Millimeter Wave Specific Challenges mmWave Design Challenges Informational

How do I manage signal routing in a multilayer PCB at millimeter wave frequencies?

Q: What about differential routing at mmWave?

Differential microstrip or stripline is used for mmWave signals in some architectures (especially RFIC interfaces that use differential balanced outputs): the differential pair must maintain tight coupling (consistent pair spacing) for common-mode rejection. At 28 GHz: the pair width + gap must fit within the tight dimensional tolerances. A 100-ohm differential pair on 5 mil RO4003C: each trace ≈ 7 mil, gap ≈ 5 mil (total pair width ≈ 19 mil). Advantages: common-mode noise rejection, reduced radiation (the fields from the two traces partially cancel). Disadvantages: wider total routing width (two traces + gap vs one trace), and the requirement for excellent balance (the two traces must be identical in length and environment to within a fraction of a wavelength).

Signal routing at millimeter-wave frequencies on multilayer PCBs requires extreme precision and electromagnetic awareness. Key challenges and solutions: (1) Controlled impedance: at 28+ GHz, the trace dimensions for 50-ohm impedance are very small. On a 5-mil dielectric (RO4003C, Dk = 3.55): microstrip width ≈ 11 mil (0.28 mm). On Rogers RT/duroid 5880 (Dk = 2.2, 5 mil): microstrip width ≈ 15 mil (0.38 mm). These narrow traces require: tight etching tolerance (±0.5 mil for ≤ ±5% impedance variation), controlled copper roughness (VLP or HVLP foil to minimize loss), and precise dielectric thickness control (±5% for ≤ ±3% impedance variation). (2) Layer assignment: route mmWave signals on the outer layers (microstrip) or on embedded layers between ground planes (stripline). Microstrip: lower loss than stripline (no top ground plane to induce eddy current) but more exposed to radiation and coupling. Stripline: better isolation and shielding but higher loss (the return current flows on two ground planes, increasing the conductor loss). For mmWave: microstrip is generally preferred for signal traces (lower loss). Use stripline only when isolation is critical (feed networks in arrays, sensitive signal paths near digital circuits). (3) Trace length minimization: every millimeter of trace at mmWave adds loss. At 28 GHz on RO4003C: microstrip loss ≈ 0.2-0.5 dB/cm (depends on copper roughness and surface finish). A 5 cm trace: 1-2.5 dB loss. This is a significant portion of the total system loss budget. Design rule: keep all mmWave traces as short as possible. Place the RFIC adjacent to the antenna. Minimize the distance between the PA and the antenna feed. (4) Bends and discontinuities: every bend creates a parasitic effect. A 90° microstrip bend: the outer corner has excess area (capacitive loading), causing a reflection. At 28 GHz: the reflection is significant (S11 ≈ -15 to -20 dB for an unmitigated 90° bend). Mitigation: use 45° mitered bends (cut the outer corner at 45°). The optimal miter: remove 50-70% of the corner area. Result: S11 < -25 dB at 28 GHz.

Category: Millimeter Wave Specific Challenges

Updated: April 2026

Product Tie-In: mmWave Components, Substrates, Packaging

mmWave PCB Signal Routing

PCB signal routing at mmWave is more like RF circuit design than traditional PCB layout. Every trace, via, and bend must be treated as a designed electromagnetic structure.

Technical Considerations

(1) Microstrip: the standard for mmWave PCB routing. Trace on the top layer, ground plane on the layer below. Advantages: lower conductor loss (only one ground plane), easy component mounting (the trace is on the exposed surface), and straightforward impedance calculation. Disadvantages: open top (radiation loss at mmWave, coupling to nearby structures, and sensitivity to nearby objects like mold compound or covers). Loss at 28 GHz on Rogers RO4003C (VLP foil, immersion silver): 0.2-0.35 dB/cm. (2) Stripline: trace embedded between two ground planes. Advantages: enclosed structure (no radiation, excellent isolation, immune to external objects). Disadvantages: higher conductor loss (the return current is shared between two ground planes, increasing the total conductor loss by approximately 40-60%), difficult component mounting (the trace is buried; vias are needed to bring the signal to the surface for component attachment). Loss at 28 GHz on RO4003C: 0.3-0.5 dB/cm (40-50% higher than microstrip). (3) Grounded coplanar waveguide (GCPW): the trace is on the top layer with ground copper on both sides and a ground plane below. The coplanar grounds provide additional return current paths and improve isolation. Advantages: good isolation (the coplanar ground shields the trace from adjacent structures), tunable impedance (the gap between the trace and the coplanar ground provides an additional dimension for impedance control). Disadvantages: the coplanar ground must be stitched to the bottom ground plane with vias (without stitching, the coplanar mode couples to a slot-line mode, creating resonances). Loss: similar to microstrip (the coplanar ground does not significantly increase loss if the gap is > 3× the trace width).

