Power Pin ERC Errors KiCAD 6

I have the folowing:

This reports an ERC error on pin 4 stating:
“Input Power pin not driven by any Output Power pins”

Pin 4 on the device is of course a Power Input pin definition. The +5V is from the default library and that is also a Power Input pin definition. Seems in order for this not to generate the error, the +5V symbol should be called a Power Output pin.

Where is +5V coming from, a regulator or something else designated a power output? If say just a connector, then you need a PWR_FLAG.

Voltage regulators such as the LM7805 have a “power output pin”, because that is where power comes from. If you do not have a voltage regulator on your PCB, for example because power comes from an connector (and external power supply), then you have to add a PWR_FLAG symbol to your +5V net. I prefer to put these PWR_FLAG symbols near the connector that brings power onto the PCB.

1 Like

So I have to do this whenever power comes from a connector?


Seems like something to just clutter up the schematic. Another quirk for KiCAD compared to every other schematic capture software I have used. Is there a way to “hide” this from showing up on a pdf/print of the schematic?

There are several ways to hide it.
One of the neatest is to set the pin type of your power connector to the “power output” type.

In KiCad V6 you can also simply disable the ERC messages for "Input pin not driven by any Output pins. You can find this in: Schematic Editor / File / Schematic Setup / Electrical Rules / Violation Severity / Connections

In itself it is a useful thing though. I would not call it

It is an uncommon feature. Other EDA suites probably do not check for this error at all.
In KiCad, it is a feature that (unfortunately) leads to many questions / confusion. A part of the problem is that the ERC in KiCad can not look “through” schematic symbols such as fuses, jumpers, net-ties, filter inductors and chokes, and therefore re-issues this error any time such a schematic symbol is inserted between a power source and a power consumer.

1 Like

Meh, that’s a minor nuisance compared to horrible schematics I’ve seen. E.g. power and GND pointing every direction. The ones I hate are those that just present every IC separately and using only labels to connect them.

You don’t have to. Another option might be to create a custom connector symbol which has the power output pins actually set to “power output”, this will make KiCad happy.

You can also create a edited copy of the PWR_FLAG symbol that looks less annoying, for example make it smaller and remove/hide the text.

If you’re using a lot of chokes, current sense resistors, net ties, zero-ohm-links and so on, placing lots of PWR_FLAGs might be annoying and I would probably disable that warning.

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.