Microstrip Width From Zo Calculator

Microstrip Geometry Estimator from Target Zo

Microstrip Width From Zo Formula

Formula

\[ A = \frac{Z_0}{60}\sqrt{\frac{\varepsilon_r + 1}{2}} + \frac{\varepsilon_r - 1}{\varepsilon_r + 1}\left(0.23 + \frac{0.11}{\varepsilon_r}\right) \\ \frac{w}{h} = \frac{8e^{A}}{e^{2A} - 2} \]

Where:

\(Z_0\) — target characteristic impedance (Ω)
\(\varepsilon_r\) — relative permittivity (dielectric constant) of the substrate
\(h\) — substrate height, i.e. the dielectric thickness between the trace and the ground plane (mm)
\(w\) — required trace width (mm)
\(A\) — dimensionless intermediate term

This is Wheeler's synthesis equation for a microstrip line. It inverts the standard impedance analysis formulas, so instead of computing \(Z_0\) from a known geometry, it directly yields the width-to-height ratio \(w/h\) that produces the desired impedance.

Microstrip Width From Zo – Calculation Example

Example: a 50 Ω single-ended microstrip on 1.6 mm FR-4 with a dielectric constant of 4.5.

\[ A = \frac{50}{60}\sqrt{\frac{4.5 + 1}{2}} + \frac{4.5 - 1}{4.5 + 1}\left(0.23 + \frac{0.11}{4.5}\right) = 1.382 + 0.162 = 1.544 \]

\[ \frac{w}{h} = \frac{8e^{1.544}}{e^{2 \cdot 1.544} - 2} = \frac{8 \cdot 4.683}{21.93 - 2} \approx 1.880 \]

\[ w = 1.880 \times 1.6 = 3.01~\text{mm} \]

Result: the required trace width is approximately 3.01 mm.

How to Use the Calculator

Enter the Characteristic impedance \(Z_0\) you want to achieve, in ohms. For most RF and high-speed single-ended traces this is 50 Ω.
Enter the Dielectric constant \(\varepsilon_r\) of your substrate. Standard FR-4 is typically 4.3–4.7 depending on frequency and manufacturer; high-frequency laminates range from about 2.2 (PTFE) to 10 (alumina).
Enter the Substrate height \(h\) in millimetres — the thickness of the dielectric layer between the copper trace and the ground plane, not the total board thickness.
Read the Required Trace Width in the result field. The calculation updates instantly as you change any input.

What Is Microstrip Impedance Synthesis?

A microstrip is a flat conductor on the outer layer of a printed circuit board, referenced to a ground plane beneath the dielectric. Because the field lines are split between the substrate below and air above, a microstrip behaves as a transmission line with a characteristic impedance \(Z_0\) determined by the trace width \(w\), the substrate height \(h\), and the dielectric constant \(\varepsilon_r\).

Most textbook formulas run in the “analysis” direction: you know the geometry and compute the impedance. This calculator solves the inverse, more practical problem — synthesis: given the impedance your system requires, what trace width should you draw? If you need to check an existing trace instead, use the Microstrip PCB Impedance calculator, which runs the calculation in the forward direction.

Controlling \(Z_0\) matters because every driver, receiver, and connector in a high-speed link is designed around a specific impedance. If the trace impedance deviates from it — typically beyond about ±10 % — part of the signal reflects at each discontinuity, causing ringing, overshoot, EMI, and bit errors. This is why controlled-impedance routing is standard for USB, HDMI, Ethernet, PCIe, DDR memory, and RF circuits. The 50 Ω target is the near-universal convention for single-ended RF work because it is a good compromise between power handling and loss in coaxial systems.

The result is best interpreted as a starting point: the calculator gives the width for an ideal, infinitely thin copper trace. Real boards add effects (trace thickness, solder mask, etch back) that shift the impedance by a few percent, so treat the output as a first-pass value to refine before fabrication.

