Non-Global Power Symbols?

I just found out that the Power symbols are global.

What is the “recommend” way to have a label with a graphic symbol for local power on individual sheets?

Or, if there is no recommend way, how do you do it?


There is no “recommended” way. A Power Symbol defines a net label, and that net-naming ability exists only with power symbols. You can’t assign a net name to a pin in a non-Power Symbol.

Just give the name a local label that makes sense.


I personally don’t like that method because the common global power symbols are very easy to visually recognize for what they are.

Every time I post a question here I do in fact attempt to search for the answer before posting; on this forum and a few others. Today, I found an answer to a similar question on another forum, I forget which one.

I tinkered around with KiCad and the power symbols and decided on a method based upon that forum answer.

My power symbol was the typical arrow and the text “+5V”.

I have 5 hierarchical sheets. I decided to edit the +5V power symbol to read “+5V_1” through “+5V_5”.

I considered using “+5V_0” for the ROOT page, but didn’t want to spend the time making those changes; but in a way it seems it might be more logical that way. As such, it would indicate on the top page that there is more then 1 power source of that voltage.

Comments welcome.

1 Like

Same as @Andy_P.
Local or hierarchical labels.

1 Like

I realize this is an old post, but in case others find this post in search of how power symbols work: The answer quoted here is not really correct.

A Power Symbol connects to a power net only by virtue of having a pin that has particular qualities:

  1. The pin has its name set to the net name of interest. The name of the power symbol should be set to the same name as the pin to reduce confusion for users, but that is not necessary. Setting the name of the power symbol does not determine the net to which the pin connects. (So you can’t create power symbols for a new net solely by renaming the symbol.)

  2. That pin has its visibility set to False. It is not obvious why the “visible” attribute causes “define and connect to a net”, but it does.

  3. The pin’s type should be set to Power In. Somewhere else on the net there should be a component with a pin that supplies a Power Out to the net.

  4. This invisible pin mechanism can be applied to any symbol, For example, it is applied to 7400-series TTL components, so that they connect to the GND and VCC nets without explicitly drawing their wiring. That was a popular style of schematic back when a product might consist of hundreds of TTL chips, and there was only a VCC/GND supply . There’s nothing special about power symbols per se.