How to Design Cavity PCB

07 October 2026
New

Cavity PCB design creates a controlled-depth recess inside a multilayer printed circuit board to place components, expose selected copper surfaces, reduce local package height, or create a controlled mechanical and thermal interface. A reliable PCB cavity design starts by defining cavity depth, floor layer, sidewall geometry, component clearance, copper keepouts, routing, vias, fabrication tolerances, and the required inspection method before routing is finalized. Typical production designs may use 0.30–2.00 mm cavity depths, 0.10–0.25 mm sidewall clearances, 0.20–0.30 mm mechanical vias, 50/50–75/75 µm HDI routing, and 50 Ω or 90/100 Ω controlled-impedance structures. The key engineering principle is simple: a cavity is not only a mechanical pocket; it changes the local PCB stackup, thermal path, dielectric geometry, routing space, and manufacturing process.

What Is Cavity PCB?

Characteristics and Structure

A Cavity PCB is a multilayer PCB containing a machined or otherwise controlled-depth opening that removes selected dielectric and copper layers without cutting through the entire board.

A typical structure may contain:

Top copper layer
Rigid dielectric
Internal signal layers
Cavity opening
Cavity floor
Internal copper reference plane
Bottom copper layer

For example, a 1.60 mm multilayer PCB may use a 0.80 mm cavity that stops above an internal reference layer. The remaining 0.80 mm structure forms the cavity floor.

The cavity can therefore change only part of the Z-axis structure while preserving the mechanical integrity of the complete PCB.

Why Create a Cavity?

Common engineering objectives include:

Reducing total package height.
Embedding or partially recessing components.
Creating an RF component pocket.
Improving thermal contact.
Exposing a copper heat-spreading surface.
Creating a controlled-depth mechanical interface.
Integrating high-density packaging into a smaller enclosure.

A cavity is most valuable when the removed PCB thickness solves a specific mechanical, thermal, or electrical constraint.

PCB Cavity Design Rules

Define Fabrication Drawings

A cavity should never be defined only by an outline on the top copper artwork.

The fabrication drawing should identify:

Cavity X/Y dimensions.
Cavity depth.
Cavity floor layer.
Finished board thickness.
Sidewall tolerance.
Component clearance.
Copper keepout.
Routing restrictions.
Surface-finish requirements.
Inspection method.

A cavity drawing may specify:

Finished depth: 0.80 ±0.05 mm
Opening: 12.00 × 8.00 mm
Sidewall tolerance: ±0.10 mm
Floor layer: L4
Minimum component clearance: 0.20 mm

The exact tolerance must match the selected machining process.

Use Dedicated Mechanical Layers

The cavity geometry should have its own fabrication definition.

Dedicated CAD layers can identify:

Cavity milling boundary
Final cavity boundary
Depth-control boundary
Tool-entry region
Component keepout
Copper keepout

This prevents the cavity from being interpreted as an ordinary copper-layer opening.

The fabrication drawing and CAD database should contain the same cavity reference dimensions. A 10.00 mm cavity in the CAD file and a 10.10 mm cavity in the mechanical drawing creates an avoidable manufacturing ambiguity.

Apply Clearances and Keepouts

Cavity Sidewall Clearance

Copper should not normally terminate directly at a machined cavity wall.

A practical starting clearance is approximately:

0.15–0.25 mm for standard cavity features
0.25–0.50 mm for aggressive mechanical routing
Larger clearance where tolerance stack-up is significant

For a cavity with ±0.10 mm positional tolerance and ±0.05 mm routing tolerance, a nominal 0.10 mm copper clearance can become insufficient after process variation.

The clearance must therefore include the complete tolerance stack rather than relying on nominal CAD dimensions.

Component Clearance

The component body, solder fillet, and assembly tooling must all fit inside the cavity.

For a 0.40 mm-pitch BGA placed inside a cavity, the component keepout should account for:

Package body tolerance
Placement tolerance
Solder spread
Cavity-wall tolerance
Rework access

A nominal 0.10 mm gap may be insufficient for production assembly even when the component physically fits in the CAD model.

Routing and Vias

Routing Near Cavities

Routing around cavities requires both electrical and mechanical planning.

