Originally published on AtlasPCB Engineering Blog
The connector launch — where a PCB trace connects to a coaxial connector, board-to-board interconnect, or cable assembly — is one of the most commonly underestimated impedance discontinuities in high-speed PCB design. In our DFM reviews, we see connector launch-related impedance violations in roughly 40% of designs operating above 6 GHz. The irony is that engineers spend significant effort optimizing their trace routing, material selection, and via transitions, only to lose 3-5 dB of return loss budget at the connector interface because the launch pad geometry was left at the connector manufacturer's default recommendation.
This guide covers the electromagnetic principles behind launch pad design, provides practical design rules for common connector families (SMA, SMPM, board-to-board), and explains the fabrication considerations that determine whether your simulated launch performance translates to production reality.
Why Connector Launches Are the Weak Link
To understand why launches are problematic, consider the geometric reality. A 50-ohm microstrip trace on standard FR-4 (Dk 4.2, 8 mil dielectric) has a width of approximately 0.15mm (6 mil). An SMA connector center pin pad requires 0.7-1.0mm diameter to accept the pin and provide adequate solder fillet area. That represents a 5:1 to 7:1 width expansion happening over a very short distance.
This geometric expansion creates excess capacitance. The larger pad area couples more strongly to the ground planes below and beside it, reducing the local characteristic impedance from 50 ohms down to 35-42 ohms in the pad region. For signals at frequencies where this impedance dip spans a significant fraction of a wavelength, energy reflects back toward the source. At 10 GHz, a wavelength in FR-4 is approximately 15mm, and even a 1mm launch region represents nearly 7% of a wavelength — enough to generate measurable reflections.
The problem compounds because the connector itself contributes its own discontinuity. The pin-to-barrel geometry inside the connector is optimized for 50 ohms but transitions to the PCB through solder or press-fit interfaces that add inductance. The total launch discontinuity is the combined effect of the PCB pad geometry and the connector mechanical interface — and the designer controls only the PCB side.
Ground Via Placement: The Return Current Foundation
The most critical and most frequently overlooked aspect of connector launch design is ground via placement. Every high-frequency signal requires a low-impedance return current path in close proximity to the signal conductor. At DC and low frequencies, this return path can take any route through the ground system. Above 1 GHz, the return current concentrates directly beneath (for stripline) or beside (for microstrip) the signal trace due to proximity effect.
At the connector launch, the return current must transition from the ground plane beneath the trace to the connector shell or ground pins. This transition happens through the ground vias surrounding the signal pin. If these vias are too far from the signal pin, or if there are too few of them, the return current takes a longer path, creating excess inductance that appears as a high-impedance spike in the TDR response.
For SMA connectors operating to 18 GHz, ground vias should be placed within 0.5mm of the signal pad edge, with at least four vias arranged symmetrically around the signal pin. Each via should be a full-depth plated through-hole connecting all ground layers. The via diameter should be 0.3mm or larger to minimize via inductance, and the vias should connect to the connector ground tabs or shell pads with short, wide traces.
For higher-frequency applications using SMPM (to 65 GHz) or 1.85mm connectors (to 67 GHz), ground via spacing must tighten to 0.2-0.3mm from the signal pin edge. At these frequencies, the ground vias themselves can resonate if they are too long relative to wavelength, so via depth becomes a consideration — backdrilling or blind vias may be necessary to eliminate stub resonances in the ground return path.
In our fabrication process, we routinely drill ground vias at 0.2mm diameter with 0.15mm finished hole size for high-frequency launches. This requires laser drilling or precision mechanical drilling with tight positional tolerance. When reviewing designs for RF connectors, we verify that ground via-to-signal-pad clearance meets both the electrical requirement (close proximity) and the fabrication requirement (minimum 0.15mm drill-to-copper clearance for mechanical drilling, 0.1mm for laser).
Anti-Pad Geometry: Tuning Local Impedance
Anti-pad relief — enlarging the ground plane clearance around the signal pad — is the most effective single technique for compensating the excess capacitance at a connector launch. The principle is straightforward: by moving the ground plane edges further from the pad, you reduce the parallel-plate capacitance and raise the local impedance back toward 50 ohms.
For a standard SMA launch pad of 0.9mm diameter on 8-mil FR-4, the default anti-pad might be 1.4mm (0.25mm annular clearance). Enlarging this to 1.8-2.2mm raises the local impedance by 5-10 ohms, partially compensating the pad capacitance. The optimal anti-pad size depends on the specific stackup, but a good starting point is 2.0-2.5 times the pad diameter for the ground layer immediately adjacent to the signal layer.
