Vias on Exposed Pads

[Ignasi Soler]

Hi Robert,

When adding vias in exposed pads for thermal considerations, do you also use tented vias?
Is there any good reason to do it in one or the other way?

Thanks and regards

Ignasi

[Paul van Avesaath]

I would not use tented via's in exposed pads. espacially not when applying them underneath a component.
for thermal concideration (if the exposed will be soldered) just do the normal via;s
if you want to stop the tin seeping through you should go for plugged via's.

if it is just a larger polygon plane that you want to connect to a ground plane for thermal reasons then i don't think it matters either way.

[Ignasi Soler]

Hi Paul, thanks for your comments.

[robertferanec]

The VIAs under exposed pad will automatically not have mask as the whole area is unmasked because of the PAD. We do not add extra mask on the pad / via. However, you may want to consider size of the hole in that VIA (e.g. we often use 0.2mm), so solder will not flow on the other side of PCB (or you can use plugged/filled VIAs as suggested by Paul ... but we never do it, it adds cost to PCB manufacturing and we do not have problems not filling up the VIAs in exposed pads ... once I had problems with it, when I left the holes too big, but not since).

[Paul van Avesaath]

I mentioned the plugged via's because in some cases the designs has BGA components were it is nescesarry to have them any way.. since it is a proces step it does not really mather how many via's you use it for.. ususally i add a line in a mechanical layer status they have to do them all if via plugging is needed.. an 18-8mil via wont have any leak through of solder in any case.. I have seen it with 24-12 though..