Microstrip Impedance Calculator

Characteristic Impedance of Microstrip Line

Microstrip Impedance Formula

Formula

\[ Z_0 = \frac{87}{\sqrt{\varepsilon_r + 1.41}} \; \ln\!\left( \frac{5.98\,h}{0.8\,w + t} \right) \]

Where:

\(Z_0\) — characteristic impedance (Ω)
\(\varepsilon_r\) — relative dielectric constant of the substrate (dimensionless)
\(h\) — substrate height, i.e. the dielectric thickness between the ground plane and the trace (mm)
\(w\) — width of the copper trace (mm)
\(t\) — thickness of the copper layer (mm)

This closed-form approximation estimates the impedance of a microstrip line — a flat conductor separated from a ground plane by a dielectric slab — from its geometry and the substrate material. Trace thickness enters through the effective conductor width \(0.8w + t\), which accounts for the fringing fields at the trace edges.

Microstrip Impedance – Calculation Example

Example: a 1 mm wide copper trace on a 1.6 mm thick FR-4-like substrate with a dielectric constant of 4.5 and 35 µm (0.035 mm) copper thickness — the default values of the calculator.

\[ \varepsilon_r + 1.41 = 4.5 + 1.41 = 5.91, \qquad \sqrt{5.91} = 2.431 \]

\[ \frac{5.98\,h}{0.8\,w + t} = \frac{5.98 \times 1.6}{0.8 \times 1 + 0.035} = \frac{9.568}{0.835} = 11.456 \]

\[ Z_0 = \frac{87}{2.431} \times \ln(11.456) = 35.78 \times 2.439 \approx 87.27~\Omega \]

Result: the characteristic impedance is approximately 87.27 Ω.

How to use the calculator

Enter the Dielectric constant \(\varepsilon_r\) of your substrate (4.4–4.5 for FR-4, 2.2 for PTFE, 3.0 for RO4350B — check the datasheet of your laminate).
Enter the Substrate height \(h\) in mm. This is the dielectric thickness between the ground plane and the signal layer, not the total board thickness.
Enter the Trace width \(w\) in mm.
Enter the Trace thickness \(t\) in mm (0.035 mm for 1 oz copper, 0.070 mm for 2 oz).
Read the Characteristic Impedance in ohms (Ω). Adjust the trace width until the impedance matches your target, e.g. 50 Ω.

What is microstrip impedance?

A microstrip line is the most common controlled-impedance structure on a PCB: a flat copper trace running on an outer layer, with a solid ground plane beneath it and dielectric material in between. Because part of the electromagnetic field travels through the dielectric and part through the air above the board, a microstrip behaves as a transmission line with a well-defined characteristic impedance \(Z_0\).

When a high-frequency or fast digital signal travels along a trace whose impedance differs from the impedance of the driver, receiver, or connectors, part of the signal is reflected at every discontinuity. These reflections cause ringing, overshoot, crosstalk and bit errors. Matching \(Z_0\) to the system impedance — most often 50 Ω, or 90/100 Ω differential for high-speed pairs — is therefore a fundamental requirement in RF design, high-speed digital routing, and any interface with controlled-impedance specifications such as USB, Ethernet, PCIe or DDR memory.

The result of this calculator tells you what impedance a given geometry will produce. In practice designers usually work the other way: they pick a target impedance and iterate the trace width until the calculator converges on it. Wider traces lower the impedance, thicker substrates raise it, and a higher dielectric constant lowers it.

For embedded signal layers sandwiched between two ground planes, the geometry is a stripline rather than a microstrip — see the Stripline Impedance Calculator. For routing rules on paired traces, the PCB Microstrip Crosstalk Calculator is also useful, and a broader treatment of geometry-based impedance estimation is available in the Microstrip PCB Impedance Calculator.

