VIPPO PCB Design Guide: Via Size, Pad Layout, BGA Routing and DFM

VIPPO (Via-In-Pad Plated Over) is a PCB technology that places a via directly inside a component pad, then fills and plates over the via to create a flat surface for component assembly. Compared with a conventional via-in-pad structure, VIPPO can reduce the surface area needed for BGA breakout routing and support higher routing density.

VIPPO is commonly used with fine-pitch BGA packages, HDI PCBs, high-density computing hardware, networking equipment, and other designs where PCB space is limited. However, VIPPO is not simply a matter of putting a via inside a pad. The design must also account for BGA pitch, pad size, via diameter, stackup, routing rules, filling, planarization, copper plating, and manufacturing tolerances.

This guide covers the main VIPPO PCB design considerations, including via size, pad layout, BGA fanout, via filling, copper capping, DFM, and common reliability concerns.

What Is VIPPO in PCB Design?

VIPPO stands for Via-In-Pad Plated Over. It places a via directly inside a component pad and uses a filled and plated-over structure to create a relatively flat solderable surface.

In a conventional BGA fanout, the via is normally placed outside the component pad. A short trace connects the BGA pad to the via before the signal moves to an inner layer.

The basic structure is:

BGA Pad → Short Trace → Via → Inner Layer

As BGA pitch becomes smaller, the space available for this type of breakout decreases. VIPPO changes the routing structure to:

BGA Pad → VIPPO Via → Inner Layer

The via occupies the same area as the component pad, removing the need for a separate escape trace between the pad and via.

A VIPPO structure normally requires via filling, surface planarization, and plating over the filled via. IPC-4761 provides guidance for protected and planarized via structures, including planarized and capped configurations.

For a broader overview of VIPPO technology and its applications, SLLPCB also covers the topic in its VIPPO PCB Guide.

When Should You Use VIPPO?

VIPPO is not required for every BGA or high-density PCB.

If a BGA has enough routing space for a conventional dog-bone fanout, using VIPPO may only add manufacturing cost and process complexity without providing a meaningful layout benefit.

VIPPO becomes more useful when:

• BGA pitch is small
• Conventional fanout cannot escape all required signals
• Routing channels are limited
• PCB size is constrained
• The design requires high routing density
• HDI technology is already required
• Direct connections from BGA pads to inner layers are needed
• A shorter interconnect path is useful for certain high-speed nets

BGA Pitch and VIPPO

BGA pitch is one of the main factors that determines the available fanout strategy. As pitch decreases, the space between adjacent pads becomes smaller, making conventional dog-bone routing more difficult. Current HDI design guidance shows why fine-pitch BGA designs often move from mechanical vias toward microvias and via-in-pad structures as pitch and routing density increase.

The following table can be used as an initial engineering reference:

BGA Pitch	Typical Routing Situation	VIPPO Consideration
1.27 mm	Large breakout space	Usually unnecessary
1.00 mm	Conventional fanout often possible	Depends on routing requirements
0.80 mm	Routing space becomes tighter	May be useful
0.65 mm	Dog-bone fanout becomes more difficult	Often worth considering
0.50 mm	Very limited breakout space	Often combined with HDI
0.40 mm	Extremely dense routing	Advanced HDI/VIPPO often required

These are not universal manufacturing rules. The actual transition point depends on BGA pad size, trace width, spacing, via geometry, layer stackup, and the PCB fabricator’s process capability.

VIPPO Via Size and Design Rules

Via size is one of the most important parameters in VIPPO design.

A smaller via can release more routing space around a BGA, but smaller vias also place greater demands on drilling, laser processing, filling, plating, and registration.

The main parameters include:

• Finished hole diameter
• Drill diameter
• Via pad diameter
• Annular ring
• Aspect ratio
• Layer-to-layer registration
• Via filling capability
• Copper plating thickness
• Dielectric thickness

Mechanical VIPPO Vias

For mechanically drilled VIPPO structures, the practical via size depends heavily on board thickness, copper thickness, aspect ratio, drilling capability, and filling process.

As an early design reference, engineers may evaluate ranges such as:

Parameter	Typical Engineering Reference
Finished hole	0.20–0.30 mm
Advanced mechanical via	About 0.15–0.20 mm
Via aspect ratio	Often controlled around 8:1 or lower
Annular ring	About 0.075–0.10 mm or more
Via pad diameter	Determined by the BGA pad and manufacturing tolerance

These values should not be treated as universal minimum manufacturing limits.

For example, whether a 0.15 mm mechanical hole is practical depends on board thickness, copper weight, hole depth, drilling process, plating, and the fabricator’s actual capability.

