Thermal Via vs Signal Via Design

Vias are the unsung heroes of PCB design—those tiny plated holes that connect layers and make complex routing possible. But not all vias serve the same purpose. Understanding the difference between thermal vias and signal vias is crucial for effective thermal management and signal integrity.

Get this wrong, and you could end up with a board that overheats, generates noise, or fails prematurely. Let's break down the key differences, design rules, and when to use each type.

Signal Vias vs Thermal Vias: The Basics

Signal Vias

Signal vias carry electrical signals between PCB layers. Their primary design goal is signal integrity—minimizing impedance discontinuity, crosstalk, and signal degradation.

Sized for signal frequency and impedance
Often use anti-pads to isolate from planes
Placement affects routing and crosstalk
May need back-drilling for high-speed

Thermal Vias

Thermal vias conduct heat away from components to other layers or heat sinks. Their primary design goal is thermal conductivity—maximizing heat transfer through the PCB.

Sized for thermal conductivity
Connected to copper planes/pours
Placed directly under heat sources
Often filled or plugged

Quick Comparison

Signal Via vs Thermal Via Characteristics
Characteristic	Signal Via	Thermal Via
Primary Purpose	Carry electrical signals	Conduct heat
Typical Diameter	8-12 mil	10-20 mil
Typical Drill	6-10 mil	8-15 mil
Aspect Ratio	8:1 to 12:1	4:1 to 8:1
Filling	Usually open	Often filled
Plating	Standard (0.8-1 mil)	Thicker preferred
Array Pattern	Single or few	Grid array
Plane Connection	Isolated or single	Maximum copper

Thermal Via Design Guidelines

Thermal vias are essentially heat pipes through your PCB. Their effectiveness depends on several factors:

1. Via Size and Plating

Bigger vias conduct more heat, but there's a practical limit. The thermal conductivity comes from the copper plating on the barrel wall, not the air or fill material inside.

Thermal Via Size vs Heat Conduction
Via Drill	Finished Size	Thermal Resistance	Relative Performance
8 mil	6 mil	~95°C/W	Fair
10 mil	8 mil	~85°C/W	Good
12 mil	10 mil	~75°C/W	Better
15 mil	13 mil	~65°C/W	Best
20 mil	18 mil	~55°C/W	Excellent

2. Via Array Pattern

A single via won't cut it for serious heat transfer. Thermal vias are used in arrays under thermal pads and heat-generating components.

Recommended Via Array Density
Application	Via Pitch	Coverage
LED drivers	40-50 mil	15-25%
Power MOSFETs	30-40 mil	25-35%
Voltage regulators	35-45 mil	20-30%
High-power ICs	25-35 mil	30-40%

Rule of Thumb: Place thermal vias on a 1mm (40 mil) grid under exposed pads. Tighter grids improve thermal performance but increase manufacturing cost. Most fabs recommend minimum 25-30 mil pitch.

3. Via Filling Options

Thermal vias under exposed pads need special attention to prevent solder wicking during assembly:

Via Filling Options for Thermal Vias
Method	Cost	Thermal	Best For
Open (tented)	Low	Good	Non-critical pads
Plugged (epoxy)	Medium	Fair	General use
Filled + plated	High	Excellent	High-power devices
Copper-filled	Very High	Best	Maximum thermal

Signal Via Design Guidelines

Signal vias are all about maintaining signal quality as signals transition between layers. The key concerns are impedance discontinuity, parasitic capacitance, and inductance.

1. Via Impedance Considerations

Every via introduces a capacitive discontinuity because the barrel passes through reference planes. For high-speed signals, this can cause reflections and signal degradation.

Signal Via Impact by Frequency
Signal Speed	Via Impact	Mitigation
<100 MHz	Negligible	Standard via OK
100 MHz - 1 GHz	Moderate	Smaller vias, ground vias
1-5 GHz	Significant	Via optimization required
>5 GHz	Critical	Back-drilling, HDI vias

2. Ground/Return Vias

For controlled impedance signals, every signal via should have nearby ground vias to provide a low-inductance return path. This is especially important for differential pairs.

Ground Via Placement Rules:

Place ground vias within 20-30 mils of signal vias
For differential pairs: ground via between and on each side
Maintain ground via stitching along high-speed routes
Connect ground vias to all ground planes

3. Anti-Pads and Clearances

Signal vias need anti-pads (clearances) in reference planes to prevent shorts. But larger anti-pads mean more impedance discontinuity.

