What is an ideal layout for a normally-open solder jumper?

Question

We would like to make a normally-open solder jumper between two 50x50mil unmasked square pads. I've seen this kind of thing by others and would like to replicate it in our layout. We tried a simple layout with ~10mil spacing between 50x50mil pads, each with a solder mask expansion of 1.5mil. The result was surprisingly difficult to bridge.

Ultimately these are the goals:

1. The jumper should not bridge with a "normal" amount of solder paste. (We are not using a stencil, but for example's sake, lets consider a "normal amount" to be that which would be deposited with a 5-mil thick stainless stencil.)
2. It should bridge with even more solder paste, but (subjectively) we want to balance accidentally bridging vs needing a large solder blob.
3. When we bridge, we wish to bridge by manually placing a larger amount of solder paste (by syringe) over the jumper and heat it with hot air.

This is approximately they layout we are thinking, but are unsure of the spacing and stub sizes. Both the stub and the 50x50mil pads are unmasked:

Questions:

1. What would be an ideal solder mask spacing between the stubs that protrude from the 50mil pads?
2. Should there be solder mask expansion around the pad, and if so, how big?
   • Should there be a negative solder mask expansion?
3. How wide should the stub be in the vertical direction as pictured above?
4. How far should each stub protrude toward the other in the horizontal direction?

Answer 1

Take this layout:

 |¯¯\ \¯¯|
 |__/ /__|

Just make the arrows better than I did here :D

Slide with solder left to right to close, right to left to open. Reduce the gap to a minimal safety size. I'm sure they're already defined in the standard CAD programs libraries.

From Jumper pads for I2C addressing

Answer 2

The correct answer is probably: there exists no ideal layout.

Or at least none which the PCB CAD and/or manufacturer will approve. Usually the default clearance area around a pad/trace is too wide to enable a correctly done solder joint, which more or less requires no air gap at all. Regardless if you use solder mask or not there.

The result was surprisingly difficult to bridge.

Bingo. I have tons of production experience from these and therefore I can tell you with some confidence that they will be a recurring quality problem. The design itself assumes that the technician makes a poor, cold joint on purpose. The result can then be one of two options:

• Either you get a poor, cold joint as per design, in which case the connection is questionable.
• Or you get a correctly wetted joint, which either creates a not connected gap or at best "hanging by a thread". In which case the connection is questionable.

Either way, you get something unsuitable for oxidation, shock, vibration and so on. By design.

Furthermore you can likely forget about using hot air/oven and solder paste because, as you have noted, that makes it even more difficult to create the poor, cold joint you are looking for. Essentially the cold joint has to be applied by hand soldering.

The even dumber version of this is the one where you expect the technician to cut open a default-shorted trace between the pads using a scalpel. Which may leave copper residue behind, or worse, cut down into copper in the layers below.

So my conclusion from long use of various "solder bridges" is simply that they are bad engineering. I've banned these in new designs within my organization. But mind that my experience is exclusively from industrial/automotive/outdoors environments.

Consider using a component instead. Some examples of alternatives:

• Through-hole header strip with jumpers.
• Through-hole header strip which is not actually mounted, but instead a 'U' shaped, gold-plated/flash tin piece is placed in the holes and soldered.
• Decent quality dip-switches (washable recommended, no matter if you actually wash the PCB or not)
• 0 ohm SMD resistors

Answer 3

I have soldered a fair bunch of such jumper pads open/close, and in my experience they are all inferior (take longer to rework) compared to SMD pads on which you can place a zero-Ohm resistor. Either the gap is easy to close but getting it open again requires you to remove excessive solder, or it's easy to open by just sliding the solder iron in the direction of the gap (vertically for your sample picture), but closing it requires making a rather big blob which by Murphy's law always sticks to unrelated pads nearby. And then there will be this one board which looks like the pads are bridged but electrically they are not, and you'll lose an hour to find out what's wrong.

In production, zero-Ohm resistors are way more reliable than solder bridges.

One thing to consider: always connect such pads with thin traces of a certain length, don't connect them to a GND plane or a thick trace directly, or with heat relief spokes / vias. Long traces allow you to remove the zero-Ohm resistor by heating only one pad. A strong thermal link will require you to heat both pads with a heat gun or a pincette soldering tip.

Answer 4

A slit circle works pretty well if it isn't too small and the gap is reasonable. It can be opened and closed a few times without much risk.

The best size and gap size depends a bit on how "gummy" the solder is. Eutectic 63/37 SnPb is a bit harder to use to bridge a larger gap compared to some of the lead-free solders, but a circular shape (with solder mask) keeps the solder all piled up in one place so the bridging is not an issue. Clearing it with a flick of the iron might be a bit more difficult if the gap is too small. Most of the ones I see on eval boards etc. are on the small size compared to what is best, in my opinion.

Of course if you can use a switch or a 0Ω resistor or a leaded 0Ω jumper it's better, and it's always best to keep users as far away from the PCB as possible especially with a hot soldering iron in their grubby paws.

Answer 5

In production, zero-Ohm resistors are way more reliable than solder bridges.

That's the most important bit of advice to give. Solder bridges are not OK even for development boards/early prototypes. Just put a proper switch in there. I'm not even bothering with jumpers on 0.1" headers for a lot of things. Mechanical PCB-mount toggle switches that will do fine in low use are cheap and plentiful.