Accuracy, assumptions and practical tips

Valid range: this approximation is most accurate for aspect ratios of roughly \(0.1 \leq w/h \leq 2\) and dielectric constants up to about \(\varepsilon_r \approx 10\). Very wide traces, very thin substrates, or exotic ceramics reduce the accuracy — field solvers give more precise results for such cases.
Uniform dielectric assumed: the model assumes a homogeneous substrate and a trace of constant width. Solder mask covering the trace lowers the impedance slightly (typically by 1–3 Ω), because it replaces air with a higher-permittivity material.
Copper roughness and etch profile: real traces have trapezoidal cross-sections and rough surfaces; both shift the impedance slightly. Fabricators typically guarantee ±10 % impedance tolerance, or tighter with a controlled-impedance stackup.
Use manufacturer data: the dielectric constant of FR-4 varies with resin content, frequency and thickness (typically 4.2–4.8). Always use the value from the laminate datasheet at your operating frequency.
Discontinuities matter: vias, bends, layer transitions and gaps in the ground plane cause reflections that a uniform-line formula cannot capture. Keep the reference plane continuous under the trace and prefergentle bends (two 45° bends instead of one 90°).
Matching networks: when a source and load cannot both be matched by the trace alone, an PI Network Impedance Matching or a T Matching Network can transform the impedances.

Frequently Asked Questions

What trace width gives 50 Ω on standard FR-4?

For 1.6 mm FR-4 (εr ≈ 4.5) with 1 oz copper, a 50 Ω single-ended trace is roughly 2.9–3.0 mm wide. On a 0.8 mm core the width drops to about 1.5 mm, and on a 0.2 mm layer it is near 0.37 mm. Because the result depends on the exact dielectric constant and stackup, always verify by entering your own dimensions and iterating the width until the calculator reads 50 Ω.

How do I convert trace dimensions from mils to millimeters?

1 mil equals 0.0254 mm, so a 6 mil trace is 0.152 mm and a 4 mil trace is 0.102 mm. Going the other way, divide millimeters by 0.0254. Copper thickness is usually specified in ounces: 1 oz ≈ 1.37 mil ≈ 0.035 mm, 2 oz ≈ 2.74 mil ≈ 0.070 mm, and ½ oz ≈ 0.017 mm. Enter all dimensions in the same unit system — mixing mils and mm is one of the most common mistakes.

Can I use this calculator for differential pairs like USB or LVDS?

Not directly. This tool computes single-ended impedance. A tightly coupled differential pair has a differential impedance of roughly 2·Z₀·(1 − k), where k is the coupling factor between the two traces. As a rule of thumb, two traces each designed for about 55–60 Ω single-ended, routed close together, land near the typical 90–100 Ω differential target. For exact results use a differential impedance model or a field solver.

What is the effective dielectric constant, and why doesn't this formula use it?

Because part of the field in a microstrip travels through air and part through the substrate, the line behaves as if it were filled by an ε_eff between 1 and εr — for FR-4 typically around 3.2–3.6. The formula on this page folds that effect into its empirical coefficients, so you enter the raw substrate dielectric constant from the datasheet, not ε_eff. You need ε_eff separately when calculating wavelength or propagation delay along the trace.

Why does my measured impedance differ from the calculated value?

Common reasons: solder mask over the trace (lowers impedance by 1–3 Ω), trapezoidal etch profile making the trace effectively wider, wrong εr for your laminate, and using total board thickness instead of dielectric height to the reference plane. Fabricators normally guarantee only ±10% impedance tolerance, so a measured value a few ohms off is normal. If you need tighter control, order a controlled-impedance stackup and consult the fab house's impedance coupons.

Does this formula work for traces on inner layers between two ground planes?

No. An inner trace sandwiched between two reference planes is a stripline, a different structure with lower impedance for the same width because all of its field is inside the dielectric. This calculator is only for outer-layer microstrip. Using it for embedded traces will significantly overestimate the impedance — use a stripline impedance calculator instead.

How does frequency affect microstrip impedance?

The characteristic impedance is fairly constant with frequency, but the dielectric constant of the substrate is not — FR-4 drops from about 4.4 at low frequencies to around 4.2 in the GHz range, and resin content and glass weave also matter. This raises the calculated impedance slightly at high frequencies. Use the datasheet εr measured near your operating frequency, and for designs above roughly 5 GHz consider low-loss laminates and field-solver verification.