One important subtlety: the anti-pad on the reference ground layer (the layer providing the return current for the signal trace approaching the pad) has the strongest effect. Anti-pads on more distant ground layers contribute less but still matter for tight impedance targets. For designs targeting better than -20 dB return loss above 10 GHz, anti-pads should be specified on at least the two ground layers closest to the signal layer.
The fabrication consideration here is that anti-pad size affects isolation between adjacent launches. If two SMA connectors are placed at 10mm center-to-center spacing (common on test fixtures and RF boards), excessively large anti-pads may overlap, creating a ground void between the two launches that compromises isolation. In our DFM review, we verify that anti-pad enlargements maintain at least 0.3mm ground copper between adjacent anti-pads for adequate isolation.
Trace Taper Design: The Gradual Transition
The connection between the controlled-impedance trace and the connector pad should never be an abrupt step. A well-designed taper provides a gradual impedance transition that distributes the discontinuity over a length comparable to or longer than a quarter wavelength, converting what would be a concentrated reflection into a distributed, lower-amplitude return.
For a linear taper connecting a 0.15mm trace to a 0.9mm pad, the taper length should be at least one-quarter wavelength at the maximum operating frequency. At 20 GHz on FR-4 (effective permittivity approximately 3.0), the quarter wavelength is about 2.2mm. A taper length of 2-3mm therefore provides adequate transition for most sub-20 GHz applications.
The taper profile (linear, exponential, or Klopfenstein) matters for ultra-wideband applications but makes negligible difference below 20 GHz for practical PCB geometries. A simple linear taper is easiest to implement in standard PCB CAD tools and provides adequate performance for the vast majority of designs we fabricate.
One practical fabrication note: very narrow trace tapers at the trace end (below 75 µm) become challenging for standard photolithography processes. If your controlled impedance trace is already at the minimum feature size for your manufacturing process class, the taper should begin at the trace width and expand toward the pad — never narrow below the trace width. In our standard process, we achieve 75 µm (3 mil) minimum trace width reliably, so tapers terminating at this dimension are fully manufacturable.
Stackup Considerations for Launch Optimization
The PCB stackup fundamentally constrains launch performance because it determines the dielectric thickness, reference plane locations, and via aspect ratios available to the designer. Certain stackup choices inherently support better launches.
Thin dielectric layers beneath the launch signal layer reduce both the controlled-impedance trace width and the reference plane distance, making anti-pad tuning more effective. A 4-mil dielectric between signal and ground (versus 8 mil) halves the 50-ohm trace width and provides a closer reference plane that responds more sensitively to anti-pad geometry changes. However, thin dielectrics also increase pad capacitance for a given anti-pad size, so the net benefit depends on the specific geometry.
The signal layer choice matters as well. Surface-layer launches (microstrip) allow connector pins to solder directly to the top copper without via transitions, eliminating via discontinuity. However, microstrip is more susceptible to radiation loss at high frequencies and less shielded from external interference. Internal-layer launches (stripline) provide better shielding but require a via transition from the connector pin to the internal signal layer, adding discontinuity that must be managed.
For designs above 25 GHz, we recommend discussing launch layer strategy during the stackup review phase. The choice between surface-layer and embedded-layer launches significantly affects both signal integrity and fabrication complexity, and making this decision early avoids costly redesigns.
Practical Design Rules by Connector Family
SMA Connectors (DC to 18 GHz)
The standard SMA connector remains the workhorse for RF test, instrumentation, and moderate-frequency communications. For SMA launches on standard 62-mil FR-4 boards, the following rules provide reliable performance to 18 GHz with return loss better than -15 dB.
Signal pad diameter should be 0.7-0.9mm for standard SMA pin dimensions (0.32mm center conductor diameter). Ground vias of 0.3mm finished hole size should be placed at four locations symmetrically around the signal pad at 0.5mm center-to-center from the signal pad center. Anti-pad relief on the first ground layer should be 1.8-2.0mm diameter. The trace taper from 50-ohm trace width to pad edge should be 1.5-2.0mm long with a linear profile.
For edge-launch SMA connectors (the most common type), the signal trace should approach the pad in the same direction as the coaxial center pin to minimize the bend discontinuity. Side-entry approaches add a 90-degree bend at the launch that creates additional reflection, particularly above 12 GHz.
SMPM / GPPO Connectors (DC to 65 GHz)
SMPM (also known as GPPO or Mini-SMP) connectors demand significantly tighter launch design. The smaller pin geometry (0.14mm center conductor) and higher operating frequency require ground vias within 0.2-0.3mm of the signal pad, anti-pads of 0.6-0.8mm on adjacent ground layers, and trace tapers of 0.5-1.0mm. These dimensions push against standard PCB manufacturing limits and often require advanced fabrication processes.
