Newbie here.
When I run the ERC I´m getting error: Input power pin not driven by any Output Power pins for each of my power and ground connections.
I tried to make it go away by changing some of them by PWR flags. It worked but apparently I´d have to change all of the 3V3 and GND to PWR flags. Is this the only way to fix it?
Is it an issue with Kicad 6?
Should I use Kicad 5 instead?
I´m running Kicad 6 on Windows 10.
You don’t need to swap the 3V3/GND symbols for PWR_FLAG. Instead you need to add a single PWR_FLAG to each power/ground net in addition to the existing 3V3/GND power symbol.
The reason you get an error is that ERC wants every “power input” pin to be connected to a “power output” pin on the same net, to make sure that the “power input” pin is getting power from somewhere. In some cases, like when your circuit is powered from a connector, there won’t naturally be a “power output” pin, so you can add a PWR_FLAG to tell ERC that you actually are powering the net (PWR_FLAG is really just an output power pin with a little diamond drawn on top).
Hello gkeeth,
Thanks for the reply. It did work for one +3.3V and one GND, however now when I do it for others I get error: Pins of type output and Power output are connected.
What should I do?
Check your symbol. Is FR/pin15 defined as an input?
Looks like you have a few problems.
Your selected error suggests you have at least two PWR_FLAGs connected to 3V3 - you only need one.
The next errors suggest you have a bunch of pins set as bidirectional when they should be input or power input. PAD should be power input as it’s a ground pin, and FR seems like it should be an input based on my quick read of the datasheet.
You only need one pwr_flag per net, ie one for 3.3V and one for GND. Placing multiple flags also creates errors. You should not place one at every 3.3V symbol and so on.
Ideally place the flags where your power really is input into the system, like near a DC connector or behind a fuse or whatever.
The warning is essentially telling you that you have defined a 3.3V net but KiCad isn’t sure where the power actually comes from. The flag essentially says “I looked at it and the power comes from here”.
You don’t need power flags if you use power sources that kicad recognizes, like if you have voltage regulators or battery symbols that have their pins set as power output.
When possible, rather than adding the PWR_FLAGS to the wires on the main schematic which could confuse a reader not familiar with KiCad, I’ve been adding a legend near the title block.
Another alternative to avoid PWR_FLAG symbols is to modify the appropriate symbols so they act as power output. For example if you have a DC-Connector where your PCB gets power, don’t use a generic connector symbol (with passive pins), but create one yourself where the pins are set to power output.
If you use fuses or inline resistors for current measurements, that quickly gets messy, though, You can also simply disable the warning if it gets annoying.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.