Performance Analysis

At 28+ GHz: every via transition between layers adds 0.2-0.8 dB loss and degrades the return loss. Minimize the number of via transitions: ideal mmWave routing uses zero via transitions (all traces on one layer). If transitions are needed: use blind microvias (shortest possible via, minimum inductance). Add ground via fences around signal vias (quasi-coaxial transition). Optimize the via antipad size with EM simulation. Add compensation structures (pads or stubs) to match the via impedance to 50 ohms. Each via transition should be simulated in 3D EM and the S-parameters verified: target IL < 0.3 dB and RL > 15 dB at the design frequency.

Performance verification: confirm specifications against the application requirements before finalizing the design
Environmental factors: temperature range, humidity, and vibration affect long-term reliability and parameter drift
Cost vs. performance: evaluate whether the application demands premium components or standard commercial grades

Interface compatibility: verify impedance, connector type, and mechanical form factor match the system architecture

Design Guidelines

(1) Registration tolerance: the alignment between layers in the PCB fabrication has a tolerance of ±1-2 mil. Misregistration shifts: trace position relative to ground plane (changes impedance), via position relative to pad (can break the connection if excessive), and coupled-line gap dimensions (critical for couplers and filters). For mmWave: specify the tightest registration tolerance available from the fabricator (typically ±0.5-1 mil for high-end fabricators). (2) Solder mask: at 28 GHz, the solder mask dielectric (Dk = 3.5-4.5, loss tangent = 0.02-0.04) over the microstrip trace adds loss and shifts the impedance. Options: remove solder mask from all mmWave trace areas (solder mask defined opening, SMDO). Leave bare copper or apply immersion silver. This eliminates the solder mask loss and impedance shift. Apply solder mask only over non-RF areas (digital traces, power planes, non-critical pads). Some designers use a selective solder mask process to leave mmWave areas bare while protecting the rest of the board.

Common Questions

Frequently Asked Questions

Can I use FR-4 for 28 GHz routing?

No. FR-4 is unsuitable for mmWave because: (1) High loss tangent: tan_d = 0.020-0.035 at 28 GHz. This creates approximately 1-2 dB/cm dielectric loss alone (in addition to conductor loss). A 3 cm trace: 3-6 dB dielectric loss. (2) Dk variation: Dk = 4.0-4.8 (±10%). The impedance is unpredictable. (3) Dk anisotropy: the glass-fiber weave creates different Dk values along and across the weave. This causes impedance variation along the trace. Use RF laminates: Rogers (RO4003C, RO4350B, RT/duroid), Taconic (TLY, CER-10), Panasonic Megtron 7 (for lower-cost digital + RF designs). For system boards where only a few mmWave traces exist: use a hybrid stack-up with Rogers laminate for the mmWave layers and FR-4 for the digital layers.

How do I handle test points at 28 GHz?

Standard test pads (1-2 mm pads with probing access): the pad capacitance and the probe inductance create a significant impedance discontinuity at 28 GHz. Options: (1) SMPM/GPPO connectors: use miniature board-edge or surface-mount RF connectors rated to 40+ GHz. These provide a calibrated, repeatable connection for VNA measurement. (2) Probe pads: design specific probe pads compatible with microwave wafer probes (GSG or GSGSG configuration). The pad layout matches the probe pitch (typically 150-250 um). EM-simulate the probe pad to ensure < 0.1 dB additional loss. (3) Contactless probing: use a near-field probe above the trace to non-invasively measure the signal level and phase. This does not provide calibrated S-parameters but is useful for troubleshooting. (4) Built-in test couplers: include a -20 dB directional coupler in the mmWave path. The coupled port connects to a test pad. This provides a -20 dB attenuated version of the signal at a test point without disrupting the main signal path.

What about differential routing at mmWave?

Differential microstrip or stripline is used for mmWave signals in some architectures (especially RFIC interfaces that use differential balanced outputs): the differential pair must maintain tight coupling (consistent pair spacing) for common-mode rejection. At 28 GHz: the pair width + gap must fit within the tight dimensional tolerances. A 100-ohm differential pair on 5 mil RO4003C: each trace ≈ 7 mil, gap ≈ 5 mil (total pair width ≈ 19 mil). Advantages: common-mode noise rejection, reduced radiation (the fields from the two traces partially cancel). Disadvantages: wider total routing width (two traces + gap vs one trace), and the requirement for excellent balance (the two traces must be identical in length and environment to within a fraction of a wavelength).

Keep Reading