Stripline Impedance Calculator

Embedded PCB Stripline Impedance Estimator

Stripline Characteristic Impedance Formula

Formula

\[ Z_0 = \frac{60}{\sqrt{\varepsilon_r}} \cdot \ln\!\left( \frac{4H}{0.67\,\pi\,(W + T)} \right) \]

Where:

\(Z_0\) — characteristic impedance (Ω)
\(\varepsilon_r\) — relative permittivity (dielectric constant) of the substrate
\(W\) — trace width (mm)
\(T\) — copper trace thickness (mm)
\(H\) — distance from the trace center to each ground plane, i.e. half of the total substrate height (mm)

This closed-form approximation gives the characteristic impedance of a symmetric stripline: a flat conductor of width \(W\) and thickness \(T\) embedded in a uniform dielectric exactly midway between two ground planes. A wider or thicker trace lowers the impedance, while a larger spacing \(H\) or a lower dielectric constant raises it.

Stripline Impedance – Calculation Example

Example: a 0.2 mm wide, 35 µm thick copper trace is routed symmetrically between two ground planes, 0.2 mm of dielectric (\(\varepsilon_r = 4.5\), typical for FR-4) on each side.

\[ Z_0 = \frac{60}{\sqrt{4.5}} \cdot \ln\!\left( \frac{4 \times 0.2}{0.67\,\pi\,(0.2 + 0.035)} \right) = 28.28 \cdot \ln\!\left( \frac{0.8}{0.4946} \right) = 28.28 \cdot \ln(1.617) \approx 13.59~\Omega \]

Result: the characteristic impedance is approximately 13.59 Ω.

To reach a more typical 50 Ω target with this stack-up, you would need to reduce the trace width or increase the spacing to the ground planes.

How to Use the Stripline Impedance Calculator

Enter the Dielectric Constant (\(\varepsilon_r\)) of your substrate material — 4.3–4.5 is typical for FR-4; use the value from your laminate datasheet if available.
Enter the Trace Width (\(W\)) in mm. This is the copper width set in your PCB layout tool.
Enter the Copper Thickness (\(T\)) in mm. Standard 1 oz copper is 0.035 mm; 0.5 oz is 0.017 mm and 2 oz is 0.070 mm.
Enter the Dielectric Height (\(H\)) in mm — the distance from the trace to each ground plane. If the total dielectric thickness between the two planes is 0.4 mm, enter 0.2 mm.
Read the Characteristic Impedance (\(Z_0\)) in ohms, then adjust the inputs until you hit your target impedance.

What Is Stripline Impedance?

A stripline is a transmission line in which the signal conductor is fully embedded in a dielectric layer between two reference (ground) planes, typically on an inner layer of a multilayer PCB. This contrasts with microstrip, where the trace runs on an outer layer with air above it. Because the field is confined entirely within a homogeneous dielectric, stripline has no air interface, which gives it a well-defined, frequency-independent characteristic impedance and excellent immunity to crosstalk and electromagnetic interference.

The characteristic impedance \(Z_0\) is the ratio of voltage to current for a wave travelling along the line. When a driver, receiver, or intervening trace has a different impedance, part of the signal reflects at the discontinuity. Reflections cause ringing, overshoot, timing errors, and false clocking in digital systems, and standing waves and power loss in RF circuits. Matching \(Z_0\) to the system impedance — most commonly 50 Ω, or 100 Ω differential for differential pairs — is therefore a basic requirement of high-speed and RF design.

The result tells you what impedance the trace will present. If it is below target, widen the geometry gap (increase \(H\)) or narrow the trace; if it is above target, do the opposite. Note that in a symmetric stripline \(H\) is half the total dielectric thickness between the planes, so the trace must be centered — an off-center trace is an asymmetric stripline and follows different equations. For differential pairs routed as stripline, use the stripline differential impedance calculator instead, because the coupling between the two traces changes the odd-mode impedance.

