Microstrip Line Characteristic Impedance Calculation in uSimmics (formerly QucsStudio) [2026]

This guide explains how to use the Line Calculation tool in uSimmics (formerly QucsStudio) to compute the characteristic impedance of a microstrip transmission line. It covers the physical parameters that govern impedance, how to enter substrate data, and how to solve both forward (width → impedance) and inverse (impedance → width) problems.

What You’ll Learn
1. Characteristic Impedance
2. Why Characteristic Impedance Matters
3. Parameters That Govern Microstrip Impedance
4. Computing Characteristic Impedance with uSimmics (formerly QucsStudio)
5. Calculation Result Example
Summary
Related Articles

What You’ll Learn

What characteristic impedance is and why it matters in PCB design
Which physical parameters affect characteristic impedance (trace width, dielectric constant, substrate height, etc.)
How to launch and use the Line Calculation tool in uSimmics (formerly QucsStudio)
How to enter substrate parameters (εr, tanδ, copper thickness) correctly
How to compute trace width for a target impedance, and how to back-calculate impedance from a known trace width

1. Characteristic Impedance

Characteristic impedance is the ratio of voltage to current in a transmission line for a traveling wave. Measured in ohms (Ω), it is an intrinsic property of the line’s geometry and materials — independent of line length.

An analogy: just as fluid flow in a pipe depends on pipe diameter and material, electrical signal flow on a PCB trace depends on the trace’s physical dimensions and the surrounding dielectric. Characteristic impedance quantifies this relationship.

2. Why Characteristic Impedance Matters

When the impedances of a signal source, transmission line, and load are all equal, signals travel with minimal reflection and loss. A mismatch causes part of the signal to reflect, leading to:

Signal reflections: Reflected waves return to the source, degrading signal fidelity
Data errors: Increased ringing and undershoot in high-speed digital signals
Increased EMI: Standing waves from reflections become sources of unwanted radiation

Impedance control is especially critical for high-speed digital signals (above 1 Gbps) and RF signals (UHF and above). The standard characteristic impedance for RF systems is 50 Ω.

3. Parameters That Govern Microstrip Impedance

Trace Width (W)

Trace width is inversely proportional to characteristic impedance — wider traces give lower impedance, narrower traces give higher impedance. For 50 Ω design, there is an optimal width that depends on substrate material and thickness.

Trace Thickness (T)

The conductor (copper foil) thickness. Thicker copper reduces impedance slightly by widening the effective current path. Common values are 18 µm (0.5 oz) and 35 µm (1 oz).

Substrate Dielectric Constant (εr)

The relative permittivity of the substrate material. Higher εr slows signal propagation and lowers impedance. Representative values:

Substrate Material	εr
FR-4	4.2–4.8 (typically 4.5)
Rogers RO4003C	3.55
PTFE (Teflon)	2.1–2.2
Alumina	9.5–10

Substrate Height (H)

The thickness of the dielectric between the trace and the ground plane. A thicker substrate reduces capacitance and increases impedance.

Loss Tangent (tanδ)

The dielectric loss factor. It does not directly affect characteristic impedance but does affect transmission loss (insertion loss). Low tanδ materials are required for high-frequency applications.

Conductor Resistivity

The electrical resistivity of the conductor (copper: 1.72 × 10⁻⁸ Ω·m). The effect on characteristic impedance is negligible, but it contributes to transmission loss.

4. Computing Characteristic Impedance with uSimmics (formerly QucsStudio)

Example Calculation Conditions

Parameter	Value
Substrate material	FR-4
Dielectric constant (εr)	4.5
Substrate height (H)	1.5 mm
Copper thickness (T)	35 µm (1 oz)
Target impedance	50 Ω

Step 1: Launch Line Calculation

From the menu bar, select Tools.
Click Line Calculation to open the tool.
The Line Calculation window appears.

Step 2: Select Transmission Line Type

From the choice dropdown, select Micro Stripline.
The parameter input fields for microstrip geometry are displayed.

Step 3: Enter Substrate Parameters

Enter the following values in the Properties section:

Parameter	Value	Description
εr	4.5	FR-4 relative permittivity (verify with substrate datasheet)
tanδ	0.02	FR-4 loss tangent (affects high-frequency insertion loss)
Resistivity	1.72 × 10⁻⁸	Copper resistivity (Ω·m)
Conductor µr	1	Relative permeability of copper
Roughness	Per substrate spec	Surface roughness — becomes significant at GHz frequencies
T	35 µm	Copper foil thickness
H	1.5 mm	Dielectric thickness

Enter the operating frequency in the Parameters field (e.g., 915 MHz or 2.4 GHz).

Step 4: Compute Impedance or Trace Width

Forward calculation (W → Z₀):
1. Enter the desired trace width in the W field under Dimensions.
2. Click Calculate (or the tool updates automatically).
3. The corresponding characteristic impedance Z₀ is shown.

Inverse calculation (Z₀ → W):
1. Enter the target impedance (50 Ω) in the Z₀ field.
2. The required trace width W is computed automatically.

5. Calculation Result Example

Using the conditions above (FR-4, εr = 4.5, H = 1.5 mm, T = 35 µm), achieving 50 Ω characteristic impedance requires a trace width of W = 2.77624 mm.

Use this value as the trace width specification in your PCB layout to realize the intended impedance.

Summary

Characteristic impedance is a fundamental parameter for maintaining signal integrity in PCB design. uSimmics (formerly QucsStudio)’s Line Calculation tool allows you to compute characteristic impedance instantly from trace and substrate parameters, and to back-calculate the trace width needed for a target impedance. Integrating this tool into your PCB design workflow enables accurate impedance control that minimizes signal reflections, reduces losses, and maximizes signal delivery efficiency.