What is PCB Transmission Loss? A Complete Engineer’s Guide to Signal Attenuation

I’ve been designing high-speed PCBs for over a decade, and if there’s one topic that keeps coming up in every 5G, data center, or RF project, it’s transmission loss. Whether you’re routing 25 Gbps SerDes channels or designing a 77 GHz automotive radar, understanding how signals attenuate on your board isn’t optional anymore—it’s fundamental.

In this guide, I’ll walk you through everything you need to know about transmission loss in PCBs, from the physics behind it to practical techniques for minimizing signal attenuation in your designs.

Understanding Transmission Loss in PCB Design

Transmission loss refers to the reduction in signal strength as electrical energy propagates along a PCB trace. When a signal travels from a driver to a receiver, some of that energy gets converted to heat or radiates away rather than reaching the destination. This signal attenuation becomes increasingly problematic at higher frequencies, which is exactly why modern high-speed designs require such careful attention.

The total transmission loss in a PCB transmission line consists of several components working together. The industry typically expresses this as insertion loss (αt), which combines conductor loss (αc), dielectric loss (αd), radiation loss (αr), and leakage loss (αl). In practical designs, leakage loss is negligible due to the high volume resistance of PCB materials, and radiation loss mainly affects thicker substrates at very high frequencies.

For most engineering purposes, the equation simplifies to:

Transmission Loss = Conductor Loss + Dielectric Loss + Scattering Loss

This relationship forms the foundation for all signal integrity analysis in high-frequency PCB design.

The Four Primary Causes of Transmission Loss

Conductor Loss: When Copper Works Against You

Conductor loss stems from the resistance of copper traces and reference planes. At DC and low frequencies, current flows through the entire cross-section of a conductor. But as frequency increases, something interesting happens—current starts concentrating near the surface of the conductor. This phenomenon, called the skin effect, dramatically increases the effective resistance of your traces.

The skin depth (δ) decreases with frequency according to a well-established relationship. At 1 MHz, skin depth in copper is approximately 66 μm. By 10 GHz, it drops to just 0.66 μm. This means your 1 oz copper trace (35 μm thick) becomes essentially irrelevant for high-frequency signals—only that thin outer layer carries current.

From a practical standpoint, this explains why increasing copper weight doesn’t help high-frequency designs. Instead, you need wider traces to provide more surface area for the current to flow.

Dielectric Loss: The Material Makes the Difference

Dielectric loss occurs within the substrate material itself. As electromagnetic fields propagate through the dielectric, molecular polarization causes energy dissipation. Two material properties govern this behavior:

The dielectric constant (Dk or εr) determines signal propagation speed and impedance. Lower Dk values mean faster signal propagation and generally better performance.

The dissipation factor (Df or tanδ) directly measures how much energy the material absorbs. Standard FR4 has Df values around 0.02 at 10 GHz, while premium materials like Rogers RO4350B achieve values below 0.004.

Unlike conductor loss, which increases with the square root of frequency, dielectric loss increases linearly with frequency. At frequencies above 5-10 GHz, dielectric loss often becomes the dominant loss mechanism in low-loss designs.

Scattering Loss: The Hidden Contribution

Scattering loss is the lesser-known contributor that only recently gained recognition in the signal integrity community. This loss occurs at the interface between copper conductors and dielectric materials where surface roughness creates non-ideal boundaries.

PCB manufacturing intentionally roughens copper surfaces to improve adhesion between layers. This roughening creates micro-scale peaks and valleys that force high-frequency currents to travel longer paths, increasing resistance beyond what smooth copper would exhibit.

Research has demonstrated that copper roughness can increase losses by up to 20% at high frequencies, making copper profile selection a critical design decision.

Radiation Loss: Energy Escaping the Transmission Line

Radiation loss represents energy that escapes from the transmission line structure and radiates into space. This loss depends on substrate thickness, frequency, and dielectric constant. Microstrip lines are particularly susceptible because their fields aren’t fully contained.

Thinner substrates and higher Dk values reduce radiation loss by better confining electromagnetic fields. Stripline structures virtually eliminate radiation loss since fields are contained between ground planes.

