Technical Article

PCB Material Properties and Their Impact on Performance of High Frequency Boards

July 05, 2023 by Dr. Steve Arar

Understanding PCB material parameters such as relative permittivity and loss tangent allows us to discuss some important considerations for choosing the right material when designing a high-speed/high-frequency application.

Important Parameters of a PCB Material

Some of the most important material parameters that affect the line’s attenuation are: 

  • the relative permittivity (εr or Er or Dk) of the dielectric material
  • the loss tangent (tan(δ) or Df) of the dielectric
  • conductor resistance which is affected by the skin effect and surface roughness 
  • and finally the fiberglass weave composition of the PCB.

A good understanding of these properties and the loss mechanisms in transmission lines can help us choose the right PCB material for our application. Material selection is the first step in the PCB design process. Today, designers of high-speed digital boards and RF products can choose from dozens of controlled-Dk and low-loss PCB materials. Many laminate suppliers have developed proprietary resin systems. 


Use a Low Dk and tan(δ) Material to Reduce Losses

For a low-loss transmission line, the dielectric loss in dB per inch is given by the following equation:

\[\alpha_d \text{(dB per inch)} = 2.32 f \ tan(\delta) \sqrt{\epsilon_r}\]

Equation 1.


where f is frequency in GHz. As can be seen, the dielectric loss is directly determined by the dielectric constant and loss tangent of the material. Therefore, we can use a material with lower tan(δ) and εr to limit ⍺d as much as possible. Three material choices that are recommended for very high Gbps transceivers are Nelco 4000-13EPSI, Rogers 4350B, and Panasonic Megtron 6. Figure 1 below compares the loss tangent of these materials with some other common materials.


Loss tangent as function of frequency for different PCB materials.

Figure 1. Loss tangent as function of frequency for different PCB materials. Image used courtesy of Intel


Use a Low-Dk Material to Reduce the Board Thickness

To better understand how using a low-Dk material allows us to reduce the board thickness, consider the stripline shown in Figure 2.


A stripline configuration

Figure 2. A stripline configuration. Image used courtesy of Sierra Circuits



The most popular approximation for the characteristic impedance of a stripline, recommended by the IPC, is:

\[Z_0 = \frac{60}{\sqrt{\epsilon_r}} ln \big ( \frac{2b+t}{0.8w+t} \big )\]

Equation 2.


  • t is the metal thickness (mil)
  • w is the line width (mil)
  • b is the plane-to-plane spacing (mil)


For a fixed Z0 and trace width w, if we use a material with larger εr, then we have to increase the spacing between the planes. In other words, a larger εr can increase the overall thickness of the board. In a high density board with many signal layers, this can significantly increase the board thickness. A thicker board means that your design needs vias with a larger aspect ratio. The aspect ratio of a via is its length divided by its diameter.

For example, if you have a board with a thickness of 0.2” and a via drill diameter of 0.02”, then the aspect ratio is 10:1. What is the difficulty of having a large aspect ratio? Recall that in order to provide electrical connectivity, the interior of the via needs to be covered with copper using a plating solution. Figure 3 shows the cross-section of a plated hole with an aspect ratio of 15:1.


Cross-section of a high-aspect plated hole with a 15:1 ratio

Figure 3. Cross-section of a high-aspect plated hole with a 15:1 ratio. Image used courtesy of C. Coombs


Most PCB manufacturers have the capability to create vias with an aspect ratio ranging between 6:1 and 8:1. With higher aspect ratios, plating becomes more and more difficult because the inner portions of the via barrel can have a thinner copper coating. This can even make the center of the via more prone to cracking under thermal stresses. Therefore, with larger aspect ratios, you might have to use more expensive PCB manufacturing techniques and have reliability concerns with your final board. The choice of a lower-Dk material can somewhat alleviate these issues. 


Dielectric Constant Changes With Frequency

The dielectric constant of a PCB material is a function of frequency. Figure 4 below shows the frequency dependency of the dielectric constant of some common PCB laminates.


Dielectric constant as a function of frequency.

Figure 4. Dielectric constant as a function of frequency. Image used courtesy of Altium


What are the consequences of Dk variations? The dielectric constant affects two important parameters: the characteristic impedance and wave velocity. The propagation velocity of a signal through a transmission line is given by:

\[v_p = \frac{c}{\sqrt{\epsilon_r}}\]

where c is the speed of light in a vacuum.

Due to Dk variations, different frequency components of the signal can experience slightly different signal velocities, leading to signal dispersion. Also as Dk decreases with frequency, the characteristic impedance of the line increases (Equation 2). This consequently degrades signal reflections at higher frequencies. Hence, it is desirable to use materials that have a flatter Dk versus frequency response over the frequency range of interest.    

Figure 4 shows that the Dk versus frequency response of FR4 family of materials exhibits a relatively larger variation. That’s why it is recommended to avoid this type of material in high speed/high frequency applications (another reason for this is the high dielectric loss of FR4 family of PCB laminates). Note that, unfortunately, most manufacturers specify the Dk values at only a few specific frequencies. 


