PCB Impedance Calculator
Estimate the characteristic impedance of a trace, or solve for the width that hits your target. Four structures: microstrip, stripline, differential microstrip, and coplanar waveguide.
When a trace becomes a transmission line
At DC, a trace is a resistor. As the edge rate gets faster, the same trace becomes a transmission line: the voltage no longer arrives at the far end at the same time, and reflections appear if the impedance changes. The usual rule of thumb is to treat a trace as controlled impedance when its electrical length is longer than about one-sixth of the rise-time edge.
In practice, the interfaces tell you. USB 2.0, USB 3.x, HDMI, Ethernet, PCIe, DDR memory, MIPI, and RF feeds all specify an impedance and a tolerance. If you are designing one of those, the question is not whether to control impedance but which stackup and geometry gets you there.
The four structures
Microstrip
A trace on an outer layer with one reference plane below. The field is partly in the dielectric and partly in the air (or solder mask), which is why the effective Er is lower than the laminate Er and why solder mask matters.
Stripline
A trace buried between two reference planes. The field is fully inside the laminate, so the impedance is more stable and the structure radiates less. The relevant height is the plane-to-plane distance, not the distance to one plane.
Differential microstrip
Two coupled traces on an outer layer. The differential impedance is not simply twice the single-ended impedance; the gap controls the coupling. Narrow gaps lower the differential impedance and increase crosstalk sensitivity to spacing tolerance.
Coplanar waveguide
A signal trace with ground on the same layer on both sides, optionally with a backside ground. CPW is common in RF because it keeps the return current close to the signal and is less sensitive to substrate thickness. The gap to ground is part of the geometry.
The variables that actually move the number
- Dielectric height. Impedance is roughly logarithmic in h; a 10% stackup error moves the impedance several percent. This is the variable fabricators control most tightly.
- Er. FR-4 is not a single number. Resin content, glass style, frequency, and temperature all move it. Use the laminate supplier's value at your operating frequency, not a generic 4.4.
- Copper thickness. 1 oz versus 2 oz changes the width needed for the same impedance. Plating adds thickness on outer layers, so the finished geometry is not the same as the artwork.
- Solder mask. Mask loads the exposed field on microstrip and CPW, lowering impedance by a few percent. Include it in the field model if the target is tight.
- Etch and width tolerance. A ±1 mil width tolerance on a 5 mil trace is ±20%. The fabricator's etch process and the artwork compensation matter as much as the calculator.
How to talk to the fabricator
Send three things with the Gerber: the target impedance, the tolerance, and the reference plane for each controlled layer. A stackup drawing with layer thicknesses and Er values is better than a note that says “control impedance.” If the board has a test coupon, say so; if it does not, ask whether the fabricator will add one.
For digital interfaces, ±10% is common. For RF and tight high-speed links, ±5% is achievable with a defined stackup and coupon, but it costs more. The fabricator's field solver is the authority; this page is for choosing a starting geometry and catching obvious mistakes before the stackup review.
Common mistakes
- Using the core Er for a prepreg layer, or the other way around. They are often different materials with different resin content.
- Using the distance to one plane for stripline instead of the plane-to-plane distance.
- Ignoring the solder mask on microstrip and CPW.
- Changing the differential gap without re-checking the single-ended impedance of each line.
- Routing a controlled-impedance trace across a split in the reference plane. The return current has to detour, and the impedance is no longer controlled.
- Trusting a calculator without a stackup review. The calculator does not know the fabricator's actual laminate, plating, or etch.
Frequently asked questions
When do I need controlled impedance?
When the rise time is short relative to the trace length, or when the interface specifies it. As a rule of thumb, treat a trace as a transmission line when the electrical length is longer than about one-sixth of the rise-time edge. USB, HDMI, Ethernet, DDR memory, PCIe, and RF feeds normally require controlled impedance.
How accurate is this impedance calculator?
It is an engineering approximation, typically within about 10–15% for ordinary geometries. The real impedance depends on the fabricated stackup, copper roughness, etch taper, solder mask, and the field solver used by the fabricator. Use this tool to choose a starting width; let the board shop confirm the final stackup with a coupon or field solver.
What Er should I use for FR-4?
Most FR-4 laminates are specified around 4.2–4.6 at 1 MHz. At higher frequencies the effective Er drops, and the value depends on resin content, glass style, and frequency. Ask the laminate supplier for the Er at your operating frequency, and use the same value the fabricator uses in its stackup.
Why does solder mask change impedance?
Solder mask has a different dielectric constant from air (typically 3.3–3.8), so it loads the trace and lowers the impedance slightly. The effect is larger on microstrip than on stripline because the field is exposed. A field solver or the fabricator's coupon should include the mask; simple calculators often ignore it.
What impedance tolerance should I specify?
±10% is common for digital interfaces; ±5% is achievable for RF and high-speed boards with a defined stackup and test coupon. Tighter tolerance costs more because the fabricator has to control etch, laminate thickness, and plating more tightly. Specify the tolerance with the target and the reference plane.
Can I use this for differential pairs?
Yes, for an initial estimate. The differential model uses the single-ended microstrip impedance of each line and the gap-to-height ratio. Real differential impedance also depends on the pair's symmetry, the reference plane, and the coupling length. For USB, HDMI, or 100Ω Ethernet, confirm the final geometry with the fabricator's field solver.
Stackup review
Send the stackup, get a real impedance check.
Tell us the target, the laminate, and the layer count. We will propose a stackup, run the geometry through the field solver, and quote the board with the impedance coupon included.