A typical HDI PCB cavity design may use:

50/50–75/75 µm line/space
0.20–0.30 mm mechanical PTH
75–100 µm laser microvias
50 Ω single-ended impedance
90 or 100 Ω differential impedance

Traces should remain outside the machining allowance unless the design specifically requires copper exposure.

Routing immediately beside a cavity wall can create:

Reduced dielectric thickness
Increased mechanical stress
Etching exposure
Impedance discontinuity
Potential copper damage during machining

Via Placement

Vias near cavities require a larger engineering margin than ordinary vias.

A practical starting clearance is:

0.20–0.30 mm from standard cavity boundaries
0.30–0.50 mm where machining tolerance is relatively high
Greater clearance where high-speed routing or thermal expansion is involved

For a 0.25 mm mechanical via located 0.20 mm from a cavity edge, even a small positional shift can reduce the remaining copper land between the drill and the machined wall.

A via should therefore be dimensioned against the actual cavity machining tolerance, not only the PCB CAD grid.

Identify IPC Cavity Types

Cavity Classifications

Cavity structures can be classified according to depth and the layers removed.

Cavity type	Typical structure	Main application
Surface cavity	Removes top dielectric/copper	Recessed components
Partial-depth cavity	Stops at internal layer	Package height reduction
Buried cavity	Internal recessed region	Embedded components
Through cavity	Cuts through PCB	Mechanical openings
RF cavity	Controlled pocket and reference structure	RF/microwave
Thermal cavity	Exposes copper or heat path	Power electronics

The classification should describe the physical construction rather than treating every milled opening as the same manufacturing process.

Controlled-Depth vs Through Routing

Feature	Controlled-depth cavity	Through cavity
Depth	0.30–2.00 mm typical	Full board thickness
Floor	Preserved PCB layer	No PCB floor
Z-axis control	Critical	Less critical
Tool depth	Precisely controlled	Profile controlled
Internal layer risk	High	Lower after complete removal
Component recessing	Excellent	Not applicable
Thermal interface	Excellent	Depends on construction

Controlled-depth machining is significantly more demanding because the manufacturer must remove a known thickness while preserving the electrical and mechanical function of the remaining layers.

HDI Integration

High-Density Interconnect PCB With Cavities

Cavities can be combined with HDI PCB technology when conventional surface area is insufficient.

A representative structure may use:

10 PCB layers
2 sequential HDI build-up layers
60/60 µm line/space
75 µm laser microvias
0.25 mm mechanical PTH
100 Ω differential pairs
0.80 mm cavity depth
1.60 mm overall PCB thickness

The cavity can create additional Z-axis packaging space while HDI provides the XY routing density.

This combination is useful for:

Fine-pitch BGA
RF modules
Camera electronics
High-speed processors
Compact power modules

Z-Axis Interconnection

Cavity structures also create new Z-axis relationships.

A component recessed into a cavity can connect to:

Surface pads
Microvias
Via-in-pad structures
Buried vias
Internal copper planes

A 75 µm microvia can connect a cavity-associated pad to an adjacent HDI layer while preserving routing density around the cavity.

The challenge is registration.

A cavity machined from one side and a microvia registered from another process must both reference the same layer geometry. Excessive cumulative tolerance can reduce the available landing-pad margin.

Cavity Design PCB Benefits

Profile Reduction

A 1.60 mm PCB with a 0.80 mm cavity can recess a package by approximately 0.80 mm relative to the surrounding surface.

For compact electronics, that reduction can determine whether the package fits under an enclosure wall.

The benefit becomes larger when several PCB layers and package interfaces are vertically constrained.

Thermal Management

A cavity can expose or approach an internal copper plane.

For example:

Internal copper: 35–70 µm
Thermal via: 0.20–0.30 mm
Copper thermal area: 5–20 mm²
Cavity depth: 0.50–1.00 mm

A thermally conductive interface can then connect a recessed package to an internal heat-spreading structure.

However, removing copper near a thermal region can reduce heat spreading. The thermal design must therefore define whether the cavity is intended to expose copper or isolate it.

