As the pitch of BGA, CSP, and LGA packages becomes smaller, less surface area remains available for routing and vias on a printed circuit board. Conventional dog-bone fanout works well for many standard BGAs, but in high-density or fine-pitch layouts, designers may no longer have enough space to place vias outside the component pads.
A common solution is to place the via directly inside the component pad. This is called Via-in-Pad.
However, placing a via in a pad does not complete the design. If the pad will be used for direct SMT soldering, an untreated opening can draw solder away from the joint and reduce soldering quality. To create a flat, solderable surface, PCB fabrication commonly fills the via, cures the fill, planarizes the surface, and plates copper over the opening. This structure is commonly called VIPPO, or Via-in-Pad Plated Over.
Via-in-Pad and VIPPO are often discussed together, but they are not identical. Understanding their relationship helps designers make better decisions for BGA fanout, HDI routing, and other high-density PCB applications.
What Is the Difference Between Via-in-Pad and VIPPO?
The simplest way to understand the difference is to separate the two concepts.
Via-in-Pad (VIP) describes the location of a via.
Instead of placing the via next to a component pad, as in a conventional fanout, the via is located directly inside the pad.
VIPPO describes how that Via-in-Pad is subsequently fabricated.
When a pad must directly support a soldered component, the PCB fabricator typically fills the via, cures the fill, planarizes the area, and plates copper over the top. This restores a continuous, flat pad surface where the original opening was located.
In simple terms:
> Via-in-Pad answers “Where is the via?” VIPPO answers “After placing the via in the pad, how do we make the pad reliably solderable?”
The term POFV, or Plated Over Filled Via, is also common in the PCB industry. It emphasizes the fabrication structure—a filled via with copper plated over it—and is closely related to VIPPO.
A conventional via sits outside the pad. Via-in-Pad places the opening inside the pad, while VIPPO fills and plates over that opening to create a continuous soldering surface.
| Item | Conventional Via | Via-in-Pad | VIPPO |
|---|---|---|---|
| Via location | Outside the pad | Inside the pad | Inside the pad |
| Via filling | Usually not required | Depends on the application | Usually required |
| Copper plated over the surface | No | Not necessarily | Yes |
| Flat solderable pad surface | Not applicable | Not necessarily | Yes |
| Common applications | General PCB routing | Dense routing, thermal pads | BGA, CSP, LGA, HDI, and similar designs |
| Manufacturing complexity | Lower | Moderate | Higher |
Why Do PCB Designs Use Via-in-Pad?
Via-in-Pad is not used simply to make a PCB appear more advanced. Its main value is solving the space limitations that conventional routing encounters in high-density designs.
Fine-Pitch BGA Fanout Space Is Limited
Conventional BGA routing often uses a dog-bone structure:
BGA pad → short trace → via → inner layer
This method is simple, mature, and relatively economical.
As BGA pitch decreases from 1.0 mm and 0.8 mm to 0.65 mm, 0.5 mm, or smaller, however, the routing space between adjacent pads shrinks quickly. There may no longer be enough room to route a short trace from every pad to a separate via.
Via-in-Pad allows a connection to transition directly from the BGA pad to an internal layer without reserving additional surface area for dog-bone fanout. This is its most typical application.
There is no universal rule such as “every BGA below 0.8 mm pitch must use VIPPO.” The decision must consider BGA land size, trace width and spacing, via diameter, annular ring, layer count and PCB stackup, HDI and microvia capability, and the fabricator’s process limits.
More Surface Routing Space for High-Density PCBs
Placing the via inside the pad eliminates the surface trace that would otherwise connect the pad to an external via.
This is especially useful in HDI boards, portable devices, compact control boards, and designs with high-I/O-count BGAs. In layouts with very high routing density, Via-in-Pad may determine whether the entire breakout can be completed, rather than merely saving a small amount of area.
Shorter Signal or Power Connections
Via-in-Pad can also remove the short surface trace between a pad and its via.
For some high-speed signals and power or ground connections, a shorter transition can reduce parasitic inductance and avoid an additional routing stub. This does not mean that every high-speed PCB should use Via-in-Pad. If conventional via placement already meets signal-integrity, routing, and manufacturing requirements, adding the VIPPO process only to shorten a small distance may not be justified.
