ROG Blog

The Rog Blog is contributed by John Coonrod and various other experts from Rogers Corporation, providing technical advice and information about RF/microwave materials.

The Role of PCB Materials in Printed-Circuit Impedance

August 10, 2017

Printed circuits for high-speed and high-frequency applications rely on fine-featured transmission lines for signal transmission. Three of the most commonly used transmission-line technologies for these applications are microstrip, stripline, and grounded coplanar-waveguide (GCPW) transmission lines. Ideally, the loss through these transmission lines is minimal, and this requires an electrical impedance that is consistent and without interruptions, and with a value most appropriate for the types of signals to be transferred through the circuit. Variations from the nominal impedance of a circuit can result in increased insertion loss, increased return loss, higher radiated energy, degraded signal integrity (SI), and degraded rise time. A number of factors can affect the impedance of a PCB, including the physical and electrical characteristics of the circuit and circuit material, but by reviewing and better understanding these variables, their effects can be minimized.

Several different types of impedance are associated with high-speed, high-frequency PCB transmission lines, including wave impedance, input impedance, characteristic impedance, and frequency-dependent impedance. For RF/microwave circuits, for example, a characteristic impedance of 50 Ω is typically used for low-loss performance. The characteristic impedance, Z0, of a circuit can be defined as the ratio of voltage to current for a wave propagating in one direction without interference from any other wave in the circuit. In mathematical terms, it is simply

Z0 = V(x)/I(x)

where V(x) is voltage and I(x) is current. To include the effects of inductance (L) and capacitance (C) as required for high-frequency/high-speed circuits, the characteristic impedance for microstrip can be determined by the square root of inductance divided by capacitance:

Z0 = (L/C)0.5

where C is a function of the product of the circuit substrate dielectric constant (Dk) and the area between the signal plane and the ground plane divided by the substrate thickness, or C = (Dk area)/thickness. For thicker substrates, the capacitance decreases and the impedance increases. The lower capacitance is less supportive of the flow of electrons needed for current flow. For thinner substrates or substrates with higher Dk, the capacitance increases and the impedance decreases in support of greater current flow. A wider conductor will increase the area and achieve the same effect.  

This relationship for impedance, relating inductance and capacitance, is lossless, with no frequency dependence. To account for the numerous inductances and capacitances of complex circuits, such as differential circuits, a more comprehensive relationship can be used. This relationship is frequency dependent and does include conductor loss and dielectric loss:

Z0 = [(R + jωL)/(G + jωC)]0.5


ω = 2πf is the angular frequency;
G is related to dielectric loss; and
R is related to conductor loss.

Inductance and capacitance have opposite effects on a circuit’s impedance. An increase in inductance can cause an increase in impedance, while an increase in capacitance can result in a decrease in impedance. For example, in a 50-Ω system in which impedance variations may reach 45 Ω at one time and 55 Ω at another, the decrease in impedance may be due to an increase in capacitance while the rise in impedance may be the result of an increase in inductance.

The physical characteristics of transmission lines can affect capacitance and impedance, which in turn impact circuit impedance. As conductors are made narrower, the inductance increases and the impedance increases. As conductors are made wider, the capacitance increases and the impedance decreases.

Sudden changes in impedance or differences in impedance are problematic for maintaining high performance in high-speed/high-frequency circuits. Such changes can occur at any transmission-line junction, such as between a coaxial connector and the feed point of a PCB. The change in impedance can cause reflections of RF/microwave signals or high-speed digital signals back to the signal source. This results in less energy delivered to the load as well as with the reflected energy interfering with the propagation of forward energy from the source to the load.

Tracking Transmission Lines

For high-speed/high-frequency circuits, an ideal signal path maintains the same impedance throughout, such as a 50-Ω characteristic impedance, with minimal losses in energy along the path. Most of these signal paths use microstrip, stripline, or GCPW, which may be integrated into complex multilayer circuits. Closed-form equations are available to determine the impedances of these circuit structures, although field-solving techniques typically provide more accurate results.

A closed-form equation to determine the impedance for microstrip, for example, is

Z0 = [87/(Dk +1.41)0.5 ]{ln[5.98H/(0.8W + T)]}


H is the thickness of the dielectric substrate;
W is the width of the transmission line; and
T is the thickness of the transmission-line copper layer. 

To ease the calculations, the MWI-2017 impedance-modeling software is available to download for free from the Rogers Corp. Technology Support Hub.

The calculations for finding the impedance of stripline transmission lines are similar to those for microstrip:

Z0 = [60/(Dk)0.5]{ln [1.9B/(0.8W + T)]}


B is the thickness of the dielectric substrate from ground plane to ground plane;
T is the thickness of the stripline conductor; and
 W is the width of the stripline conductor.

GCPW is a somewhat more complex than microstrip or stripline, with correspondingly more complex closed-form equations for predicting impedance. But again, the free MWI-2017 software provides a quick and straightforward way to perform the calculations based on proven closed-form equations.

Delving into Differences

The physical characteristics of high-speed/high-frequency circuits play significant roles in determining PCB impedance, since differences in substrate thickness, copper conductor thickness, and conductor width lead to differences in impedance in such circuits. To explore the effects of differences in these parameters, various microstrip test circuits were fabricated using a

20-mil-thick substrate with 2-mil-thick copper and 43-mil-wide conductor (50.07 Ω characteristic impedance) as a baseline. One of the other substrates had a slightly lower dielectric constant (Dk), one had a 1-mil-thick copper conductor, one had an 18-mil-thick substrate, and one had a 42-mil-wide conductor, to explore what the changes in physical parameters would do to the impedance in each case. The thinner substrate exhibited significantly lower impedance, the use of a circuit material with lower Dk resulted in a minimal difference in impedance, the thinner copper conductor provided only slightly lower impedance, and the narrower conductor also led to only slightly lower impedance.

Copper conductor surface roughness is yet another PCB parameter, although it is not always considered when analyzing different circuit variables for impedance. Smoother copper conductor surfaces exhibit lower conductor losses than copper conductors with rougher surfaces, but how do they affect impedance? For one thing, rougher copper surfaces will slow the velocity of a wave propagating through the circuit. The slower wave is perceived by the circuit as a higher effective Dk, even if the Dk of the circuit material itself has not changed.

As is apparent, a number of variables can affect the impedance of high-speed/high-frequency circuits, including substrate thickness, copper thickness, conductor width, and Dk. A number of additional factors can influence PCB impedance. For example, absorbed moisture can decrease the impedance of microstrip lines since water has a high Dk. Circuit substrate materials with high moisture absorption will suffer these effects on impedance, especially in conditions of high relative humidity (RH). This blog is based on a presentation that will be given by the author, John Coonrod, at the PCB West Conference & Exhibition on September 13th. The presentation will provide additional information on the variables that affect PCB impedance.

Do you have a design or fabrication question? Rogers Corporation’s experts are available to help. Log in to the Rogers Technology Support Hub and “Ask an Engineer” today.

Post a comment to this article