RF PCB Stackup Planning

Cavity RF Stackup | Embedded MMIC Recess Design

A cavity RF stackup recesses an MMIC or bare die into the PCB so its RF pads sit coplanar with the top trace layer, shortening wire bonds and cutting parasitic inductance at millimeter-wave frequencies. This guide covers cavity depth control,…

Milled cavity in a multilayer RF PCB exposing the copper ground plane

What Is a Cavity RF Stackup?

A cavity RF stackup is a multilayer PCB construction in which one or more pocket-shaped recesses are machined or laminated into the board so that an MMIC die, filter element or other component sits below the surface plane. The die’s RF pads end up coplanar with—or within 25 µm (1 mil) of—the surrounding microstrip traces, which keeps wire-bond lengths under 300 µm and limits parasitic inductance to well below 0.1 nH per bond at 77 GHz. This approach is standard in automotive radar front-ends, satcom T/R modules and phased-array tiles wherever flip-chip or conventional surface mount cannot meet the electrical or thermal budget.

Why Embed an MMIC in a Cavity?

Cross-section of a cavity RF stackup with embedded MMIC die

Surface-mounted MMICs on a flat board force the wire bond to arc upward and back down, adding length and therefore inductance. At 24 GHz that extra inductance is tolerable; at 77 GHz it shifts the match enough to cost 1–2 dB of gain. A cavity eliminates the height difference. Additional benefits include:

  • Shorter thermal path. The die sits closer to the ground plane or a coin-embedded heat spreader, reducing junction-to-board thermal resistance by 30–50 % compared with surface mount on the same laminate.
  • Lower profile. Recessing the tallest component lets the overall module height shrink, critical in conformal phased arrays.
  • Improved shielding. The cavity walls act as a partial waveguide-below-cutoff enclosure, containing stray fields from the die.

For multi-chip imaging radar boards that cascade several MMICs, cavity embedding keeps inter-chip trace lengths short and symmetric—an approach detailed further in guides on cascaded radar MMIC architectures.

Anatomy of a Cavity RF Stackup

Layer Arrangement

A typical 6-layer cavity RF stackup for a 77 GHz radar front-end looks like this:

Layer Function Material Example Thickness
L1 (top) RF signal, microstrip traces RO3003 (Dk 3.00, Df 0.0013) 5 mil (127 µm)
L2 Ground / cavity floor Copper + prepreg 0.5 oz Cu
L3 Stripline routing RO4350B (Dk 3.48) 6.6 mil (168 µm)
L4 Ground Copper 1 oz Cu
L5 Power / control FR-4 or low-cost thermoset Variable
L6 (bottom) Ground / thermal pad Copper 1 oz Cu

The cavity is milled through L1 and its underlying prepreg, stopping at L2 copper. This makes L2 both the die-attach ground and the microstrip reference plane. Boards that combine low-loss RF laminates on top with standard FR-4 below follow a mixed-Dk stackup philosophy to control cost.

Cavity Depth Control

Depth accuracy is the single hardest fabrication parameter. Most controlled-depth milling processes hold ±50 µm (±2 mil); laser-ablated cavities in thin laminates can reach ±25 µm. The target depth equals the total dielectric removed minus the desired step between the die pad and L1 traces. For a 200 µm thick MMIC on a 127 µm dielectric, the cavity floor should sit 73 µm below the L1 surface if the goal is perfect coplanarity—tight enough that a ±50 µm tolerance demands careful stackup planning. The cavity and back-drill PCB capabilities page discusses achievable tolerances in more detail.

Ground-Plane Continuity Under the Cavity

Removing dielectric to form the cavity interrupts the return-current path on L2 at the cavity edges. Two countermeasures are standard:

  1. Plated cavity walls. The milled sidewalls are metallized during the board’s plating cycle, stitching L1 ground copper to L2 and forming a continuous shield.
  2. Via fencing. A ring of ground vias at λ/20 spacing surrounds the cavity perimeter, suppressing parallel-plate modes between L1 and L2 that would otherwise radiate at the gap.

Both techniques also help with the MMIC die-attach ground path, ensuring the epoxy or solder preform under the die sees low-impedance ground on all sides.

Laminate Selection for Cavity Stackups

The RF layer must survive the milling process without delamination or smearing. PTFE-based laminates (Rogers RO3003, Taconic TLY) machine cleanly and offer Df below 0.002 at 77 GHz, but they are soft and require controlled feed rates. Thermoset hydrocarbon laminates like RO4350B are stiffer and easier to mill, though their Df (~0.004 at 10 GHz) limits use above about 40 GHz in loss-critical paths. Use the database below to compare Dk and Df across candidate materials at your operating frequency.

Loading Dk Df Laminate Database…

For example, selecting RO3003 shows a Dk of 3.00 ± 0.04 and Df of 0.0013 at 10 GHz—values that translate to roughly 0.15 dB/cm microstrip loss at 77 GHz on a 5 mil substrate. If the link budget allows 0.3 dB/cm, the less expensive RO4350B may suffice, saving 40–60 % on laminate cost. A broader comparison of high-frequency substrates is available in the high-frequency PCB materials guide.

