Holes/vias in SMT pads

[jmatt]

I posted this on the Listserver, but got a limited response, so I thought I'd try here.

We've been able to avoid putting holes in SMT pads up to now but are starting a project string that most likely will require this.

What are any rules, reqirements, suggestions, guidelines, pitfalls, etc, etc we need to know or be aware of when we do this?

Thanks....

[randychase]

My perception is that it is an option that can work. I have placed vias on sm pads when I have had to. But doing it places a burden (cost!) on the assembly shop. In very general terms, small proto or low volume boards might be okay, but the higher the volume the worse of an idea this is.

I would not build these holes into the library, but place them afterwards. I think it would be best to still place them as far away from the center of the land as possible and to use the smallest via one can.

Everything is a compromise and trade off when trying to squeeze ten pounds of stuff in a 5 pound bag...and all the solutions will have costs associated with them. For me, the use of vias in the SM pads is a last gasp solution.

Check out this link:
http://www.laservia.com/PDF/smi97.pdf

[Tom]

Vias in SMT pads will work OK following certain rules:

1. Never place the hole in an area on the pad where the component lead makes contact. Place the hole on the outer edge of the Toe. In the case of a chip component, place the via in the outside corner of the pad.

2. Make all the holes as small as possible and make them a unique size so that the manufacturer can plug them with silver epoxy (which is a good condutor also). If you do not plug the holes, paste mask will melt down into them causing problems on the opposite side of the board.

[jmatt]

Tom,

On the part about not putting a hole where a comp lead contacts it, I've now heard two different viewpoints:

The first can be summed up like this: "Use a minimal non-plugged hole (.010" or smaller diameter). You can place the hole where the lead will cover it, because the part will cap the hole and prevent or reduce wicking away of solder. Do not place the hole where it will only be partially covered, and do not tent the hole on the opposite side of the board. This is to prevent any outgassing from moving the part."

I've actually seen a board layed out that way. So I know it's doable anyway. Don't know if there were any assembly problems.

and

Basically what you said (with a plugged hole), with outgassing the reason given for the hole to not be under the part.

I know that a close relationship with my assembler is required here regardless.

I'm going to affect a company policy here, so I want to make the best decision here. What do you think?

[Tom]

I think we all need a little education in this area. My original response was take right out of an article by Jim Blankenhorn in PCD Magazine 2 years ago.

We really need to get the assembly shops involved and get the straight answer and a solution to this issue. Then once we have the correct information we need to publish it so everyone knows the research that was done to derive the solution.

[jmatt]

Oh, after re-reading my last post - a little clarification is probably in order...

A hole doesn't have to be covered by a lead/termination, it just shouldn't be half-under a pad, this would promote wicking away the solder.

The hole can can be on the pad elsewhere. And pads not under parts could be plugged or tented on the opposite side.

[tboyer]

The best way I have seen the use of vias under pads is by using blind vias as small as possible or use a micro via. Normally if you have room on the other side of the board for a through via you have not reached a point were a via under pad must be used.
You must decide on whether to pay for a more expensive board process or pass on the cost to assembly by having some components on the bottom of the board. By using a through via under a pad and having it plugged reduces the number of board shops that will quote the job.

[jmatt]

I agree that I'd rather not do this, but there are situations where we see it as a need.

We're looking into it more as an answer to a potential problem, a last resort, or an option in extraordinary circumstances, not as an everyday design practice.

[Tom]

We are doing a PCB design right now for AMCC (the chip manufacturer) and they have a 20 X 20 BGA 1mm Pitch that is a 10 GIG Chip. The engineer has to have the termination resistors and bypass caps directly under the BGA on the bottom of the board. The only solution is blind and buried vias. I believe that we are going to see a lot of this coming up in the future as boards get faster and faster. Speaking of which, I gotta get me one of those 2 GIG computers with 120 GIG hard disk, DVD CD and a 24" Viewsonic Flat Panel monitor. Smokin'.