Labels and net names.
In KiCad, a label is a schematic symbol on itself. There are 3 kinds of labels.
- Local label.
- Global label.
- Hierarchical label.
A local label is shown as a text string that defines the name of a net and does not have additional graphics. The label is attached to a wire as soon as its attachment point (small square, by default in it’s lower left corner) is put on a wire. In that case the small square disappears.
This label is not connected to a wire, because the square in it’s lower left corner is visible:
This label is connected to a wire. Both the squares from the “open wire end” and from the label itself have disappeared.
A label can be put anywhere on the wire. In the case below the label is attached to the wire, but the square of the open wire end remains and this is harmless.
In KiCad it is perfectly legal to have multiple labels with different names in a single net. When two labels are put on a single wire, the nets get merged silently and KiCad just picks one of the label names as the net name. There are no nag screens to ask for confirmation.
When labels of different types are connected with a wire, they also get merged into a single net.
Each net that does not have a manually placed label, gets an auto generated net name. These names are considered unimportant in KiCad. They do not show up on the schematic in KiCad V5.1.x, and they are not shown in the drop down box while selecting preexisting names for labels.
In KiCad-nightly V5.99 these net names are shown in the status area at the bottom of the screen when a wire is selected:
KiCad V6 has error checking for net labels in ERC. This behavior can be set to your own preferences in: Schematic Editor / File / Schematic Setup / Electrical Rules / Violation severity, and you can suppress individual errors or warnings.