Laser-Drilled Microvia VIPPO

For finer-pitch BGA packages, laser-drilled microvias can provide much higher routing density than conventional mechanical vias.

A typical engineering evaluation may include:

Parameter	Typical Range
Laser via diameter	0.075–0.15 mm
Dielectric depth	About 0.05–0.10 mm
Microvia aspect ratio	Commonly around 1:1 or lower
Capture pad	About 0.20–0.30 mm or larger

These are reference values rather than fixed industry limits. The final geometry must be matched to the dielectric thickness, laser drilling capability, copper structure, and registration tolerance.

For example, current HDI design guidance shows that a 0.5 mm BGA can require laser-drilled microvia-in-pad structures when conventional mechanical dog-bone routing cannot fit within the available space.

This is also where HDI PCB design becomes directly relevant, because microvia diameter, dielectric thickness, layer span, and BGA fanout must be designed as one stackup problem.

VIPPO Pad Size and Via-in-Pad Layout

The VIPPO via must fit completely within the component pad while leaving enough copper around the via to accommodate manufacturing tolerances.

A simplified relationship can be written as:

Pad Diameter ≥ Via Diameter + 2 × Required Copper Margin

However, this equation should not be used by itself to determine the final BGA pad size.

The correct design sequence is:

Package Drawing → Recommended Land Pattern → PCB Pad → VIPPO Via → Registration Check → Manufacturing Review

The PCB pad should first follow the component manufacturer’s package drawing and recommended land pattern. The VIPPO via is then selected to fit within that pad while maintaining the required manufacturing margin.

This is important because enlarging a BGA pad simply to accommodate a larger via can change the solder joint geometry and may create assembly problems.

NSMD and SMD Pads

BGA packages commonly use either NSMD or SMD pad structures.

Pad Type	Structure	VIPPO Consideration
NSMD	Solder mask opening is larger than the copper pad	Common in BGA designs
SMD	Solder mask defines the pad edge	Used for specific package and process requirements

The choice affects solder mask clearance, pad geometry, solder joint formation, and manufacturing tolerance.

For fine-pitch BGA designs, the pad structure should therefore be based on the package manufacturer’s recommended land pattern rather than selecting NSMD or SMD only because a VIPPO via needs to fit inside the pad.

VIPPO BGA Routing Strategy

One of the main advantages of VIPPO is that it reduces the surface area required for BGA breakout.

Conventional Dog-Bone Fanout

A conventional dog-bone fanout normally uses:

BGA Pad → Short Trace → Via → Inner Layer

This structure is relatively simple and usually has lower manufacturing complexity.

It works well when there is enough space between BGA pads to accommodate the trace, via pad, annular ring, and required clearances.

As BGA pitch decreases, however, this space becomes increasingly difficult to maintain.

VIPPO Fanout

VIPPO changes the structure to:

BGA Pad → VIPPO → Inner Layer

The short escape trace between the BGA pad and via is removed.

This can provide more routing space around the BGA and can reduce the number of routing layers needed in some designs.

Routing Method	Surface Space	Fine-Pitch BGA	Manufacturing Complexity
Dog-bone	Higher	More suitable for larger pitch	Low
Conventional via-in-pad	Lower	Suitable for some fine-pitch designs	Medium
VIPPO	Very low	Highly suitable	High
VIPPO + microvia	Lowest	Suitable for very fine pitch	Very high

Fine-pitch BGA routing often requires a combined decision about pad size, via size, trace/space, and stackup. Microvia-in-pad is one of the main techniques used when conventional fanout cannot provide enough routing channels.

VIPPO Design for 0.8 mm, 0.65 mm and 0.5 mm BGA

Different BGA pitches can require very different fanout strategies.

0.8 mm BGA

A 0.8 mm BGA can often be routed with conventional fanout, depending on the pad diameter, trace/space, via size, and layer count.

VIPPO may still be useful when:

• the BGA has a high pin count
• board space is limited
• the design needs fewer routing layers
• the stackup already uses HDI
• routing density is high

There is no need to use VIPPO simply because the package is a BGA.

0.65 mm BGA

At 0.65 mm pitch, the available routing space becomes more restrictive.

Depending on the land pattern and PCB design rules, a conventional dog-bone fanout may require smaller vias, tighter trace/space, or additional routing layers.

VIPPO can eliminate the short surface trace between the BGA pad and via and provide more room for escape routing.

For this pitch, the decision should be made together with the stackup rather than after routing has already started.

