Hi everyone, I`m designing my first PCB and have problems with filling the ground plane under the IC. I made a Copper Zone and tried to fill it with “b” but don’t know why the pads are not connecting to the rest of the ground fill.
Is this a problem caused by the footprint of the IC or am I just doing it wrong? It seems like a small part is filling but filling the whole GND pad of the ic
Best Fabian
There are two different issues here.
The first is caused by the small pad spacing of your 64 pin square IC.
The default clearance for new zones is 0.508mm and this prevents your zone from reaching (for example) pad 19. (You can see the zone is trying to reach it by the little stub extending from it). The solution for this is to use a smaller clearance for the zone (“Freiraum” here set to the default 0.508mm).
The other issue is Pad 65. I assume you want to connect it to GND, (you put a via there), but that pad is not in the netlist. All pads that are part of a netlist, have the name of the netlist printed under the pad number, and the “GND” net name is missing in your schematic.
The fix for this is to go back to your schematic, add pin 65 to your schematic symbol and update the PCB again.
A third issue I just noticed is that you tried to draw the exact outline of your zone. I did not see this earlier because it’s unusual. Kicad keeps a clearance (defined in the zone) and it stays away from anything it should not touch. So you can for example just draw a simple rectangular zoneoutline.
Thank you for the quick reply, Issues fix 
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.
