Electrical Engineering Stack Exchange is a question and answer site for electronics and electrical engineering professionals, students, and enthusiasts. It only takes a minute to sign up.
Sign up to join this community
What does it mean to kicad that a pin is driven?
I have a 12V rail connected to a battery positive terminal in kicad. Kicad says the 12V rail is not driven. Why does it say that? In fact, it tends to shift around depending on whenever I redraw the wire and run a design rules check on it. I'm trying to make sure the board has a battery input, when it is drawn up on PCBnew.
The Electrical Rules Check tries to ensure that everything that is connected to a single net fits together. The quick summary is that a valid net has
power_in, power_out) or data (input, bidi, output) pins, not a mixture of thempower_out for power nets, bidi or output for data nets)power_out or output)So a power network needs exactly one power_out connected to it.
A known limitation is that connectors' pins are defined as passive, because that doesn't immediately lead to a conflict with anything else connected to the same net, so the connector that the power supply is connected to cannot be marked as having a power_out pin to placate the ERC.
The PWR_FLAG pseudo-component provides a single power_out pin, so you can avoid the warning here. The ERC will complain if the same net has two PWR_FLAGs, or a PWR_FLAG and some other component with a power_out pin (such as a linear regulator).
In KiCad the power nets (grounds and sources) should be marked with special symbol "PWR_FLAG" which is located under "power ports" category.
