PCB DesignJanuary 15, 20268 min read

Microstrip Impedance Design Guide: From Theory to PCB Layout

A practical guide to designing controlled-impedance microstrip traces on PCBs. Covers the Hammerstad-Jensen equations, material selection, manufacturing tolerances, and how to verify your design.

Why 50Ω Matters

The 50Ω impedance standard emerged from a compromise between power handling (which favors lower impedance) and insertion loss (which favors higher impedance around 77Ω). For RF work, 50Ω is the near-universal standard. For video, 75Ω. For some logic signals, 100Ω differential is common.

When trace impedance doesn't match the source or load, reflections occur. At DC and low frequencies this is harmless — signals travel slowly enough that the transient dies before causing damage. But above roughly:

f_{critical} = \frac{v_p}{20 \cdot l}

where *v*ₚ is propagation velocity (~0.6c on FR4) and *l* is trace length, impedance control becomes important. For a 10cm trace on FR4, this is approximately 900 MHz.

The Hammerstad-Jensen Equations

Most online calculators use the simplified IPC-2141 equations, which are accurate to about ±5%. For manufacturing, use Hammerstad-Jensen (1980) with Wadell corrections, which achieve ±1% accuracy.

For a narrow trace (W/H < 1):

Z_0 = \frac{60}{\sqrt{\varepsilon_{eff}}} \ln\left(\frac{8H}{W_e} + \frac{W_e}{4H}\right)

For a wide trace (W/H ≥ 1):

Z_0 = \frac{120\pi}{\sqrt{\varepsilon_{eff}} \left[\frac{W_e}{H} + 1.393 + 0.667 \ln\left(\frac{W_e}{H} + 1.444\right)\right]}

where *W*ₑ is the effective width (accounting for copper thickness) and *ε*eff is the effective dielectric constant.

Material Selection

Material	εᵣ	tan δ	Use case
FR4 standard	4.2–4.5	0.020	General digital, <1 GHz RF
FR4 high-frequency	3.9–4.1	0.015	DC–3 GHz
Rogers 4003C	3.38 ±0.05	0.0021	RF, microwave to 10 GHz
Rogers 4350B	3.48 ±0.05	0.0037	RF, microwave to 10 GHz
PTFE (PTFE/glass)	2.10–2.55	0.0009	Microwave, mmWave
Alumina 96%	9.6	0.0001	High-power RF, hybrids

FR4's dielectric constant varies with frequency (4.5 at 100 MHz → 4.1 at 10 GHz) and with the glass weave. For critical RF designs above 1 GHz, specify a controlled-Dk laminate.

Manufacturing Tolerances

A typical PCB manufacturer holds these tolerances:

Trace width: ±0.05mm (2 mil) for standard, ±0.025mm (1 mil) for controlled impedance
Dielectric thickness: ±10% standard, ±5% for impedance-controlled stackups
Copper thickness: ±10%

Combined, these produce an impedance variation of roughly ±10% on a standard order and ±5% on an impedance-controlled order. If you need better than ±5%, you need to specify it explicitly and expect a higher cost.

Practical Design Rules

Target 50Ω for RF, 100Ω differential for high-speed digital. On a standard 1.6mm FR4 board with 1oz copper:

50Ω single-ended ≈ 2.8mm trace width
100Ω differential ≈ 0.12mm spacing between 1.8mm traces

Keep reference planes solid. Voids, slots, or splits under a controlled-impedance trace change the local impedance unpredictably. Route RF traces away from board edges and connectors that might be cut near the reference plane. Stitch vias around RF traces. For microstrip, add ground vias every λ/20 on either side of the trace to suppress parallel-plate resonances. Match discontinuities. Connector launches, vias, and pads all create impedance discontinuities. Compensate with pad size reduction (anti-pad) or void out the reference plane slightly at via transitions.

Verification

Use our Microstrip Impedance Calculator to compute your trace dimensions, then confirm with your board house's stackup impedance calculator. For production, request a test coupon — a separate trace with the same geometry that can be measured with a TDR (time-domain reflectometer) to verify actual impedance before assembly.

← Back to Blog