In our facility, SMPM launches typically require laser-drilled ground vias (0.1mm holes), controlled-depth drilling for stub management, and tight registration tolerance (±25 µm) to maintain symmetry. We recommend discussing SMPM launch requirements during the DFM review to ensure your design aligns with achievable tolerances.
High-Speed Board-to-Board Connectors (56 Gbps PAM4+)
Modern high-speed connectors from suppliers like Samtec, TE Connectivity, and Molex operate at 56-112 Gbps per lane using PAM4 signaling. These connectors have proprietary footprint recommendations that include specific via patterns, anti-pad shapes, and trace routing constraints. In most cases, following the connector vendor's reference design for the launch footprint provides adequate performance.
However, vendor recommendations assume a specific stackup (often their reference board stackup) that may not match your production design. When adapting vendor footprints to a different stackup, the anti-pad dimensions and ground via positions require adjustment. The ground via distance should maintain the same electrical length (time of flight) rather than the same physical distance when moving to a different dielectric thickness.
TDR Validation and Manufacturing Verification
Time Domain Reflectometry (TDR) is the primary measurement technique for validating launch performance. A well-designed launch appears on a TDR trace as a smooth transition between the connector impedance (50 ohms) and the trace impedance (50 ohms) without sharp spikes or dips exceeding the design tolerance (typically ±5 ohms for standard applications, ±2 ohms for high-performance).
For production verification, we recommend including a TDR test coupon on the panel that replicates the connector launch geometry without the connector installed. This coupon allows measurement of the PCB contribution to launch impedance independently of connector variation. The coupon should include the full launch geometry: pad, anti-pad, ground vias, and taper — but terminate in a matched trace for time-domain measurement.
Manufacturing variables that affect launch performance include drill registration (affects ground via symmetry), etch compensation accuracy (affects trace taper profile), and copper plating uniformity in the ground vias (affects via impedance). In our controlled-impedance process, we hold drill registration to ±50 µm and etch tolerance to ±0.5 mil, which maintains launch impedance within ±3 ohms of design target for most geometries.
Common DFM Mistakes We See in Launch Designs
After reviewing thousands of high-frequency board designs, certain launch-related errors appear repeatedly. The most common is simply using the connector manufacturer's default land pattern without any impedance optimization — these patterns are designed for mechanical reliability (adequate solder fillet, proper pin retention) rather than electrical performance. Adding anti-pad relief and ground via optimization to an existing land pattern typically improves return loss by 5-10 dB without changing the mechanical interface.
The second most common mistake is asymmetric ground via placement. For a four-via ground pattern, placing three vias on one side and one on the other creates a return current imbalance that converts common-mode noise and degrades isolation. Ground vias should be distributed symmetrically around the signal axis.
The third frequent issue is routing the trace to the connector at an angle rather than straight on. Any bend within 2mm of the launch pad adds its own reflection that compounds with the launch discontinuity. Route signal traces straight into connector pads for the final 3-5mm whenever board geometry permits.
When to Invest in Full-Wave Simulation
For designs operating below 10 GHz with standard SMA connectors, the design rules in this guide provide adequate launch performance without full-wave electromagnetic simulation. Following the ground via, anti-pad, and taper guidelines will yield return loss better than -15 dB in most cases.
Above 10 GHz, or for designs requiring better than -20 dB return loss, full-wave simulation (HFSS, CST, or similar) of the complete launch geometry becomes worthwhile. The simulation should include the connector model (most vendors provide S-parameter models or 3D geometry files), the PCB stackup, and the specific anti-pad and via geometry. This investment pays for itself by eliminating the prototype-measure-redesign cycle that otherwise consumes 2-4 weeks per iteration.
For production volumes above 100 boards, we recommend investing in launch simulation to optimize yield. A marginal launch that passes at room temperature may fail impedance testing at temperature extremes due to dielectric constant shifts, making production testing more stringent than prototype validation.
Reviewed by AtlasPCB Engineering Team — with direct experience fabricating RF connector launches for applications from 2 GHz GPS modules to 67 GHz millimeter-wave test fixtures.
If you are designing RF boards with SMA, SMPM, or high-speed connector launches and want to discuss impedance optimization during DFM review, AtlasPCB fabricates controlled-impedance boards with launch geometries validated by TDR measurement. We hold drill registration to ±50 um and etch tolerance to ±0.5 mil for consistent launch performance.
Top comments (0)