Does anyone know how to fix this: When I load a GND symbol from the Kicad 8 power library and I connect it to a PWR_FLAG symbol from the Kicad8 PWR_FLAG library I get the error:
“Input Power pin not driven by any Output Power pins.” I searched all pages and this is the only PWR_FLAG symbol I have. Even if I change the PWR_FLAG from Bidirectional to Output I still get the same error. I also checked the GND symbol from the Kicad power library and it has attribute of Input.
PS: Even if I leave the PWR_FLAG and GND symbols unchanged and make the main GND input connector/pin an Output, I still get that error message.
I am quite certain you did not do this.
Just to verify, I also did it, and ERC does give an error, but it is a completely different one.
What most likely happened on your side, is that you messed with KiCad’s default libraries in some way (Normally they are read-only, and that is for good reasons) And then you did “other things”, which resulted in KiCad using the symbols that you broke.
I’ve got a question for you, and if you can figure out the answer, then you are already halfway to the solution:
In KiCad’s default library, the pin in the Device:GND symbol is set to be a power input. Why is this done?
This is weird, and I agree with Paul that there’s something wrong with your library. There’s one pin in the standard PWR_FLAG of KiCad and its type is Power Output, not Bidirectional. Be careful with terminology: Power Output and Power Input are different than Output and Input. The GND and other related symbols have one pin which is of type Power Input, not Input.
My PWR_FLAG was getting pulled from a different library of symbols I got from original older kicad drawings. I removed that and got PWR_FLAG from the Kicad 8 library and it fixed that problem but caused a new warning: Power Output pins connected to Bidirectional pins on GND net connections.
You make it easier for us if you post the exact error message you get, and don’t turn the words around. When I create the problem I think you are having by connecting an SN74ALVC164245DGG (Which has bidirectonal pins) to your (recreated) schematic construction I get:
Note that the two lines under the warning give details about which pins KiCad thinks are the cause of the problem. And in this case KiCad is correct. It’s not good practice to connect a bidirectional pin to a power output.
I am guessing that your GND symbol has a similar problem as your PWR_FLAG.
Open the properties of the GND symbol, and then look at the Library link at the bottom. This symbol should be from the power library.
You can also use: Schematic Editor / Tools / Edit Symbol Library Links. This gives a spreadsheet like overview of all used symbols, and you can also use it to replace symbols with those from other libraries.
Sorry, I’m retarded at linguistics. I updated the PWR_FLAG to be from the “power” library in the Kicad8 “share” folder of library files, when before I was using an old PWR_FLAG that was pulled in from a schematic originally drawn with Kicad 4 or 5 I think. Now I get 19 instances of “Warning: Pins of type Power output and Bidirectional are connected.” All 19 warning arrows are pointing at the PWR_FLAG connection and each instance of the warning also lists a symbol connected to GND, like a resistor or connector. I checked and as best I can tell I have replaced all GND symbols (from the old drawing converted to Kicad 8) to the new GND symbol from the Kicad 8 “power” library. However, all the other symbols, like resistors and connectors are still what was pulled in from the older version schematic converted to Kicad8. I’m hoping there is an easier fix than manually replacing each symbol from the old Kicad version schematic.
Those warnings are not problematic, you’ll always get them because a bidirectional pin is a potential output and should not be connected to a power output directly.
You can turn off the warning in ERC setup. You’ll find it under “File”, “Schematic setup” (V7). Might be somewhere else in V8.
What signal type should be used for a pin of a connector used for Output of GND so as not to conflict with a PWR_FLAG of type Power Output that is connected to the GND net? Is there something else that is supposed to stop the conflict?
ERC is not a “smart” system, it just follows some simple rules. And the rules are defined by Schematic Editor / File / Schematic Setup / Electrical Rules / Pin Conflicts Map
Pins for connectors and resistors are by default set to the passive pin type.
I also checked this with an old project for which I made the schematic in KiCd V4 or V5. Back then I carefully made the project independent of all of KiCad’s default libraries, and later upgraded the project. Pins of resistors, capacitors and connectors and such are all set to the passive pin type, as they should. The “passive” pin type is commonly used for all pins for which there is no clear other alternative. “Passive” is the most permissive pin type and it can be connected to nearly all other pins without ERC complaining. From the matrix you can see that the only warning is if it gets connected to an Unspecified Pin.
It is unlikely this changed for you during the conversion from the KiCad V6 project. It’s more likely that those symbols were taken from some other library when the project was created, or someone changed them somewhere in the last 3 years.
From all appearances, you have a problem with old symbols that were assigned very strange pins.
From V6 onwards, symbols used in the schematic are stored in the *.kicad_sch file, and it’s no longer possible to trace where they came from. Certainly not from the standard KiCAD symbol library, but rather from a heavily personalised one.
What paulvdh said, “passive” is the right pin type for connectors et al.
You can always have a look at: Schematic Editor / Tools / Edit Symbol Library Links. It should list both a library name and a symbol name for all symbols. Even though all used symbols are embedded inside the schematic itself, the links likely still point to the external libraries.
If the links point to the default library names, then: Schematic Editor / Tools / Update Symbols from Library still works. If the library links are broken, then you can use that previous dialog to repair them, and then update the schematic.
But overall, it may be better to not spend too much effort on ERC in this project. If you want to use ERC, then do this in the next project, and then keep an eye on it and make sure it works from the beginning. So that starts with the library setup.
If you want to experiment with changing these things in your current project, then make sure you have backups you can revert to for if you make some gross errors.