Signal Integrity

A cavity changes local dielectric geometry.

If a 50 Ω microstrip normally uses a 100 µm dielectric spacing to its reference plane, machining away part of the dielectric can substantially alter impedance.

High-speed cavity designs should therefore evaluate:

Reference-plane distance
Local dielectric thickness
Dielectric constant
Trace width
Copper thickness
Cavity depth
Cavity wall proximity

A cavity should never be treated as electrically invisible.

Design and Fabrication Considerations

Tolerances and Planning

Cavity manufacturing involves several tolerance sources:

Lamination thickness
Copper thickness
Board bow and twist
Milling depth
Tool wear
XY positioning
Registration
Surface finish thickness

For a target cavity depth of 0.80 mm, a practical drawing might specify 0.80 ±0.05 mm when the manufacturing process supports that capability.

The tolerance should not be tighter than the verified production process.

If a design requires 0.80 ±0.02 mm, the manufacturer may need specialized depth-controlled machining, additional metrology, or tighter material-thickness control.

Tool Selection

Common cavity production methods include:

CNC mechanical milling
Controlled-depth routing
Laser machining
Sequential lamination construction
Combination mechanical and laser processing

Mechanical milling is commonly suited to larger cavities with straight or radiused walls.

Laser processing can create smaller or more localized structures but introduces its own considerations involving ablation, heat-affected regions, debris, and depth control.

The selected process should follow cavity dimensions, depth, material stackup, wall geometry, and required surface condition.

Standards

IPC Design Framework

Cavity PCB requirements should be controlled through the applicable PCB design, performance, acceptability, and fabrication documentation rather than relying on a generic cavity dimension.

Relevant IPC standards include:

IPC-2221C — Generic Standard on Printed Board Design
IPC-2222 — Sectional Design Standard for Rigid Organic Printed Boards
IPC-6012F — Qualification and Performance Specification for Rigid Printed Boards
IPC-A-600 — Acceptability of Printed Boards
IPC-TM-650 — Test Methods

IPC-2221 establishes general PCB design principles, while IPC-2222 addresses rigid organic printed-board construction. IPC-6012 addresses rigid-board qualification and performance.

The fabrication drawing should additionally define cavity-specific requirements that are not sufficiently described by a generic board standard.

Quality Control

Cavity Inspection

Cavity inspection should verify both depth and XY geometry.

A production inspection plan can include:

Cavity depth measurement
Cavity length and width
Wall position
Floor-layer integrity
Copper exposure
Internal-layer damage
Burr inspection
Surface roughness where specified
Board thickness
Via-to-cavity clearance
Electrical continuity
Controlled impedance where applicable

For high-density cavity PCB structures, cross-section analysis can verify whether the cavity stopped at the intended layer.

First-Article Control

For a new cavity design, the first article should establish:

Actual cavity depth.
Actual cavity wall position.
Remaining floor thickness.
Internal copper condition.
Via clearance.
Component fit.
Thermal interface.
Electrical performance.

A cavity depth that measures correctly at one location but varies by 0.10 mm across a large area can still create assembly problems.

Large cavities therefore benefit from multiple-point depth measurement rather than a single center-point measurement.

Early Collaboration

Design Before Fabrication

A Cavity PCB should be reviewed by the fabrication engineer before the final Gerber release.

The engineering review should confirm:

Stackup
Cavity layer
Cavity depth
Machining method
Tool diameter
Corner radius
Copper keepout
Via clearance
Component clearance
Impedance
Thermal structure
Inspection method

A 5.00 mm cavity corner cannot be machined with a 1.00 mm-radius cutter without producing a different internal geometry.

Tool diameter therefore belongs in the mechanical design discussion.

Real Factory Case

12-Layer HDI Cavity Board

A representative production case involved a 12-layer high-density interconnect PCB used for a compact processing module.

The construction included:

12 total copper layers
2 HDI sequential build-up layers
60/60 µm minimum line/space
75 µm laser microvias
0.25 mm mechanical PTH
100 Ω differential impedance
1.60 mm finished PCB thickness
0.70 mm controlled-depth cavity
8.00 × 12.00 mm cavity opening
35 µm internal copper planes

The cavity was designed to reduce package height while allowing the component thermal pad to interface with an internal copper heat-spreading structure.

