Copper fills (zones in KiCad) should usually be connected to the pads which they surround or touch if they belong to the same net. Sometimes this doesn’t happen, and there can be several reasons.
The connection can be either solid or with thermal reliefs. When a zone is created, or afterwards, this can be selected in the Properties dialog with Pad connections option. One option is “None”, so if this has been selected, the zone may be left unconnected.
This zone option can be overridden in the footprints. Each footprint has similar set of options in its Properties -> Local Clearance and Settings. It can follow zone the option selected in the zone or override it.
Each pad has this same set of options, too, and pads can inherit it from their footprint if there’s no need to change it for that one pad. Otherwise the pad setting overrides both the zone’s and the footprint’s setting.
So, if a zone doesn’t connect to pads, check these zone/pad connection settings in:
- zone properties
- footprint properties
- pad properties.
(Screenshot from v5.99 pad Properties.)
If it still doesn’t connect, the problem can be in some numerical values. If the connection is made with thermal reliefs, they have their own values in the above mentioned properties for zones and individual pads. Again, the pad properties override the zone properties. Make sure the values are sensible.
A zone has also its own values for generic clearance and minimum width. If they are too large there may not be enough room for the zone to fill.
(Screenshot from v5.99 zone Properties.)
The last possibility is some other clearance value which prevents the zone filling. If a nearby pad or an item in another net has large clearance value which overlaps with the problematic pad, the zone may not connect. Detecting this is easier if you make the clearance lines visible from the PCB editor’s Preferences then try the outline modes for different kinds of items in the left hand toolbar.