Assumptions, Limitations, and Practical Tips

Symmetric geometry. The formula assumes the trace lies exactly midway between two infinite ground planes. If the trace is closer to one plane than the other, the true impedance will be lower than calculated.
Homogeneous dielectric. The entire field is assumed to be in a single material with constant \(\varepsilon_r\). Glass-weave effects in FR-4 can shift the effective permittivity by a few percent, varying along the trace.
Approximate closed form. This equation is a simplified approximation most suitable for narrow traces (roughly \(W \lesssim 0.5H\) after accounting for thickness). Errors grow for very wide traces; for sign-off on production designs, verify with a 2D field solver or your fabricator's impedance coupon data.
Manufacturing tolerances matter. Etch-back makes finished traces trapezoidal and narrower than drawn; resin content and prepreg flow vary \(\varepsilon_r\) and \(H\). A ±10 % impedance tolerance is a realistic production spec.
Units must be consistent. \(W\), \(T\), and \(H\) only appear as ratios, so any consistent unit works — but keep all three in the same unit (the calculator uses mm).
Interconnect design doesn't end at Z0. Once the line impedance is set, matching networks (see the PI network impedance matching and T matching network calculators) may still be needed to transform between impedances at the terminations.

Common Substrate Materials

Material	Typical \(\varepsilon_r\) (at ~1 GHz)
FR-4 (standard glass epoxy)	4.3–4.6
High-Tg / low-Dk FR-4	3.8–4.2
Rogers RO4350B	3.48
Rogers RO4003C	3.38
PTFE (Teflon)	2.0–2.2
Isola FR408HR	3.68

Always confirm the dielectric constant at your operating frequency with the laminate datasheet — \(\varepsilon_r\) decreases slightly with frequency in woven-glass materials.

Frequently Asked Questions

How do I calculate stripline impedance by hand?

Plug your values into the formula and work through it in three steps. First compute the denominator term \(0.67\pi(W+T)\). Then divide \(4H\) by that result to get the logarithm's argument, and take its natural log (ln, not log₁₀). Finally multiply by \(60/\sqrt{\varepsilon_r}\). Double-check that \(W\), \(T\), and \(H\) are all in the same unit before you start, otherwise the ratio inside the logarithm is wrong.

What is a good stripline impedance value?

Most single-ended high-speed and RF systems target 50 Ω, while differential stripline pairs typically target 100 Ω differential (about 50–60 Ω odd-mode per trace, depending on spacing). Values far from the system impedance cause reflections, so aim for the target within your tolerance — realistically ±10 % in production due to etch and laminate variations. There is no universally "good" number; it must match the driver, receiver, and termination impedance of your system.

Why is my stripline impedance lower than the same trace as microstrip?

Because the entire field is in the dielectric instead of partly in air. Air has \(\varepsilon_r = 1\), which raises microstrip's impedance for identical geometry. A symmetric stripline is surrounded by substrate with the full \(\varepsilon_r\), roughly \(\sqrt{\varepsilon_r}\) times more capacitance per unit length, so the same trace dimensions give a noticeably lower impedance. A trace that is 50 Ω as microstrip will usually need to be narrower, or placed farther from the planes, to reach 50 Ω as stripline.

Can I use mils or inches instead of mm?

Yes — the formula only uses the ratios of \(W\), \(T\), and \(H\), so any unit works as long as all three are in the same unit. The calculator labels the fields in mm, so if you work in mils, convert first (1 mil = 0.0254 mm). Copper thickness is often quoted in ounces: 0.5 oz ≈ 17 µm, 1 oz ≈ 35 µm, 2 oz ≈ 70 µm (0.017, 0.035, 0.070 mm).

What if my trace is not centered between the two ground planes?

Then it is an asymmetric (dual-plane) stripline, and this calculator no longer applies. An off-center trace sits closer to one plane, increasing capacitance and lowering the real impedance compared to the symmetric result. As a rule of thumb, the trace "sees" the nearer plane more strongly, so the impedance falls toward the value the near plane alone would produce. Use a dual-stripline or asymmetric-stripline equation, or better, a 2D field solver, for off-center routing.

What are the most common mistakes when using this calculator?

The most frequent error is entering the total dielectric thickness between the planes instead of the half-height \(H\) — that doubles \(H\) and inflates the result. Other common slips: mixing units (mils for width, mm for height); using log₁₀ instead of ln when computing by hand; ignoring copper thickness, which matters for narrow traces; and entering \(\varepsilon_r\) of a vacuum (1.0) or of air instead of the laminate. Also verify that your trace is actually routed on an inner layer between two planes.

Why does my fabricator's impedance coupon show a different value?

Production geometry differs from your drawing. Etch-back makes finished copper trapezoidal and narrower at the top, prepreg resin content shifts \(\varepsilon_r\) and \(H\), and glass-weave skew varies the local permittivity along the trace. Together these easily produce 5–10 % deviation from a closed-form estimate, especially for wide traces. Treat this calculator as a design starting point; for sign-off, rely on your fabricator's stackup model, their coupon measurements, or a 2D field solver such as the one built into your layout tool.