How do I implement advanced copper fill techniques?


I’m interested in making boards that look like this one. How can I expand power and ground runs so that they fit together like a jigsaw puzzle?


Why do you want to do as shown in the image?

If you really want to do this, use two zones on the same layer, and change each zones priority level to achieve the desired results.


Hi, thanks for your comment.

I do lots of work with audio signals and it’s important to partition off ground planes as well as steer current.




The jigsaw puzzle pours shown in the photo will have next to no effect on “steering” audio frequency currents; this is mostly affected by the selected schematic design.


Are you sure you understood the situation? of course the shape of the zone steers current; current can’t go where there’s no copper. There are “slots” inside one zone in the picture. It’s common practice to separate analog and digital parts of the ground plane having only one small connection point.

@mlaflare, Zones are polygons, so you just add corners and drag the control points util you get the desired shape. Open the right mouse button menu of a zone and get familiar with the options. You can add and remove corners. You can also add cutouts to zones. As Sprig told, each zone has priority level which tells which zone avoids another one.


Splitting ground (or star ground) only helps if you fully understand all problems that come with it. You are for example not allowed to cross over the gab between the grounds with a signal that contains or is suseptible to high frequencies (> 10kHz) as that would create a slot antenna.
This is why it might be better to use a single uninterrupted ground plane on an inside layer. The separation of “currents” is then controlled by the placement of components (Ground currents take the path of least inductance. For high frequency directly under the signal they originate from.)


Well, I may be wrong, but I’m fairly confident that the slots in the zone shown will have little affect on audio frequency currents.


You are (can be) very wrong here indeed.
Take for example a 100W audio amplifier, which can deliver peak currents of well over 10A, but also has pretty sensitive inputs. Such high currents will cause significant voltage drops over the tracks they run through (inclding a GND plane) and such currents must be separated from the ground paths of the input signal.


@paulvdh I hope this is just a language/forum presentation issue.

Changing the shape of a Filled Zone, or adding a slot, will not control (“steer”) the direction of the resulting currents from that physical copper pour, in the image provided by the OP, at audio frequencies in such a small space of board.

I don’t believe this is so. Even your post contains the solution; which I hinted back with:

Just like the OP provided the schematic above:

You agreed with the comment that:

Then you twist the post to suggest that the OP meant high currents from 100+Watt amplifiers; which was never mentioned, or suggested, in the OP.

Then you make your own claim which is absolutely incorrect:

KiCad comes with the software called PCB Calculator. A knowledgeable PCB designer would use such a tool to ensure that the copper thickness and trace width were sufficient to provide the minimum desired voltage drop for any circuit with a sensitive parameter/s.


This is a cool tool: but I cannot see it in my installation. Is it a plug-in?
Where can I find & add it?
thnx Sprig.


The calculator icon on the main project window in KiCad:


oh, lordy!
do I have eye for sight or what!
thnx: yes I see it…


Sometimes other constraints come into play and the designer doesn’t have the luxury of unlimited trace width or 10oz copper. Splitting power and ground planes is a well known technique for keeping large or noisy currents (all the way down to DC) out of sensitive areas of the PCB.

Cuts and splits can be implemented using the copper pour outline, or by using keepouts.


This thread is getting ridiculous.

Once again, it is not difficult to make use of KiCad’s calculator tool.
Shown are the calculations for 5oz copper:

Or, with 2oz copper:

OMG! That is 139 million inches to handle that power!

No, not really, it ends up being a 0.14in/3.5mm trace; and this is assuming that the source drive voltage is only as high as 10Volts for the above assumptions after the OP’s initial provided information.



Did you notice the 100mV drop over the track in the PCB calculator?
This is very significant for audio, and connecting a track for a feedback loop to the “start” or to the “end” can completely destroy an audio circuit, or any other low-noise circuit were voltage drops of uV over tracks can be important.



Sometimes mV matter.


I’m won’t argue on ground topology.
A practical technic to separate GND and AGND is to use net-ties. Doing so will allow to use DRC to force minimum width, separation, etc, for tracks and even for polygons.


Thanks! I found a video explaining the concept and it appears to be a great trick. I’ll give it a try on a future board.


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