Electronics > KiCad

Best way to implement jumpers in KiCad?

(1/2) > >>

John B:
I want to implement some manual jumper points on a 2 layer board, mainly power rails and such, but I'm having trouble finding what the best way to implement it is.

Ideally I would like KiCad to recognise both end points of a jumper as the same net, but I would like 2 separate footprints. Eg, something like 2 separate plated through holes, but KiCad would automatically recognise them as connected (maybe through an invisible layer that isn't included in the gerbers?)

That way you could place either footprint anywhere in the PCB and the DRC would still recognise that anything connected to those pads are also connected to one another. (so you dont end up with "islands" of unconnected nets)

retiredfeline:
I haven't seen any good way of doing this, especially if the nets are connected is conditional on the jumper. But why require them to be the same net? It only elicits a warning from ERC (not DRC) if a net is not driven. Judicious use of the PWR_FLAG (inappropriately named for this use case) should satisfy ERC.

julian1:
Have you seen how a net-tie symbol works in kicad? It breaks a net, but is electrically closed, because the footprint pads are joined by a copper trace.

You could probably achieve what you want using the inverse approach.  ie Create a symbol with two pins, where both pins share the same pin number (eg 1) so the net is not broken. Then adapt an open (when unpopulated) footprint jumper (smd R) by assigning both pads the same number.

In general such tricks should be avoided, because they break assumptions and add to complexity.

golden_labels:
You may use labels to directly name your nets. If wires bear the same label, they are treated as a single net.

Alternatively you may divide your schematic and simply put a jumper with both ends connected to nothing except the same power symbol (e.g. VCC). Preferably close to a segment that describes the power supply — for clarity. Of course that symbol will also need PWR_FLAG, but it only has to be placed once for the whole schematic and most likely you already have it in the power supply section.

The downside of both approaches: in PCB editor you will get no warnings if you connect your devices to the wrong side of the jumper.

pierreraymondrondelle:

--- Quote ---Ideally I would like KiCad to recognise both end points of a jumper as the same net, but I would like 2 separate footprints. Eg, something like 2 separate plated through holes, but KiCad would automatically recognise them as connected (maybe through an invisible layer that isn't included in the gerbers?)

That way you could place either footprint anywhere in the PCB and the DRC would still recognise that anything connected to those pads are also connected to one another. (so you dont end up with "islands" of unconnected nets)
--- End quote ---

Please have a look to this post: https://forum.kicad.info/t/multiple-pcbs-from-single-schematic-take-2/32798/17, from messages #14 to 17 & 19. The trick is to fool kicad with both the symbol and the footprint.

Navigation

[0] Message Index

[#] Next page