myself 
Maybe youâll find humor in thisâŚ
I was a Rocket Engineer and one day I was assigned to solve a problem on a Laser-Firing system for the Air-Force. A small 20-Million Dollar portion of a 500-Million Dollar defense project.
I arrived at Norton Air-Force-Base and was ushered to a Top-Secret meeting. Though arriving on-time, all attendants were already seated.
Stars & Strips seated at the head of the table, 14 Engineers and Scientists (all with PhDâs) seated on one side of a long table and I sat alone on the other side.
The meeting started and documents were passed out. The leader of the âgroup of 14â quickly got to the âmeatâ of the design and the assumed problem. These folks designed it, built it, tested it and, knew every dotted âiâ and crossed âtâ. I was assigned to this the night before and knew nothing.
There was something on the very first page that I didnât understand and after 10 minutes of my silent listening, I asked the question, âIâm looking at the first page, how does this get turned On?â
I saw Eyeâs rolling and smirks that read, âWho is this dope with long hair and corduroy jacket?â Their lead said, âBy the Switch on the first-page youâre looking atâ, he said.
I waited a moment to ensure those 14 geniusâs were looking at the Switch, too. Nobody said anything so, I said, âThat switch isnât going to turn On anythingâ.
Still, nobody said a thing except for their lead who asked in a manner conveying insult to me for my stupidity, âWhy not?â
I replied, âSee that line going to the High-Voltage, itâs also going to Groundâ.
I watched 14 Jawâs drop and still have that mental picture.
Those 14 geniusâ couldnât pack-up and leave the room fast enough and I was left alone with Stars & Strips, âYouâre reputation preceded you. Iâve been watching you. When I saw you kept turning back to the first page, I knew you saw something and I waited and watchedâ.
10-minutes later I was escorted by Military-Police to the Airportâs back-end adjoining Norton AFB and ushered into a hanger where my Ticket was stamped and told by the only other person in the building as she looked out the Window, âTheyâre bringing your plane around from boarding-gate, have a good flightâ she said as we saw the fully loaded Delta-737 pull-up for me.
1 Like
Thatâs a good story.
But forgive me for being stupid, is the upshot that I shouldnât do things like pouring ground without analysing their effects?
Youâre not being stupid, not at all.
I was reminded of the story by (and, I donât mean to imply anything about anybody) âWhat ifâsââŚâCouldâ⌠all the possibilities (like, Pie-In-The-Sky that could happen, are Important to consider but, need (IMHO) a healthy dose of commonsense consideration.
And, I try to start from the foundation of the matter-at-hand⌠Ground-Planeâs are important for many designâs, environmentâs, etc⌠If I were wondering about the Ground-Plane (pour), Iâd do my own homework using real-world documentation/booksâŚetc⌠Then, I would âKnowâ what I needed to learn⌠Perhaps mostly because I was born at the end 1940âs when technology was simple and âhow to learnâ was taught in school, unlike in todayâs iPhone worldâŚ
ADDED: In other-words, Iâd want to know:
⢠Why are GND-Planes used
⢠When are they used
⢠When are they Not used
⢠Is my design similar to those situations and environment of usageâŚ
1 Like
Youâre right about the education part (Iâm in 3rd year of college).
As for ground pours working in space, I guess they do.
Purpose? Prevent board warping and also due to the fact that adding a ground via for a component fills that region with the ground pour.
And yeah thanks for the general advice
Just to give and idea about Warping & Curiosity and, Iâm not suggesting you do something like this though, perhaps a classmate (primarily a Mechanical Engineering student) could helpâŚ
I did this Example in FreeCAD 5yrs ago when the FEM software was in a less stable version⌠I did not include the PCB re deflection/etcâŚ
You can use the KSU Workbench in FreeCAD to load the PCB, Traces/Pad and parts and do FEM
1 Like