Easiest way for one to one connections

[Phozer]

I have a silly question but i want to make a one to one connection of those two Connectors. How do i do that in the easiest way possible?

With Net names? Or put them on top of each other? That seems to connect them (the circles go away).

[Jonathan_Haas]

Would probably be easier to use symbols that have the connections all on one side and then just mirror one.

[eelik]

Intriguing question. I tried what Jonathan suggested. It takes about one or two minutes to edit the KiCad symbol:

1. Select all pins from one side using box selection.
2. Mirror with X.
3. Move with M.
4. Select all graphics next to pins which were left after moving the pins.
5. Move them.
6. Select the graphic rectangle body.
7. Drag one corner to make it taller.

And that’s it. You have to save it to a personal library.

It’s OK to connect symbols directly together without using wires, although it’s easy to copy and paste identical wires directly between the symbols, and wires may look better or “more professional”.

In any case editing the symbol is much quicker and easier than drawing good looking wires for the original symbols:

Writing labels can’t be automated easily, either.

EDIT: on second thought, there already exist Conn_01x40 symbols, why not use them… The only upside of creating your own is that you can easily see the difference between left and right side pins because they are grouped together. You know what you need.

[Piotr]

@eelik

although it’s easy to copy and paste identical wires

I would rather use INS key.

@eelik

Writing labels can’t be automated easily, either.

When you place label ‘WIRE1’ and then press INS key you will get WIRE2, WIRE3,… WIRE10, WIRE11 and so on placed just like you need them (depends on some settings, but default is OK).

[retiredfeline]

You could also draw the connections through one of the connectors. Nothing says the wires have to avoid the inside of the connector symbol. Here’s what I did in my schematic.

Of course this works only when there is one column.

[paulvdh]

The simplest way is to put the two connectors on top of each other, and then drag them apart, but you have to do it diagonally, or you will short the left and right pins of the connectors.

Therefore, single row headers are easier. 40 pin single row headers are also default symbols, so no need to modify it. It is good to practice a bit with rotating and mirroring blocks of pins in schematic symbols. I also do this regularly with for example I/O ports of microcontrollers, to have them appear on my schematic where I want them.

With Single row headers, you can simply:

1. place two of them on your schematic.
2. Mirror one, and place the connection points on top of each other.
3. Drag it aside a bit, and wires appear.

Using the repeat function with the [Ins] key, as piotr mentioned is also a function you should get familar with.

[Munyua_wa_Mugo]

Connect one of them then use mirror to finish everything. Or you can use label symbols in all pins and link pins with similar labels together.

[Phozer]

Thanks for your advice. I thought that i couldn’t assign a 2x20 Footprint to a Conn_01x40, but that’s possible. So i placed the two Conn_01x40 facing each other, drew the first line and completed the other 39 lines with insert. Then i assigned the 2x20 Footprint to the symbol.