PCB thermal vias move heat from a hot component pad into internal copper, bottom-side copper, or an external heat sink. However, adding more holes does not guarantee a cooler component.
The complete heat path may contain resistance in the component package, solder joint, surface copper, via barrels, internal planes, thermal interface material, heat sink, and surrounding air. Therefore, thermal vias improve performance only when the rest of that path can receive and release the transferred heat.
Designers should select via diameter, quantity, pitch, plating, fill, and pad treatment from the actual power loss and allowable component temperature—not from one universal array pattern.
What Are PCB Thermal Vias?
PCB thermal vias are plated holes that primarily transfer heat between copper layers.
Designers usually place them:
- Inside an exposed component pad
- Around a thermal pad
- Beneath a power component
- Between top and bottom copper areas
- Above an external heat sink
- Near a high-current hot spot
- Under LEDs, processors, regulators, or power modules
A thermal via may use the same drilling and plating process as an ordinary electrical via. However, its placement and quantity support a thermal objective rather than signal routing.
A typical heat path follows this sequence:
Semiconductor Junction → Package Exposed Pad → Solder Joint → Top Copper → Thermal Via Barrels → Internal Or Bottom Copper → Heat Sink Or Air
If any part of this chain has excessive thermal resistance, adding more PCB thermal vias may provide only a small improvement.
How Do PCB Thermal Vias Transfer Heat?
FR-4 conducts heat poorly compared with copper. Therefore, heat moves slowly through the laminate thickness.
A plated via replaces part of that laminate path with a copper cylinder. Although the center of an open via contains air, its plated barrel creates a much more conductive vertical path.
PCB thermal vias normally perform two connected functions:
Vertical Heat Conduction
The copper barrel moves heat through the PCB thickness.
Lateral Heat Spreading
The via delivers heat into internal or bottom copper planes. Those planes then distribute the heat across a larger area.
Consequently, the receiving copper matters as much as the via itself. A dense via array connected to a very small bottom pad may simply move heat into another local hot spot.
When Do PCB Thermal Vias Work Well?
Thermal vias provide the most value when:
- The component transfers substantial heat through an exposed pad.
- A large internal or bottom copper area can receive the heat.
- The board connects to a heat sink or metal enclosure.
- The via barrels make solid copper-plane connections.
- The pad and solder joint provide adequate contact.
- Airflow can remove heat from the receiving area.
- The array distributes heat across the source pad.
- The design controls solder wicking and voiding.
They provide less value when:
- The package releases most heat through its top surface.
- The receiving copper area remains too small.
- A thermal relief restricts every via-to-plane connection.
- The heat sink lacks contact with the bottom copper.
- Thick dielectric separates useful copper structures.
- Solder voiding reduces contact under the exposed pad.
- Another thermal resistance already dominates the system.
Therefore, component package data should guide the starting design.
Infineon notes that thermal-via diameter and quantity depend on power consumption, final application, PCB construction, and thermal requirements in its package assembly recommendations.
How Many PCB Thermal Vias Do You Need?
No universal quantity works for every component.
The required number depends on:
- Component power dissipation
- Maximum junction temperature
- Ambient temperature
- Package thermal resistance
- Thermal-pad dimensions
- PCB thickness
- Via drill diameter
- Barrel plating thickness
- Via fill material
- Copper-plane area
- Copper thickness
- Airflow
- Heat-sink performance
- Thermal interface material
- Acceptable cost
Start with the component manufacturer’s recommended land pattern when one exists. Then compare that design with the actual board stackup and cooling structure.
More Vias Produce Diminishing Returns
The first few vias often produce the largest improvement because they replace a poorly conductive FR-4 path with copper.
However, nearby vias begin to share the same heat-spreading region. As the array grows, the package, solder joint, copper planes, or heat sink may become the dominant resistance.
Consequently, increasing an array from four to nine vias may produce a meaningful improvement, while increasing it from 25 to 30 may change the final component temperature very little.
Thermal simulation or prototype measurement should confirm high-power designs.
How To Estimate Thermal Via Resistance
Designers can estimate the ideal axial thermal resistance of a hollow plated via with:
Rθ Via ≈ L ÷ (kCu × π × D × t)
Where:
- Rθ Via = approximate via-barrel thermal resistance in °C/W
- L = via length in meters
- kCu = copper thermal conductivity, approximately 385–400 W/m·K
- D = approximate plated-hole diameter in meters
- t = barrel copper thickness in meters
This simplified formula assumes that the plating thickness remains small relative to the via diameter.
