[Solved] Pins representation


Hi all,

I would like to know what kind of symbol I should use.

I tried using the pwr_flag for Vin and Vout

and I having error

Thanks in advance.


From where did these signals come?

I would modify the symbols to define their pin types as Power Output. That eliminates the need for a Power Flag.


What i was initially thinking was having a pin header on the schematic and run through the rule check I got errors and I went to search on the forum and found out I need power flag.

What I want is to be able to translate to pcbnew for the input and output.

May I ask by modifying is to edit through part library editor?


A pin header is fine – usually the pins are defined as type Passive, so yes, you will need to put a power flag on the nets connected to pins you wish to use for power.

Looking back at your first post, it’s a complaint about pins on a Power Symbol that have no driver. But I don’t see any Power Symbols other than GND. But yes, the Power Flag solves that problem.


This might not always be the best idea.
I had a kicad workshop recently where a guy did this. I manually checked his board. I found that he has no power supply for his components. ERC did not complain because he simply changed the electrical type of a few pins.

In my mind the best option is to use the power flag. (near where the power is supplied to the board. It is not a good idea to connect all power symbols do a power flag at a central location.)


ERC can’t predict that the user won’t connect a power supply to the product … and except for a batter-powered gizmo, nothing on a board is really a “power output.” To be pedantic about it, anyway.

That said: there was previous discussion about DC power jacks (the usual sort of 2.1mm pin/5mm barrel) things, and whether to declare the pins as Power Input or Passive, and arguments for both options are compelling. One can split the baby and have the pins on the library part be Passive, and when the part is instantiated in the design, they can be changed to be Power Output. (Being aware, of course, that if the part is changed, the new part will have to have its pins modified the same way.)


Could I use a general power flag and place it on the Vin line?


There is only one Power Flag. Everything else in the power.lib library is a Power Symbol.

There are important differences that you must understand.

A Power Symbol declares a global net whose name is given in the symbol (VCC, VDD, whatever). It has exactly one pin whose type is defined as Power Input. Since it is a Power Input, in order to satisfy ERC the net must be connected to a pin defined as Power Output.

The Power Flag does not declare a net. Its pin is defined as a Power Output. Its purpose is to satisfy the ERC requirement mentioned just above. For example, say your design as an AC input which goes into a rectifier which feeds the input of a voltage regulator. That regulator’s VIN pin is likely defined as Power Input, but is a rectifier a “power output?” Strictly speaking, no, and the diodes (and the smoothing cap) have their pins defined as Passive, so ERC will complain: “No driver found for Power Input Pin1 on U1.” Placing a Power Flag on the rectifier output net satisfies ERC, because you (as the designer) “know” that the input power for the regulator comes from the AC input though the rectifier.

Got it?


@Andy_P I have put the power flag at the input and how do I set the output of the connector on the schematic? Do I change the value or do I have to manually change the pins on the connector?

Thanks in advance.


I’m not quite sure what you ask.


I’m sorry I should be more clear, how do I define the pin as power output? I place the power flag and the pin is define as power input.

The error stated that power input is not driven but the connection is going to the output. Or do I have to put power flag at the output?

I kinda confuse on the input and output of the symbol, I wanted to have input and output using the pin header and I could not seem to change the pins behavior unless I have to go to the edit with the library editor.


I place a power flag near voltage source part. It is much faster.