via in pad

onsdag den 16. oktober 2019 kl. 01.40.33 UTC+2 skrev John Larkin:

you can get the via filled and plated over

Right, but that adds a lot of process steps to the board fab, something like 15 by one account. Sounds expensive.

--

John Larkin         Highland Technology, Inc 

lunatic fringe electronics

• Seems even solder has problems filing a 4 mil hole. Then again it matters not.

I once accidentally put a via in the middle of a 0.5mm pitch BGA pad. The via sucked the whole ball away, even though the volume of the via was less than the ball volume. The board was rescued by cleaning the remaining solder out of the via and forcing a stiff steel wire through the via until it contacted the underside of the BGA. Fortunately this was only a prototype. I may still have the X-ray images.

The bottom line: use plugged vias in pads under BGAs.

John

Your production cost is a small part of your total cost so it shouldn't be a bank buster. You're able to justify the cost of LT parts, so filled vias should be on the menu where it gives any advantage at all.

snipped-for-privacy@notreal.com wrote in news: snipped-for-privacy@4ax.com:

He can manage the via by placing mask over them. Being in a pad negates that, so he can manage those that are 'in pad' areas by ignoring them. A 4 mil via does NOT soak up enough solder to worry about.

Worried, add a mil to the stencil thickness. A bit cheaper than having them filled by the fabs or your production floor.

Or, place a via in all four locations so the wicking effect is equal on all four and thus the attachment integrity is the same across all four.

My experience is the opposite. I only have one data point because I took care never to make that mistake again.

John

AlwaysWrong insists on being wrong.

Always.

I think you will be surprised by how much trouble you will have with this.

I would highly recommend having them filled and plated by the board house. The modern ones do this all the time and are well setup for it, so the cost shouldn't be significant enough to gamble against the trouble you will bring yourself.

Did you do via in pad on BGAs?

What happened?

--

John Larkin         Highland Technology, Inc 

lunatic fringe electronics

My experience is with vias in pad for 1.27 pitched BGAs but it should be relevant.

You should not worry about how much solder is soaked up into the via, it is negligible (even with 0.2mm holes as we have been doing it for decades now). However you do have to worry about solder balls flowing through the hole entirely, leaving nothing to connect the BGA pad to the PCB pad. Happens when a solder ball comes coldly attached to the BGA case; about

1 ball in 100 in my experience are like that. The remedy is simple - just bake the BGA balls up with enough decent flux prior to putting it on the board so there are no cold balls. For our low quantity products this is not an issue, don't know if it would be one for you. But trying to bake the BGA right away onto a board with holes in the pads (we do all BGA pads with holes) is almost 100% sure to get you into trouble.

Dimiter

====================================================== Dimiter Popoff, TGI

======================================================

I accidentally put a via in the middle of a pad. It was 0.5mm pitch BGA package. The ball completely disappeared. Production of the prototype was done by a very competent UK contract manufacturer (the one who now makes Raspberry Pis). I may be able to find an X-ray image.

John