0.50 mm BGA

A 0.50 mm BGA is a common point where conventional fanout becomes much more difficult.

For example, one current HDI design analysis shows how a 0.5 mm BGA with a small land pattern can quickly exceed the available geometry for mechanically drilled dog-bone routing, making laser microvia-in-pad a practical alternative.

A 0.50 mm BGA design may therefore require:

• VIPPO
• Laser microvias
• HDI build-up layers
• Stacked or staggered microvias
• Tighter registration control
• Fine trace/space rules

0.40 mm BGA

A 0.40 mm BGA requires even tighter control of via geometry, trace/space, and layer registration.

For these designs, VIPPO may be combined with laser microvias and advanced HDI structures.

The design review should confirm:

• BGA land pattern
• Pad diameter
• Laser via diameter
• Via pad diameter
• Pad-to-via registration
• Dielectric thickness
• Fill capability
• Copper cap
• Surface flatness
• Trace/space capability

At this level of density, the PCB fabricator should be involved before the layout is finalized. Fine-pitch BGA design guidance also recommends checking the fabricator’s supported via geometry and tolerances before selecting the final structure.

VIPPO Via Filling, Planarization and Copper Cap

The reliability of a VIPPO structure depends heavily on how the via is filled and how the surface is finished.

A typical manufacturing sequence is:

Drilling → Via Filling → Planarization → Copper Plating/Capping → Surface Finish

Via Filling

VIPPO vias may use different filling approaches depending on the PCB construction and required performance.

Common approaches include:

• Resin filling
• Conductive filling
• Copper filling

The choice depends on thermal requirements, reliability, process capability, and cost.

VIPPO should therefore not automatically be described as requiring solid copper filling in every application. The key requirement is a suitable filled structure that can be planarized and plated over for the intended assembly process.

Planarization

After filling, the surface needs to be controlled so that excessive material does not remain above the surrounding copper and the via does not create an unacceptable depression.

IPC-4761 describes planarized via protection as a structure where excess plugging or fill material is removed to produce a co-planar surface.

Planarity matters because the VIPPO surface may become part of the actual BGA soldering surface.

Poor surface control can affect:

• Solder paste deposition
• BGA ball placement
• Solder joint formation
• Assembly yield
• Local solder volume

Copper Cap

After filling and planarization, copper plating creates the final plated-over surface.

The copper cap connects the filled via to the component pad and provides a solderable surface.

For fine-pitch BGA applications, copper cap thickness, uniformity, and surface flatness should all be controlled as part of the fabrication process.

VIPPO DFM Requirements

VIPPO requires more manufacturing control than a standard through-hole via.

Before releasing a VIPPO design for production, the following items should be reviewed:

DFM Item	Why It Matters
Via diameter	Determines drilling and filling feasibility
Drill tolerance	Affects via location and registration
Aspect ratio	Affects plating and filling
Annular ring	Provides manufacturing margin
Pad diameter	Must match the package land pattern
Via fill	Controls the internal via structure
Fill voids	Can affect reliability
Planarity	Important for BGA soldering
Copper cap	Creates the plated-over solderable surface
Layer registration	Critical for fine-pitch structures
Surface finish	Must be compatible with assembly

For HDI designs, the fabricator should also confirm laser drill depth, laser hole diameter, location tolerance, fill and cap options, planarization capability, and supported microvia stacking structures before layout is finalized.

For broader fabrication requirements, the design can also be reviewed against the available PCB manufacturing capabilities before production release.

VIPPO Reliability and Common Failure Modes

VIPPO is not reliable simply because a via has been filled and plated over. The entire via, pad, plating, and assembly structure must be controlled.

Common problems include:

Failure Mode	Possible Cause	Control Direction
Solder wicking	Open or poorly filled via	Use an appropriate filled and plated-over structure
Surface dimple	Poor filling or planarization	Control fill and surface flatness
Fill void	Incomplete filling	Control filling process and inspection
Registration error	Drill or layer misalignment	Control registration tolerance
BGA solder defect	Pad or cap surface variation	Optimize pad and surface structure
Thermal reliability issue	Incompatible via structures	Review stackup and via construction

Solder wicking is one of the main reasons open vias are generally avoided directly inside BGA solder pads. A filled and plated-over structure provides a controlled surface and prevents solder from freely entering the via barrel during reflow.

For thermal-pad applications, VIPPO also has its own design considerations. IPC-7093A specifically includes a section for VIPPO thermal pad design, showing that via-in-pad structures need to be considered together with the assembly process rather than treated only as a routing feature.