How Frequency Affects Transmission Loss

The relationship between frequency and transmission loss isn’t simple—it’s actually the sum of two different frequency dependencies:

Loss Type	Frequency Relationship	Dominant Range
Conductor Loss	Proportional to √f	Lower frequencies (below 5-10 GHz)
Dielectric Loss	Proportional to f	Higher frequencies (above 10 GHz)
Scattering Loss	Complex relationship	Becomes significant above 1 GHz
Radiation Loss	Increases with f	Very high frequencies on thick substrates

This frequency dependency explains why different design strategies work at different speeds. At 3-5 GHz, impedance matching and trace geometry dominate performance. Above 10 GHz, material selection becomes the primary factor.

Material Selection for Low Transmission Loss

Choosing the right PCB material is often the most impactful decision for managing transmission loss. Here’s a comparison of common materials:

Material	Dk @ 10GHz	Df @ 10GHz	Best Application	Relative Cost
Standard FR4	4.2-4.8	0.015-0.025	Low frequency, cost-sensitive	1x
High-Speed FR4 (IS408HR)	3.6-4.0	0.008-0.012	Mid-speed digital, 10-25 Gbps	2-3x
Megtron 6	3.4	0.004	High-speed digital, 25-56 Gbps	4-6x
Rogers RO4350B	3.48	0.0037	RF/Microwave, 5-40 GHz	5-8x
PTFE (RT/Duroid)	2.1-2.5	0.001-0.002	Microwave, mmWave	8-15x

A common misconception is that you always need exotic materials for high-frequency work. In my experience, standard FR4 performs adequately for many WiFi applications below 5 GHz, especially on smaller boards. The key is matching material capability to actual performance requirements.

Copper Roughness and Surface Profile Selection

Surface roughness has become one of the most discussed topics in high-speed design, and for good reason. The table below shows typical roughness values for different copper types:

Copper Type	Roughness (Rz)	Applications	Signal Integrity Impact
Standard ED	6-8 μm	General purpose, up to 3 GHz	High loss at frequencies above 1 GHz
Low Profile (LP)	4-5 μm	Mid-speed digital, 3-10 GHz	Moderate improvement
Very Low Profile (VLP)	2-3 μm	High-speed digital, 10-25 GHz	Significant loss reduction
Hyper VLP (HVLP)	1-2 μm	25+ Gbps, mmWave	Minimal roughness impact up to 20 GHz
Rolled Annealed (RA)	<1 μm	Highest performance RF	Best available, highest cost

The skin depth at 1 GHz is approximately 2.1 μm. When copper roughness exceeds this value, the rough surface creates additional path length for current flow, directly increasing conductor loss. This is why standard ED copper with 6-8 μm roughness causes noticeable performance degradation above 1 GHz.

PCB Stack-up Optimization Strategies

Your stack-up design significantly impacts transmission loss through several mechanisms. Here are practical approaches I use in my designs:

Dielectric Thickness Selection: Thicker dielectrics allow wider traces for the same impedance, reducing resistive losses. However, they also increase radiation loss on microstrip lines. Finding the balance requires simulation.

Trace Width Optimization: Wider traces mean lower resistance and lower conductor loss. A 20% reduction in Dk can enable 23% wider traces at the same impedance, potentially reducing insertion loss by 13%.

Fiberglass Weave Considerations: The glass weave pattern affects both Dk uniformity and loss. Tighter weaves (1080, 2116) provide more uniform dielectric properties. For differential pairs, angling traces at 5-15 degrees relative to the weave can reduce skew caused by Dk variations.

Reference Plane Quality: Solid, unbroken reference planes minimize return path inductance and keep currents flowing directly under signal traces.

Practical Design Techniques for Reducing Transmission Loss

Beyond material selection, several design practices help minimize transmission loss:

Keep Traces Short: This sounds obvious, but trace length optimization through component placement often gets overlooked. Every unnecessary inch of trace adds to your loss budget.

Minimize Via Transitions: Each via represents a discontinuity that contributes to both insertion loss and return loss. Layer assignment that minimizes via count improves performance.

Use Appropriate Trace Structures: Stripline offers lower loss than microstrip at equivalent dimensions due to better field containment. Edge-coupled stripline differential pairs often outperform broadside-coupled configurations.

Consider Surface Finish Impact: ENIG (electroless nickel immersion gold) adds a nickel layer that increases skin effect losses compared to pure copper finishes. At very high frequencies, finishes like ENEPIG or copper OSP may perform better.

Impedance Matching: While technically return loss rather than transmission loss, impedance discontinuities cause reflections that reduce the power reaching your receiver.

