PCBWay issue with QFN solder bridge, what to do?

[wraper]

Lead free solder is typically not prone to wicking away from under a chip when using small holes (like 0.4mm vias). Or put differently: I have had a lot (thousands) of boards produced with small vias under QFNs and I have yet to see a board where the solder has reached the other end of the board.

IME it wicks to other side with 0.3mm vias if there is exposed copper to receive that solder. The best is plugging the vias but it costs a lot. On the other hand tenting on other side is completely free and usually is good enough. Sometimes vias get tented on top side instead of expensive plugging, right under the chip to completely eliminate the wicking. However it's only applicable for larger chips if vias are not populated densely.

[VEGETA]

They gave me the price for plugging with risen, it is 240$!!! no way I am paying that. I wonder if I ordered 100 boards, what will the price be for plugging xD

however, does removing the 4 cornered vias help eliminate this? i mean they are the only ones with solder paste above them.

I am not familiar of how to tent one side of a via in kicad... tenting them in both sides may eliminate the issue but maybe won't be firm soldering


what to do now?

[ataradov]

however, does removing the 4 cornered vias help eliminate this? i mean they are the only ones with solder paste above them.

No, the solder will flow. But that's another thing you can control. If in practice it turns out that vias capture some of the solder, you can increase the openings in the stencil, basically compensating for the lost solder.

what to do now?

Don't overthink it, just order the boards with the simplest and cheapest process and see how the soldering goes.

[VEGETA]

I think I will order them without filling for now.

I wanted something to be fully working and guaranteed for production. I don't want a good prototype then when it comes to production it would not work or some units do not work properly...etc since I cannot test all units.

for now I will order them without filling... can you suggest something for future? I mean for production, covering the vias will be relatively affordable so yes i can fill them. but gotta guarantee if they are filled, the soldering, electrical, thermal performance to be good.

For example, I can increase the 4 solder paste areas to be more... maybe slightly more than the footprint? please check the attached image for illustration. 2 images for 2 suggestions.

[ataradov]

I wanted something to be fully working and guaranteed for production.

Everybody wants that, but you can't have this in most cases on the first try. That's why you do prototypes - to figure out what can go wrong. And then before mass production you do small engineering runs to figure out what may go wrong during mass production.

PCB assembly itself is not a guaranteed process that just works 100% of the time, it may need to be adjusted for a specific board. Most of the time things just work, but sometimes they don't.  And only assembly house will be able to tell you their confidence level that your specific design will not have issues.

I don't want a good prototype then when it comes to production it would not work or some units do not work properly...etc since I cannot test all units.

can you suggest something for future?

You can just see how evaluation goes and do nothing if it seems to work. You can also see if thermal performance is an issue in your case and if you really need all those vias.

For example, I can increase the 4 solder paste areas to be more... maybe slightly more than the footprint?

All of this is tuned during the engineering runs. But generally it is not a great idea to just add more solder. The issue here is that if you don't explicitly plug the holes, they may still get plugged at random, so the amount of solder they will take will vary.

None of this is exact science and you have to deal with issues as they come up from design to design. Or commit to the most expensive manufacturing process. It is up to you to estimate what will cost more.

Also, the prices for big orders would drop, of course, so may be having smaller holes or plugged vias would be acceptable. You need to get quotes for the actual quantities you will want, don't try to guess based on the prototype prices.

Also, without prototypes, what makes you sure your design is even functional? You already almost made the boards with the wrong footprint. What makes you so sure that the reset of the footprints are correct?

You will have to build something to do the tests, and that's a good opportunity to observe how the boards behave during assembly. 

[VEGETA]

your suggestion seemed ok with me. I mean using smaller holes and plugging them then use good amount of solder to fully seal and solder the IC... all this durring manufacturing the production units.

if this batch of just 2 assembled boards worked, which it will unless something majorly wrong is there.... i will make another small batch of say 5-10 assembled boards using the 0.2mm hole vias (exactly the same as datasheet) and plugged holes.

if that also worked, then i will use it for all production in the future.

i just wanted to do one iteration of prototypes instead of 2, but as you said, can't get it right the first go.

