Signal integrity guide
RF and high-speed PCB design: materials, signal integrity and EMC
Fast edges and radio frequencies turn copper traces into transmission lines, antennas and resonators. This guide covers the decisions that matter most — laminate choice, return paths, crosstalk, vias, power delivery and emissions — and explains what to tell us when your board needs special materials or controlled impedance.
Get an instant quoteWhen a board counts as high-speed or RF
A 10 MHz microcontroller can have a signal-integrity problem, and a 100 MHz bus can be perfectly fine. What decides it is how fast the edges switch and how long the traces are — not the clock frequency printed on the datasheet.
Rise time sets the bandwidth
Length versus edge
RF is about wavelength
| Rise time (10–90%) | Approx. bandwidth (0.35 ÷ rise time) | Approx. critical length on FR-4 (outer layer) |
|---|---|---|
| 5 ns | 70 MHz | ≈ 125 mm |
| 1 ns | 350 MHz | ≈ 25 mm |
| 300 ps | ≈ 1.2 GHz | ≈ 7–8 mm |
| 100 ps | 3.5 GHz | ≈ 2–3 mm |
Values are rough guidance for planning only; the real propagation speed depends on the effective dielectric constant of your stack-up. Modern logic families often switch in well under a nanosecond, so check the edge rate in the IBIS model or datasheet rather than assuming the clock frequency tells the story.
Dielectric constant (Dk) and loss (Df): when FR-4 is enough
Two laminate properties matter most for fast signals. Dk (dielectric constant, also called relative permittivity) sets impedance and propagation speed. Df (dissipation factor, or loss tangent) sets how much signal energy turns into heat in the material. Both change with frequency, so always compare datasheet values at a frequency close to your own.
| Material class | Typical Dk (around 1–10 GHz) | Typical Df | Usually suitable for |
|---|---|---|---|
| Standard FR-4 (glass-epoxy) | ≈ 4.0–4.6 | ≈ 0.015–0.025 | Most digital designs, USB 2.0, 100 Mb/1 Gb Ethernet, short links up to a few Gb/s, sub-GHz and 2.4 GHz radios with short RF traces |
| Mid-loss / improved FR-4 | ≈ 3.7–4.2 | ≈ 0.008–0.012 | Longer multi-Gb/s links, PCIe-class and fast memory buses on larger boards |
| Low-loss / very low-loss laminates | ≈ 3.0–3.8 | ≈ 0.002–0.008 | Long 10 Gb/s+ channels, backplanes, high-end networking |
| RF laminates (ceramic-filled hydrocarbon, PTFE-based) | ≈ 2.2–3.6, tightly controlled | ≈ 0.001–0.004 | Antennas, filters, couplers, power amplifiers, microwave and mmWave circuits |
Signs that FR-4 is enough
Signs you need a better material
Dk tolerance matters as much as Dk
Glass weave effect
Hybrid stack-ups
Return paths and reference planes
Every signal current has a return current flowing back to its source. At high frequency that return current flows in the plane directly under the trace, because that is the path of lowest inductance. Most signal-integrity and EMC problems start when this return path is interrupted.
A solid plane under every fast signal
Do not cross splits or slots
Watch via clearance chains
Changing layers
Prefer ground over power as reference
Keep fast nets off the board edge
Crosstalk, spacing and differential pairs
Crosstalk is unwanted coupling between neighbouring traces through their electric and magnetic fields. It grows with parallel length and edge speed, as traces get closer together, and as they sit further from their reference plane.
