Kicad Ground Pads are not completey connected with Ground plane

Question

I have the upper layer of my board set up as GND copper plane.

However, when GND pads are connected to the GND plane, they are not completely connected to GND. Rather, a cross is formed on the pad. For example:

I wanted the whole pad connected to GND. How can I change that?

Answer 1

No Thermal Relief - Do you really want to do that?

Thermal reliefs are enabled by default for a reason. Large copper planes act like an excellent heatsink for the circuit board. This is both a blessing and a curse - pads connected to the plane can be more difficult to solder, desoldering is a bigger problem - in the worst case, a through-hole pad connected directly to a ground plane can be a repair/rework nightmare.

The problem is less serious for surface-mount pads, since reflow soldering usually heats the entire board evenly. But you may still encounter solderability problem, especially during the assembling and reworking of a prototype by hand.

There's a tradeoff between performance and solderability. If you don't have any special electrical or thermal requirements - such as better thermal conductivity for heat dissipation, a continuous ground plane or lower impedance for high-speed circuit, etc. - it's recommended to enable thermal reliefs.

Disable Thermal Reliefs Globally

To disable thermal relief for all copper pads in the entire ground pour, click the copper zone to highlight it on the screen, then press E to open the property dialog window.

In the property window, one can see the "Pad Connections" options:

• Solid: disable thermal reliefs entirely
• Thermal reliefs: enable thermal reliefs
• Reliefs for PTH: only enable it for through-hole pads.

Disable Thermal Reliefs Locally

To disable thermal relief for a single copper pad, click the copper pad of a specific component, until only the copper pad zone is highlighted on the screen (but not the entire component, you may need to click the pads multiple times before that happens). Then press E to open the pad dialog window.

In the property window, one can see the "Connection to Copper Zone" options. The default setting is to follow the setting of the entire component, but it can be overridden too.

Answer 2

That is perfectly normal. It is called a "thermal break" - it provides some thermal isloation between the pad and the plane. Without that thermal break, you would have to heat a large area of the plane to get the solder on the component to stick to the copper plane.