PCB Impedance Calculator
Calculate PCB trace impedance for microstrip, coated microstrip, stripline and differential pairs from your stackup geometry and dielectric constant. Solve the reverse problem too: enter a target impedance such as 50 ohm or 100 ohm differential and get the exact trace width you need. Includes a to-scale cross-section diagram, propagation delay, capacitance and inductance per unit length, critical trace length, and a manufacturing tolerance analysis showing how etch and dielectric variation move your impedance.
Your ad blocker is preventing us from showing ads
MiniWebtool is free because of ads. If this tool helped you, please support us by upgrading for ad-free browsing and more daily uses, or allowlist MiniWebtool.com and reload.
- Allow ads for MiniWebtool.com, then reload
- Or upgrade for ad-free browsing and higher daily limits
About PCB Impedance Calculator
The PCB Impedance Calculator works out the characteristic impedance of a printed circuit board trace from your stackup: trace width, copper weight, distance to the reference plane, and the dielectric constant of the laminate. It covers surface microstrip, soldermask-coated microstrip, symmetric stripline, and edge-coupled differential pairs — and it works in both directions, so you can either check a trace you already have or ask it for the exact width that lands on 50 Ω, 90 Ω or 100 Ω differential.
What Is PCB Trace Impedance?
Every trace running over a reference plane is a small transmission line. Its characteristic impedance Z0 is the ratio of voltage to current a travelling wave sees, and it is fixed entirely by geometry and materials — not by how long the trace is. Widen the trace and impedance falls; move the plane further away and impedance rises; switch to a laminate with a higher dielectric constant and impedance falls again.
It matters because a signal that meets a change in impedance reflects part of its energy back toward the driver. Those reflections show up as overshoot, ringing and eye-diagram closure. When the driver, the trace and the receiver all sit at the same impedance, the energy keeps moving forward and the edge arrives clean.
Microstrip vs Stripline: Which One Are You Routing?
Trace on an outer layer with one reference plane below. Part of the field runs through air, so the effective dielectric constant is well below the laminate value and the signal is fast. Easy to route and to probe, but it radiates and picks up noise.
The same structure with soldermask over the top. The resin replaces air above the trace, raising the effective dielectric constant and pulling impedance down by roughly 1–3 Ω. Ignore it and a 50 Ω design ships at 47–49 Ω.
Trace buried between two planes. The entire field is inside the laminate, so the effective dielectric constant equals Er, the signal is slower, and the trace must be much narrower for the same impedance. Radiates almost nothing.
Two coupled traces driven with opposite polarity. The coupling drops the odd-mode impedance, so differential impedance is always less than 2 × Z0, and it falls further as you tighten the gap.
PCB Impedance Formulas
This calculator deliberately avoids the IPC-2141 logarithmic approximations that most free tools still use. Those are convenient but drift several percent outside a narrow validity window — which is a problem when your fabricator quotes a ±10 % impedance window.
K is the complete elliptic integral of the first kind. In the wide-trace limit this reduces exactly to the parallel-plate result \( Z_{0} = 94.15\,B / (W\sqrt{\varepsilon_{r}}) \).
