via's masked or unmasked

[cyberstace]

Hi all, I have a question, should via's in general be covered with solder mask or tinned? My company seems to tin all their via's, but I worry about this under FPGA's. Any pro and cons for this?

[randychase]

I used to tin them all. It was handy to have some extra tinned holes for rework or modification.

But the downside is when things get tight and you have to use silkscreen legends on vias. The silkscreen is much better on a masked via.

And if the vias are under parts, or your clearances are tight, you will have less chance of problems with masked vias.

The only time now I clear the vias of mask is on the occasional thru-hole pcb I do.

[petehouwen]

We used to tent vias. Then we had concerns about outgassing during soldering. Tenting one side only causes flux entrapment. Now, we do not tent vias. If they need to be closed, the wave solder process will close most vias (except the really larage ones). If your board is not going to be waved, you can add vias to the paste mask. BUT, we still tent vias under BGAs, to eliminate sodler paste problems.

[Tom]

Here are some tips from our manufacturers:

1. Tenting vias are OK up to a 0.35mm (.014") hole.

2. Via holes that are larger than 0.35mm can still be covered 80% but need a solder mask clearance that is 0.15mm (.006") larger than the hole to create a 0.075mm (.003") annular ring. If you are going to wave solder the entire board you need to discuss this with your assembly shop because of the outgassing issue, but most boards today that are 90% SMT get "Selective Wave" just for the through hole parts.

3. Why Tent? There are several reasons to tent (cover) vias with solder mask and one is so that when you apply silkscreen, the white ink does not get all over exposed metal. We do a lot of large dense boards with a couple thousand parts and thousands of vias with ref des and silkscreen outlines all over the vias. Typically, in good PCB design practice, you move the ref des off all non-tented vias, like Test Points. If we had to move every ref des off every via it would get ugly, if not impossible.

4. You absolutely need to tent all vias under BGA's. Most assembly shops will reject boards with exposed vias under BGA's because it causes solder bridges that cannot be easily seen except through x-ray. PCB manufacturers cannot go back and add additional solder mask on selective vias under BGA's after the boards have been finished. We tried it, failed and had to rebuild new boards. Our assembly shop rejected a batch of boards that had exposed vias under BGA's and they came back to my office. I sent the boards back to the manufacturer to try and "Patch up" (cover) the exposed vias and the manufacturer failed.