Anti-Pad Sizing Guidelines
Via Drill	Min Anti-Pad	Typical Anti-Pad
8 mil	20 mil	25 mil
10 mil	24 mil	30 mil
12 mil	28 mil	35 mil

When to Use Each Type

Use Thermal Vias For:

Exposed thermal pads on ICs, regulators, and power devices
LED thermal management - high-power LEDs need heat extraction
Power semiconductors - MOSFETs, IGBTs, and rectifiers
Heat spreader connections - linking to internal copper planes
Bottom-side cooling - transferring heat to heatsinks

Use Signal Vias For:

Layer transitions in signal routing
BGA/fine-pitch breakout - escaping from dense packages
Differential pair routing - with proper ground via placement
Power distribution (with proper current calculations)
Ground stitching - maintaining reference plane integrity

Thermal Vias Under Exposed Pads: Best Practices

Many modern ICs have exposed thermal pads on the bottom that require both electrical connection (usually ground) and heat extraction. Here's how to do it right:

1. Calculate Required Via Count

Use our Via Current Calculator to determine how many vias you need for both current capacity and thermal transfer. Typical thermal pads need 4-16 vias depending on power dissipation.

2. Choose Via Pitch

Space vias 1.0-1.2mm apart for optimal thermal performance. Tighter spacing improves heat transfer but complicates manufacturing. Never place vias closer than 0.5mm center-to-center.

3. Consider Solder Wicking

Open vias under solder pads can wick solder during reflow, creating voids and weak joints. Solutions: via tenting, plugging, filling, or using solder mask dams.

4. Connect to Internal Plane

Thermal vias should connect to a large copper area on inner layers (usually ground plane) to spread and dissipate heat. The effectiveness depends on plane size and copper weight.

Thermal Via Array Recommendations by Package
Package Type	Typical Pad Size	Via Count	Via Pitch
QFN 3x3	1.5mm × 1.5mm	4-6	0.8-1.0mm
QFN 5x5	3mm × 3mm	9-12	1.0-1.2mm
QFN 7x7	5mm × 5mm	16-25	1.0-1.2mm
DPAK/D2PAK	6mm × 8mm	12-20	1.5-2.0mm
TO-263	5mm × 10mm	15-25	1.5-2.0mm

Via Current Capacity: Signal vs Thermal

While thermal vias are optimized for heat transfer, they also carry current (usually to ground). Here's how current capacity compares:

Single Via Current Capacity (1oz plating, 10°C rise)
Via Type	Drill Size	Current Capacity
Signal via	8 mil	~0.5 A
Signal via	10 mil	~0.7 A
Thermal via	12 mil	~0.9 A
Thermal via	15 mil	~1.2 A
Thermal via (filled)	15 mil	~1.8 A

For high-current applications, you'll need multiple vias in parallel. See our Via Sizing Guide for detailed calculations.

Common Mistakes to Avoid

❌ Using signal via rules for thermal pads

Thermal pads need arrays of vias, not single vias. A 5mm thermal pad with one via in the corner won't transfer meaningful heat.

❌ Leaving thermal vias open under BGA pads

Open vias under BGA pads cause solder to wick away, creating voids. Always tent, plug, or fill thermal vias under solderable pads.

❌ Forgetting ground vias for high-speed signals

A signal via without nearby ground vias creates a discontinuity in the return path. At high frequencies, this causes EMI and signal integrity issues.

❌ Using the same via size for everything

Signal vias can be smaller (8-10 mil) to minimize capacitance. Thermal vias should be larger (12-20 mil) to maximize heat transfer. Use appropriate sizes for each purpose.

Design Checklist

Thermal Via Checklist

☐ Via array under all thermal pads
☐ Via pitch 1.0-1.2mm (40-50 mil)
☐ Connected to internal ground plane
☐ Vias plugged or tented if under solder
☐ Via count matches thermal requirements
☐ Current capacity verified

Signal Via Checklist

☐ Via size appropriate for signal speed
☐ Ground vias near high-speed signal vias
☐ Anti-pad size minimized
☐ Back-drilling considered for 5+ GHz
☐ Via stub length acceptable
☐ Differential pairs have symmetric vias

Summary

Thermal vias and signal vias serve different purposes and require different design approaches. Signal vias prioritize electrical performance—small size, minimal capacitance, controlled impedance. Thermal vias prioritize heat transfer—larger size, maximum copper, array placement.

Use our Via Current Calculator to determine the right via count for your current and thermal requirements. For trace width calculations to match your vias, check out the Trace Width Calculator.