[westfw]

I don't know how much good those "thermal vias" are going to do without a substantially more "solid" ground plane on the other side of the PCB.  A lot of those SMPS chips seem to assume a 4-layer board with the bottom layer being almost solid ground plane.

For maximum heat sinking, you WANT the vias to get filled with solder - a solder-filled via should be significantly more thermally conductive than a via with just plating or non-metallic fill.  I don't know how to balance that with the "wicking" problem that others are concerned about :-(

[VEGETA]

I don't know how much good those "thermal vias" are going to do without a substantially more "solid" ground plane on the other side of the PCB.  A lot of those SMPS chips seem to assume a 4-layer board with the bottom layer being almost solid ground plane.

For maximum heat sinking, you WANT the vias to get filled with solder - a solder-filled via should be significantly more thermally conductive than a via with just plating or non-metallic fill.  I don't know how to balance that with the "wicking" problem that others are concerned about :-(

the bottom layer is all ground plain, which is what you mentioned here.

the boards are on route to me, without resin filling. and from picture it looks like there is no wicking or spillage.

balance is what we do here xD  so kindly mention you balancing theory 

[VEGETA]

Hello

the boards arrived in Amman Jordan but will need time to get to me, will examine then but from pictures sent by manufacturer there does not seem to be any leakage.

However, I asked for a quotation of just PCB manufacturing using 3 options and here are the results:

1- via on pad without filling (our current options):
5 pieces     = 44.14 USD.
20 pieces   = 53.65 USD.
100 pieces = 93.81 USD.

2- via on pad with copper filling (what is considered to be the best):
5 pieces     = 431.09 USD.
20 pieces   = 431.09 USD.
100 pieces = 486.61 USD.

3- via on pad with resin filling:
5 pieces     = 268.79 USD.
20 pieces   = 268.79 USD.
100 pieces = 349.94 USD.


huge price increase as seen! components + assembly for 20 boards is about 500$ while it is about 1400$ for 100 boards. selling this for 50$ seems ok if I choose no filling and 100 quantity as it seems, especially that there is customs which is a giant monster here!

for 100 quantity: without filling = ~1500$ -> = 15$ per one unit + 5$ per unit as approx. customs = 20$ per unit total. sold for 50$ is kinda ok. however going for filling will make it harder. resin will make it about 23$ per unit and copper will make it more than 25$.

for 20 quantity: without filling = ~550$ -> ~35$ per unit including customs...

is 20 quantity as above good for first batch?

what will you do if you are in this situation?


if i got them as non filled, then checked the boards manually to remove the leaked solder will it be ok? or maybe reflow it from the bottom using soldering iron.

for your kind suggestions.

[ataradov]

For small quantities like this, I'd go with the cheapest option. If something fails on a couple units, you can always manually rework them. The real issue starts when you need to make 1000+ of them.

[VEGETA]

For small quantities like this, I'd go with the cheapest option. If something fails on a couple units, you can always manually rework them. The real issue starts when you need to make 1000+ of them.

so you did some manual reworking in the past? what about my suggested reworking by soldering iron is it good enough.

I don't think I will ever make +1000 at once, at least not in foreseeable future. actually, for 100 it is kinda ok financially, just not good enough for making good profit margin. I assume 1000 or more is going to be really negligible loss of money if we choose copper filling.

[ataradov]

What you will have to do depends on the nature of the issues you will get. There is a high chance that you won't get any issues.

Don't overthink it. You have the hardware on a way, just wait and see.

[VEGETA]

Hello all, as I mentioned here: https://www.eevblog.com/forum/projects/my-psu-design-ripple-and-noise-with-picture-measurements/msg4518794/#msg4518794

the project works as intended and there were no problems in spillage and so on, actually the holes are extremely small and I think it is kinda impossible for solder to spill from there... very narrow.

the 3.3v rail has nice clean 5-10mv p-p total noise\ripple... but the 5v rail is significantly bad at about 40mv p-p which is shocking to me!

I am trying to know the root problem as seen in my last post there, which I suspect it is due to long travel of the 5v signal then routed by a via under 3.3v ferrite bead.

for your help if you can.

I was VERY close to finally wrap this and start production... so hyped