How do I force to use wire names?

I have some wires with labels where the wire name is being replaced by the part pin name.

How do I force the label I applied to the wire instead of the name of the pin?

Here VINT is the name of the Pin in the Symbol while 5V is the hierarchical name.

Here VBUS is the Pin name of the USB connector, and USB_SS3_VBUS is the label in the wire that connects this pin

It looks like Kicad is choosing the wrong name (for me) as its default choice.

KiCad does not use auto generated names if a label is present.
All power symbols are global net label names.
I’m almost certain that “VINT” is a local label somewhere.
Same for “VBUS”.

I am confused by:

Unless you have defined those schematic symbols as power symbols. (which is probably a bad idea).

Auto generated net names have the form of: “Net-R4(Pad1)”

1 Like

Cool. I could track this symbol U19 may be the culprit.

It connects both problematic wires.
Also both B1 and C2, are a stack of other pins.
They are all power inputs if this is important

Also, removing the symbol or disconnecting it from 5V and USB_SS3_VBUS fixes both issues.

Now, this component looks good.
It is not a power symbol. It is updated with the library too.

Its properties look fine.

Pins do not look wrong too.

I have these messages on this component. I did not know that components had this info.
But they look normal unless I am misunderstanding something.

[Off-Topic] This extra. This window is malformed.

Ah, this last window says it all.

Hidden power pins will drive their pin names on to any connected nets.

This looks wrong. Why something hidden has precedence over visible things?
Also, since the pins are stack up, the visible pin should dive the name. Not the hidden pins.
Also, if the wire has labels on it, it should override this, for sure.

This is a legacy issue and it’s the way the global power port symbols work. (You could examine the global “5V” or “GND” symbol).
For this reason it’s advised to not use hidden power pins inside of normal symbols.

see also the schematic-documentation Schematic Editor | 6.0 | English | Documentation | KiCad , section “hidden power pins”.

1 Like

Ah, I see. Makes sense but, I have some particular configs here:

  • I am not using global labels.
  • In one place I am using a hierarchical label.
  • In the second place I am using a local label.

Well, if hidden pins are the issue here and since there is this legacy issue, I will fix my symbol.

Thanks @mf_ibfeew

Why? Based on what do you do this statement? I am asking to understand the issue.

Stacking pins is a Kicad feature. So, if it is a feature, the issue I am describing is a bug since I am forcing naming the the wires with a (local) label and also with a hierarchical label.

Power symbols and pins are bit of an organically grown wart in KiCad.

I think the recommended workaround is to only set the visible pin to a power input, and set the stacked pins to “passive”.


Ah, then this is the thing. Thanks @paulvdh

Update: Yeah, this definitely solved this issue. I thought only Power Output had issues regarding being stacked.

Sure but, partially correct. If you stack power output they are connected even before you think about connecting them in the schematics, and this will cause the issue you are saying where 2 things are driving at the same time.

I did not know that similar issue (with a different ERC message) could appear by stacking power input pins. It is an issue, but it is not kind of the same, since the issue is related with the name of the wire. And this is a Warning and not an Error too.

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.