All VCC become GND

Hi all,

My Little Arduino Shield: I annotated all components, run the ERC, generated the net and saved the schematic. Everthing went fine, no error or warning indication whatsoever appeared.

But when I clicked the Pcbnew, all VCC related pads had changed to GND. In the Pcbnew’s List no VCC was listed and hence even a manual correction was impossible.

I’d appreciate help.


  1. List item (688 Bytes)

sorry , 1st upload was empty (688 Bytes)

You need to archive the project and upload it. You have just supplied the project header file

1 Like

Next try with an Eeschema.jpg file.
I didn’t dare to try a 3rd time with the KiCad files, since it wasn’t clear to me which of all (!) files were to upload providing the necessary problem description.

This is just a theory, but it looks like there are hidden pins on the U1 Units. I think that because you apparently are connecting to something with the VCC and Ground wires. I wonder if all 4 of the units for the U1 symbol have hidden VCC and GND pins on the top and bottom and by stacking them like that you have inadvertently connected them. (If so, I can now add this to my reasons why I eschew hidden pins in anything but power symbols…)

To test this, try separating each of the U1 Units by one grid space and send to the PCB again. See if your VCC pins are now VCC pins instead of GND pins.

Not related to your issue, I do have an observation and a question about your circuit…

  • It looks like you applied the PWR_FLAG symbols somewhat randomly (probably to resolve ERC errors?). While your implementation works, maybe if you move the PWR_FLAG symbols to the source of its connected power net (where the electrons are coming from) you can take advantage of the otherwise visually useless PWR_FLAG symbol to indicate the source of power. For example, move the +12Vs PWR_FLAG from the voltage input of the buck regulator to the cathode of the diode.


  • Speaking of the buck regulator… Why do you have it’s GND connection unconnected? Why are you taking the output (Vin) on the FB (feedback?) pin instead of the OUT pin? There might be a good answer to this as I haven’t bothered to look up a datasheet for that buck regulator. I’m just confused trying to reconcile your usage to the symbol’s pin names.

Looking for an error with the jpeg schematic is difficult. Could you send the whole project folder in a zip file?

Try to highlight (2nd icon on the right toolbar) the GND wire in order to check if the VCC wire is also highlighted.

You made may day with your advice to separate the part-symbols of my
sn7407 Hex Buffer. Retrospectively it seems to be obvious and certainly
all pundits had known it anyway.

However the power pins of the IC are - hidden or not - denoted as implicitly
connected to VCC and GND, respectively. This means to me no ecplicit wiring is required
as long as appropriate VCC and GND labels are specified in the
schematic. At this point I have to stand up for the TINA Design and
Analysis tool. Although TINA features sophisticated electrical analysis
and simulation of the schematic, there is no such bizarre thing like
‘connected but not driven pins’ and ‘power flags’ needed in addition to
power supplies and labels. For my Hex Buffer I had simply defined a Macro
to - implicitly - take care of all the hidden pins and later invisible

Besides the power flag concept which I account as legacy I pay all
respect to those who made this amazing KiCad tool work and available to
the open source comunity. Especially the powerfull and instant
interaction between schematic and pcb made me to stop using Tina

Back to my problem and following the given hint, in a first try I took
the IC apart and wired each module separately. Ugly but it worked.
In a next attempt all wires were removed and the modules piled up in a
staggered stack, hoping for the magic ‘implicit connections’ to the existing VCC and GND
power flags. Negative.
After making the hidden pins visible I noticed they are labled in upper/lower case letters.
Although ERC makes a remark and accepts VCC and Vcc as look-alike, Pcbnew doesn’t tolerate the spelling difference.
Finally I attached an extra label /Vcc/ to the VCC power flag and an
extra label /gnd/ to the power flag GND and - the implicit connection

The solution might not receive absolution from KiCad founders, but
after hours of wasted time for such a simple matter I will stay with it.

Concerning the buck regulator I have to postpone the issue till next
Thanks for all attempts to help solving my prob.

There is a technique to break the power pins of an IC out on an additional unit. In the very long FAQ entry Tutorial: How to make a symbol there is a walk through of creating a multi-unit symbol (6th post on the thread) and the second half of it shows how to create a power-pin only unit on a multi-unit symbol.

In addition to the above FAQ entry, you may want to read these two (in addition to any others you want to read…):

And instead of simply looking through the un-ordered list of FAQ entries, here is the post with the index of FAQ items (including items that aren’t in the FAQ forum area):


@SembazuruCDE is correct, the 7407 units are drawn shorting the hidden VCC and GND pins.
I am another hidden pin hater and always draw a separate power unit on these hex and octal parts. This error keeps happening.

1 Like

The power flag stuff might be badly communicated but it is far from legacy. It is a very powerful check against a common mistake. Maybe it should de made even more powerful by allowing to define valid supply ranges.

What is however legacy is the use of hidden power pins to supply ICs. We have not (yet) come around to fix this for all symbols of the official library.

1 Like

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