For several identical vias sharing heat evenly:
Rθ Array ≈ Rθ Via ÷ N
Where N represents the number of vias.
However, this equation calculates only the ideal barrel contribution. It does not include heat spreading, solder, package, laminate, plane, heat sink, airflow, or interface resistance.
Illustrative Calculation
Assume:
- PCB thickness: 1.60 mm
- Plated-hole diameter: 0.30 mm
- Barrel copper thickness: 25 µm
- Copper conductivity: 390 W/m·K
Approximate barrel area:
π × 0.00030 × 0.000025 = 2.36 × 10⁻⁸ m²
Approximate thermal resistance of one via:
0.00160 ÷ (390 × 2.36 × 10⁻⁸) ≈ 174°C/W
Ideal resistance for nine parallel vias:
174 ÷ 9 ≈ 19.3°C/W
Ideal resistance for 16 parallel vias:
174 ÷ 16 ≈ 10.9°C/W
These values do not represent junction-to-ambient thermal resistance. Instead, they show why one small hollow via provides limited vertical conduction and why an array performs better.
They also show why board thickness and plating thickness matter.
What Thermal Via Diameter Should You Use?
A larger plated hole provides more copper circumference and can reduce barrel thermal resistance.
However, larger holes also:
- Consume more pad area
- Remove solderable copper
- Increase solder-wicking risk
- Need larger annular rings
- Reduce routing space
- Limit via density
- May weaken a small exposed pad
Smaller vias allow a denser array and reduce solder loss through each opening. However, they increase drilling complexity and may require laser drilling when the diameter becomes too small for the board thickness.
Therefore, the best diameter depends on the complete array rather than one via.
Texas Instruments commonly shows vias of 0.3 mm or less with approximately 1 mm pitch in its PowerPAD layout guidance. However, TI also instructs designers to follow the device-specific datasheet.
Consequently, 0.3 mm and 1 mm should serve as a package-specific starting reference—not a universal PCB rule.
How Should PCB Thermal Vias Be Spaced?
Thermal via pitch must balance heat transfer, solderable area, copper continuity, and manufacturing capability.
If vias sit too far apart:
- Heat must travel farther through the surface copper.
- The center of the pad may remain hotter.
- The array may not use the complete pad effectively.
If vias sit too close together:
- Heat-spreading regions overlap.
- Additional vias provide smaller benefits.
- The pad loses continuous solderable copper.
- Drilling and plating become more difficult.
- Solder wicking can increase.
- Copper between holes may become too narrow.
Therefore, distribute the array across the heat-source area rather than concentrating every via in one location.
Check the finished copper between adjacent pads, not only drill-center pitch.
Where Should You Place PCB Thermal Vias?
The shortest thermal route normally places vias directly beneath the component’s exposed pad.
However, via-in-pad creates additional soldering requirements. If the budget or fabrication process cannot support suitable via treatment, designers can place vias immediately outside the solderable pad and connect them through wide copper.
Vias Inside The Thermal Pad
Advantages include:
- Short heat path
- Efficient use of pad area
- Direct connection to the heat source
- Compact layout
Possible risks include:
- Solder wicking
- Reduced solder coverage
- Package tilt
- Increased voiding
- Solder protrusion on the opposite side
- Higher fill-and-cap cost
Vias Outside The Thermal Pad
Advantages include:
- Lower solder-wicking risk
- Simpler PCB fabrication
- More continuous solderable pad area
- Easier stencil control
However, heat must travel laterally through the top copper before reaching the vias. Therefore, keep the connection short and wide.
The correct choice depends on component power, pad size, available area, manufacturing budget, and assembly yield.
