Microstrip Transmission Lines Impedance Calculator
Estimate the characteristic impedance of a microstrip transmission line from the dielectric constant, substrate height, trace width and copper thickness. Enter your PCB stack-up values to get Z0 in ohms for RF and high-speed design.
Microstrip Line Characteristic Impedance Tool
Microstrip Transmission Line Impedance Formula
Where:
- \(Z_0\) — characteristic impedance (Ω)
- \(\varepsilon_r\) — relative permittivity (dielectric constant) of the substrate
- \(\varepsilon_{\mathrm{eff}}\) — effective permittivity seen by the line
- \(h\) — substrate height between trace and ground plane (mm)
- \(w\) — trace width (mm)
- \(t\) — trace (copper) thickness (mm)
- \(e \approx 2.71828\) — Euler's number
Because part of the field propagates in air above the board, the line behaves as if it were filled by a dielectric with \(\varepsilon_{\mathrm{eff}}\), which always lies between 1 and \(\varepsilon_r\). The trace-thickness term in the narrow-trace formula accounts for the extra copper that effectively widens the line.
Microstrip Transmission Line Impedance – Calculation Example
Example: a 1 mm wide trace on a 1.6 mm thick substrate with \(\varepsilon_r = 4.5\) and 0.035 mm (1 oz) copper — the calculator's default values.
\[ \frac{w}{h} = \frac{1}{1.6} = 0.625 \leq 1 \quad \Rightarrow \quad \text{use the narrow-trace formula} \]
\[ \varepsilon_{\mathrm{eff}} = 2.75 + 1.75 \cdot \frac{1}{\sqrt{1 + 12 \cdot 1.6 / 1}} = 2.75 + \frac{1.75}{\sqrt{20.2}} \approx 3.139 \]
\[ t \cdot \ln\!\left(1 + \frac{4e}{t/w}\right) = 0.035 \cdot \ln(311.66) \approx 0.201 \text{ mm} \]
\[ Z_0 = \frac{60}{\sqrt{3.139}} \cdot \ln\!\left( \frac{8 \cdot 1.6}{1 + 0.201} \right) \approx 33.86 \cdot \ln(10.66) \approx 33.86 \cdot 2.366 \approx 80.09 \, \Omega \]
Result: the characteristic impedance is approximately 80.09 Ω.
How to Use the Calculator
- Enter the Dielectric constant of your PCB material (e.g. 4.5 for typical FR-4).
- Enter the Substrate height — the thickness of the dielectric layer between the trace and the ground plane.
- Enter the Trace width of the copper trace.
- Enter the Trace thickness — the copper weight of the trace (0.035 mm for 1 oz copper, 0.07 mm for 2 oz).
- Read the Characteristic Impedance in ohms; use the result to adjust the width until you hit your target impedance.
What Is Microstrip Impedance and Why It Matters
A microstrip transmission line is a flat conductor on the surface of a printed circuit board, with a ground plane on the opposite side of the dielectric layer. It is the most common controlled-impedance structure in modern PCBs because it is easy to fabricate, easy to probe, and gives reasonable performance from DC into the lower gigahertz range.
The characteristic impedance \(Z_0\) is the ratio of voltage to current for a wave travelling along the line. When a high-speed or high-frequency signal encounters a change in impedance — at a driver output, a connector, or a trace of the wrong width — part of the signal is reflected back toward the source. These reflections cause ringing, overshoot, timing errors, and EMI, and they can corrupt data on digital buses just as they detune RF amplifiers and filters.
Most systems standardise on 50 Ω (RF and test equipment) or 90–100 Ω (differential pairs such as USB, LVDS, and Ethernet). To hit these targets you must set the trace geometry correctly: wider traces lower the impedance, thicker substrates raise it, and higher dielectric constants lower it. A trace of about 3 mm width on 1.6 mm FR-4 comes close to 50 Ω; on the same board a 1 mm trace, as in the example above, sits near 80 Ω.
If you work with embedded traces between two ground planes instead, use the Stripline Impedance calculator; for a similar surface-trace geometry solved differently, see the Microstrip PCB Impedance calculator. Keeping uncoupled traces apart also matters — the PCB Microstrip Crosstalk calculator helps you check spacing, and the PI Network Impedance Matching calculator can help when a source and line simply cannot be made equal.
Assumptions, Limitations and Practical Tips
- Quasi-static model: the formulas are accurate for electrically thin substrates (typically up to a few GHz for ordinary FR-4 thicknesses). At higher frequencies, dispersion makes \(Z_0\) frequency-dependent and full-wave tools are more reliable.