Vias Under Thermal Pads
Vias are also commonly placed under QFNs, power devices, and other exposed thermal pads. These thermal vias can help transfer heat from the top layer to internal copper layers or the bottom side of the board.
Thermal vias and VIPPO used under BGA solder pads are not exactly the same design problem. Some thermal vias may remain partially open, while others require plugging or filling. The appropriate treatment depends on the SMT process, solder-paste volume, and thermal requirements.
Why Should an Open Via Not Be Left in a Solder Pad?
This is the key reason for using VIPPO.
If a conventional plated-through via is placed directly in a BGA pad without filling or copper capping, molten solder can flow down the via barrel during reflow. This effect is commonly called solder wicking.
For a relatively large solder joint, a small loss of solder may not be obvious. In a fine-pitch BGA or CSP, however, the solder volume on each pad is already limited. Solder drawn into the hole can cause:
- Insufficient solder at the joint
- Inconsistent BGA ball height
- Increased voiding
- Unstable joint geometry
- Local open circuits or reduced reliability
An unfilled opening also interrupts the pad surface.
In an open Via-in-Pad, molten solder can migrate into the barrel. A filled and plated-over VIPPO structure retains solder on a flat pad.
By filling, planarizing, and replating the via, VIPPO closes the original opening. The component sees a continuous, flat copper pad, so solder is much less likely to flow into the via during the SMT and reflow process.
How Does VIPPO Create a Flat, Solderable Pad?
The exact process sequence may vary among PCB manufacturers, but the basic VIPPO fabrication logic usually includes these stages:
Drilling → Copper Plating → Via Filling → Curing → Planarization → Copper Plating → Surface Finish
The via progresses from an empty drilled hole to a plated, filled, planarized, and copper-capped pad.
1. Drilling and Hole-Wall Copper
The hole is first formed using the appropriate process for a conventional via or microvia. Copper is then deposited and plated on the hole wall.
2. Via Filling
The hole is filled with a material appropriate for the structure and end use. Common options include:
- Non-conductive epoxy fill
- Conductive fill
- Copper-filled microvia
Conductive fill should not automatically be considered better than non-conductive fill. For many conventional VIPPO applications, non-conductive fill satisfies the structural and soldering requirements. Conductive fill should be selected only after considering heat transfer, current, the via structure, and the fabricator’s validated process.
3. Curing and Planarization
After curing, the fill material may leave a slight protrusion. The surface is then planarized so that the via and surrounding pad area are relatively flat.
4. Copper Capping and Surface Finish
After planarization, copper is plated over the via to form a continuous surface layer. From the top, the original hole has effectively disappeared and the component sees a complete pad.
The specified final finish—such as ENIG, OSP, or immersion silver—is then applied. Finish availability and suitability should be confirmed against the board construction and assembly requirements in the manufacturer’s PCB manufacturing capabilities.
Via-in-Pad or Conventional Dog-Bone Routing: Which Should You Choose?
Not every BGA requires Via-in-Pad. When sufficient space is available, conventional dog-bone routing remains a mature and economical solution.
If standard fanout already satisfies routing, signal-integrity, and reliability requirements, dog-bone routing is usually the simpler choice. VIPPO provides the most value when conventional methods are constrained by space or performance.
| Comparison | Dog-Bone Routing | Via-in-Pad / VIPPO |
|---|---|---|
| Surface routing space | Uses more space | Uses less space |
| Fine-pitch BGA suitability | Becomes limited as pitch decreases | Better suited to high-density designs |
| PCB fabrication flow | Simpler | More complex |
| Via filling | Usually not required | Usually required for VIPPO |
| Surface-planarity requirement | Lower | Higher |
| PCB cost | Lower | Usually higher |
| HDI applications | Usable | Very common |
If conventional fanout meets all requirements, it is usually the practical default. VIPPO becomes valuable when the traditional method begins to limit the overall PCB architecture.
What Should Designers Consider When Using Via-in-Pad and VIPPO?
Consider the Via Type Together With the Stackup
Via-in-Pad can use a through via or a blind microvia.
Microvias are common under high-density BGAs because they can connect adjacent build-up layers while using a smaller land area. The permitted layer span and the use of staggered or stacked structures are closely related to the HDI stackup.