Open, Tented, Plugged, Or Filled Thermal Vias
Via treatment affects soldering, cost, reliability, and thermal performance.
| Via Treatment | Main Benefit | Main Limitation | Typical Use |
|---|---|---|---|
| Open Via | Lowest Cost And Simple Processing | Solder Can Wick Into The Hole | Vias Outside Solderable Pads |
| Tented Via | Mask Covers One Or Both Ends | Mask May Not Reliably Seal Larger Holes | Small Vias Outside Critical Pads |
| Resin-Plugged Via | Reduces Solder Movement | Surface May Remain Uneven | Controlled Non-Pad Applications |
| Resin-Filled And Capped Via | Flat Solderable Surface | Higher Cost And More Processing | Via-In-Pad |
| Conductive-Filled Via | Adds Fill Conductivity | Material Performance Varies | Specialized Thermal Or Electrical Design |
| Copper-Filled Microvia | Strong Thermal And Electrical Path | HDI Cost And Process Limits | Dense High-Performance Designs |
Our PCB via filling article explains why plugging, filling, capping, and tenting describe different processes.
Does Nonconductive Resin Improve Heat Transfer?
Nonconductive resin fill often improves assembly control because it prevents solder loss and supports a plated cap.
However, the resin normally conducts much less heat than copper. Therefore, the copper barrel still carries most of the heat.
A nonconductive fill should not support a thermal claim unless the calculation includes the fill material’s documented thermal conductivity.
Does Conductive Fill Equal Solid Copper?
No. Conductive epoxy may contain metal particles, but its thermal and electrical conductivity usually remain below solid copper.
Copper-filled microvias or copper-plated structures can provide a stronger thermal path. However, they require different fabrication processes and cost.
Therefore, specify the actual fill material instead of writing only “conductive fill.”
PCB Thermal Vias And Via-In-Pad
When PCB thermal vias sit inside an SMT pad, the design becomes a via-in-pad structure.
A basic open via-in-pad can pull molten solder away from the package interface. As a result, the joint may contain less solder, more voiding, or uneven package standoff.
Filled and plated-over via-in-pad, often called VIPPO, creates a flat solderable surface and provides better process control.
However, VIPPO adds:
- Filling
- Planarization
- Copper capping
- Additional inspection
- Longer lead time
- Higher cost
Therefore, not every thermal pad needs full VIPPO. Small open vias, carefully segmented stencil apertures, or vias outside the solderable region may work for some assemblies.
Our via-in-pad article explains when VIPPO provides enough assembly and routing value to justify the additional process.
PCB Thermal Vias And Solder Paste
The thermal-pad stencil pattern controls solder volume and gas escape during reflow.
One large stencil opening can deposit excessive paste and trap flux volatiles. Therefore, assemblers often divide the thermal-pad aperture into several smaller windows.
This windowpane pattern can:
- Control total paste coverage
- Reduce component floating
- Provide gas-release channels
- Limit void size
- Balance solder across the pad
- Reduce paste loss into open vias
However, the assembler must coordinate aperture placement with the thermal-via pattern. A stencil opening directly above a large open via can feed solder into the barrel.
The component supplier’s package guidance provides a useful starting point. Nevertheless, production trials and X-ray inspection may require aperture adjustments.
Should Thermal Vias Use Thermal Relief?
Normally, no.
PCB thermal vias should move heat into internal or bottom copper. Thermal-relief spokes intentionally restrict heat flow into those planes.
Therefore, thermal vias generally need solid, full-circumference connections.
This rule differs from soldered through-hole component pins, which may need relief spokes to reach soldering temperature.
The previous PCB thermal relief article explains this functional difference.
A CAD library or global plane rule can accidentally apply relief spokes to every via. Consequently, designers should inspect the actual plane connection for each thermal array.
How Copper Planes Affect Thermal Via Performance
Thermal vias only transfer heat to another location. Copper planes spread and release that heat.
Important plane variables include:
- Area
- Copper thickness
- Number of connected layers
- Connection continuity
- Plane position
- Distance from the heat source
- Air exposure
- Heat-sink contact
- Nearby heat sources
Increasing copper area often provides a meaningful thermal improvement. However, the benefit eventually reaches a limit because convection, enclosure temperature, or another resistance controls the system.
Likewise, heavier copper can improve lateral heat spreading. Nevertheless, adding copper weight to every layer may cost more than improving the heat sink, airflow, or thermal interface.
The PCB copper thickness article explains how copper weight affects heat spreading, etching, current, and manufacturing cost.
How PCB Thickness Affects Thermal Vias
A thicker PCB creates a longer thermal-via barrel. Therefore, its axial thermal resistance increases when all other variables remain the same.
For example, a 3.2 mm board creates approximately twice the barrel length of a 1.6 mm board.
However, the thicker board may also contain more copper layers and larger internal planes. Consequently, the final thermal result depends on the complete structure.
