surface solderable link design - NO and NC by paste screen only

[julianhigginson]

So, I'm doing a board where I wanted a few different options for configuring a few different circuits on the board, and I had the idea that rather than using a bunch of 0R resistors, it might be fun to try and make some surface solderable links that are NO and NC by design, where the only difference is in the paste screen.

I have done cuttable link components with PCB traces in the past, though find they get pretty hard to operate on, even at 0603.. and you're pretty committed to any NC's made for the life of your PCB board version - so my current standard approach is just making links using 0R 0402 parts. And it's not such a horrible option, but it's nice to try new things sometimes.

So, I made a footprint that's a bit smaller than a standard 0402 footprint, opened soldermask over the whole area of the part, and extended the pads close together so I have an 0.15mm (6 mil) copper gap (the default min gap of the board I am aiming for)

The NO version has normal solder right over the pads (though I could reduce that or even take it off completely, they will be ENIG finish)
The NC version has solder right across both pads and bridging them. overall a similar amount of paste to a pretty regular SOT23 pad

Now, to be honest I'm not 100% sure this will work. I'm thinking that due to lack of solder volume coming through the paste screen, it may not reliably make the NC links after reflow. But, I'm also not 100% sure it won't work either..

If it doesn't work, I expect it's not going to be the end of the world - I'll just have 6 prototypes that need a bit of touching up before I can use them, but if anyone has any suggestions for how this is a massive mistake and I should just go back to 0402 links before I ruin everything. Or how it might be modified to work better and take up similarly small board space. Or even just general thoughts on the topic of reconfigurable prototype circuits, I'd love to hear.

[Berni]

You will need a verry big paste opening to get enough solder on it.

Whats wrong with 0 Ohm? They cost next to nothing

[Rerouter]

To increase your chances, you want the surface area of the pads to be very small, with a wide paste aperture, so the paste draws to them, but is too big to remain on the pad, using pad shapes with sharp corners will also encourage the paste to spill from there, e.g. 2 L shaped pads against each other.

However I foresee this approach leading to rouge solder balls across your design,

[julianhigginson]

Hmm.. solder balls are no fun. Unmade NC links are one thing, but I'd rather not get lots of solder balls on a board that also has fine pitch leaded parts on it...


Nothing particularly "wrong" with 0402 0R parts, though they do cost money to buy, source, ship, handle, and place... And they take time to rework if you want to change them. dropping and lifting a blob of solder seems like it would be faster.

But mostly I thought it'd be interesting to do something new, more to have as another option in my toolbox than as something 100% necessary today.

[Rerouter]

If you want to just go with solder blobs, then you should use a different pad design anyway, I tend to use 2 interlocked "U" shapes with solder mask between, as its really easy to form a fillet, and breaks clean with desolder braid.

[chickenHeadKnob]

If you want to just go with solder blobs, then you should use a different pad design anyway, I tend to use 2 interlocked "U" shapes with solder mask between, as its really easy to form a fillet, and breaks clean with desolder braid.

Or a chevron, (a triangle in a Vee). This is what is on stm nucleo boards to set options.

[julianhigginson]

If you want to just go with solder blobs

well, first up I want them to be defined as either NC or NO in my design so I can have them set either way in normal production, and ideally have them reliably form as intended when the solder paste is reflowed.

After that, I'd like to be able to quickly adjust them if I need

you should use a different pad design anyway, I tend to use 2 interlocked "U" shapes with solder mask between, as its really easy to form a fillet, and breaks clean with desolder braid.

cool! what sort of size are these?
Do you get solder balls forming much?

[julianhigginson]

Or a chevron, (a triangle in a Vee). This is what is on stm nucleo boards to set options.

Aaah, yes! I have some of those boards kicking about. Will have a look ASAP.
Do you know if they set them to both NO and NC configuration in production, or are they always N.O. links that are easy to manually solder if you want to make them?

[chickenHeadKnob]

Or a chevron, (a triangle in a Vee). This is what is on stm nucleo boards to set options.

Aaah, yes! I have some of those boards kicking about. Will have a look ASAP.
Do you know if they set them to both NO and NC configuration in production, or are they always N.O. links that are easy to manually solder if you want to make them?

Normally open on the underside of the stlink-2 portion and on the target portion as well. Documented in the user manual:https://www.st.com/content/ccc/resource/technical/document/user_manual/98/2e/fa/4b/e0/82/43/b7/DM00105823.pdf/files/DM00105823.pdf/jcr:content/translations/en.DM00105823.pdf

[Rerouter]

For mine, they are always NO on the PCB, just 1 design,

The traces are 0.4mm wide, with a 0.2mm gap.  The U shape means at the edge the solder tends to overlap the center trace before it gets big enough to roll away,

Still never used it as paste defined, just manual spotting. but the goal is to have the solder fall over a gap where you want it to, and not escape, the only way I can think to make it reliable is to give it enough copper to be able to pile up on if it moves, while still wanting to jump the gap, My best guess would be something like this with no solder mask apart from on the center Via.

Blue is meant to be copper, purple the paste later,

[Philfreeze]

See the attached picture for how we do it, the bottom one is the current version and seems to work better but it is also a lot bigger.
The top jumper is exactly as big as a 0402 footprint and works good enough (I think we have a bit more paste on it than I did (I recreated the footprint because I am at home).

[PCB.Wiz]

Now, to be honest I'm not 100% sure this will work. I'm thinking that due to lack of solder volume coming through the paste screen, it may not reliably make the NC links after reflow. But, I'm also not 100% sure it won't work either..

You are right it will not yield 100%, but when that happens, some paste is better than none when it comes to the manual touch-up.
We've use 0402 with paste as a pre-primed jumper, but we do not 'hope' it will bridge, we just use the paste as a manual soldering aid.

If you want better yields, the co-axial design above looks better, as it 'gives the solder paste little choice' - I'd expect anything will not give 100%

[mdszy]

For whatever it's worth, I found this on the internet as well. Look like some pretty decent SMD jumper designs.