Symbol and footprint for "bodge wire"?

Anybody have a good way to put a bodge wire in a schematic, and suitable footprint for it?

This is kind of like a two-pin option jumper or zero-ohm resistor (for which there are symbols and footprints) but doesn’t have a typical footprint… just a physical piece of wire that connects between two existing pads. Two pads that are some random distance apart.


When I wanted to add such wires in my 2 layer PCB (it was before I started to use KiCad) I just changed PCB to 4 layers (only in software, I didn’t send extra layers to PCB factory) and used one layer for these connections using pads (instead of vias) to jump to that layer. Then this layer picture was a instruction what points have to be connected with wires (I had only 3 wires at those PCB). I didn’t show those wires at schematic (like it would simply be connection made on extra layer).

Huh! That idea certainly has promise!

I was hoping to make the “bodge wire” a component so it would

(a) show up in the BOM.
(b) preserves the separate net names of the nets that are joined by the bodge.

But I do see how your “bodge layer” scheme deals with the variable length aspect.

Isn’t this similar to the question one sided PCB people* ask about how to design with jumpers, with the same solution as given above, a “jumper” layer?

* People who use one sided PCBs, not people made of one sided PCBs. :rofl:

PS: I suppose there could be different solutions depending on whether it’s an intentional bodge or not. Normal wire for the former, symbol for the latter.

Aren’t they electrically the same net?
If you route a track swapping layers several times you don’t mark vias on the wire at schematic.

As I know KiCad allows (at least I have read something like this about KiCad V4) to modify footprint after placing it at PCB. So you probably can have one bodge wire footprint and then move its pads on the PCB.
But I prefer my method assuming this wires as being extra layer. I had only one such PCB with 3 wires. Later the IC manufacturer issued new IC revision and I was able to route it using only one layer (second is continuous GND). If you have lot of such wires than having them automatically listed in BOM has advantages so …

I made this Bodage Wire a couple of years ago, Footprint and 3D-STEP.

It’s size is 42mm X 3mm

Here’s the footprint - you can Edit it but can’t Edit the 3D-Step. The Step isn’t important for anything other than a Photo so, it’s not needed…
Bodge_40x3mm.kicad_mod (1.2 KB)
BodgeWire_40x3mm.step (14.5 KB)

With respect to a Footprint/Symbol, a Bodage is nothing more than a drawing of a Trace and placing Pads on each end…

Footprints can link to 3D-STEP and/or WRL so, you can do this if wanting a different size…

• Start a New PCB
• Draw a Track of desired Width/Length on the PCB Top layer
• Add Pads (THT or SMD) to each End of the Track
• Draw a PCB shape on Edge-Cut layer
• Place Origin (Drill) at center of the PAD
• Export STEP

Now, load the STEP into the Footprint

Screenshot shows original and a newly added one done as described above… I left it placed at 90deg for visual clarity…


So what Symbol do you use this with?

Also, am I correct in assuming that since your footprint has two separately-numbered pins, it does not connect the two pins electrically, so far as DRC is concerned? (This happens to be what I want, though I can imagine the opposite in other situations.)

I agree with you 50% :slight_smile:

There are some times when the bodge wire is an intended part of a single net you established on the schematic, or the bodge wire is to fix a mistake in the PCB that omitted an intended track for a single net.

Other times, the bodge wire might implement a later-defined option or fix. For example, in some application it turns out that you get better noise performance if you bridge “Analog Ground” and “Digital Ground” at a particular location, but you want to keep the rest of the nets separate. (like you might do with a Net Tie, but it’s an added physical wire).

So both options are interesting.

Your point:

modify footprint after placing it at PCB.

Yes, that seems like a good way to accommodate the random length needed.

And for those wondering, if you place more than one of a particular footprint on a PCB, each one is separately editable. (ie: You’re not just editing a single “project-local” library footprint.)

I make my own Symbol(s) and they are so simple to make… Plenty of Posts and Tutorials on making symbols. They can be as simple as a single line or, complicated… you decide what you want them to be.

Regarding the Terminal Numbers… That’s also up to you - they can be the same or different. And, for DRC/ERC you can create Rules and/or set clearances/etc or, Ignore the errors…