Warning: Pins of type Power input and Unspecified are connected

[hbadilla]

Hello.

I’m having trouble resolving the warnings that appear in this model. I really don’t understand what’s causing them. I need help to understand and solve the issue. This is my first model in KiCad and with PCBs in general.

I previously read similar topics, but I didn’t find any information that helped me to solve it. I appreciate any help you can provide.

I am using Kicad 7.0.7 in windows

Best regards.

[retiredfeline]

Welcome to the forum.

You got the U3 symbol from an Internet library, right? Those symbols often do not have the correct pin types assigned. Probably they were lazy and just left them all Unspecified.

You have to edit the symbol and assign the correct pin types to pass ERC. Start with the official documentation here: Schematic Editor | 7.0 | English | Documentation | KiCad

[davidsrsb]

In this case, connectors correctly unspecified - there is now way to “know” it is a power input.
The solution is to add a PWR_FLAG to the net

[hbadilla]

Thanks for your answer retiredfeline.

I’m not sure if I’m interpreting correctly. Before writing the post, I had reviewed the information in the attached image. As I understand it, GND and VDD are power inputs, and that’s correct, right?

Kind regards.

[hbadilla]

Hello davidsrsb

I watched a video where they were precisely showing the PWR_FLAG. I added one for GND and another one for +3V3. The error and warning messages related to +3V3 were resolved. However, the errors and warnings related to GND are still ongoing.

Regards.

[hbadilla]

Indeed, the power_flag for GND is defined as power_output. Remember, I am new to KiCad.

[retiredfeline]

@hbadilla

GND and VDD are power inputs

Yes that’s correct. However the symbol that has the Unspecified pins is J5 (not U3 as I said). All the pins should be Passive.

[paulvdh]

@davidsrsb

In this case, connectors correctly unspecified - there is now way to “know” it is a power input.

Dealing with “unspecified” pins is a nuisance. Schematic Editor / File / Schematic Setup / Electrical Rules / Pin Conflicts Map Generates warnings for nearly all possible connections to an “unspecified” pin:

In KiCad’s default libraries, connector pins are set to Passive, which may be “less correct”, but it avoids a lot of nuisance.

[hbadilla]

I changed J5 (now J1) to passive, and almost all warnings disappeared. I have already resolved the remaining warnings. Thank you very much for the help.

[hbadilla]

Thanks paulvdh for this info. Now I know where to check first.

BR

[retiredfeline]

In general it’s difficult to assign anything but Passive to connector pins since they are non-specific. In some cases one might know that they are always another type, say a power socket pin might be Power Output. It might improve error detection a little.

[Piotr]

@hbadilla

However, the errors and warnings related to GND are still ongoing.
…
Indeed, the power_flag for GND is defined as power_output.

It is probably correct (not 100% sure as I am not using ERC at all).
The problem is that all power pins (including GND, VCC, +3V3,…) are power inputs. It is to allow you to connect them all together. What ERC checks in that subject are:

• if the net containing power inputs has also one power output,
• if there are no more than one power output at the net.

So if you don’t have at schematic something that has power output pins (what is typical for most schematics I think) than for example all pins connected to GND (including GND symbols themselves) are power inputs and ERC issues a warning or error (I don’t know). What is lacking is one power output pin connected to this net. So if power_flag connected to GND has power output pin than it is probably correct.