Footprint not connected to Symbol

Version: 5.1.2-f72e74a
OS: Ubuntu Linux

I have created a Circuit diagram and connected the Symbols to their proper Footprins via the assign PCB footprints diagramm. There are three connectors in the PCB. Two 2x5 PinHeader and one 2x30 PinHeader

For the 2x5 I chose the Vertical Version (Conn:02x05_Odd_Even : Connector_PinHeader_2.54mm:PinHeader_2x05_P2.54mm_Vertical) all is fine and dandy.
For the 2x30 I chose the Horizontal version (Conn_02x30_Row_Letter_First : Connector_PinHeader_2.54mm:PinHeader_2x30_P2.54mm_Horizontal)
When loading the Netlist there is a ratsnest to both 2x05 but none what so ever to the 2x30.
Do i have to specify which via is a1?

Without screenshots of the schematic and the layout it is difficult to answer. We don’t know how the connectors are wired in the schematic.

Or better if you could attach the project.

1 Like

Well there is your problem. The symbols pin numbers must fit the footprints pin numbers. The footprint you chose uses odd/even numbering while the symbol uses bga style numbering.

Use the _OddEven symbol for connecting with pin headers.

More details: How does KiCad know which symbol pin represents which pad of the footprint?


If your schematic wires are properly connected to the 2x30 connector the small circles around the pins disapear.

Then run an ERC check in Eeschema, does it complain about unconnected pins?
Then, while transfering the netlist to Pcbnew, carefully read all warnings and error messages.

I suspect that the 2x30 pin connector on the PCB is somehow not recognised by Eeschema. You can simply delete it and then when you transfer the netlist to Pcbnew again, it should also import a new 2x30 pin connector from the library.
If it does not do this, then the link to the footprint for the 2x30 pin connector in Eeschema is faulty. You should then choose the right footprint for it before transfering the netlist & components to Pcbnew.

It is a normal process to do this multiple times when schematics evolve. During import in Pcbnew you can even choose if you want to keep or delete unused components during import.

Your info is correct in general but i doubt it is the problem here. As mentioned above the most likely problem is that the wrong symbol was chosen for the footprints.

This does indeed look like a wrong footprint:

To me this does not read as it would have anything to do do with the odd/even numbering.

If none of the nets connect to the connector, then the whole footprint is somehow not recorgnised.

This is because the symbol selected uses pin numbers like a1, a2, … b1, b2, …
The footprint uses 1,2,3 (no matter what order on they are in there will be not a single match resulting in no schematic connection being transferred over to the layout.)

Missing connection can of course be additional problems. But there is as of yet no evidence that this is the case (only if changing the symbol does not resolve the issues could we say anything in that direction with any amount of certainty)

Good reason.
If the schematic pin numbers has letters and digits, and the PCB footprint only has digits then there is no way the nets can be connected by KiCAd.

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