Designing the Cavity: Step-by-Step

Radar module PCB with multiple MMIC cavities and via fences
  1. Define die height and pad coplanarity target. Get the MMIC thickness from the foundry datasheet (typical: 75 µm, 100 µm, 150 µm or 200 µm for GaAs/GaN). Decide the maximum allowable step between die pad and board trace—25 µm is a good default for 25 µm diameter gold wire bonds.
  2. Calculate required cavity depth. Cavity depth = (L1 dielectric thickness + prepreg thickness) − (die thickness − coplanarity target). If the number is negative, the die is thinner than the stackup above L2 and you need a pedestal or thicker die-attach layer.
  3. Size the cavity footprint. The cavity floor must exceed the die outline by at least 150 µm (6 mil) per side for pick-and-place tolerance, plus clearance for the epoxy fillet. Add another 250 µm if plated walls are specified.
  4. Place the via fence. Ring the cavity with ground vias on λ/20 centers at the highest operating frequency. At 77 GHz in RO3003 (effective wavelength ≈ 2.24 mm), that means vias every 112 µm—tight, but achievable with laser-drilled microvias.
  5. Verify thermal path. If the MMIC dissipates more than 1 W, consider a copper coin or filled thermal vias under the cavity floor. Model junction temperature with the actual stackup thermal conductivity, not a generic value.
  6. Add alignment features. Include fiducials on L1 referenced to the cavity center so the die bonder can place the MMIC to ±25 µm.

The RF PCB stackup library contains downloadable cavity stackup templates for 24 GHz and 77 GHz radar that can serve as a starting point.

Design Checklist for Cavity RF Stackups

Before releasing Gerbers, run through the checklist builder below. Enter your cavity dimensions, laminate choices and bond-wire parameters; the tool flags common omissions such as missing keep-out zones, unspecified depth tolerances and absent via fences.

Loading Design Checklist Builder…

A completed checklist should confirm at minimum: cavity depth and tolerance noted on the fab drawing, L2 copper weight specified (0.5 oz minimum for die attach), plated-wall or via-fence requirement called out, and die-attach material (conductive or non-conductive epoxy, or AuSn preform) identified. Missing any one of these is the most common cause of first-article failure on cavity boards.

Common Pitfalls

  • Ignoring prepreg flow into the cavity. During lamination, prepreg resin can flow into an open cavity and raise the floor. Specify no-flow or low-flow prepreg (e.g., Rogers 2929 bondply) for the layer directly above the cavity floor.
  • Skipping X-ray verification. After lamination, X-ray the cavity area to confirm L2 copper is intact and no resin pooling has shifted the effective depth.
  • Over-milling into L2 copper. Controlled-depth routing that cuts into the ground plane raises DC resistance and can create resonant slots. Specify a minimum remaining copper thickness of 18 µm (0.5 oz) on the fab drawing.
  • Neglecting moisture sensitivity. Exposed cavity surfaces absorb moisture, raising Dk locally. Bake boards at 105 °C for 4–6 hours before die attach per JEDEC J-STD-033D moisture-sensitivity guidelines.

Frequently Asked Questions

How deep can a PCB cavity be milled?

Production controlled-depth milling typically handles cavities from 100 µm (4 mil) to about 1.5 mm (60 mil) deep with ±50 µm tolerance. Deeper pockets are possible but require slower feed rates and in-process depth gauging, adding cost.

Can FR-4 be used for the cavity layer?

FR-4 can physically form a cavity, but its Dk variation (4.2–4.8 depending on resin content and frequency) and high Df (0.020 at 10 GHz) make it unsuitable for the RF signal layer. It is commonly used for non-RF power and digital layers below the cavity in a hybrid stackup.

Is a copper coin necessary under every cavity?

Not always. For MMICs dissipating under roughly 0.5 W, filled thermal vias on a 0.5 mm grid beneath L2 ground copper provide adequate heat spreading. Above 1 W, a press-fit copper coin brazed or adhesive-bonded into the stackup is the safer choice, as described in Rogers RO3000 series application notes on thermal management.

What wire-bond length is acceptable at 77 GHz?

Keep bond wires under 300 µm total length (pad to pad). Each 100 µm of 25 µm diameter gold wire adds roughly 0.07 nH, which at 77 GHz represents about 34 Ω of reactance—enough to degrade a 50 Ω match by more than 1 dB if uncompensated.

How do I specify a cavity on the fab drawing?

Call out cavity X-Y location, outline dimensions, target depth with tolerance (e.g., 150 µm ± 50 µm), reference copper layer, wall finish (plated or bare), and corner radius (minimum 200 µm for mechanical milling). Include a cross-section sketch showing the cavity relative to the full stackup.

Ready for a quotation?

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

Upload Gerber