Assumptions, Limitations and Practical Tips

Valid range: the synthesis formula used here is accurate for \(w/h \lt 2\), which covers the common cases (impedances below roughly 60–70 Ω on typical FR-4). For very narrow, high-impedance traces where \(w/h \gt 2\) would be needed in the alternate branch of Wheeler's equations, results become less reliable.
Zero trace thickness: copper thickness (e.g. 35 µm for 1 oz copper) is ignored. Thicker copper lowers the impedance slightly, so the actual impedance will be a few ohms lower than the target; many fab houses provide corrections.
Solder mask: a conformal coating over the trace raises the effective dielectric constant and typically lowers the impedance by 2–5 Ω. Many stackup tools let you model this explicitly.
Frequency dependence: \(\varepsilon_r\) of FR-4 falls with frequency (roughly 4.5 at low frequency to about 4.2 in the GHz range). Use the value quoted for your operating frequency.
Single-ended only: this calculator handles single-ended traces. Differential pairs (USB, HDMI, LVDS) need coupled-line models — see the Stripline PCB Differential Impedance calculator.
Inner layers differ: traces sandwiched between two dielectric layers are striplines, not microstrips, and follow different equations — use the Stripline Impedance calculator for those.
Final verification: before committing a design, confirm the width with your PCB manufacturer's stackup data or a 2D field solver, since resin content, glass weave, and etch tolerances all play a role.

Keep in mind that impedance control is only one part of signal integrity. Spacing to neighbouring traces affects crosstalk, which you can estimate with the PCB Microstrip Crosstalk calculator, and source/load mismatches may still require matching networks.

Frequently Asked Questions

How do I convert the result from millimetres to mils or inches?

Divide the width in mm by 25.4 to get inches, or multiply by 39.37 to get mils (thousandths of an inch). For example, a 3.01 mm trace equals roughly 118.5 mils. If you work in mils, you can also enter the substrate height in mm by first converting it — 1.6 mm FR-4 is about 63 mils, a common 2-layer board thickness.

Why does a higher target impedance require a narrower trace?

A narrower trace has less capacitance per unit length to the ground plane and higher series inductance, and since \( Z_0 = \sqrt{L/C} \), the impedance rises. Conversely, making a trace wider increases capacitance and lowers impedance. This is also why increasing the substrate height \( h \) (moving the ground plane farther away) raises impedance for the same width — the field coupling weakens.

What trace width is typical for a 50 Ω line on standard FR-4?

On 1.6 mm FR-4 (\(\varepsilon_r \approx 4.5\)) a 50 Ω trace is about 3 mm wide. On a 4-layer board with a 0.2 mm dielectric to the ground plane, the same 50 Ω needs only about 0.37 mm. The width scales almost linearly with height, so thin dielectrics give conveniently narrow traces for dense routing.

Should I use the dielectric constant from the datasheet or an effective value?

Use the relative permittivity \(\varepsilon_r\) of the laminate itself, not the effective permittivity. Because a microstrip's fields are partly in air, the effective value that appears in analysis formulas is lower — roughly \((\varepsilon_r + 1)/2\) to \(\varepsilon_r\) depending on geometry. Wheeler's synthesis equation already accounts for the air region internally, so entering the effective value would double-count the correction.

What happens if I ask for a very high impedance, like 100 Ω?

High impedances push the required width-to-height ratio below the formula's accurate range, and at some point the trace becomes impractically narrow — under etching tolerances or even below fab minimums. A 100 Ω single-ended line on thin FR-4 may need a width thinner than 0.1 mm. In practice, high impedances are usually achieved as differential pairs, where the odd-mode impedance of each half is what matters.

My fabricated board measures a few ohms off — what went wrong?

Small deviations are normal. The formula assumes zero copper thickness and no solder mask; real 35 µm copper and mask coverage typically pull the impedance 2–5 Ω below target. Etch taper also makes traces trapezoidal rather than rectangular. Most fabricators offer an impedance coupon: a test trace on your panel that they measure with a TDR before shipping, and they will adjust widths to hit the target.

Is this the same calculation my PCB CAD tool performs?

Conceptually yes, but CAD stackup editors usually use more complete models — Hammerstad and Jensen, or the IPC-2141 variants — that include copper thickness, trapezoidal etch, and solder mask layers. Expect a few percent difference between this calculator and your tool. Use this result as a starting point, then let the tool or fab house refine the final width.

Microstrip Impedance From Zo Calculator