Hi,
I want to create a split ground plane. This would be like opening a rectangular hole in a ground plane. And put another rectangular filled region inside that rectangular hole.
In other words, it would look like concentric rectangles.
Any guidance on how to do this?
Thank you
Another option is to use a rule area to create a keep out zone:
This method is mostly useful if you want to connect the inner zone to the same net as the outer zone.
If you want to connect the inner zone to another net, then just drawing the zones on top of each other and working with zone priorities as Naib mentioned may be a better solution. The inner zone should then have a higher priority, so it’s drawn first, and the zone around it will automatically keep a clearance from the higher priority zone.
Thank you, I used the rule.
But I would like to understand how to do this with zones and priorities. it is a little hard to make out the sequence of steps from your images.
In the example below I drew two overlapping zones. In the properties of the highlighted zone (on B.Cu, just as the other) I set the Zone Priority Level to 5. For the other zone, it’s left at the default (which is zero). “5” has a higher priority, so this zone is filled first, and the other zone maintains a clearance from it, just as it does with tracks from other nets, and Edge.Cuts.
Neat. I might guess that they need to have different net names. Presumably I could connect them through a 0 ohm resistor and they will still remain separated.
In my case, the regions are going to connect to each other through a narrow area around one through-hole pin. So, I might guess the software will see that as one net and loose the separation between them?
Yes, they must have different net names. If the names are the same, then the zones will just merge together. You could use a zero ohm resistor in the schematic, but that would also require you to put it on the PCB. KiCad does have a special mechanism to have continuous copper with different net names, and that is called a net tie. KiCad has both schematic symbols and footprints for net ties.
