Electrical Engineering Stack Exchange is a question and answer site for electronics and electrical engineering professionals, students, and enthusiasts. Join them; it only takes a minute:

Sign up
Here's how it works:
  1. Anybody can ask a question
  2. Anybody can answer
  3. The best answers are voted up and rise to the top

I was looking at an example board schematic provided by TI and I noticed something rather curious: vias were placed directly on SMD pads. Is this a normal/acceptable practice to follow? Or is it recommended/better to put a short trace and then have a via?

share|improve this question
up vote 23 down vote accepted

Vias in the pads are useful in high speed designs since they reduce trace length and therefore inductance (i.e. the connection goes straight from pad to plane rather than pad-trace-via-plane)
You have to check whether your PCB house can do this though, and it may cost more (via will need to be plugged and plated over to provide a smooth surface) If you can't put the via in the pad, putting directly adjacent and using more than one can help reduce inductance.

They are also useful for Micro-BGA designs, where space is very limited and traditional fanout techniques cannot be used.

A via-in-pad (or capped/plated via) is not to be confused with a "tented via", which is a standard via with soldermask covering the hole (hence "tented")

To illustrate the advantage, here is an example of a TQFP footprint fanout with standard vias and via-in-pads:

Via-in-pad comparison

It's easy to see why the via-in-pad version is preferable for high speed designs that need to keep inductance low.

The reason it's more expensive is due to the complex process (compared to standard vias) and potential problems (e.g. plating bulging with expansion of plug, or dimpling)
This document discusses various plugging techniques.

Here is a run through of the process:

enter image description here enter image description here enter image description here enter image description here enter image description here enter image description here enter image description here enter image description here

share|improve this answer

In general it's bad practice: the solder paste may get sucked in the via capillarily, leaving too little to solder the part's connection. I would place the via as close as possible next to the pad, with a narrow connection which won't draw the solder paste from the pad.

There's a technique called tented via which avoids this by covering the top of the via, but it's covered with solder mask, so that's not usable on a pad.

Fake Name comments that I forgot to mention plugged vias, and they may indeed be a solution. I didn't mention them at first because I've never used them, and can't comment on possible pitfalls. Oli's answer has a very nice illustration of the technique and everything just screams "expensive!" (anywhere between very expensive and Damn Expensive™). You may need plugged microvias though for a small pitch BGA, like 0.5 mm.

Staggered microvias don't require plugging and the copper caps, but are buried vias, so also expensive.

enter image description here

share|improve this answer
You forgot plugged vias, which are vias filled with a conductive compound, most commonly conductive epoxy, and plated over. – Connor Wolf Sep 2 '12 at 9:36
@Fake - Added to my answer. Thanks for the feedback. – stevenvh Sep 2 '12 at 10:14
It would be nice if you could credit the source of the image you used. – Armandas Sep 27 '12 at 13:22
@Armandas - sorry, no can do :-(. This is from the Google images cache, the source page doesn't seem to exist anymore. That's also the reason for the reduced size, the original must have been larger and better readable. – stevenvh Sep 27 '12 at 13:30

When ordering PCBs to be manufactured, you can expect the vias to be drilled slightly off. Depending on how far this "slightly" is, the via might mess things up.

I'm sure TI has the best quality PCB manufacturing available. If you're using a cheap PCB manufacturer though, you may expect some visible imperfections.

Sometimes putting vias on pads is recommended. A power component soldered on to the PCB will very often have numerous vias connecting its big thermally conductive ground pad to the GND trace on the bottom layer. In high frequency designs you have to take into account the trace lengths of your PCB. It may sometimes be beneficial to put a via directly on a pad to reduce trace length.

share|improve this answer
agree with via on pads for heat. I have used vias on the large pad of a D2Pak regulator to get the heat down to the ground plane – justing Sep 1 '12 at 23:46

It is sometimes done with BGA devices, or to minimise inductance. The vias need to be plugged, which is very expensive.

share|improve this answer

No, no, no, no, no. Don't place vias on the pads*. The solder will suck into the via and create a faulty soldering. The solder joint will not have enough solder to be reliable.

This practice is expressly forbidden in any company taking their work seriously. I have worked e. g. at a major manufacturer of telecom equipment: Don't even think about via-in-pad.

I have seen a number of such solder joints. And I have seen such joints crack up after a while, losing contact.

In our design rules I have defined this as no-go. There shall be at least 100um solder mask between the pad and the via, exactly to avoid this problem.

If your assembly house makes sloppy work they will let you do this. If they are careful they will ask you to move the vias out of the pads.

*Exceptions: -Certain RF applications may need the pad in the via, but then the common practice is to use many vias.

-BGAs may require via-in-pad because there may not be enough space to route the board otherwise.

-Certain pads for power dissipation use vias in the big pad to conduct the heat away.

share|improve this answer

Your Answer


By posting your answer, you agree to the privacy policy and terms of service.

Not the answer you're looking for? Browse other questions tagged or ask your own question.