A fabrication note that says "fill the vias" leaves the supplier to choose between tenting, plugging, filling and capping. Those are four different processes with different flatness, and only one of them allows a BGA ball or a printed thermal pad to sit directly on the via. When a filled via still wicks solder at reflow, the note was usually the problem, not the process.
The seven types, and what each one delivers
IPC-4761 names the via protection options so that a buyer and a board supplier can agree on one. The practical difference is how flat the pad ends up and whether solder can enter the barrel.
| Type | What is done | Surface at the pad | Where it is enough |
|---|---|---|---|
| I | Tented both sides with mask | Mask over the hole | Non functional vias away from pads |
| II | Tented one side, covered the other | Mask over the hole | Vias near a board edge or a connector |
| III | Plugged, material in the barrel, not full | Visible depression | Vias that must not stay open but carry no ball |
| IV | Plugged and covered with mask | Mask over the plug | Vias under a shield can or a stiffener |
| V | Filled, ends open or slightly recessed | Fill visible, dimple allowed | Thermal vias where paste is not printed over |
| VI | Filled and covered, with mask or with a plated finish | Covered, not necessarily planar | Vias that must not see solder but need no ball on top |
| VII | Filled and capped with plated copper | Planar, solderable pad | Any via inside a pad that receives a ball or paste |
Type VI is where most notes go wrong, because the covering step differs between suppliers: some cover with mask, some with plating. If the via sits in a pad that gets paste, do not write Type VI and hope. Write Type VII and state the dimple and cap thickness.
Where a via has to sit in the pad
| Package or feature | Why the via moves into the pad |
|---|---|
| 0.4 mm pitch BGA | Pad and gap no longer leave room for an escape trace and a via between balls |
| WLCSP at 0.35 to 0.4 mm | Same geometry, and the die shadow blocks routing on the surface |
| QFN thermal pad | Heat has to leave through the board, so vias sit under the paste area |
| Package on package | No through hole may pass under the upper package outline |
| RF module ground ring | Shortest return path, and a via just outside the pad adds inductance |
| Stacked microvia in HDI | The next lamination lands on the filled via, so it must be planar and plated |
The numbers to put in the fabrication note
- Type per via group. Name the groups, for example "all vias inside BGA pads Type VII, all other vias Type I". A blanket instruction gets a blanket process.
- Fill material. Non conductive epoxy for electrical and general work, copper paste where thermal or current carrying matters. The two behave differently under thermal cycling, so the choice belongs in the note.
- Dimple. The depression left after planarization. SUPERB PCB holds 10 micron or less on filled and capped vias. Customers who ask for 25 micron are specifying a cheaper process, which is fine as long as it is written down.
- Cap plating. Type VII needs a plated copper cap thick enough to survive assembly. 20 to 25 micron is a common range. Ask for the microsection at first article rather than a statement.
- Cure before cap. The fill must be cured before plating, otherwise the cap blisters at reflow. Ask for the cure schedule with the lot.
- What must not be filled. Test points, wire bond pads and press-fit holes take no fill material.
What goes wrong when the type is wrong
| Failure | Mechanism | Prevention |
|---|---|---|
| Solder wicks down the barrel, joint starves | Via still open at the pad, or plug not full | Type VII, dimple limit, paste print checked with SPI |
| Blowholes and spatter at reflow | Fill not fully cured, moisture held in the resin | Cure verification, bake before assembly on old stock |
| Head in pillow on the ball above a via | Deep dimple takes paste away from the ball | Dimple at 10 micron, paste volume verified over the via |
| Voids over a thermal pad | Air trapped in the fill and under a large aperture | Window pane aperture, smaller thermal vias, longer soak |
| Cap lifts after thermal cycling | Poor adhesion, resin smear before plating | Plasma desmear, microsection, thermal cycle on the first lot |
On RF boards one more item matters: a filled via in a ground pad changes the local capacitance, so the antipad and the pad geometry have to be checked with the fill in place. That is a stackup question answered before the panel is released, not after the impedance coupon fails.
What SUPERB PCB can hold
SUPERB PCB fills and caps vias to 10 micron dimple or less on HDI and high layer count builds, with the fill completed before final finish so the pad is planar when paste reaches it. Laser drilling runs 0.075 to 0.15 mm with 0.05 mm on request, mechanical drilling 0.15 to 6.35 mm, HDI goes to 1 to 3 stages and ELIC to 30 layers, the high layer count line reaches 68 layers with up to seven lamination cycles. Controlled impedance holds plus or minus 5 percent, or 2 percent on critical nets, and microsections from the fill and cap step ship with the lot when the drawing asks for them.
- FR-4 process parameters: drill sizes, via fill and plating limits, and the numbers to quote in a fabrication note.
- PCB capability: drill sizes, aspect ratio, layer counts and the limits in one table.
- AOI and X-ray inspection: how a filled via and the joint above it are checked.
Frequently asked questions
Is Type VII needed for every filled via?
No. A buried via that never meets a pad can be Type V. A via under a ball, under a printed thermal pad, or under the next lamination of a stacked microvia needs a planar cap, which means Type VII.
Can a plugged via be used under a BGA ball?
It should not be. Plugging leaves a depression measured in hundreds of microns, the plug material can pump during reflow, and the paste that should form the joint goes into the hole instead. The result is a joint that looks placed and fails inspection.
Does filling change the stackup?
Not the layer count, but it adds process steps: fill, cure, planarize, then cap plating before final finish. That affects cost and lead time, and it has to be planned with the lamination sequence on stacked microvia builds.
Next step
Send the Gerber data, the stackup and a note listing which vias carry a ball or sit under a paste printed pad. The reply states the IPC-4761 type per via group, the dimple and cap thickness that will be held, and the inspection evidence that ships with the first lot.