Copper pour/filled zone disappears after DRC run

I have a PCB project where there is an elevated island. I more or less finished designing the board but for some reason, when I want to run a DRC test, the GND copper pour on the island entirely disappears.

Could someone help me with this? I am at a loss. old_PCB.kicad_pcb_v3.kicad_pcb (309.7 KB)

(alternatively, since I am happy with the island itself but I just want to move the island up a bit, If there is a way I can selectively redo copper pour, (performing GND copper pour on the main board’s copper layers only, that would be wonderful).

I do not know how to keep the island, as it is not connected to any pad/net, the job of the DRC is to remove it, I could not find any configuration to keep it, maybe throw a dummy pad on the bottom layer to keep the DRC happy.

Well if the island is anyway not attached to any net, maybe it can get its own net name that way you are able to redo the GND zone, without interfering with your Island.

Maybe this will help: How to create a power plane (using zones), especially the Appendix.


I think I found a workaround (I just learned how to refill individual copper layers)

Regarding the island being not connected, the two copper layers have vias (some for grounding and others for signals)

Did i miss something here? I am not sure why you think the island is not connected to anything…

As you can see in the FAQ article, it must be connected to a pad directly or indirectly. It’s not connected to a pad even indirectly through vias. It’s connected to a zone in B.Cu but that’s not connected to a GND pad, either.

1 Like

If it wasn’t clear: it must be connected to a pad in the same net, of course. The signal vias don’t affect in this case because the vias must belong to the GND net.

If you add a through via which connect the F.Cu zone to the other GND zones they will be filled. (This is of course just an example which shows how it works.)

You mean with the context menu ?

I’m curious, how did you fill up the zone in first place?

I’ve got KiCad V5.1.6 and the board seems to render normally when I turn all copper layers on, also after re-calculating zone boundaries with b.

Also lots of DRC errors.
About half of them are about “Micro Via’s” (Check your PCB manufacuturer. Those things are expensive).

Most others seem to be because you’re halfway some kind of move operation.

I wonder why you have choose microvias for the vias for the fannout did you for the middle device. Are you sure you really want that?

Is this intentionally made as a four layer board? It looks like you are only routing on two layers. To be it looks like they layer you have is something you want on In1.Cu and not In2.Cu.

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