Filled Zone question

Running into this issue I don’t understand with the back copper fill.

Why are these gaps here and why do they not fill in even when I make another filled zone to cover them ?

They are surrounded by traces on the same layer, so there is no way for the zone to connect into those ‘islands’.


Or are you referring to the pattern of circular holes?

1 Like

Circular holes are okay, they are part of a footprint. Just the larger areas that are blank.

Is there anyway to fill those in or is that just how it has to be in order to work ?

If I select No Net, they do fill. Not sure if that would cause an issue or not.

If you move some tracks aside so the fenced off areas can be reached they will get filled automatically. If you’ve moved a track aside so the “blank” area can be reached by the zone, you must press “b” to re-calculate the zone boundaries.

But having those area’s filled is not a worthy goal on itself.
For copper (power supply) zones to be actually usefull, they MUST be continuous, and not be cut to pieces by long tracks through them.

It seems that you have completely missed the point of the zones, and how to use them (That’s OK for a beginner, everybody has to learn). The Zones are an important part of EMI controll. Mandatory EMI regulation in EU (Every electronic device must compy) was a big push for 4-layer boads to have bigger and un-interupted copper fills on the power planes which were hard to do with 2 layer boards.
4 layer boards are often easier to design than 2 layer boards with proper EMI control.


That does make sense. I was just trying to save etching solution by not taking off the copper. Not sure where I read that but it stuck in my mind. Not making the boards myself but thought it was good practice to save the production facility etching solution, as that also saves time.

Savig etching chemicals is 5% of wanting zones. EMI control is the other 97%. The difference is filled by some other small things.

To prevent boards from warping during manufacturing it is also advisable to have a similar amount of copper on both sides (or on each pair of layers for multy layer designs).

1 Like

That makes sense. Mainly aesthetic at this point but I can connect them with vias. The very small sections aren’t worth the time but the larger areas can now be filled in.

Thank you once again @paulvdh for helping me learn something new about KiCad and design.

Not really that much of an issue for modern fabrication.

Is this still an issue? I assumed this is only a problem in wave soldering.

Regarding the zone itself:

In general a copper plane really only works if it is not interrupted. It is not some magical feature that makes a good ground connection just by being there. With that many interruptions one would really need a copper zone on the other side as well and make sure that there are connections on the other layer where the currently shown layer is interrupted.

I made a few example connections in this screenshot (Just for one interruption and indicated it with something that looks like traces but in reality this would be another zone on top.)
The best result is possible if you have vertical connections mainly on one layer and horizontal on the other. (Your diagonal would break this system a bit.)

To be honest your board looks like being layed out by an autorouter. Here a few examples of where you should really invest more time:

1 Like

You will need to spread the tracks so that the fill gets a chance to actually find some space to execute the fill.

Also place some additional vias for the fill to connect to other layers where tracks cannot be repositioned.

When it comes to fills there is always hand work required. KiCad won’t move the tracks for you in that context. At least not for now.

This was done 99% by FreeRoute. I actually have no idea what I’m doing on this project and am trying to learn from a similar project by building my own version from square one. Cleaning up everything as more is learned and more things are pointed out. Thank you everyone.

Based on that result ‘freeroute’ sucks :-1:

1 Like

Well, it is free. Keep in mind I still have no idea what I’m doing and am learning as I go. Have to start somewhere.

Warping / deforming of boards is not only caused by wave soldering.
Some time ago I saw some vid’s about PCB production from eurocircuits, and PCB’s deform during of the the pressing and curing of the resins. In hindsight this sems very logical. The press puts a lot of force on the PCB, and is hot and the resins partially liquify during, or at least get soft. Big copper planes will be pretty stiff, while on layers with no planes at all, the tracks and pads may be pressed a bit to the sides. (Distances would be very small, maybe a 10th of a mm, but even that can be important in high resolution PCB’s.

Undoing the mistakes from a badly routed PCB can be more work than manually laying all tracks on a PCB, especially if you have done a bunch of boards and have experience with it.
I do not see the problem of the circles Rene made. A far biggr problem are all the long vertical tracks, which cut the GND plane (I assume it is GND) into little pieces. In his first screenshot Rene presented a solution by via stitching the GND plane together again over such long vertical slots, but a much better solution is to not draw the long vertical slot through the GND plane at all. Most of the vertical track should have been on the other side of the PCB, and the same for all the other vertical (and diagonal) tracks.

Not necassarily. When a beginner in PCB design just “starts an autorouter” and let it rip through the whole board the results are bound to be bad. To get good results out of any autorouter, you have to know how to use it. I do not have much experience with autorouters myself, but from what I have seen autorouters generally make a big mess of a PCB really quick. I do not like them much. I also design relatively small and simple PCB’s. Autorouters are probably more usefull with very complex PCB’s and where 2 layers are completely reserved for Pwr and GND planes.

I do however like the interactive router in KiCad very much, Especially shoving tracks and via’s aside to make room to squeeze in just that extra last track.

Agreed. Auto routers are a messy lot.

Worked with half a million dollar calay systems with hardware router. They get the job done but messy. Always plenty of clean up by hand required.

Worked with protel, orcad, eagle, They all do something.

Abandoned eagle in favour of KiCad just last year and have not looked back other than to import some eagle projects.

Pcbnew has some wild sides for now, though no big issues in general.

I wanted to add my own small contribution as a power designer. It is true that long traces breaking up the ground plane can interfere with the ability of a ground plane to suppress EMI (and in fact they degrade the operation of the plane for probably all purposes).
But even the partially broken copper zone can be helpful for spreading heat and to reduce DC voltage drop in the ground or power plane. Except possibly where high voltage is concerned, I think it is better to fill unused areas with grounded copper rather than leave them bare. The information regarding a copper zone not filling if it is not connected … I sort of noticed that and it is good to know about. The only other point concerns any unconnected copper zone…I have learned to mistrust anything which introduces an unknown variable. In this case…the voltage on the floating zone is unknown so I would rather either connect it to something (probably ground) or 2nd choice is to delete it.

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.