Dielectric Constant Changes With Resin Content

The PCB material is a fiber/resin composite that can use different densities of weaves (Figure 5).


Figure 5. Image used courtesy of NWES


The dielectric constant of resin is less than that of the fiber. That’s why increasing the resin content reduces the effective Dk of the PCB laminate. Figure 6 shows how the dielectric constant of the FR408HR laminate changes with resin content.


Relative permittivity as a function of PCB laminate resin content.

Figure 6. Relative permittivity as a function of PCB laminate resin content. Image used courtesy of Isola


Therefore, in addition to the frequency of measurement, the laminate supplier should also specify the corresponding resin content. Table 1 gives the dielectric constant of a Hi Tg FR4 laminate for different constructions and resin contents at two different frequencies (1 MHz and 1 GHz). 


Table 1. Delectric constant of different Hi Tg FR4 laminates. Data used courtesy of Nelco via Altium



Resin Content

en @ 1 MHz

er @ 1 GHz


1 x 106





1 x 1080





1 x 2113





1 x 106 + 1 x 1080





1 x 2116





1 x 106 + 1 x 2113





1 x 2116





1 x 1080 + 1 x 2113





1 x 106 + 1 x 2116





2 x 2113





2 x 2113





1 x 7628





2 x 2116





2 x 7628





This table clearly shows that a given laminate thickness can have different dielectric constants. For example, the dielectric constant of a 0.004” thick laminate can vary from 4.11 to 4.54. The reason is that the available variants for a 0.004” thick laminate use different styles of woven glass and have different glass-to-resin ratios.


Fiber Weave Effect

As shown in Figure 5, PCB laminates and cores are made from woven glass impregnated with resin. This makes the material intrinsically inhomogeneous and anisotropic. In other words, certain areas of the board might be glass-dominated whereas some other regions are resin-rich. This can cause problems in demanding applications. To better understand this, consider the two traces shown below.


High-res image of woven glass PCB material.

Figure 7. High-res image of woven glass PCB material. Image used courtesy of Isola


In the above figure, trace 1 is over a fiber bundle while trace 2 is over a resin-rich area. This shows that depending on location, two traces on the same board can experience different effective dielectric constants.  As a result, the signal velocity for the two paths on the same board might not be the same, which can lead to timing skew in a high speed board. There are several different glass weave styles some of which are shown in Figure 5. As you can see, the non-uniformity of the material depends on the type of glass weave and size of the gaps in the weave. A sparsely woven material, such as 106 and 1080 glass cloth, produces a larger timing skew compared to more tighter weave styles. Exacerbated EMI and loss issues are two other undesired effects of sparsely woven materials. 

In addition to using glass weave styles with a more uniform distribution of glass, we can also use some trace routing techniques to have a more consistent Dk across the board. For example, we can route traces at an angle with respect to fiber warp/fill and/or use a zig-zag routing style to somewhat mitigate the glass weave effect. Note that a zig-zag routing consumes valuable board space and increases the loss due to the use of longer traces, while only partially solving the problem. To learn more about this effect, please refer to this Isola presentation


The Loss Tangent of the Board

Figure 8 below compares the loss vs frequency performance of some PCB materials. As you can see, certain materials are significantly less lossy than others. This information could help us decide which material could possibly perform better at higher speeds. As we go to higher and higher frequencies, materials that are less lossy and provide a flatter Dk versus frequency response should be employed.


Loss versus frequency for common PCB materials.

Figure 8. Loss versus frequency for common PCB materials. Image used courtesy of Sierra Circuits


Figure 9 below shows how the use of a PCB laminate system with low loss tangent can increase the cost of the PCB. As a point of reference, FR406 in this figure is the Hi Tg FR-4 material manufactured by Isola Corporation.


Lower loss tangent in PCB design typically requires higher costs.

Figure 9. Lower loss tangent in PCB design typically requires higher costs. Image used courtesy of Lee W. Ritchey


Popular Misconception About FR4 Boards

At this point it’s worthwhile to mention that, contrary to popular belief, the term “FR4” does not specify a particular PCB laminate with known dielectric constant or any other performance metrics. FR4 materials are a broad class of glass-weave resin-impregnated materials that are used as PCB substrates. There is a historical basis for its use as a laminate designator. In the early years of PCB technology, there were two original material choices: polyimide and epoxy-based materials. The term FR4 was the name used to refer to the latter group. FR4 came to mean “not polyimide” but it doesn’t specify a dielectric constant or any other performance metrics.


Use Simulation Tools and Measurements for Greater Accuracy

The data provided by laminate suppliers along with the first-order loss equations we have discussed in previous articles allow us to have an initial assessment of the material performance at the frequency of interest. However, it should be noted that when losses are important to us, we usually need analytical tools to have a more accurate estimation of the losses of the specific material being used over the operating frequency range. If there is a lot of money involved, we might not be able to trust even the simulated performance. In this case, we’d better build a test board with the real circuit to examine the actual performance of the material. It’s also important to make sure that the same laminate is used throughout the entire production cycle from prototype through to full production.


Featured image used courtesy of Adobe Stock