If the stackup is not confirmed until after layout is complete, the selected via span or microvia structure may prove impossible to manufacture. For complex HDI designs, confirm the stackup and routing assumptions with the fabricator early. SAYFU’s published HDI PCB capabilities provide a starting point, but the complete design still requires engineering review.
Microvia reliability also requires deliberate review. IPC has documented reliability concerns in demanding stacked-microvia structures, so “smaller” or “more layers” should not be treated as automatically better.
Do Not Apply One “Standard Via Size” to Every Design
There is no single Via-in-Pad diameter that suits every PCB.
The appropriate dimensions depend on component-pad geometry, finished-hole size, drilling method, board thickness, annular ring, copper-plating requirements, and layer structure. For fine-pitch BGAs in particular, the via and pad combination should be confirmed during layout, not changed only after the Gerber package is complete.
Specify Which Vias Require Filling and Plating Over
Gerber data shows geometry but may not fully communicate manufacturing intent. If a design contains VIPPO structures, the fabrication drawing or fab notes should clearly identify:
- Which vias are Via-in-Pad
- Whether filling is required
- The required fill type
- Whether the vias must be plated over or capped
- The via layer span
- Finished-hole or drill requirements
- Applicable standards or special requirements
For filled and capped vias, the fabrication notes can reference the relevant structure in IPC-4761. In that guide, a filled and capped via is identified as Type VII. The final acceptance criteria should still be agreed between the customer and fabricator and tied to the applicable procurement documentation.
Surface Planarity Matters
After VIPPO processing, the pad surface should not have excessive depressions or protrusions.
Fine-pitch BGAs use many small pads with limited solder volume, so local planarity variation can directly affect solder-joint consistency. VIPPO therefore means more than plugging a hole. Filling is only one stage; planarization, copper plating, inspection, and process control are equally important.
Common Via-in-Pad Problems Found During DFM Review
Via-in-Pad is not an unusual PCB structure, but several recurring issues should be checked before release.
The Layout Shows Via-in-Pad but Does Not Define the Treatment
A Gerber file may show a via inside a pad, but the PCB fabricator cannot safely infer whether it should remain open, be resin-filled, be plugged, be capped, or be plated over.
If the pad will directly support a BGA solder joint, the required treatment should be explicit in the fabrication information.
Via Geometry Does Not Match Manufacturing Capability
A small pad paired with an oversized mechanical drill may not leave enough annular ring or may fail to meet plating and filling requirements. This issue is normally avoidable through early DFM review.
Thermal Vias Are Treated as Identical to VIPPO
Both structures can place vias inside pads, but their objectives and SMT requirements differ.
Thermal vias primarily transfer heat, while Via-in-Pad under a BGA emphasizes routing density and a solderable surface. Whether the vias must be completely filled and copper-capped depends on the specific assembly requirement.
The HDI Stackup Is Confirmed Too Late
A layout may be completed around a particular microvia span even though the chosen fabricator supports a different build-up structure. The result can be a complete redesign of the breakout. For complex BGAs, confirming the stackup earlier usually reduces later modification cost.
When Is VIPPO a Good Choice?
Fine-Pitch BGA, CSP, and LGA Packages
This is the most typical use case. When package pitch is too small for practical dog-bone fanout, placing the via inside the pad can create additional routing channels and improve breakout feasibility.
High-Density HDI PCBs
In space-constrained HDI boards with complex interlayer connections, Via-in-Pad combined with microvias can move signals quickly into internal routing layers.
High-I/O-Count Components
Even when BGA pitch is not extremely small, a device with many I/Os can create enough routing density to require Via-in-Pad for escape routing.
Signals or Power Networks Sensitive to Connection Length
For some high-speed, RF, power, or ground connections, Via-in-Pad can shorten the connection path. The choice should be based on defined signal-integrity or power-integrity requirements, not on an assumption that VIPPO always improves electrical performance.
Products With Strict PCB Size Limits
Portable electronics, communication modules, and embedded control boards often need to fit substantial functionality into a small board area. Via-in-Pad can reduce the surface space consumed by component breakout.
When Might Via-in-Pad Be Unnecessary?
Via-in-Pad is a design tool, not a symbol of PCB technology level.
If BGA pitch is generous, board area is sufficient, dog-bone fanout is easy to complete, and the routing, signal, thermal, and power requirements do not justify a more complex structure, conventional vias are usually simpler.