Board thickness also affects drilling aspect ratio. A very small mechanical drill through a thick PCB may challenge plating reliability.
Therefore, the fabricator should review:
- Production drill size
- Finished hole size
- Board thickness
- Aspect ratio
- Barrel copper requirement
- Filling process
- Connected plane layers
- Reliability class
PCB Thermal Vias For Common Components
QFN And DFN Packages
These packages often transfer a large portion of their heat through the exposed center pad.
Use the component datasheet to define:
- Thermal-land dimensions
- Via diameter
- Via array
- Stencil coverage
- Electrical net
- Acceptable voiding
- Recommended copper area
Power MOSFETs
Power MOSFET packages may transfer heat through an exposed drain pad, source pad, or thermal tab.
Because the exposed pad may carry a switching voltage, the connected copper and thermal vias can also affect EMI and electrical clearance.
Therefore, do not automatically connect every thermal pad to ground.
LEDs
High-power LEDs need a low-resistance path from the thermal land into copper or a metal-core substrate.
FR-4 thermal vias may work for moderate power. However, demanding lighting products may require aluminum PCB, copper coin, insulated metal substrate, or an external heat sink.
Voltage Regulators
Regulators often use an exposed ground pad as their main thermal path.
Place vias according to the datasheet and keep high-(dv/dt) switch-node copper separate from the thermal-ground structure.
Processors And FPGAs
Large BGA devices may need many ground and power vias for electrical reasons in addition to thermal transfer.
Thermal design should account for package escape routing, via fields, internal plane distribution, heat sinks, and airflow.
Manufacturing Risks With PCB Thermal Vias
Insufficient Barrel Plating
The thermal calculation may assume a barrel thickness that production does not consistently achieve.
Therefore, drawings should define the applicable finished copper or hole-wall requirement when thermal performance depends on it.
Excessive Aspect Ratio
Small drills through thick boards can create difficult plating conditions. Poor barrel coverage reduces both thermal transfer and reliability.
Solder Wicking
Open vias within solderable pads can remove paste from the component interface.
Trapped Voids
Incomplete filling or poorly controlled tenting can trap gas, chemistry, or voids.
Uneven Capping
Via-in-pad surfaces must remain flat enough for reliable paste printing and component seating.
Drill Density
A very dense array can reduce laminate and copper between holes. It may also increase drill wear and cost without providing a proportional thermal improvement.
Incorrect Plane Connections
Thermal-relief spokes or missing internal pads can disconnect the array from useful heat-spreading layers.
What Haode Reviews Before Manufacturing
A useful DFM review connects the thermal design with both PCB fabrication and assembly.
Haode can review:
- Production drill diameter
- Finished via size
- PCB aspect ratio
- Annular ring
- Hole-wall copper
- Via pitch
- Copper remaining between vias
- Fill and cap requirements
- Solder-mask treatment
- Thermal-pad geometry
- Stencil compatibility
- Internal-plane connections
- Copper thickness
- Stackup
- Reflow and X-ray requirements
However, the OEM or thermal engineer should define the allowable junction temperature, operating power, ambient conditions, and required system thermal resistance.
The PCB manufacturer can confirm that the structure is buildable. It cannot determine the final product temperature without complete operating and mechanical data.
How To Validate PCB Thermal Vias
Thermal-via performance should be validated on a production-representative assembly.
Verify The Fabricated Structure
Use appropriate inspection to confirm:
- Drill and finished-hole size
- Barrel plating
- Fill quality
- Copper cap
- Plane connection
- Pad flatness
- Internal-layer registration
Microsection analysis can verify critical filled or plated structures.
Inspect The Solder Joint
X-ray inspection can evaluate:
- Thermal-pad voiding
- Solder loss into vias
- Uneven solder coverage
- Package alignment
- Large localized voids
Measure Temperature
Use:
- Thermocouples
- Calibrated infrared imaging
- Component temperature sensors
- Case-temperature measurement
- Power-cycling tests
- Environmental testing
Emissivity can distort infrared readings from shiny metal surfaces. Therefore, use a controlled measurement method.
Compare Controlled Variants
For critical designs, compare prototypes with different:
- Via counts
- Via patterns
- Copper areas
- Fill methods
- Heat-sink interfaces
- Airflow conditions
Quantitative comparison provides more evidence than assuming that the densest array performs best.
