RF PCB Resources by Frequency Context

L Band PCB | 1–2 GHz Material and Design Guide

A practical guide to designing L band PCBs operating between 1 and 2 GHz, covering laminate selection, controlled-impedance layout, loss budgeting, and common pitfalls for GPS, telemetry, and radar applications.

Microstrip trace routed to an SMA connector on an L band RF PCB

What Is an L Band PCB?

An L band PCB is a printed circuit board engineered for signals between 1 and 2 GHz. This frequency range covers GPS/GNSS receivers (1.575 GHz), Iridium and Globalstar satellite links, air-traffic-control radar (1.03–1.09 GHz), and a growing number of telemetry and electronic-warfare systems. At these frequencies, wavelengths range from roughly 150 mm down to 75 mm, so trace lengths on a typical 50 × 50 mm board are already a meaningful fraction of a wavelength and controlled impedance is mandatory.

Compared with higher microwave bands, L band is forgiving on dielectric loss but unforgiving on cost discipline: choosing an exotic low-loss laminate where standard FR-4 or a mid-tier high-frequency material would suffice wastes budget without measurable performance gain. The sections below walk through how to make that call.

Where L Band Sits in the RF Spectrum

Four-layer PCB cross-section showing RF signal and ground plane layers

L band (1–2 GHz) sits between the sub-GHz band used for LoRa and ISM radios and the S band (2–4 GHz) used for weather radar and some satcom links. The moderate frequency means that conductor loss (resistive loss in copper traces) often dominates over dielectric loss, which reverses the priority compared with boards at C band and above. Understanding this loss split is the first step in choosing a laminate.

Material Selection for 1–2 GHz

At L band, the dielectric constant (Dk) of the substrate sets trace width for a given impedance, while the dissipation factor (Df) determines how much signal energy the board absorbs per unit length. Because dielectric loss scales with frequency, a laminate’s Df matters less at 1.5 GHz than at 10 GHz. That opens the door to cost-effective materials that would be inadequate at higher bands.

Material Tiers for L Band

Tier Examples Dk (typical) Df (typical, 1 GHz) When to Use
Standard FR-4 Shengyi S1000-2, Nanya NP-175F 4.2–4.5 0.018–0.022 Low-cost consumer GPS, short RF paths (< 30 mm)
Low-loss FR-4 Panasonic Megtron 4, Isola I-Tera MT40 3.4–3.7 0.005–0.009 GPS/GNSS front-ends, moderate-length feed networks
PTFE / ceramic-filled Rogers RO4350B (Dk 3.48, Df 0.0037), Arlon 25N 2.2–3.5 0.001–0.004 Radar, satellite transponders, phased-array feeds

For many L band products—think a single-chip GPS receiver on a drone flight controller—standard FR-4 with a well-controlled Dk tolerance (±5 %) is enough. The total dielectric loss over a 25 mm microstrip at 1.575 GHz on 0.5 mm (20 mil) FR-4 is roughly 0.15 dB, which disappears into the noise figure budget of a modern LNA. Switch to a CubeSat transceiver board with a multi-element patch antenna feed network spanning 100 mm, and that same FR-4 costs you 0.6 dB or more—enough to justify a move to RO4350B or an equivalent.

Nanya Laminates

Nanya offers a range of FR-4 and enhanced laminates that are widely available and competitively priced. For L band designs where cost is the primary driver, use the selector below to find a Nanya grade that meets your Dk and thickness requirements.

Loading Nanya Material Selector…

If the selector returns NP-175F or NP-170TL, you have a standard-loss glass-reinforced epoxy suitable for short RF traces at L band. For anything with Df below 0.010, check that the quoted Dk tolerance is tight enough for your impedance target—±3 % is preferred for 50 Ω microstrip.

Arlon Laminates

Arlon’s ceramic-filled and PTFE-based laminates serve the higher end of L band design: radar T/R modules, satellite payload boards, and military IFF transponders where loss, phase stability, and thermal reliability all matter. Use the tool below to compare Arlon grades by Dk, Df, and operating temperature.

Loading Arlon Material Selector…

A result such as Arlon 25N (Dk 3.38, Df 0.0025 at 10 GHz) is well suited to an L band radar feed network that must also survive –55 °C to +125 °C thermal cycling per IPC-6012 Class 3 requirements. Its Df at 1.5 GHz will be even lower than the 10 GHz datasheet value, giving comfortable margin.

Stackup and Controlled Impedance

Most L band boards use four to six layers. A common four-layer stackup places the RF signal on Layer 1, an uninterrupted ground plane on Layer 2, a power or low-speed signal layer on Layer 3, and a second ground on Layer 4. The critical dimension is the dielectric thickness between Layer 1 and Layer 2: for 50 Ω microstrip on RO4350B (Dk 3.48), a 10 mil (0.254 mm) core yields a trace width of approximately 22 mil (0.56 mm) using 1 oz (35 µm) copper.

Microstrip vs Stripline at L Band

  • Microstrip — preferred for antenna feeds, filters, and anything that must radiate or be probed. Easier to tune post-fabrication. Slightly higher radiation loss, but negligible below 2 GHz.
  • Stripline — preferred for internal routing of LO and IF signals where shielding from adjacent layers is needed. Requires two reference planes, increasing layer count.

At L band, radiation loss from open microstrip is small enough that stripline is rarely chosen for the RF path itself. Reserve it for sensitive clock or local-oscillator distribution where isolation to adjacent digital layers matters.

