I have a footprint that I would like two different sized connectors attached to the same pin out. How can I add traces between the to parallel hole rows (connect them).
Must I make some type of separate schematic & pcb layout then import it in order to have connected holes?
All I see in the footprint editor is the ability to add pads but no traces?
that’s how I do this:
I needed an universal 3.81 mm socket for a simple 12V input option besides the 8 pole connector (layout):
And that’s how this works in the schematic (take note of the 12V local label):
If I understand your footprint correctly, you have the pads close enough that they overlap.
If that is the case, I would not be able to do this because one of the connectors i need to
use has an external shell requiring some space. Please clarify 
There is a way, maybe not a good way. KiCad discourages creating such traces, by disabling the option, and putting a warning message to say it is “very dangerous”. So things might go very wrong later. e.g Things like DRC and Freeroute get confused or throw errors. But given the caveat, you can create a polyline on a silk layer, and then edit its properties to be on a copper layer.
An intermediate way is to use SMD pads to create traces, this is safer but somewhat tedious, and you are restricted to horizontal and vertical lines. You may get DRC errors (pad near pad).
Personally I would not create traces in the footprint, but simply give pads that should be connected the same number. Then join them in pcb layout. This is slightly more work but a much safer option.
Wow!
That is a perfect answer… a workaround, with a clear explanation, and why I don’t want to do it!!!
That really gave me the big picture. So I guess I need to revert to making a part. I guess I will
have to read up on how to do this.
Any pointers on where I would find info on making a part would be appreciated. This dual connector
is something that I will need on quite a few circuits and I would like to only have to figure the spacing
out one time.
I did put traces in there between the pads that needed connection.
I just moved the pads so close together as I need space for a PE copper fill area otherwise they would be further apart as the connector housing of the 3.81 mm sticks over the edge of the pcb.
I did understand you so that you want two connectors connected to the same nets and I would solve that by creating a couple of labels and place the connector on the schematic right next to the other.
In the layout then just put traces between the pins that get connected from the schematic. If the connectors have the same pitch this is piece of cake, if not it needs more space naturally (or one get’s lucky or creative as I did there).
I’d also have an example for a SDcard and uSDcard slot going to the same tracks and being a population option:
Any of Chris’s videos on youtube that deal with footprints should help you there or the online help for KiCAD (might be using older KiCAD versions though, so be aware of that).
Try searching for titles such as:
As for ‘hardcoding’ the 2 different physical connectors into one footprint/symbol (together they are called a part) I don’t know.
You will get trouble in your BOM as you get one entry for 2 potential parts only and as @bobc pointed out DRC will not be thrilled about it either.
As for figuring out the spacing (if it is really that complicated) you could make you a footprint for just that purpose with markings on some of the custom layers that depict where your 2 connector footprints should be positioned?
That way you get all the goods without much extra fuzz.
As exact position markers I suggest to use little crosses that align with the anchors of the footprints (note the 2 tiny blue crosses on those SDcard footprints up there?), as those will be referencing the origin of the footprint.
Then just some outline for both footprints together and you got your placement help that you can load into PCBnew when you need it.
