IntelCAD team

Via in Pad: PCB Design Rules, Filling and Capping Guide

Via in pad explained: when to use it, filled and capped vias (VIPPO), solder wicking, cost, IPC-4761 types, and design rules for BGA and QFN layouts.

Cutaway of a multilayer PCB under a BGA package showing filled, copper-capped vias drilled directly through the SMT pads

Short answer: Via in pad means drilling a via directly inside a component’s copper pad instead of routing a short trace from the pad to a via beside it. It saves space and shortens the electrical path, which makes it the standard way to fan out fine-pitch BGAs and to pull heat out of QFN thermal pads. The catch is solder: an open via in a pad wicks solder away from the joint, so for SMT pads the via is normally filled with resin or copper and plated over flat, a process often called VIPPO (via in pad plated over). Use it when pitch, signal integrity or heat demand it, and spec the filling clearly in your fab notes.

Cutaway of a multilayer PCB under a BGA package showing filled, copper-capped vias drilled directly through the SMT pads
Cutaway of a multilayer PCB under a BGA package showing filled, copper-capped vias drilled directly through the SMT pads

What is via in pad?

In a conventional layout, every SMT pad connects to a via through a short trace called a dog-bone. Via in pad (also written via on pad or pad on via) removes the dog-bone and places the via inside the pad itself. The via barrel connects the pad straight down to inner layers or to the other side of the board.

That sounds like a small change, but it changes how the board is built. A plain through-hole via is an open, plated hole. If you put an open hole in an SMT pad, the paste melts during reflow and capillary action pulls it down the barrel. To prevent that, the fab fills the via, planarizes it and plates copper over the top so the pad is flat and solid again. That extra fill-and-cap step is the main cost of via in pad, and it is why you should use it on purpose rather than everywhere. It sits in the same family of choices as blind and buried vias, and the two are often combined in HDI boards.

When should you use via in pad?

Via in pad earns its cost in four common situations:

If none of those apply, a dog-bone with a standard via beside the pad is cheaper and easier to build.

Open via in pad vs filled and capped via in pad

Cross-section comparing an open via in a pad wicking solder away from a lead with a filled, copper-capped via under a flat, full solder joint
Cross-section comparing an open via in a pad wicking solder away from a lead with a filled, copper-capped via under a flat, full solder joint
OptionWhat the fab doesGood forRisk
Open (unfilled) via in padNothing extra; plated hole left openRarely acceptable on SMT pads; sometimes tolerated in large thermal pads with tiny drillsSolder wicking, voids, starved joints, paste on the far side
Tented or plugged viaSolder mask or plug covers one or both endsVias next to pads, not inside themTrapped chemistry, outgassing, uneven pad surface
Resin-filled, copper-capped (VIPPO)Fill with non-conductive epoxy, planarize, plate copper overBGA pads, QFN thermal pads, most via in pad workHigher cost and lead time; needs clear fab notes
Copper-filled viaFill the barrel with plated copperMicrovias and high-current or high-thermal viasHighest cost; usually limited to small drills

The key point: for any via inside an SMT pad that gets solder paste, ask for filled and capped vias. Open vias in pads are the source of most via in pad assembly failures, from voided BGA balls to QFNs that float on uneven solder.

Via filling and IPC-4761 types

Fabs describe via protection using IPC-4761, which lists types from simple tenting to full fill and cap. In practice you will see a few names:

Write the type into your fab notes rather than writing “via in pad” and hoping. A clear note such as “All vias in SMT pads: non-conductive epoxy fill, planarized, copper capped per IPC-4761 Type VII” removes ambiguity at quote time. The solder mask layer and the surface finish both sit on top of the cap, so flat ENIG or ENEPIG pads pair well with VIPPO under fine-pitch BGAs.

Via in pad design rules

These rules keep via in pad buildable and reliable:

  1. Size the drill to the pad. A common starting point is a finished drill of about 0.2 to 0.3 mm in a BGA pad, with an annular ring your fab supports. Check your fab’s standard via size table before you lock the footprint.
  2. Keep the via centered. An off-center via makes uneven solder fillets and can break out of a small pad.
  3. Use the same rule for every pad in a footprint. Mixing filled and open vias under one BGA leads to uneven ball collapse.
  4. Watch aspect ratio. Thick boards with small drills are hard to plate and fill. Long, thin barrels may push you toward blind or laser microvias instead.
  5. Plan thermal pad grids. For QFN thermal pads, use a regular via grid, filled and capped, and segment the paste stencil so the part does not float.
  6. Mark it in the stackup and notes. Via in pad affects your PCB stackup, lamination sequence and price. Put it in the drawing so it is quoted correctly.
  7. Ask the fab early. Capability for filled and capped vias varies, and some fabs only offer it on certain stackups or finishes.

What via in pad costs

Via in pad adds process steps: filling, curing, planarizing and a second plating cycle. Expect a higher price per board and a longer lead time than a dog-bone design with standard vias. On dense boards that is often still the cheaper choice overall, because it can save routing layers, shrink the board or avoid HDI build-ups. The decision is a trade-off between process cost and the layers and area it saves, which is why it belongs in your DFM review and not only in routing.

Common via in pad mistakes

Add a via in pad line to your PCB design review checklist so these get caught before Gerbers go out.

Where AI and DFM checks help

Via in pad errors are usually mismatches between the layout and the notes: a via inside a pasted SMT pad with no fill and cap specified, a footprint that mixes open and filled vias, a drill that breaks the annular ring, or an aspect ratio the chosen fab cannot fill. All of these can be checked automatically. An AI-assisted DFM pass reads footprints, drill data, stackup and fab notes together, finds every via that lands inside a pad, and flags the ones that will wick solder or cannot be built as specified, before the board is quoted.

That is the IntelCAD angle on via in pad: not just a definition, but a check tied to the actual pads, parts and fab notes on your board.

FAQ

What is via in pad in PCB design?

Via in pad places a via directly inside a component’s copper pad instead of connecting the pad to a nearby via with a short trace. It saves space and shortens the electrical path, and is common for fine-pitch BGAs and thermal pads.

Do vias in pads need to be filled?

For SMT pads that receive solder paste, yes in most cases. An open via wicks solder away from the joint, so fabs fill the via with resin or copper and plate it over to make a flat pad.

What is VIPPO?

VIPPO stands for via in pad plated over. The via is filled, planarized and capped with copper so the pad is flat and solderable, which is the usual way to build via in pad for BGAs.

Does via in pad increase PCB cost?

Yes. Filling, planarizing and extra plating add cost and lead time. On dense boards it can still lower total cost by saving routing layers or board area.

Can I put a via in a QFN thermal pad?

Yes. A grid of filled and capped vias in the thermal pad moves heat into internal planes. Segment the paste stencil so the part does not float during reflow.

Next step

Want every via that lands in a pad found and checked against your fab notes before you send Gerbers? Start Your Design with IntelCAD for AI assisted PCB design and manufacturability checks.

Design your next board by describing it.

Start Your Design