Removing the filling, curing, planarization, and copper-capping steps generally reduces manufacturing complexity, lead time, and process risk while helping control cost.
The right question is not:
> “Is VIPPO better than a conventional via?”
It is:
> “Does this PCB need VIPPO to meet its routing or performance requirements?”
What Should You Tell the PCB Manufacturer When Ordering VIPPO Boards?
If the design requires Via-in-Pad or VIPPO, avoid relying on a single email note that says only “VIPPO required.” Define the key requirements in the fabrication drawing or related manufacturing files.
Via Definition
Identify exactly which vias are VIPPO rather than asking the fabricator to infer them from Gerber geometry.
Layer Span
State which layers are connected by each through via, blind via, or microvia.
Hole Requirements
Specify drill size, finished-hole size, or microvia dimensions as applicable.
Via Fill
State whether non-conductive fill, conductive fill, copper filling, or another mutually agreed process is required.
Plated-Over Requirement
If the Via-in-Pad will serve as a component solder pad, explicitly require plating over or capping.
Surface Finish
Specify the required finish, such as ENIG, OSP, or immersion silver.
For a complex HDI PCB, also provide the confirmed stackup. Defining these details before production is usually more efficient than resolving them through engineering questions after fabrication has begun.
Why Does VIPPO Increase PCB Cost?
VIPPO usually costs more than a conventional through via because it adds real manufacturing operations, not because of an “advanced process” label.
After drilling and plating, a conventional via has largely reached its required structure. VIPPO still requires:
Via filling → curing → planarization → additional copper plating → surface inspection
If a PCB contains many Via-in-Pad locations, the manufacturer must also control fill quality, pad planarity, and copper-cap consistency across the board and production panel.
Actual cost depends on the number of VIPPO vias, via diameter, board thickness, HDI stackup, microvia structure, PCB size, surface finish, and panel utilization. A fixed statement such as “VIPPO adds 20%” cannot accurately describe every project.
For a conventional PCB, VIPPO may add unnecessary cost. In a dense BGA design that cannot be routed without Via-in-Pad, however, that cost is part of the required PCB architecture and may even be offset by avoiding a larger board or additional layers.
FAQ
Are Via-in-Pad and VIPPO the Same Thing?
Not exactly. Via-in-Pad describes a via located inside a component pad. VIPPO usually refers to a Via-in-Pad that has been filled, planarized, and plated over to create a complete solderable surface.
Must Every Via-in-Pad Be Filled and Copper-Capped?
No. If the pad directly supports a BGA, CSP, LGA, or similar component, the Via-in-Pad normally requires appropriate treatment to prevent solder wicking and create a flat soldering surface. Thermal vias and vias in non-soldered areas may have different requirements.
Is Conductive Via Fill Always Better Than Non-Conductive Fill?
No. Fill material should be selected according to thermal transfer, current, via structure, and the validated PCB fabrication process. Many conventional VIPPO applications do not require conductive fill.
Can VIPPO Be Used With Microvias?
Yes. This combination is common in HDI and fine-pitch BGA designs. The microvia dimensions and structure must still be coordinated with the specific HDI stackup and reliability requirements.
Does VIPPO Always Make a PCB More Expensive?
Compared with a conventional via in the same construction, VIPPO generally adds manufacturing operations and therefore increases cost. If Via-in-Pad enables BGA fanout or avoids additional PCB layers, however, cost should be evaluated at the full layout and stackup level rather than as the price of one isolated process.
Conclusion
Via-in-Pad moves signal, power, or thermal connections directly into the PCB within a limited area.
When a via is located in a component pad that must be soldered, an open via is often unsuitable. Solder can enter the hole and the pad surface is no longer continuous.
VIPPO uses via filling, planarization, and copper plating to restore a flat, continuous soldering surface. That is why it is widely used with fine-pitch BGAs, CSPs, LGAs, and HDI PCBs.
The goal is not to select the most complex process. Designers should decide whether Via-in-Pad is genuinely required by package pitch, routing density, stackup, electrical requirements, and manufacturing capability.
If conventional dog-bone routing meets the requirements, it is usually the simplest and most economical solution. When PCB density exceeds the limits of conventional fanout, Via-in-Pad and VIPPO become practical and valuable design tools.