Trace Geometry and Transitions

Keep these layout rules in mind for any L band PCB:

  1. Ground plane continuity — no splits, slots, or via stitching gaps under the RF trace. A 1 mm slot in the return plane at 1.5 GHz creates a measurable impedance bump and radiates.
  2. Via transitions — when moving an RF signal between layers, use a ground-via fence (minimum four vias) around the signal via, spaced no more than λ/20 apart (≈ 4 mm at 2 GHz). Back-drill or use blind vias to eliminate stubs longer than 20 mil.
  3. Connector launch — SMA and MMCX connectors are standard at L band. Taper the pad geometry to match the connector’s center-pin diameter to the trace width over 1–2 mm; an abrupt width change creates a capacitive discontinuity visible on a TDR.
  4. Bend radius — use mitered or curved bends with a radius ≥ 3× trace width. At 1.5 GHz the added reflection from a right-angle bend is small (often below –30 dB), but it compounds in a long feed network.

Loss Budget Example: GPS L1 Front-End

GPS L1 ceramic patch antenna on a PTFE laminate PCB

Consider a GPS L1 receiver at 1.575 GHz with an external patch antenna, a SAW filter, an LNA, and a 30 mm microstrip run on 10 mil RO4350B:

Element Loss / Gain
Antenna-to-board transition –0.15 dB
30 mm microstrip (RO4350B) –0.08 dB
SAW filter insertion loss –1.8 dB
LNA gain +18 dB
Post-LNA 20 mm microstrip –0.05 dB

Total pre-LNA loss is about 2.0 dB, dominated by the SAW filter, not the PCB. Swapping RO4350B for standard FR-4 would add roughly 0.12 dB to the two microstrip segments—measurable but unlikely to change system performance. This is why many commercial GPS modules ship on FR-4: the board loss is a rounding error next to the filter.

The calculus changes for an L band attenuator or power-divider network where the RF path is 150 mm or longer and every tenth of a dB matters to the link margin.

Thermal and Mechanical Considerations

L band radar transmitters can push several hundred watts through the board. At these power levels, copper weight and thermal via density under power-amplifier pads become critical. Use 2 oz (70 µm) copper for PA supply planes and add a thermal-via array (0.3 mm drill, 1 mm pitch) under the device ground paddle. For PTFE-based laminates, note that the coefficient of thermal expansion (CTE) in Z can exceed 200 ppm/°C above Tg; specify a filler-loaded grade (e.g., Rogers RO4350B datasheet lists Z-axis CTE of 32 ppm/°C) to protect plated through-hole reliability.

Common Pitfalls

  • Over-specifying the laminate — choosing PTFE for a simple GPS patch antenna that could run on low-loss FR-4 doubles the board cost with no measurable sensitivity improvement.
  • Ignoring moisture absorption — standard FR-4 absorbs up to 0.15 % moisture by weight, which raises Dk and detunes narrowband filters. For outdoor or space-qualified L band boards, ceramic-filled laminates with < 0.02 % absorption are safer.
  • Neglecting the ground plane — a split ground under a 50 Ω trace at 1.5 GHz shifts impedance by 5–15 Ω depending on slot width. Always run a DRC check for reference-plane voids under RF traces.
  • Stub resonances from through-hole vias — a 62 mil (1.57 mm) via stub resonates near 24 GHz, well above L band, so back-drilling is usually unnecessary at these frequencies unless the same board carries higher-band signals.

Design Checklist

  1. Define the RF path length and acceptable insertion loss to choose a material tier.
  2. Lock Dk tolerance to ±3 % or better; request the fabricator’s Dk test coupon data at 1–2 GHz.
  3. Set stackup with an unbroken ground plane directly below the RF layer.
  4. Calculate trace width for 50 Ω (or system impedance) using the laminate’s actual Dk at 1.5 GHz, not the 1 MHz catalog value.
  5. Place ground-via fences around every layer transition and along board edges near RF traces.
  6. Specify surface finish: ENIG for wire-bondable pads, immersion tin or OSP for standard soldering; avoid HASL on fine-pitch RF pads.
  7. Add test coupons for impedance verification per IPC-2141 and request TDR data with the deliverable.

FAQ

Can I use FR-4 for an L band PCB?

Yes, for short RF paths under about 40 mm and applications where 0.1–0.2 dB of extra loss is acceptable—most consumer GPS and telemetry receivers qualify. Use a grade with a published Dk at 1 GHz and request ±5 % or tighter tolerance.

What trace width gives 50 Ω at 1.5 GHz?

It depends on the substrate. On 10 mil RO4350B (Dk 3.48) with 1 oz copper, the answer is approximately 22 mil (0.56 mm). On 10 mil FR-4 (Dk 4.3), it drops to about 18 mil (0.46 mm). Always verify with your fabricator’s impedance calculator using their actual measured Dk.

Is back-drilling needed at L band?

Rarely. A 62 mil via stub resonates near 24 GHz, far above the 1–2 GHz operating range. Back-drilling becomes relevant only if the same board also carries signals above about 6 GHz, such as on a multi-band 5.8 GHz ISM layer.

How does L band PCB design differ from S band?

The main difference is loss sensitivity. At S band (2–4 GHz), dielectric loss roughly doubles and trace dimensions shrink, making laminate Df and etch tolerance more critical. L band designs have wider traces, lower loss, and more material flexibility.

What surface finish is best for L band RF pads?

ENIG (electroless nickel / immersion gold) is the default for its flat pad coplanarity and solderability. For cost-sensitive builds, immersion tin works well. Avoid hot-air solder leveling (HASL) on fine-pitch RF pads because the uneven surface degrades impedance control at the connector launch.

Ready for a quotation?

Send your requirements for a material, stackup and manufacturing review. Price and schedule are confirmed for your project.

Upload Gerber