RF PCB Design Resources

RF Connector Launch Design | SMA to 1.85 mm

A well-designed RF connector launch is the difference between a clean −25 dB return loss and a resonant spike that kills your channel. This guide covers footprint geometry, ground via fencing, and anti-pad sizing for SMA, 2.92 mm, and 1.85…

SMA edge-launch connector soldered to an RF PCB with visible ground via fence

What Is an RF Connector Launch?

An RF connector launch is the physical transition where a coaxial connector’s center pin meets a PCB transmission line—microstrip, grounded coplanar waveguide (GCPW), or stripline. The launch geometry controls the impedance discontinuity at that boundary. A poor launch adds reflections (high return loss), radiates stray energy, and sets the usable bandwidth ceiling of the entire signal chain. A good launch maintains better than −20 dB return loss across the connector’s rated bandwidth while keeping insertion loss under 0.3 dB per transition up to at least 26.5 GHz for SMA, 40 GHz for 2.92 mm, and 67 GHz for 1.85 mm interfaces.

Connector Families at a Glance

Cross-section of a vertical-launch RF connector through a multilayer PCB
Interface Rated Frequency Center Pin Ø (typ.) Mating Compatibility Common Use
SMA DC–18 GHz (mode-free), usable to ~26.5 GHz 1.27 mm (50 mil) 3.5 mm Wi-Fi, sub-6 GHz 5G, test fixtures
2.92 mm (K) DC–40 GHz 0.91 mm (36 mil) SMA, 3.5 mm Radar, satcom, mmWave test
1.85 mm (V) DC–67 GHz 0.51 mm (20 mil) 2.4 mm 77 GHz automotive radar, 5G FR2

Mating compatibility matters for measurement: a 2.92 mm connector mates with any SMA cable, so you can prototype at lower cost and move to precision 2.92 mm adapters for final characterization. A 1.85 mm connector mates with 2.4 mm, not SMA—mixing the two will damage the smaller pin.

Edge-Launch vs Vertical-Launch vs End-Launch

Edge Launch (Through-Board)

The connector body clamps to the board edge. The center pin slides into a channel milled into the board edge and solders to a surface trace. This is the most common topology for frequencies above 10 GHz because the transition is short and the ground path is continuous through the connector’s flange bolted to the ground plane.

Vertical Launch (Through-Hole)

The connector mounts perpendicular to the board. The center pin passes through a plated via to an inner-layer stripline or to a top-layer trace. The via stub creates a capacitive discontinuity that limits bandwidth; back-drilling or using blind vias is usually mandatory above 10 GHz. Vertical launches are common in backplane and test-fixture applications where edge space is unavailable.

End Launch (Solderless Compression)

A precision connector presses its center pin against a PCB pad using a spring-loaded mechanism—no solder joint. End-launch connectors from vendors like Rosenberger and Southwest Microwave achieve repeatable performance to 67 GHz and beyond, but they require tight board-edge tolerances (±2 mil / ±0.05 mm) and specific RF DFM rules on the milled edge.

Critical Launch Geometry Parameters

Signal Pad and Anti-Pad Sizing

The signal pad width must match the connector center pin diameter closely—typically within ±2 mil (±0.05 mm). The anti-pad (clearance in the ground plane beneath the signal pad) sets the local characteristic impedance. Too small an anti-pad increases capacitance and drops impedance below 50 Ω; too large an anti-pad raises impedance and creates an inductive discontinuity. A useful starting point: set the anti-pad diameter to roughly 2.5× the signal-pad width for a microstrip launch, then tune with a 3-D EM solver.

Ground Via Fence

Ground vias surrounding the signal pad serve two purposes: they provide a low-inductance return path from the connector shell to the PCB ground plane, and they suppress parallel-plate and surface-wave modes that cause resonances. Key rules:

  • Via spacing: keep center-to-center pitch below λ/20 at the maximum operating frequency. At 40 GHz (λ ≈ 7.5 mm in free space, ~4.5 mm in RO4350B), that means ≤ 0.22 mm (8.7 mil) pitch—tight but achievable with 8 mil vias on 12 mil pitch.
  • Proximity to signal via: the first ring of ground vias should be as close to the signal pad as impedance allows. For a 2.92 mm edge launch, 20–25 mil (0.5–0.6 mm) center-to-center from the signal pad edge is typical.
  • Via diameter: use the largest drill the pitch allows. Larger vias have lower inductance per via.

Insufficient via fencing is the single most common cause of resonant dips in connector launch S-parameter sweeps. A dip at a specific frequency usually means the via fence spacing is λ/2 at that frequency—halving the pitch eliminates it.

Trace Taper and Transition Length

The connector center pin is round; the PCB trace is rectangular. A short linear taper (typically 15–30 mil / 0.4–0.75 mm long) smooths the impedance transition. Avoid abrupt width changes. For mmWave designs above 40 GHz, even the taper shape matters: a Klopfenstein or exponential taper outperforms a simple linear taper by 3–5 dB of return-loss margin.

Edge Connector Rule Checker

Use this tool to verify your edge-launch connector footprint. Enter the connector pin diameter, anti-pad clearance, ground-via pitch and count, board thickness, and target frequency. The checker flags violations of spacing and impedance rules before you commit to fabrication.

