Insert 0R footprint instead of a VIA?

[DL1AKP]

Hi there,

is any usable method there to insert a 0R 1206 footprint instead of two via’s and a wire on another layer?

I normal cut PCB’s by myself and a one-layer PCB is faster and cheaper be built.

Thanks so much for info.
Andy

[eelik]

Do you mean that you have the functionally complete schematic, then you begin routing the board, and then you want to add 0ohm resistors as you go on routing?

I would probably do it first with two layers, using vias. After completing the whole layout I would take each via pair, put a net tie symbol with the resistor footprint in the schematic to a proper location and update the board, replacing the pair of vias with the footprint.

When I think about this, if you have a simple board, it could be possible to do it even without the back-and-forth procedure. You could draw a special symbol which has two pins and empty space between them, mimicking two pads with empty space. Then you could draw the routing in the schematic so that the wires don’t intersect but go through these special symbols. Needless to say, this would be a hack and you shouldn’t normally draw wires through symbols, but this could be reasonable in your case.

[SembazuruCDE]

@eelik’s answer is good.

To give you more options to choose from, another similar idea that I’ve heard other people doing is layout as a 2 layer board but only export one layer to etch/cut. Keep the traces on the non-copper side as short as practical and straight. Use vias that match a THT wire pad, and then during assembly use the non-copper side trace layout as a guide where to solder wire jumpers. The down-side for fully SMT designs is now you will need to drill your board. Though, I suppose you could design your vias to provide a good SMT pad to solder wires to. You will be restricted to round dots, but that shouldn’t be a problem. Depending on your output path from KiCad you can skip putting the holes in the via pads.

[DL1AKP]

Hi guys,

both are good ideas. I’ll give it a try.
I know that I can use the second layer and put wires instead of the layer.
But my intention was to do it on PCB with just SMT components on it.
So solder wire jumpers are not the solution.

I just thought, there is some “button” to klick on to “place 0R resistor”.
Because I’ve seen lots of PCB with those 0R’s on it.
Maybe I thought too simple…

Andy

[pedro]

After having read the proposed solutions I think they can be mixed.

A footprint can be added without being included in the schematic. Let’s think of a 1206 smd footprint.
Route the pcb with vias and tracks on the other layer but keep the vias at a 1206 distance.
Last thing, add a 1206 footprint and place it on the vias. Vias will be covered by the pads. No need to drill holes.
Warning: just in case you decide to update pcb from schematic or modify the netlist, the new footprints must be locked. Otherwise they would be deleted because they are not in the schematic.