Measuring and Validating Transmission Loss

Validating transmission loss requires proper test structures and equipment. Common approaches include:

Vector Network Analyzer (VNA): Measures S-parameters directly, with S21 representing insertion loss. TRL (Thru-Reflect-Line) calibration provides the best accuracy for PCB measurements.

Time Domain Reflectometry (TDR): While primarily used for impedance characterization, TDR data can indicate loss through amplitude reduction along transmission lines.

Test Coupons: Include transmission line test structures on every high-speed design for characterization and quality monitoring.

Industry standards such as IPC-TM-650 provide standardized test methods for dielectric constant and loss tangent measurements.

Industry Resources and Reference Materials

For engineers wanting to dive deeper into transmission loss analysis, these resources provide valuable information:

Material Datasheets and Construction Lists

• Rogers Corporation Technical Resources: https://www.rogerscorp.com/advanced-electronics-solutions
• Isola Group Materials Database: https://www.isola-group.com/products/
• Panasonic Megtron Series Data: https://industrial.panasonic.com/

Design Tools and Calculators

• Rogers MWI Calculator: Available through Rogers Technology Support Hub
• Altium Designer Layer Stack Manager: Integrated impedance and loss calculations
• Polar Instruments SI Calculators: Professional-grade transmission line analysis

Technical Publications

• Signal Integrity Journal: https://www.signalintegrityjournal.com
• IPC Standards (IPC-2141, IPC-2152): https://www.ipc.org
• IEEE Transactions on Components, Packaging and Manufacturing Technology

Reference Books

• “High-Speed Signal Propagation” by Howard Johnson
• “Signal and Power Integrity Simplified” by Eric Bogatin
• “The Foundations of Signal Integrity” by Paul Huray

Frequently Asked Questions About PCB Transmission Loss

What is the difference between transmission loss and insertion loss?

These terms are often used interchangeably in PCB design contexts. Technically, insertion loss is the measured reduction in signal power caused by inserting a device or transmission line into a circuit, expressed in decibels. Transmission loss specifically refers to the power lost during propagation. In practice, when we measure a trace’s S21 parameter, we’re measuring insertion loss, which includes transmission loss as its primary component.

At what frequency does transmission loss become a significant concern?

Transmission loss starts becoming noticeable above 1 GHz for standard FR4 materials. Above 3-5 GHz, careful material selection becomes important. Above 10 GHz, every aspect of the design—material, copper roughness, trace geometry, via design—requires attention. For modern interfaces like PCIe Gen5 (32 GT/s) or 112G PAM-4, transmission loss is a primary design constraint.

Does increasing copper thickness reduce transmission loss?

Not for high-frequency signals. Due to the skin effect, increasing copper weight beyond what’s needed at your operating frequency provides no benefit. At 10 GHz, current only flows in the outer 0.66 μm of the conductor. Increasing trace width is far more effective than increasing thickness for reducing high-frequency conductor loss.

How do I choose between FR4 and premium materials like Rogers?

Start with your frequency and loss budget requirements. For signals below 5 GHz on boards under 10 inches, standard or high-speed FR4 often works well. Above 10 GHz, or for long traces at 5-10 GHz, premium materials become necessary. Hybrid stack-ups using Rogers or similar materials only on critical signal layers can balance performance and cost.

Can simulation accurately predict transmission loss?

Modern 2D and 3D electromagnetic simulators can predict transmission loss with reasonable accuracy when provided correct material parameters. The challenge lies in obtaining accurate material data—published Dk and Df values may not reflect the specific construction or frequency range you’re using. Correlation to measured test coupons helps validate simulation accuracy for your fabrication process.

Final Thoughts on Managing Transmission Loss

Transmission loss isn’t going away—in fact, it’s becoming more critical as data rates continue climbing. The industry is already working on 224 Gbps PAM-4 signaling, pushing loss per inch requirements toward 1.1 dB at 56 GHz. Meeting these targets requires a coordinated approach: low-loss dielectrics, smooth copper, optimized geometries, and careful via design all working together.

The good news is that the tools and materials keep improving. Material suppliers continue developing lower-loss laminates, and EDA tools provide increasingly accurate modeling capabilities. For practicing engineers, staying current with material developments and measurement techniques is essential for tackling next-generation design challenges.

Understanding the physics behind transmission loss empowers you to make informed trade-offs between performance, manufacturability, and cost. Every project has different constraints, and knowing where your loss budget is going helps you allocate resources where they matter most.