Loading Edge Connector Rule Checker…

If the checker reports a via-pitch violation, the fix is straightforward: reduce the drill size by one standard increment (e.g., 10 mil → 8 mil) to fit more vias in the same arc, or widen the ground-pad footprint if the connector body allows it. A passing result at 40 GHz with 8 mil vias on 14 mil pitch and an anti-pad clearance of 12 mil per side is a realistic baseline for a 2.92 mm launch on 6.6 mil RO4350B.

Material and Stackup Considerations

Two 1.85 mm end-launch connectors on a mmWave PCB with isolation vias

The substrate directly under the connector launch dominates performance. For SMA launches up to 18 GHz, standard FR-4 (Dk ≈ 4.2, Df ≈ 0.02 at 10 GHz) works if trace widths are controlled. Above 18 GHz, move to low-loss laminates: Rogers RO4350B (Dk 3.48, Df 0.0037) is the workhorse to 40 GHz; RO3003 (Dk 3.00, Df 0.0013) is preferred for 77 GHz automotive radar launches. Dk and Df shift with frequency, so always use the datasheet value at your operating frequency, not the 10 GHz headline number.

Board thickness at the launch matters because it sets the microstrip or GCPW trace width for 50 Ω. Thinner cores (4–6 mil / 0.1–0.15 mm) yield narrower traces that better match small connector pins. A 1.85 mm connector with a 20 mil center pin on a 10 mil core would need a trace roughly 9 mil wide on RO4350B—feasible but at the limit of standard etching tolerances.

Simulation and Validation

Every connector launch should be simulated in a 3-D full-wave solver (HFSS, CST, or openEMS) before layout release. Model the actual connector body—most vendors supply STEP and EM simulation models. Assign wave ports at the coax reference plane and the PCB trace reference plane, then sweep S₁₁ and S₂₁ across the full rated bandwidth.

Target performance benchmarks:

  • Return loss (S₁₁): better than −20 dB across the operating band; better than −15 dB up to the connector’s rated maximum.
  • Insertion loss (S₂₁): under 0.3 dB per launch at 26.5 GHz (SMA), under 0.5 dB at 40 GHz (2.92 mm), under 0.8 dB at 67 GHz (1.85 mm).
  • No resonant nulls: any dip deeper than −15 dB within the band is unacceptable and indicates a mode or via-fence issue.

After fabrication, validate with a VNA using TRL or 2x-Thru de-embedding to separate the launch performance from the trace loss. This is the only way to confirm that what you simulated matches what was built.

RF Connector Launch Isolation and Shielding

When multiple connectors share a board edge—common in multichannel receivers—crosstalk between adjacent launches can exceed −40 dB at millimeter-wave frequencies if no countermeasures are taken. A row of stitching vias between adjacent launches, combined with a keep-out zone of at least 3× the anti-pad diameter, typically provides 20 dB of additional RF isolation. For tighter requirements, add a milled slot between launches to break the surface-wave path.

Pre-Tapeout Design Checklist

Before releasing your layout, run through every launch-related rule in one pass. Enter your design parameters below and the tool builds a go/no-go checklist covering pad geometry, via fencing, anti-pad clearance, stackup compatibility, and connector mechanical keep-outs.

Loading Design Checklist Builder…

A completed checklist with zero flags means your launch geometry is consistent with the rules above. If the tool flags “anti-pad too large,” revisit your ground-plane cutout—an oversized cutout is the second most common launch defect after insufficient via fencing, and it shows up as a broad impedance hump centered on the launch in a TDR sweep.

Frequently Asked Questions

Can I use an SMA footprint for a 2.92 mm connector?

Mechanically, yes—2.92 mm connectors are SMA-compatible. Electrically, the SMA footprint’s larger anti-pad and wider via pitch will limit performance above roughly 20 GHz. For 2.92 mm performance to 40 GHz, use the connector vendor’s recommended footprint with tighter via fencing.

How many ground vias do I need around an edge-launch connector?

Enough to close the via fence with a pitch below λ/20 at the highest operating frequency. For a 26.5 GHz SMA launch, that means ≤ 0.35 mm pitch; for a 40 GHz 2.92 mm launch, ≤ 0.22 mm pitch. Typically 6–10 vias in a semicircle around each side of the signal pad.

What causes a resonant dip in my connector launch S₁₁?

Almost always a parallel-plate or surface-wave mode excited by a gap in the ground via fence. The resonant frequency corresponds to λ/2 of the open dimension. Closing the fence gap or adding a stitching via at the resonant spot eliminates the dip.

Do I need back-drilling for a vertical-launch connector?

Above approximately 10 GHz, yes. The via stub below the signal layer acts as a quarter-wave resonator. Back-drilling the stub to within 10 mil (0.25 mm) of the signal layer pushes the resonance well above the operating band. Alternatively, use blind vias to avoid the stub entirely.

What board-edge tolerance does a solderless end-launch connector require?

Most precision end-launch connectors specify ±2 mil (±0.05 mm) on the milled board edge and ±1 mil on the signal-pad location relative to that edge. Discuss these tolerances with your fabricator early—they often require a dedicated routing pass rather than standard V-scoring. Consult the IPC-2221 generic design standard for baseline edge-tolerance classes.

Ready for a quotation?

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

Upload Gerber