- Isolated trace: the calculation assumes a single trace over an infinite ground plane. Neighbouring traces, planes on the same layer, and via fences all pull the impedance down.
- Trace thickness edge case: enter a nonzero copper thickness. Setting \(t = 0\) makes the thickness-correction term undefined in the narrow-trace branch; use at least the foil thickness of your stack-up (0.035 mm for 1 oz copper).
- Solder mask: the coating above the trace has a dielectric constant near 3–4 and typically lowers \(Z_0\) by 1–3 Ω. This calculator ignores it, so budget for the drop on mask-covered traces.
- Manufacturing tolerances: etching narrows or widens traces by 10–20% of the copper thickness, and both \(\varepsilon_r\) and \(h\) vary board to board. A ±10% impedance tolerance on the drawing is realistic for standard FR-4; tighter tolerances require controlled-impedance fabrication.
Typical Dielectric Constants
| Material | Approx. \(\varepsilon_r\) (1 MHz – 1 GHz) |
|---|---|
| FR-4 (standard glass epoxy) | 4.3 – 4.7 |
| High-Tg / low-Dk FR-4 blends | 3.8 – 4.2 |
| Rogers RO4350B | 3.48 |
| PTFE (Teflon) / RT/duroid 5880 | 2.1 – 2.2 |
| Alumina (Al2O3, hybrid circuits) | 9.8 |
Manufacturers specify \(\varepsilon_r\) at a particular frequency — always use the value quoted for your design frequency, since FR-4 in particular loses dielectric constant noticeably above a few GHz.
Frequently Asked Questions
What impedance should I aim for on a microstrip trace?
Use 50 Ω for single-ended RF lines, antennas, and test instrumentation. Differential pairs (USB, LVDS, Ethernet, PCIe) typically target 90–100 Ω differential. On 1.6 mm FR-4, a single-ended 50 Ω trace needs roughly 3 mm width; thinner substrates of 0.2–0.5 mm are usually chosen for high-speed boards so traces come out a practical 0.2–0.5 mm wide. Always match the impedance your transceiver or connector standard specifies.
Can I enter dimensions in mils instead of mm?
The calculator expects millimetres, but the formulas are ratio-based: only \(w/h\), \(t/w\), and the effective permittivity matter. Convert mils to mm by dividing by 39.37 (1 mm ≈ 39.37 mil, 1 mil = 0.0254 mm). A 6 mil trace is 0.152 mm; 1 oz copper (1.37 mil) is 0.035 mm. As long as all three dimensions use the same unit consistently, the impedance result is identical.
Why does a wider trace have lower impedance?
A wider trace increases capacitance per unit length to the ground plane while lowering inductance per unit length. Since \(Z_0 = \sqrt{L/C}\), both effects push the impedance down. This is why 50 Ω lines on thin cores are narrower than on thick cores. In practice, designers iterate the trace width in the calculator until the target impedance is hit, then round to a fab-house-compatible value.
Does solder mask change the impedance?
Yes. Solder mask (εr ≈ 3–4) sits above the trace and increases the effective permittivity, typically lowering \(Z_0\) by 1–3 Ω on 50 Ω lines. This calculator models an unmasked trace, so subtract a couple of ohms from your design target for mask-covered lines, or ask your fabricator to model the mask, since its thickness and coating style (full vs. solder-dam-only) change the effect.
At what frequencies do these formulas stop being accurate?
The quasi-static Hammerstad-style model holds for electrically thin substrates — roughly up to a few GHz for standard FR-4 thicknesses. Above that, dispersion makes \(Z_0\) rise with frequency, and the dielectric constant of FR-4 itself drops noticeably. For 10+ GHz designs, mm-wave work, or thick ceramic substrates, use a 2D field solver or full-wave simulation and design-frequency material data instead.
How do I get the impedance of a differential pair from this calculator?
Calculate the single-ended impedance \(Z_0\) of one trace first, then estimate the differential impedance as \(Z_{\mathrm{diff}} \approx 2Z_0(1-k)\), where k is the coupling coefficient (typically 0.1–0.3 for tightly coupled pairs). This works as a rough check, but edge-coupled pairs interact strongly, so for real designs use a differential-aware tool or your fabricator's stack-up solver, which accounts for trace spacing directly.
What are common mistakes when calculating microstrip impedance?
Top errors include using the total board thickness instead of the height to the reference plane, entering copper weight in oz instead of mm, using a datasheet εr from the wrong frequency, and ignoring the copper thickness term for narrow traces (setting t = 0 breaks the narrow-trace formula). Also remember that nearby traces and copper pours pull impedance down by several ohms — a trace that computes at 50 Ω in isolation may measure 45 Ω on a dense board.