PCB Thermal Via Design Checklist
Before releasing the PCB, confirm:
- Does the component primarily transfer heat through its exposed pad?
- What power must the component dissipate?
- What junction-temperature limit applies?
- What ambient temperature and airflow will the product experience?
- Does the component manufacturer provide a recommended via pattern?
- Where will the vias transfer the heat?
- Is the receiving copper area large enough?
- Does the bottom copper contact a heat sink or enclosure?
- Have you estimated via-barrel thermal resistance?
- Does the design account for diminishing returns?
- Are the production drill and plating thickness manufacturable?
- Does the array preserve enough copper between holes?
- Will the vias sit inside or outside the solderable pad?
- Can open vias wick solder?
- Does the design require fill and copper capping?
- Does the stencil pattern match the via arrangement?
- Do all thermal vias connect solidly to the intended planes?
- Does board thickness create a difficult aspect ratio?
- Has the fabricator reviewed fill, plating, and cap requirements?
- Will first-article testing measure temperature and inspect voiding?
Frequently Asked Questions About PCB Thermal Vias
What Is The Best Thermal Via Size?
No universal size is best. The correct diameter depends on pad area, board thickness, plating capability, via quantity, soldering method, and thermal requirement.
A 0.3 mm diameter may provide a useful starting point for some packages, but the device datasheet and PCB manufacturer should control the final choice.
How Many PCB Thermal Vias Should I Use?
Use enough vias to meet the required thermal resistance without consuming unnecessary pad area or creating avoidable manufacturing cost.
Start with the component recommendation. Then verify the design through thermal calculation, simulation, or prototype testing.
Should Thermal Vias Be Filled?
Fill and cap thermal vias when the design places them inside a critical solderable pad and needs a flat surface or controlled solder volume.
Open vias outside the pad may not need filling.
Is Conductive Via Fill Better For Heat?
It can improve heat transfer, but performance depends on the fill material. Conductive epoxy does not have the same thermal conductivity as solid copper.
In many resin-filled vias, the plated copper barrel still carries most of the heat.
Should PCB Thermal Vias Be Tented?
Tenting may work for small vias outside solderable pads. However, solder mask alone may not reliably seal via-in-pad structures.
Use a controlled filling and capping process when assembly yield requires a flat, closed pad.
Should Thermal Vias Use Thermal Relief Spokes?
Normally no. Thermal relief restricts heat transfer, while thermal vias should conduct heat into other copper layers.
Do More Thermal Vias Always Reduce Temperature?
No. Additional vias provide diminishing returns when the component package, solder joint, copper plane, heat sink, airflow, or interface becomes the dominant thermal resistance.
Can Thermal Vias Replace A Heat Sink?
Sometimes they provide enough heat transfer for low- or moderate-power components. However, high-power products may still need a heat sink, metal enclosure, fan, copper coin, or metal-core PCB.
Can An Open Thermal Via Cause Solder Voids?
Yes. Molten solder and flux can move into an open via, reducing solder coverage or contributing to voiding beneath the package.
Does PCB Copper Weight Affect Thermal Via Performance?
Yes. Thicker copper can improve lateral heat spreading after the vias transfer heat into a plane. However, copper weight does not remove heat unless the system provides a path to air, a heat sink, or another cooling structure.
Final Recommendations For PCB Thermal Vias
PCB thermal vias form one section of a complete thermal circuit. They cannot compensate for a poor package connection, undersized copper plane, weak heat-sink interface, or inadequate airflow.
For reliable results:
- Start with component power and junction-temperature limits.
- Follow the device-specific land-pattern recommendation.
- Calculate the complete heat path, not only the via barrels.
- Use several small manufacturable vias rather than one oversized hole.
- Distribute the array across the thermal pad.
- Expect diminishing returns as the array becomes denser.
- Connect thermal vias solidly to useful copper planes.
- Coordinate via placement with stencil apertures and solder paste.
- Use fill and cap processes where open via-in-pad creates assembly risk.
- Do not assume nonconductive resin provides a copper-like heat path.
- Confirm drilling, plating, filling, and aspect ratio with the fabricator.
- Validate junction or case temperature on a production-representative PCBA.
The central design rule is:
Do Not Count Thermal Vias Until You Know Where The Heat Will Go After It Passes Through Them.
