**Estimated reading time: 5 minutes**

# Connect the Dots: Controlled Impedance and Calculations for Microstrip Structures

Modern high-speed and RF PCB design is an exciting field but it comes with its own set of challenges. Signal integrity, performance, and crosstalk become major concerns. Designers for these types of projects need to learn how to control electromagnetic interference (EMI) and compatibility (EMC), which means utilizing some interesting math and calculations.

These designs rely on controlling impedance to improve signal integrity and reduce EMI. PCB traces are there to conduct signals from one component or device to another, and when the impedance of those traces matches the characteristic impedance of a transmitting device, the maximum signal can be sent. This method limits both signal reflection and interference. However, beyond impedance there are other critical values and calculations that the designer must understand.

An impedance structure refers to physical configuration of components on a PCB, including microstrips, striplines, and coplanar waveguides. The microstrip line is the most common type of impedance structure: an external trace separated from a plane layer by a dielectric material. Microstrips are compact, allowing for greater design flexibility. They are also easy to probe and measure, making them suitable for easy fabrication and a wide range of applications.

Figure 1 shows a microstrip trace with width (w) and thickness (t). The dielectric material separating the trace from the plane has an overall thickness of h and a dielectric constant of εr.

**Key Calculations Involved in Microstrip Design **

Incorporating a microstrip line into a PCB requires calculations involving the analysis and design of transmission lines which are widely used in microwave and RF circuits. Characteristic impedance, the effective dielectric constant, and propagation are all critical pieces of information for the designer to understand.

*Characteristic Impedance *

Characteristic impedance (Z_{0}) is the ratio of voltage to current in a transmission line and is an important parameter for determining the performance of microstrip circuits (Figure 2).

The characteristic impedance of a microstrip line can be approximated as:

**h** is the height of the substrate

**w** is the width of the trace

**t** is the thickness of the trace

*Effective Dielectric Constant *

Effective dielectric constant (ε_{r}) is the relative permittivity of the substrate material as seen by the signal on the microstrip line (Figure 3). For a microstrip line, the dielectric of the material and the dielectric of the surrounding air are the two values that are used to understand the effective constant.

**ε _{r1}** is the permittivity of the substrate

**ε**is the permittivity of the air above the substrate

_{r2}**h**is the is the height of the substrate

**w**is the width of the trace

*Velocity of Propagation *

The velocity of propagation (vp) is the speed of a signal as it travels down the microstrip line—or through any transmission line. It is typically expressed as a fraction of the speed of light, due to the effective dielectric constant of the substrate material (Figure 4).

**c** is the speed of light in a vacuum: 300 million meters/second

*Propagation Delay*

Propagation delay (τ) is the time taken for a signal to travel down the microstrip line. This is a relatively straightforward equation using the velocity of propagation and the distance the signal must travel (Figure 5).

L is the length of the microstrip line

*Putting It Into Action *

To illustrate how all these equations come together, let us examine how to calculate the numbers around a fairly common design structure: a 50Ω microstrip. For this microstrip configuration, we will use the following values:

Z_{0} = 50Ω

h = 0.0146" ^{1}

t = 0.0024"

ε_{r1} = 4.1

ε_{r2} = 1.00 ^{2}

The first step is to calculate the effective dielectric constant (ε_{r}) for the external trace using the equation we discussed previously. Make sure you keep track of the output. In our example, we get:

εr = 2.808

Next, we must determine the required trace width to meet our 50Ω target. The width of the required trace will depend on the thickness of the copper layer on the PCB (t), the effective dielectric constant (ε_{r}), and the desired characteristic impedance (Z_{0}).

We next use the characteristic impedance equation discussed earlier and solve for trace width (w). You might need to use a calculator or equation solver to calculate w ^{3}.

By inputting the values we have calculated already, we find:

w = 0.030" (30 mils)

This requires another look. The resulting 30-mil trace is a little on the wide side for most designs. However, if controlling impedance is critical, then this is the measurement the design must account for. If a 30-mil trace will absolutely not work, other variables can be modified to still achieve the required impedance. For example, both material type and thickness could be altered to meet our target numbers.

*For Fun*

Since length is such an important part of the equation, it is interesting to calculate the propagation delay for a 3"- and 6"-trace. Here’s how the numbers work out:

For 3" trace, τ = 4.2 x 10-10 seconds

For 6" trace, τ = 8.5 x 10-10 seconds

*Design Tips*

**Trace Thickness (t):**The thickness of the trace should be at least 1-ounce copper (0.0014") to ensure good current handling capability. In this example, we used 1-ounce copper (0.0014") plated to 0.0024".**Trace Spacing Calculation:**To minimize crosstalk between traces, make sure the spacing between those traces is at least three times the height of the dielectric substrate.

**Tying It All Together **

These calculations will help you create 50Ω traces for high-speed and RF PCBs that provide good signal integrity and minimize loss. In addition, with these equations in your toolkit, you are ready for any variation in impedance control. However, remember that PCB substrate quality and manufacturing process accuracy will have a big impact on the performance of the transmission lines in RF circuits.

We look forward to seeing what you will design next.

**References **

- This is the standard dielectric thickness of some manufacturers’ 6-layer stackup.
- Don’t forget to account for air.
- It’s time to dust off those rules for manipulating natural logs.

*This column originally appeared in the December 2023 issue of Design007 Magazine.*

### More Columns from Connect the Dots

Connect the Dots: Designing for Reality—Lamination and MaterialsConnect the Dots: Designing for Reality—The Physical Manufacturing Phases

Connect the Dots: Designing for Reality—The Pre-Manufacturing Process

Connect the Dots: Designing for Reality: Prioritizing Manufacturability

Connect the Dots: Are You Ready for 2024?

Connect the Dots: Five Best Practices for Designing Flex and Rigid-flex PCBs

Connect the Dots: Best Practices for Ensuring PCB Design Manufacturability

Connect the Dots: Choosing the Right CAD Tool