# Why kicad schematics pin electrical type is always power input?

I was designing new schematics and decided to inspect another library downloaded from kicad official sources on Github. The one thing that cought my eye instantly was that Electrical type for both GND and VCC was POWER INPUT.

Is it meant to be that way or just a workaround for an existing problem, eg. failing DRC?

• On a symbol, you mean? – ThreePhaseEel Oct 23 '16 at 23:28
• @ThreePhaseEel yes, on a pin. – sitilge Oct 24 '16 at 7:19
• That's expected. You should only see power outputs on things like voltage regulators. – alex.forencich Mar 30 '17 at 3:08

VCC and GND are meant to be power inputs. ERC on the schematic will check that all power inputs are driven i.e. have a power output somewhere on the net. It'll also make sure you don't connect two power outputs together. An example of a power output would be the output terminal of a regulator.

The idea starts to break down if you put passives (inductors, chokes, resistors) that break up the net, but it can be helpful when used properly.

• Isn't vcc power input and gnd power output? – sitilge Oct 26 '16 at 10:56
• @sitilge No, I like to think about it in terms of whether a device requires or supplies the power. A single power net only has one output on it. For GND, the only thing power output would be the terminal to the battery's GND (or whatever else grounds the entire circuit) – mbrig Oct 26 '16 at 23:19
• I don't get why? I would like to add a VCC and a GND, which would power e.g. Arduino. VIN is power input and all 3 GNDs are too. So connecting VCC to VIN and GND to GND, is intuitive to me. But all 4 are by default power inputs. So DRC fails. How can I make simple circuit with power source connected to an Arduino? – Genom Jan 20 at 21:08

As a newbie I found this difficult to understand and it remains very non-intuitive (at least from a programmer's perspective) to have the ground (logical circuit output) "logically" defined as an input.

The answer from @mbrig put me on the right track, but I still had errors elsewhere until I understood the requirements to separately flag each power network with the PWR_FLAG symbol, explained here: KiCad pin connected to some others pins but no pin to drive it.

Create this kind of group somewhere else on your EE schema diagram, continue to use the more intuitive +#V/VCC and GND symbols in your actual main circuit, and the errors go away.