VIPPO vs Via-in-Pad vs Dog-Bone

The three structures have different design and manufacturing characteristics.

Feature	Dog-Bone	Via-in-Pad	VIPPO
Via location	Outside pad	Inside pad	Inside pad
Via filling	Not required	Not always required	Normally required
Plated over	No	Not always	Yes
Routing density	Medium	High	Very high
Fine-pitch BGA	Limited	Suitable for some designs	Highly suitable
Manufacturing cost	Lower	Medium	Higher
Process complexity	Low	Medium	High
Surface flatness requirement	Normal	Higher	High

Dog-bone fanout remains useful when the BGA has enough space for conventional routing.

Via-in-pad reduces the space between the component pad and via, but an open via inside a solder pad can create soldering problems.

VIPPO adds filling and plating over the via to create a controlled solderable surface, making it suitable for applications where the via must occupy the BGA pad itself.

When Is VIPPO Worth Using?

VIPPO is most valuable when it solves a real routing or packaging constraint.

VIPPO is a good option when:

• BGA pitch is very small
• Dog-bone fanout cannot escape the required signals
• PCB size is constrained
• Routing layer count needs to be controlled
• HDI technology is already required
• BGA routing density is high
• Direct pad-to-inner-layer connections are needed

VIPPO may not be necessary when:

• BGA pitch is relatively large
• Conventional dog-bone fanout works
• There is enough PCB routing space
• VIPPO does not reduce routing layers
• The additional manufacturing cost provides little layout benefit

The goal should not be to use VIPPO simply because it is a more advanced PCB technology. The goal is to select the simplest structure that can meet the required routing density, assembly, reliability, and manufacturing requirements.

VIPPO PCB Design Checklist

Before releasing a VIPPO PCB for fabrication, review the following items:

• Confirm the BGA pitch
• Confirm the package land pattern
• Confirm BGA pad diameter
• Select dog-bone or VIPPO fanout
• Define via diameter
• Check finished hole and drill dimensions
• Check via aspect ratio
• Check annular ring
• Check pad-to-via registration
• Define the via fill method
• Define copper cap requirements
• Check surface planarity
• Confirm the HDI stackup
• Check trace and space
• Check solder mask geometry
• Confirm surface finish
• Complete a fabricator DFM review

For high-density BGA designs, these decisions should be made during stackup planning rather than after routing is complete. The BGA pitch, via structure, and stackup directly influence whether the board can be routed within the available layer count.

FAQ

What BGA pitch usually requires VIPPO?

There is no universal BGA pitch at which VIPPO becomes mandatory. A 0.8 mm BGA can often use conventional fanout, while 0.65 mm, 0.5 mm, and smaller pitches are more likely to require via-in-pad or HDI structures. The actual decision depends on pad size, trace/space, via geometry, layer count, and fabricator capability.

What via size should be used for VIPPO?

The appropriate VIPPO via size depends on BGA pitch, pad size, layer structure, dielectric thickness, aspect ratio, and the PCB fabricator’s process capability. Mechanical VIPPO structures may be evaluated around the 0.15–0.30 mm range, while high-density HDI designs may use much smaller laser-drilled microvias. These should be treated as engineering reference ranges rather than universal minimums.

Does VIPPO require copper-filled vias?

Not every VIPPO structure requires solid copper filling. Resin or other suitable filling materials can also be used depending on the design and fabrication process. The important requirement is that the via can be properly filled, planarized, and plated over to provide the required surface for assembly.

Should VIPPO use NSMD or SMD pads?

Either structure can be used depending on the package and assembly requirements. The recommended BGA land pattern should be established first, then checked against the VIPPO via geometry, solder mask design, and fabrication capability.

What IPC standard applies to VIPPO?

IPC-4761 provides guidance for protection and treatment of PCB via structures, including planarized and capped structures. IPC-7093A also specifically addresses VIPPO thermal-pad design. The final production requirements should be agreed between the PCB designer, customer, and fabricator.

How does VIPPO affect PCB cost?

VIPPO normally increases PCB fabrication cost because it requires additional processes such as via filling, planarization, and plating. However, it can also reduce routing layers, PCB size, or routing complexity in high-density designs. The cost impact should therefore be evaluated together with the overall stackup and layout.

Can VIPPO be used with HDI PCB?

Yes. VIPPO is commonly combined with HDI structures, especially for fine-pitch BGA packages. Laser microvias, sequential build-up, and VIPPO can be used together to increase routing density and provide direct connections from BGA pads to inner layers. Current HDI guidance specifically identifies microvia-in-pad as a key technique for fine-pitch BGA breakout.