I came across this question while looking for resources on something else, and found that people in the comments are saying that there's a difference between the term "via-in-pad", which some PCB fabs say they don't offer, and simply putting a via in a pad. But they don't mention what the difference is, exactly, other than some inconclusive arguments about whether the vias are plugged or not.

I have put plenty of vias inside pads (mostly thermal vias, but also some vias that overlap pads of tightly-packed passive components) in the past and never been charged the surcharge my prototyping fab of choice claims they have for via-in-pad designs, so it's clear that they're right about there being a difference, at least.

So I'm asking here: What is "via-in-pad", and how does it differ from a via in a pad?

  • \$\begingroup\$ It's the filling. When the pad is tiny like a BGA you need that. Were any of yours BGAs? \$\endgroup\$
    – DKNguyen
    Commented Dec 16, 2022 at 15:27
  • \$\begingroup\$ Putting vias inside your pads doesn't cost extra. Plugging them so that solder stays out of the via costs extra. If you don't care about that you don't have to pay for it. \$\endgroup\$ Commented Dec 16, 2022 at 15:33
  • \$\begingroup\$ "via-in-pad" also indicates that you're concerned about the surface flatness for when your component SMT "pin" is in the vicinity of the via. Plugging (filling) the via with stuff, making sure its flat, and then plating the filled surface, all take extra steps and money... \$\endgroup\$ Commented Dec 16, 2022 at 15:36
  • \$\begingroup\$ @DKNguyen I've never used a BGA; until recently when I have to use a QFN, I've always stuck to things I can solder by hand with a soldering iron, and the very occasional hot air station. \$\endgroup\$
    – Hearth
    Commented Dec 16, 2022 at 15:37
  • 1
    \$\begingroup\$ I got hit by that surcharge for plugged vias unexpectedly on an urgent job, I have since done a re-design to get the vias back under the solder-mask. \$\endgroup\$ Commented Dec 16, 2022 at 22:22

1 Answer 1


"Via-in-pad" implies filled vias. Via-in-pad and via in a pad look different on a bare PCB. If you look at the pad with a via-in-pad, you don't see the via, because it's filled and plated over. With via in a pad you see the hole in the pad.

Via-in-pad are filled and plated flush with the pad. (Usually the vias are filled with epoxy. They can also be filled with copper.) All that involves additional manufacturing steps, and PCB fabs charge for it.

plating through
The steps 1, 2, 7, 8 are common for all plated vias. The remaining steps are the additional steps needed for a via-in-pad.
selective pluggging
plating over
solder mask
(illustrations borrowed from this excellent old answer)

The purpose of via-in-pad is to prevent solder from getting pulled into the via. This is important when pads are small, and there's nowhere else to place the via. A good example are fine pitch BGAs (0.5mm pitch or smaller). The volume of solder stenciled onto the pads and in BGA balls is small, and a via in a pad would wick it away by surface tension. The distance between the pads is small, so there's no room for a via between the pads. Not even for a micro-via. The only remaining option is to do via-in pad.

enter image description here
The BGA in this illustration has 0.4mm pitch. Illustration taken from this blog post.

Thermal vias

In case of the thermal vias (under QFN, D2PAK, and similar) the thermal pad is larger relative to the via drill diameter. If the thermal pad is large enough, and the thermal vias are small enough, there will be enough solder stenciled onto the thermal pad to attach the thermal pad, and to slake the thirst of the thermal vias too. Thus, thermal vias don't require via-in-pad, typically.

For prototyping I usually leave the thermal vias untented.
For production I tent the other side of thermal vias.

  • 3
    \$\begingroup\$ As a poor-man's alternative I've used pads on both sides of the board - that way the excess solder from the other side of the board would fill in the via and leave enough for the BGA pads to make contact. Definitely not recommended in production, but for prototyping it worked in a pinch. The pad "on the other side" can also be larger, so that it can fit more solder, and balance out the solder load on the BGA side. \$\endgroup\$ Commented Apr 14, 2023 at 22:15

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

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