“Route USB and the RF feed at 50 Ω” is one of the most common lines in the notes that come with a board. It is also one of the most under-specified: the right track width depends entirely on the stack-up the fab will actually build. This post walks through the estimate we make before we route, and why the final number always comes from the fab’s stack-up.
The geometry that sets impedance
A track on an outer layer over a solid reference plane is a microstrip. Its characteristic impedance Z₀ depends on four things:
- w — track width;
- h — dielectric thickness between the track and its reference plane (on a 4-layer board, the prepreg between L1 and L2);
- t — copper thickness (1 oz finished copper is about 35 µm);
- εr — the dielectric constant of the prepreg, which for FR-4 class materials is roughly 4.0–4.6 and drops slightly with frequency.
Board thickness, the core in the middle and the bottom layers do not matter for an L1 microstrip, as long as L2 is an unbroken plane under the track.
A first estimate: IPC-2141A
The classic closed-form approximation for surface microstrip is:
It is reasonable for w/h between roughly 0.1 and 2 and good to a few percent in that range, which makes it a useful sanity check but not a sign-off.
Worked example
Take a common 4-layer build with a 7628-style prepreg of about 0.21 mm between L1 and L2, 1 oz outer copper and εr = 4.4. We want Z₀ = 50 Ω.
- 87 / √(4.4 + 1.41) = 87 / 2.410 ≈ 36.1 Ω.
- We need ln(5.98·h / (0.8·w + t)) = 50 / 36.1 ≈ 1.385, so 5.98·h / (0.8·w + t) ≈ e1.385 ≈ 3.99.
- 0.8·w + 0.035 = 5.98 × 0.21 / 3.99 ≈ 0.315 mm, so w ≈ 0.35 mm.
That lands where most fab calculators land for this stack-up. For other prepreg thicknesses the same formula gives:
| Prepreg h | w for 50 Ω (εr 4.4) | w for 50 Ω (εr 4.2) |
|---|---|---|
| 0.10 mm | 0.14 mm | 0.15 mm |
| 0.21 mm | 0.35 mm | 0.36 mm |
| 0.36 mm | 0.63 mm | 0.65 mm |
You can reproduce every number here, and try your own stack-up, with our free impedance calculator.
The ratio w/h stays around 1.4–1.8 for 50 Ω on FR-4, which is a handy rule of thumb when you review someone else’s layout: a 50 Ω microstrip is usually a bit wider than its dielectric is thick.
How much does it move?
Around the 0.35 mm / 0.21 mm design point, the same formula gives these sensitivities:
| Change | Z₀ |
|---|---|
| Track 0.03 mm narrower (0.32 mm) | ≈ 52.9 Ω |
| Track 0.03 mm wider (0.38 mm) | ≈ 47.3 Ω |
| Prepreg 0.02 mm thinner (0.19 mm) | ≈ 46.4 Ω |
| Prepreg 0.02 mm thicker (0.23 mm) | ≈ 53.3 Ω |
| εr 4.0 instead of 4.4 | ≈ 51.8 Ω |
Two lessons follow. First, dielectric thickness matters more than most people expect: a pressed prepreg that ends up 20 µm thinner than nominal costs you almost 4 Ω. Second, etching tolerance on the track (fabs typically hold ±10–20% on fine features) is of the same order. That is why controlled-impedance boards are specified as “50 Ω ±10%” and why the fab adjusts the track width on its own CAM data to hit the target on the stack-up it actually presses.
Solder mask and plating
Solder mask over a microstrip lowers its impedance slightly — typically by one to three ohms for a normal mask thickness — because some of the field now runs through a dielectric instead of air. Plating on outer layers adds copper thickness and nudges impedance down as well. Neither is in the simple formula above; both are in a proper field solver and in the fab’s own model.
Differential pairs
For an edge-coupled pair, IPC-2141 gives a first-order estimate of the differential impedance from the single-ended Z₀ and the gap s between the tracks:
On the same 0.21 mm stack-up, this suggests about 0.25 mm tracks with a gap near 0.14 mm for a 90 Ω USB 2.0 pair. Treat that as a starting point only: coupled-line formulas are less accurate than the single-ended one, and fabs quote pairs from their own solver. Common targets are 90 Ω for USB 2.0, 100 Ω for Ethernet and most LVDS, and 85 Ω for PCI Express.
What we do in practice
- Start from the fab’s stack-up, not a generic one. Most fabs publish their standard 4- and 6-layer builds with prepreg type, thickness and εr; many have an online impedance calculator tied to those builds.
- Put the target in the net class in KiCad (Board Setup → Net Classes) with the calculated width, and for pairs the pair width and gap. We route to those numbers.
- Keep the reference plane continuous under every controlled-impedance track. A split or a slot under the track does more damage than a few microns of width.
- Order the board as impedance-controlled and state the targets in the fab notes. The fab then tunes widths on its CAM data and can provide coupon test results.
When you order routing from us, tick Controlled impedance and list the targets in the notes (for example “USB_D± 90 Ω diff, RF_OUT 50 Ω SE, reference L2”). We check the widths against your chosen fab’s stack-up before routing and record the assumptions in the evidence dossier.