Contact Us
  • Home
  • BLOG
  • Via in Pad with Epoxy Fill for RF Boards: Process and Traps

Via in Pad with Epoxy Fill for RF Boards: Process and Traps

Via in pad means the via is placed inside the component land, and on an RF board it is usually a ground via inside a thermal or shielding pad. It solves a real problem: the shortest possible path from a pad to the plane, with no stub and no trace inductance. It creates another one, because the pad now has a hole in it and the component has to be soldered over that hole. Epoxy fill is the standard answer, and the process is where most of the failures live.

1. Why RF designs use via in pad

At 6 GHz and above, a 1 mm trace from a pad to a via is about 8 pH of inductance, which is a few ohms of reactance. On a high-power amplifier ground pad, that reactance is enough to make the source impedance wrong, and no amount of tuning at the input fixes a bad ground. Putting the via directly under the pad removes the trace and shortens the return path to the plane.

On thermal pads the reason is heat, not impedance: the via array is the only path from a QFN exposed pad to the copper below. On shielding fences it is continuity: a row of vias in the pad ring keeps the shield tied to ground at the frequencies that matter.

2. The four ways to close a via in pad

MethodWhat it producesWhere it fits
Open, untentedSolder can wick into the hole during reflowNot acceptable under a component pad
Tented from one sideMask over the hole; often blows out during reflowLow-reliability, non-critical only
Filled and capped (plated over)Epoxy fill, planarized, copper plated over the fillVia in pad under fine-pitch components
Filled, not cappedEpoxy fill planarized to the pad, no plating overLarger pads, thermal arrays, cost-sensitive

The IPC-4761 via protection types describe these formally, and the type number belongs on the fabrication drawing. A drawing that says "via in pad" without naming the type leaves the choice to the fabricator, and the cheapest interpretation is not the one the assembly house needs.

3. The process, step by step

Fill. Epoxy is pushed into the via from one side, usually with a squeegee or a dedicated via-fill machine, on a board that already has its outer layer copper. The fill has to be void-free, which is a function of via diameter, aspect ratio, epoxy viscosity and the vacuum or pressure cycle.

Bake. The epoxy shrinks as it cures. A single fill usually ends up below the pad surface. Most processes fill, cure, and fill again, or use a paste with low shrinkage.

Planarize. The cured fill is ground or sanded level with the copper. This step is mechanical and it is where pad damage happens if the operator is not careful. The result should be flat within a few microns across the pad.

Plate. Where the type calls for capping, copper is plated over the fill to reconnect the pad surface. This plating has to be thick enough to survive assembly and thin enough not to change the pad geometry.

Finish. ENIG, immersion silver or whatever the board calls for goes on last, over the capped pad.

4. Where it goes wrong

Voids in the fill. A void under a pad becomes a pocket of air that expands during reflow. The result is a blowout, a solder ball under the component, or a void in the thermal path that shows up as a hot spot. X-ray is the inspection, and the acceptance criterion has to be written: what void area percentage is allowed, measured how.

Dishing. If the fill sits below the pad plane, the component does not contact the pad properly and the paste volume is wrong. If the fill sits above, the component rocks. Both produce opens or weak joints that pass X-ray and fail in the field.

Fill wicking onto the pad surface. Epoxy that spreads beyond the via onto the land reduces the solderable area. It is invisible after plating if the plating covers it, and it shows up later as a dewetting pad.

Plating over a void. The cap can look perfect and hide a void underneath. This is why cross-section, not just X-ray, is part of qualifying a via fill process.

CTE mismatch. Epoxy expands more than copper and more than the laminate. On a large thermal pad with a dense via array, the fill can push the cap up or crack the plating after thermal cycling. The via pitch and the fill material have to be chosen together.

5. Design rules that prevent most of it

Keep the via diameter small relative to the pad, so there is land left for solder. On a 0.5 mm pitch QFN thermal pad, vias of 0.2 mm with 0.4 mm pads leave enough copper. On finer pitch, the via goes outside the pad and the trade-off changes.

Do not put vias in pad on the same net at a pitch that leaves thin copper webs between them; the fill and the plating both get harder and the pad can lift.

Keep the via array inside the pad outline with a margin, so the fill and planarization do not touch the solder mask opening edge.

State the fill type, the void acceptance, the flatness tolerance and whether the via is capped, on the drawing. State the finish, because some finishes do not cover a filled via properly.

6. How we inspect it

X-ray for void percentage on a sample per panel, with the acceptance criterion agreed in advance. Cross-section on first article, through the worst-case via in the densest area, measuring fill void, cap thickness and flatness. Visual for fill bleed onto the land after plating. And an assembly trial on the first lot, because the real test of a via fill is whether the paste prints and reflows correctly over it.

The failures we see most are all in the specification, not the process: a drawing that names no fill type, a void criterion nobody wrote down, and a flatness tolerance that was never measured because nobody asked for the measurement.

Send the pad geometry and the via array and we will confirm the fill type, the flatness we can hold and the inspection we will report.

Related reading

Need a DFM check or a stack-up review on your files? Write to pcba@superb-tech.com or WhatsApp +86 133 9608 1443.