| Technique | Why it helps | Typical guidance |
|---|---|---|
| Increase spacing | Coupling falls quickly with distance | A common rule of thumb is a centre-to-centre spacing of about 3× the trace width (the “3W rule”) between fast nets; more for clocks and sensitive analog |
| Thin dielectric to the plane | Tight coupling to the plane leaves less field to couple sideways | Signal layers placed close to their reference plane crosstalk less at the same spacing |
| Shorten parallel runs | Coupled noise builds up with coupled length | Separate aggressor and victim where they run in parallel for long distances |
| Route fast nets as stripline | Inside the board, far-end crosstalk is much lower than on outer microstrip layers | Keep the most sensitive or fastest links on inner layers between two planes when possible |
| Orthogonal adjacent layers | Broadside coupling between stacked traces is strong | If two signal layers are adjacent, route them at right angles to each other |
- 1
Take the target from the chip vendor
Use the differential impedance and skew budget from the interface specification or datasheet. Common targets and how to request controlled impedance are explained in stack-up and controlled impedance. - 2
Route the pair together
Keep both traces the same width and spacing along their whole length, on the same layer, with the same reference plane. Avoid splitting the pair around a via or component. - 3
Match lengths close to the mismatch
Compensate skew with small, gentle serpentines near the point where the mismatch occurs (for example right after a bend or pin escape), not all at one end. - 4
Keep breakouts symmetrical
Fan the pair out of the chip and into the connector symmetrically, and place any AC-coupling capacitors side by side. - 5
Separate pairs from other nets
Keep other signals and other pairs further away than the gap inside the pair — a common starting point is several times the intra-pair gap.
Vias in fast signals: stubs, backdrilling and stitching
A through-hole via on a multilayer board is a short piece of transmission line with its own capacitance and inductance. At multi-Gb/s rates and in RF circuits, the via often becomes the largest discontinuity in the channel.
What a stub is
Why stubs hurt
Ways to reduce stubs
| Method | Effect on stub | Things to consider |
|---|---|---|
| Layer choice | Short stub when the signal uses most of the barrel | Free, but limits routing freedom |
| Backdrilling | Removes most of the stub; a small residual length remains | Needs drill depth and target layers stated clearly; our online calculator offers a Backdrill option on 4+ layer boards |
| Blind / buried vias | No stub at all on that span | Extra lamination and drilling steps; see the vias guide |
| Thinner board | Shorter barrels and stubs | Must still meet layer count, impedance and mechanical needs |
Ground vias next to signal vias
Stitching and via fences
Hole types, via filling and blind/buried vias are covered in vias and special holes.
Power integrity: decoupling and plane pairs
Fast chips draw current in sharp bursts. If the power distribution network cannot supply them quickly, the supply rail dips and bounces, adding jitter and noise to every signal the chip drives.
- 1
Work out a target impedance
A common first estimate is allowed ripple voltage ÷ transient current. For example, a 1.0 V rail allowed 3% ripple (30 mV) with a 2 A load step gives a target of about 15 mΩ. The supply network should stay below that across the frequency range the chip cares about. - 2
Use a close power–ground plane pair
A power plane placed directly against a ground plane with a thin dielectric forms a low-inductance capacitor that helps at high frequencies where discrete capacitors stop working. Thinner dielectric means more capacitance and lower inductance. - 3
Mix capacitor values by frequency
Bulk capacitors cover low frequencies, ceramic capacitors in the 0.1–10 µF range cover the middle, and small low-inductance capacitors plus the plane pair cover the top. Follow the chip vendor’s decoupling recommendation first. - 4
Place capacitors for low loop inductance
Put the smallest capacitors closest to the power pins, keep the pad-to-via connection short and wide, and use two vias per pad where possible. Mounting inductance often matters more than the capacitor value.Tip: Placing capacitors on the bottom side directly under a BGA often gives the shortest path.
- 5
Avoid narrow necks in the planes
Split planes for several rails should not leave thin copper bridges that fast currents must pass through; check current density and voltage drop as well (IPC-2152 covers conductor current capacity).
EMC basics
A board that works on the bench can still fail emissions or immunity tests. Most emissions come from a few places, and most fixes are cheaper at layout time than after a failed test.
