IC footprint VCC+GND

Hi everyone,

I have a problem with the layout of an dip socket.
My schematic uses a few and, or and inverter gates.
I toke the housings_DIP:DIP-14_W7.62mm footprint.
but every time I open the pcb it makes pin 7 and 14 GND.
while pin 7 should be gnd and pin 14 should be vcc.

If I show up the invicable pins in the schematic, then it is labeled correct.
As you can see on the pictures it labels pin 7 & 14 gnd and connects them together
I also have some header pins in the schematic.
vcc and gnd should be connect to the headers.

Who is able to help me?
Thank you in advance.

With kind regards,


What symbol are you using into the schematic?
Are pins 7 and 14 connected in the schematic?

The pin name labels in the schematic could be Vcc and GND, but this pins should also be connected to Vcc and GND.


Is it possible that you used a symbol form kicad’s 74xx library?
If yes: this library uses hidden pins for GND and VCC

You can connect them by turning on the visibility of hidden pins.

The approach intended by the original developers (not a good idea in my mind.):
Use the “correct” power symbols. Hidden power pins are comparable to global labels. The label name is the pin name.
So if you place a gnd power symbol all hidden power input pins named gnd are connected to this power symbol.

Best approach (the most work for you): make your own library by copying this one symbol and set the power pins to visible.
Or even better move them to their own unit such that you have your logic and power units separated. Example:
74vhc125mtcx_mu.lib (1.1 KB)

Hi Rene,

this is precisely what i was doing.
I saw on the internet that they should connect themself.
I can make the pins vissible but then i cant connect to them.

you say the best is to make my own library.
then copy the part and make the pins vissible.
can i then connect to them to?

and how do i make my own library?
that is going to be a first for me, but it is something i would like to learn.
any sugestions or links?

thanks all for your help

I just tested it, it works in version 4:
(Did you set the correct grid? It should be 50mil)
The two as screenshot:
Option 1 direct connection using a wire connected to the invisible pin.

Option 2 (The dangerous one) Connection with the use of power symbols.

The power flag is used to tell the electrical rule check (ERC) that the power is supplied by the connector.

Yes of course. (The goal is to have them behave in the same manner as the other pins you already connected.)

It is not as difficult as it may seem.
You can look at this video tutorial:
Part two is for the creation of schematic symbols.

Short version in written form:

  • Open the schematic library editor
  • Select working library (choose the library where you got your troublesome symbol from.)
  • Open the part you want to copy.
  • Create new part from current one (give it a meaningfull name different from the one in the original library. Otherwise it will not be listed, because eeschema currently selects the first part it finds with a given name.)
  • Save part to new library (store it somewhere where it makes sense for you.)
  • Add the new library to your project (as described bellow)
  • Open your new library and your part (first two steps again)
  • Edit your part as you wish.
  • Update part in library
  • Store library to disk.

To add this library to your project you need to add it under preferences->component libraries

  • First add the path to the directory holding your newly created library. (Bottom Add)
  • After that add your library.

If you want to create the symbol as i described above you can follow these steps.
(To what i showed in the last post first. This describes the edit symbol part.)

I use the 7400 symbol as an example.
If there are two screenshots next to each other, the left one is always the original (before your changes) and the right one is the result

Step 1 change the symbol properties:

After that your screen should look similar to this:

(You should have units A to E, Unit E is a copy of unit A)

Now comes the fun part. Changing our symbol such that units A to D look the same as they did before. (But without the power pins.) And unit E has our power pins.

First select edit pins per unit. (otherwise you will edit all pins that have the same position at the same time.)

Now we make it a bit easier for us. (we don’t want to draw a lot.)
Move [press M] all graphical stuff to the side (polyline and arc)

Select the whole graphical stuff at once by draging with your mouse. (box select)
right click and select copy block.
move this copy back to where you got the graphical stuff in the first place.

Open the properties [press E] of the arc and polyline and deselect common to all units for both of them.

Change to unit B.
It should look like you just moved the graphics to the side.
Again copy the graphic, move them into position and deselect common to all units in the graphic properties.
Repeat until you reach unit D. In unit D don’t copy the graphics just move them into place and again deselect common to all units.

Now A to D should look like when we started.
Change to unit E. It should look like this.

Save your changes. (Just in case you make a mistake in the next step.)
Remove the pins 1,2,3 (make sure edit pins per unit is still selected. Otherwise you will delete everything.)
Now open the properties of pins vcc and gnd [again press E] and do the following:

When you are finished with that move your pins into the middle and the reference and value field to somewhere where it makes sense. (This fields have the same position in all units. Yes this is not a good solution.)
When you are finished your unit e should look like this.

When this is done double check that the units A to D are still ok. (Only the pins VCC and GND should have vanished from this units. All other pins should be unchanged.)

If you are happy with the result save your changes und use your symbol.
(Don’t forget the safe library to disk button.)