Typical 50 Ω Trace Widths
Impedance depends on the whole stackup, so there is no universal "50 Ω width". These are computed with this tool for 1 oz copper and give a feel for the scale:
| Stackup | Structure | Dielectric | Er | Width for 50 Ω |
|---|---|---|---|---|
| 2-layer 1.6 mm FR4 | Microstrip | 1.5 mm (59 mil) | 4.5 | 2.78 mm (109 mil) |
| 4-layer 1.6 mm FR4 | Microstrip | 0.20 mm (8 mil) | 4.3 | 0.37 mm (14.4 mil) |
| 4-layer, thin prepreg | Microstrip | 0.10 mm (4 mil) | 4.2 | 0.18 mm (7.1 mil) |
| 4-layer inner layer | Stripline | 0.61 mm (24 mil) B | 4.3 | 0.20 mm (7.8 mil) |
| 6-layer inner layer | Stripline | 0.51 mm (20 mil) B | 4.2 | 0.16 mm (6.5 mil) |
Standard Impedance Targets by Interface
| Interface | Impedance | Type | Typical tolerance |
|---|---|---|---|
| RF / general signal | 50 Ω | Single-ended | ±10 % |
| Video, SDI, cable TV | 75 Ω | Single-ended | ±10 % |
| USB 2.0 / USB 3.x | 90 Ω | Differential | ±10 % |
| PCIe, SATA, DisplayPort | 85 Ω | Differential | ±10 % |
| Ethernet, LVDS, HDMI | 100 Ω | Differential | ±10 % |
| DDR3 / DDR4 data | 40–50 Ω | Single-ended | ±10 % |
| DDR3 / DDR4 clock | 85–100 Ω | Differential | ±10 % |
| CAN bus | 120 Ω | Differential | ±10 % |
Common Laminate Dielectric Constants
Er is the number most likely to be wrong in your calculation. FR4 is not a single material — it is a class, and its dielectric constant depends on the resin content and glass style of the specific prepreg or core. Always take Er from your fabricator's stackup drawing when the design is impedance controlled.
| Material | Er (approx.) | Loss tangent | Notes |
|---|---|---|---|
| FR4 (standard, 1 GHz) | 4.2 – 4.6 | 0.020 | Varies with glass/resin ratio |
| FR4 (high resin prepreg) | 3.9 – 4.2 | 0.020 | Thin prepregs run lower |
| Isola FR408HR | 3.65 | 0.0092 | Mid-loss digital |
| Panasonic Megtron 6 | 3.4 | 0.004 | Low loss, high speed |
| Rogers RO4350B | 3.48 | 0.0037 | RF / microwave |
| Rogers RO4003C | 3.38 | 0.0027 | RF / microwave |
| PTFE / Teflon | 2.1 – 2.5 | 0.0004 | Very low loss |
| Polyimide flex | 3.2 – 3.5 | 0.008 | Flexible circuits |
| Soldermask (LPI) | 3.2 – 4.0 | 0.025 | Only affects outer layers |
Why the Tolerance Analysis Matters
A calculator that returns "50.00 Ω" to two decimals is telling you about a board that does not exist. The board you actually receive has an etched trace that is a fraction of a mil narrower or wider than drawn, a prepreg that pressed a little thinner or thicker, and a laminate whose Er is only guaranteed to a range. This tool re-runs the whole model at each of those limits and shows you which one dominates.
In almost every FR4 stackup, dielectric height and dielectric constant dominate, not trace width — which is why simply drawing the trace more precisely does not buy you a tighter impedance, and why controlled-impedance boards cost more: the fabricator adjusts the trace width to compensate for the press-out thickness they actually measure.
How to Use This Calculator
- Choose the trace structure: Surface Microstrip for an outer layer, Coated Microstrip if soldermask covers it, Symmetric Stripline for a buried trace, or one of the differential options for a matched pair.
- Pick what to solve for: "Impedance from width" checks a trace you already have; "Width from target impedance" gives you the width needed to hit 50 Ω, 90 Ω or 100 Ω differential.
- Enter the stackup: dielectric height (or plane-to-plane spacing for stripline), copper weight, dielectric constant, and the trace width or target impedance. Pair spacing is required for differential modes.
- Click Calculate Impedance: the model runs instantly, with no page reload dependency on JavaScript maths.
- Read the results: the cross-section shows your geometry to scale, the gauge places the impedance against common bus targets, and the tolerance table tells you whether the design survives real manufacturing spread.
Design Tips for Controlled Impedance
Request your fabricator's impedance-controlled stackup drawing before routing. Their pressed dielectric heights and Er values are what the board will actually have.
A split or slot under a trace forces the return current to detour, which spikes the local impedance far more than any width error. Keep the plane solid under every high-speed net.
Coated microstrip is the honest model for a real board. Skipping it biases every outer-layer trace 1–3 Ω high in the calculation and low on the finished board.
Differential impedance depends on the gap. Necking down around a connector or via field changes it locally, so return to the nominal gap as fast as the layout allows.