| Common source | Why it radiates | Layout response |
|---|---|---|
| Clock and fast data lines | Harmonics of the edge rate spread far above the clock frequency | Short routes on inner layers, controlled edge rates, series termination near the driver |
| Large current loops | Loop area acts as a magnetic antenna | Solid return plane, compact switching-regulator layout with the hot loop kept small |
| Cables and connectors | Common-mode noise on a cable turns it into an efficient antenna | Filter or common-mode choke at the connector, connector shield bonded to ground |
| Slots and plane edges | Slots and edges act as slot antennas and fringe fields | Keep planes solid, stitch ground layers along the board edge |
| Switching power supplies | Fast switch nodes and diode recovery | Small switch-node copper, input/output filtering, shielding if needed |
Edge stitching
Shield cans
Filter at the boundary
Test against the right standard
Copper roughness and surface finish at high frequency
At high frequency, current crowds into a thin layer at the conductor surface (the skin effect). In copper the skin depth is roughly 6.6 µm at 100 MHz, 2.1 µm at 1 GHz and 0.66 µm at 10 GHz, so the texture and coating of that surface start to matter.
| Factor | Effect on fast signals | Typical guidance |
|---|---|---|
| Copper foil roughness | Rough foil makes current follow a longer, bumpier path once skin depth approaches the roughness height, raising loss | Low-profile (VLP / HVLP) foils are used on low-loss builds for long multi-GHz channels |
| ENIG (nickel + thin gold) | Nickel is ferromagnetic and lossier than copper; matters where current flows through the finish, mainly on exposed outer RF traces | Fine for most designs and best for flat, fine-pitch pads; for sensitive exposed RF lines, keep them under solder mask or choose a non-nickel finish where available |
| OSP | Thin organic coating, essentially no extra conductor loss | Flat and low-loss, but limited shelf life and fewer reflow cycles |
| HASL / lead-free HASL | Uneven solder thickness changes trace geometry slightly | Economical; less suited to fine pitch and precise RF pad shapes |
| Solder mask over traces | Mask adds dielectric above microstrip, lowering impedance a few percent and adding small loss | Include mask in impedance calculations; some RF designs keep mask off critical lines |
Our online calculator offers HASL (with lead), lead-free HASL, ENIG and OSP. A full comparison of finishes is in the surface finish guide.
What to send for a quote
Fast and RF boards are only as good as the information that reaches the factory. The clearer your notes, the fewer questions we need to ask before production.
| Item | What to include |
|---|---|
| Stack-up drawing | Layer order, copper weight per layer, dielectric thickness between layers and the finished board thickness |
| Material requirement | Standard FR-4 and TG, or a property-based spec (Dk and Df at a stated frequency, or an IPC-4101 / IPC-4103 specification sheet). Name an equivalent material only if you allow substitutes |
| Impedance table | Target value and tolerance, single-ended or differential, layer, trace width and gap, reference plane(s), coplanar ground gap |
| Backdrill details | Which nets or holes, the drill-from side, the deepest layer that must be kept and the maximum allowed stub |
| Via treatment | Tented, plugged, epoxy filled & capped or copper paste filled & capped — for example via-in-pad under fine-pitch RF chips |
| Edge and shielding features | Edge plating, ground keep-outs, shield-can pads and any areas that must stay free of solder mask |
| Surface finish | The finish you need and any reason it must not be changed |
- 1
Standard FR-4 up to 16 layers: price online
Rigid FR-4 boards up to 16 layers get an instant online price. For 4 or more layers you can tick Specify stack-up (impedance), add an impedance test report, and choose options such as Backdrill and edge plating. The online price includes GST and shipping, and the minimum order is 5 PCBs. - 2
Put your notes inside the files
Add a readme or fab drawing to the Gerber zip, or use the order note field. Our engineers read the production notes in your files and compare them with the options you selected. How to package files is explained in preparing your design files. - 3
RF and low-loss materials: quoted by our team
PTFE-based, ceramic-filled and other special RF laminates, hybrid stack-ups and anything outside the online options are quoted by our team. Send your files and notes through contact us and we will come back with a price. - 4
Engineering check before production
Our engineers check every file set before production. If a stack-up cannot be built as drawn or a note conflicts with the selected options, we contact you before going ahead. - 5
Testing and delivery
Every bare board gets a free 100% flying-probe electrical test for opens and shorts. Bare PCB delivery is typically 10–15 working days including express shipping within India.
Assembling an RF or high-speed board?
Frequently asked questions
Related guides
Still have a question?
Send us your files or call us — our engineers will help you choose the right options for your boards and assembly.
Streamline your innovation with
seamless PCB ordering.