The first engineering panel showed two production issues.

First, the cavity floor varied by approximately 0.08 mm across the machining area because the laminate thickness variation and machining depth were both included in the original tolerance stack.

Second, two nearby microvias were only 0.15 mm from the nominal cavity boundary. After actual machining tolerance was included, the remaining clearance was insufficient for the intended process window.

The production revision:

Changed the cavity depth tolerance from ±0.03 mm to ±0.05 mm.
Increased cavity-to-microvia clearance from 0.15 mm to 0.35 mm.
Added three cavity depth inspection points.
Moved the thermal copper boundary 0.25 mm away from the cavity wall.
Added a dedicated cavity machining layer to the fabrication package.

The revised panel produced a more consistent cavity floor and restored adequate process margin around the microvias without changing the component footprint.

The key manufacturing lesson is that the nominal CAD cavity dimension is only one part of the design. Material thickness, tool diameter, machining tolerance, registration, and internal copper position all contribute to the finished structure.

Common Design Errors

Production-Side Failures

The most common cavity PCB design errors include:

Defining the cavity only on the top copper layer.
Omitting cavity depth from fabrication drawings.
Using insufficient copper keepout.
Placing vias too close to cavity walls.
Ignoring milling-tool diameter.
Designing square internal corners that the selected tool cannot produce.
Assuming cavity depth is identical everywhere.
Routing high-speed signals through changed dielectric geometry without impedance analysis.
Using cavity dimensions tighter than the manufacturing process supports.
Failing to identify the cavity floor layer.
Ignoring laminate thickness tolerance.
Using one inspection point for a large cavity.
Treating thermal and electrical cavity requirements independently.

A cavity should be considered a controlled three-dimensional manufacturing feature rather than simply a hole that stops before the bottom layer.

Cavity PCB vs Conventional PCB

Parameter	Conventional Multilayer PCB	Cavity PCB
Surface profile	Flat	Local recessed areas
Machining depth	Usually full profile	Controlled depth
Z-axis packaging	Limited	Strong
Component recessing	No	Yes
Thermal interface	Surface based	Surface/internal possible
Manufacturing control	Standard	Depth + XY control
Internal-layer risk	Moderate	Higher near cavity
Design complexity	Moderate	High

The additional fabrication complexity is justified when the cavity produces measurable system-level value such as reduced Z-height, improved thermal transfer, or a more compact RF package.

FAQ

What Is a Cavity PCB?

Question: What is a Cavity PCB?

Answer: A Cavity PCB is a multilayer printed circuit board containing a controlled-depth recess that removes selected material while preserving the remaining PCB structure. Typical cavity depths range from approximately 0.30–2.00 mm, although the practical range depends on board thickness, material construction, machining process, and required floor thickness.

How Deep Can a PCB Cavity Be?

Question: How deep can a PCB cavity be designed?

Answer: Cavity depth depends on total PCB thickness and the required remaining floor. For a 1.60 mm board, a 0.50–0.80 mm cavity is a practical starting range for many applications. The final depth tolerance must be matched to the machining process. A requirement such as 0.80 ±0.02 mm should only be specified when the selected manufacturer has demonstrated that capability.

Can Vias Be Placed Near a Cavity?

Question: How close can vias be placed to a PCB cavity?

Answer: Vias can be placed near cavities, but the clearance must account for cavity positioning and machining tolerance. A practical starting value is 0.20–0.30 mm from a standard cavity boundary, with 0.30–0.50 mm providing greater production margin. HDI microvias may require different spacing depending on laser registration, pad diameter, cavity tolerance, and sequential-lamination construction.

Can a Cavity Improve High-Speed PCB Performance?

Question: Can a Cavity PCB improve signal integrity?

Answer: A cavity can improve signal integrity when it creates the required package geometry, controlled reference structure, or shorter electrical interconnection. However, cavity machining also changes dielectric thickness and local impedance. A 50 Ω or 100 Ω structure must therefore be analyzed using the actual cavity geometry rather than the flat-board stackup alone.