Vias under symmetric pcb pads designed to wick solder - Page 1
Forum section: electronics / general

author: nachus001
author_rank: Contributor
timestamp: April 05, 2024, 05:01:11 pm
content: HelloI have a question for a PCB design.I need to know if is it feasible to connect two pads that are aligned in top and bottom side of aPCB thru an in-pad via, and expect the via to wick some solder and get filled with it, at least partially.The connectors (top and bottom) are equal size and pin count.Eventually, I may accept that the vias don't wick solder, but in that case I'd need two vias under smd pad and I don't knowif that would solder-starve the joint.My idea is to connect two aligned connectors on top and bottom of a PCB in order to allow a pcb stackupand to avoid copper plugged vias or any other via filling procedure (more $$$)Thanks in advanceNachus

author: ataradov
author_rank: Super Contributor
timestamp: April 05, 2024, 06:22:29 pm
content: It really depends. At a typical 0.3 mm via diameter, some vias will end up as through holes and would wick some solder. But others would end up plugged with random leftovers from drilling and plating. With larger diameter they are more likely remain open. Vias that are open will wick the solder. So, your big concern here is that different vias will behave differently, making calculation of the optimal solder paste amount impossible.And another issue would be mounting of the second side after the first one is soldered. If some solder wicks, your pads will be uneven on the second side.I don't understand the part about two vias per pad. If the vias don't wick the solder, then a single via would be enough.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: April 05, 2024, 07:31:15 pm
content: I don't like it, because a partially-wicked (from both sides) via will trap gas and can create voiding or blowouts. Maybe it's less an issue here than for LGA and BGA: if that's a gull-wing style joint, the fillet probably closes up pretty quickly once a bubble goes past, and bubbles may have an easier time getting out the side fillet than they would a blind pad.You're most likely doing it by reflowing one side, then the other, in which case the vias are plugged from one side, and then for 2nd reflow, you have the geometry of a one-side-tented via that traps flux/gas.It might be viable to fill them with solder; this won't be easy to ensure with a lead-free process I think, but using larger diameter (0.4-0.5mm say?), and leaded solder, with suitable flux (if it's ENIG, pretty much any will do, but suffice it to say, a combination between solder and plating that gives good spreading), would give the best chance for it. A little excess paste may be helpful, but mind how it spreads out on heating, and it may be trading off with leaving solder beads on the surface.Could also go over it by hand before assembly and fill and inspect, or even, like, shove bits of solder wire into the holes just to be absolutely sure it's pre-loaded, but, between the large labor input, and the potentially uneven surface before pasting, that's probably worse overall.I did a design something like this some years back, it was for a gas-tight (not necessarily hermetic) joint between two grid-style connectors; I opted for blind vias, I think, and had enough room not to need filling or anything (dogbone traces). One thing that stands out in my memory, it was a, Samtec something connector I think, that suggested N2 or other inert atmosphere for reflow... fancy.Tim

author: nachus001
author_rank: Contributor
timestamp: April 05, 2024, 08:09:25 pm
content: Quote from: ataradov on April 05, 2024, 06:22:29 pmHello Ataradovsupposedly, both connectors are going to be soldered at once since some boards have parts on top and bottom. The idea is to place the vias in such geometry that they wick solderfrom both sides at once. And it they trap air inside, then put one more via per pad.The idea of solder filling is to increase their current capability, specially on the vias that conduct battery current and ground currents. I think that filling will improve the via resistance and inductance. (these are header connectors of 1.27 or 1mm pitch)For the rest of signals they will be carrying gpios, uarts,i2c/spi/can, and of course power signals. Maybe (i have to check the physical standard) there may go one or two MIPI-CSI ports, but I'm not sure as yet.Quote from: T3sl4co1l on April 05, 2024, 07:31:15 pmHi Timanother solution that came to my mind would be to use two vias per pad and divide the pad with solder mask and tent the via hole in pads, then eventually provide a third via untented and separatedfrom the pad wit its own paste mask aeperture.Nachus

author: ataradov
author_rank: Super Contributor
timestamp: April 05, 2024, 09:22:54 pm
content: Quote from: nachus001 on April 05, 2024, 08:09:25 pmThere is no technology that would allow that. Double sided boards are still populated and soldered one side at a time. The way components are mechanically held on one side while reflow happens on the other differs, but often it is just surface tension of the solder. Sometimes connectors need to se soldered as a separate step. It all depends on the overall design.Quote from: nachus001 on April 05, 2024, 08:09:25 pmFor poser pins specifically place more vias outside of the connector.

author: Doctorandus_P
author_rank: Super Contributor
timestamp: April 07, 2024, 01:26:30 am
content: You can think up a lot of weird solutions, and they may work, some may even work quite good, but the problem usually is to get them to work reliably in a production environment. What if you build 10.000 boards, and 0.2% of the board catches fires because of badly filled via's?But that said, I would probably not place such via's in pads, but design a simple footprint consisting of one THT pad, and combine that with an opening in the soldermask (stencil) to get the amount of solder in the pad that I want. Do note that (at least in KiCad) it's easy to make the solder mask cutout bigger then the pad itself. The solder paste will wick into (or at least onto) the pad during soldering. This method is sometimes also used in a production environment to get more solder onto a pad and apparently works reliably.As an alternative, you can place simple THT headers onto the PCB. Not to connect anything, but just to get a piece of metal that goes through the PCB.