I want to have a normally-closed jumper i.e. something that is connects two nets by default but that can be cut with a knife to separate the nets on the physical board and a header soldered in instead.
I think I’ve read most of the suggestions on the forum and some blogs but I have not found the solution.
What I currently have is a foot print with two through hole pads connected with a graphic line on the bottom copper layer. This works except that I cannot root to the pads on the same side where the graphic line connects the two pads, I get “Cannot start routing inside a keepout area or board outline” message.
Which is a nuisance or show stopper because that is really the side where I need to have two copper areas that are connected through this jumper.
I could live a DRC error but I cannot live without being able to route those pads on the same side where I have that normally-on bridge wire.
There are normally closed jumpers in the official lib. You can use them as a guide on how to make your own. (Will be found in the jumper library)
Be aware that these footprints need to be made differently for nearly every version of kicad so if you follow a tutorial be sure you check it is for the correct version of kicad.
Can’t comment on the routing problem, but here’s another idea:
Cutting traces with a knife (or whatever) is a crap idea in practice.
As much better idea is drilling out a via to remove the plating/connection.
I don’t know the application where you need to break a trace, it’s just a suggestion.
Use the “solderjumper” Footprints.
These are in KiCad’s default libraries (V5) and there are versions with 2 and with 3 pads, rounded and square corners etc.
solderjumper means that it is in effect normally-closed, so not what what I’m looking for
drill through idea is good and that is an option for the customer because my footprint has two through holes
Looking into the standard library was a good suggestion and the answer is that the copper that makes the bridge needs to be a polygon, not line. Apparently (my guess) there is a bug that the polygons are not included in the keep out check (or perhaps it is a feature). Anyway by using a polygon as the bridge it is possible to route those through hole pads.
As for the polygons not being checked by DRC, this overlaps with my own memory but I’m not sure about the details.
You can also have a look at the footprints in the “NetTie” library for examples of this.
If you want to go the “via” way, then you can very simply make a footprint for a single THT pad, add some silkscreen text etc. The disadavantage of this is that once it’s drilled open, it’s hard to close again.
If you use the bridged solder jumpers, you can close them again with a dab of solder after you’ve cut them open.
If you want both, then you can for example take a 0603 footprint, connect both sides with a narrow polygon and put a THT pad in the midddle. Then you can drill out the pad, and solder a 0 ohm resistor over it to repair it.
Or just use regular Resistor footprints in the first place, and you can have different configurations whether you place 0 Ohm resistors on the BOM or not.
These are the most common options.
You have to decide what fits your application best.
If you have interdigitated pads, no solder mask, and full paste cover, you should be able to come up with something that will be solder bridged during reflow (normally closed) but can be cleared with just an iron. Having to take a drill to your board sounds silly.
Depends on one’s definition. I always thought of solder jumpers are jumpers that can be closed by bridging with a blob of solder. (Instead of using header pins and a shorting block.) Usually SMT pads close together. Within that classification I recognize NO and NC solder jumpers. The NO solder jumpers are nothing more than isolated SMT pads close together and the end-user closes the jumper with a blob of solder. And the NC solder jumpers have a solder trace (apparently in KiCad a narrow copper polygon for DRC reasons) connecting the SMT pads and the end-user has to cut that trace to open the jumper, but then use a solder blob to re-close the jumper.
Easy to confuse my small brain - I guess I’m missing something…
It seems to me, you want a simple jumper from one pad to another pad. And, you want both Jumper and Silk on Bottom layers.
Regardless of which layer, you could use the Jumper/THT I show in the link I posted. However, if Not wanting a jumper with Bends, it’s the same process and Type of Pad (SMD or THT) is up to you. You can make a footprint with SMD on Back layer - easy to do (I did not bother to do it for this example - why waste time if I miss-understand your goal…)
Image below shows:
• SMD with Straight-Wire Bridge on Front layer.
• THT with Straight-Wire Bridge on Front layer.
• THT with Straight-Wire Bridge on Back layer.
@BlackCoffee You got it correctly (except I had not thought about the silk on botton, but that is a good idea). In fact the right most in you first pic is the thing.
I did look through you video, thanks.
As I tried to convey the problem is now solved and the key thing (which I only posted for posterity) is to use polygon not graphic line for the bridge, otherwise I cannot route it.
@SembazuruCDE To me Normally On is the same as Normally Closed for switches. Regardless of the definition I explained what I wanted to achieve. Most users I expect will never cut a single trace so it makes sense that the signal is routed/connected by default from factory. I only provide this possibility for the rare user who abs needs to cut it.
I (and most of the industry) use switch notation everywhere so I don’t have to think about which notation that I’m using. In my example NO didn’t mean Normally On, rather it meant Normally Open. (And your mentioning is the first time I can recall hearing a jumper state referred to as “Normally On”.) Whether a jumper is a logical on or off depends on whether one is using pull up or pull down resistors and/or whether using active high or active low logic. Though, I suppose that is why you are boiling all the details of open/closed or high/low down to your desired effect of on/off.
I’m glad you got where you were going, granted your posts above are confusing. You started this thread asking for a NC jumper:
And then after a few answers you replied back saying that you don’t want a NC jumper.