A 10 MHz clock with a 300 ps edge needs impedance control just as much as a 1 GHz clock. Use the critical length this tool reports to decide which nets matter.
Very wide traces over thin dielectrics (W/H above about 10) behave like parallel plates and become extremely sensitive to press-out thickness. Prefer a thicker dielectric instead.
Frequently Asked Questions
What is PCB trace impedance?
PCB trace impedance, or characteristic impedance Z0, is the ratio of voltage to current a signal sees as it travels down a trace above a reference plane. It is set by geometry and material, not by trace length: the trace width, the copper thickness, the distance to the reference plane, and the dielectric constant of the laminate. When a driver, trace and receiver all share the same impedance, the signal arrives without reflections.
How do I calculate microstrip impedance?
Microstrip impedance is computed from the normalized width u = W/H using the Hammerstad-Jensen model. First the air-filled impedance Z01(u) is found, then the effective dielectric constant that accounts for the field split between laminate and air, and finally Z0 = Z01(u) ÷ √εeff. A correction for finite copper thickness widens the effective trace. This calculator uses that full model, which is accurate to better than 0.2 %.
What trace width gives 50 ohms?
There is no single answer, because impedance depends on the whole stackup. On a typical 1.6 mm two-layer FR4 board with Er = 4.5 and 1 oz copper, a 50 Ω microstrip is about 2.8 mm wide. On a four-layer board with an 8 mil dielectric to the nearest plane, the same 50 Ω needs only about 14 mil. Switch this calculator to "Width from target impedance" and it solves the exact width for your stackup.
What is the difference between microstrip and stripline?
A microstrip runs on an outer layer with a reference plane on one side only, so part of its field travels through air. A stripline is buried between two reference planes, so its entire field is inside the laminate. Stripline therefore has a higher effective dielectric constant, a slower propagation delay, needs a narrower trace for the same impedance, and radiates far less. Microstrip is faster and easier to route and probe.
Does soldermask change trace impedance?
Yes. Soldermask replaces the air directly above a microstrip with a resin whose dielectric constant is around 3.2 to 4.0, which raises the effective dielectric constant and lowers impedance. The typical drop is 1 to 3 Ω, which matters when your target tolerance is ±10 %. Use the Coated Microstrip mode to include it. Soldermask has no effect on stripline because the trace is already fully buried.
What is differential impedance?
Differential impedance is the impedance seen between the two traces of a matched pair driven with equal and opposite signals, and it equals twice the odd-mode impedance. Because the two traces couple to each other, differential impedance is always less than twice the single-ended impedance, and it falls as the traces move closer together. USB uses 90 Ω, Ethernet, LVDS and HDMI use 100 Ω, and PCIe and SATA use 85 Ω.
How long can a trace be before impedance matters?
It depends on the signal rise time, not the clock frequency. A trace behaves as a transmission line once the round-trip delay approaches the rise time. The common threshold is tr ÷ (2·tpd), and a conservative design rule uses one sixth instead of one half. This calculator reports both lengths for the rise time you enter.
How accurate is this PCB impedance calculator?
The microstrip model is Hammerstad and Jensen with a thickness correction, accurate to better than 0.2 % against full field solvers. The stripline model is Cohn's exact conformal-mapping solution with a fringing-capacitance thickness correction, rather than the IPC-2141 logarithmic approximation that runs several percent low for narrow traces. In practice the dominant uncertainty is not the model but your laminate Er and etch tolerance — which is exactly what the tolerance analysis quantifies.
Why does my fabricator's number differ from this one?
Fabricators run a 2D field solver against their own measured laminate data, including resin-content-corrected Er, trapezoidal etch profile, copper roughness and the real pressed dielectric height. Differences of 1–3 Ω are normal and usually trace back to Er and pressed thickness rather than to the model. Treat this calculator as the design starting point, and let the fabricator's impedance report be the final word.
Additional Resources
Reference this content, page, or tool as:
"PCB Impedance Calculator" at https://MiniWebtool.com// from MiniWebtool, https://MiniWebtool.com/
by miniwebtool team. Updated: August 20, 2026