Conflict error between pins - how to fix?

Hi. I am new to KiCad and I have a question. I’m working on a schematic and I have run into a problem where I am getting an error about conflicting pins.

This happened because I got an error about a some pins being connected but not being “driven”. I read that had something to do with needing the pin that is supplying power to be marked as a power pin.

So, I went into the library and edited the component (a component I created) and marked the input pin as being a power input. Then I modified the component that is the power source to have some of its pins as power output pins.

This caused this warning: “Conflict problem between pins”. I want to have a Molex connector that is a 2x2 connector. Two of the pins are +12V and the other two are GND. I took the CONN 2x2 and duplicated it and saved it into a library for a Molex 39-28-1043 connector (which is a 2x2 power connector) and marked two of the pins as being “power output”. Then I added that component to my project and attached a global label to each pin that says “+12V”. The other two pins are attached to global labels “GND”.

I get the conflict error between the two +12V pins. Is this because I’m trying to attach two output pins together? I also have +12V labels on the things in my project that need +12V.

How can I resolve this?


You can only have one power output per net, so it is joining the two that is causing the problem.

Usually you only have a “power out” pin on something really simple like a linear regulator, on connectors and more complex power supplies (e.g. switch mode) they don’t work for design rule checking.

The way to get around this is to add “PWR_FLAG” from the “Place power port” tool once to each net that needs to be driven. When you place it, make sure there really is a driving source (in this case your ATX 12V connector) and then just connect the power flag to the +12V net.

The power flag component isn’t a component symbol or power port in the normal sense, it just provides a driving source for the purpose of verifying the design. Generally I put these off the page somewhere, they’ll still get taken into account when the electrical rule check is run but aren’t in the schematic output if you print/plot it.

Thanks. That solved it. I had some trouble finding the power flag, but then I found it under the list of parts that come up when you place a power port.

Thanks again.