How to Design Embedded Cavities Into Your PCB

Sometimes, when you look at a PCB, you will see a board with an interesting shape or some cutouts visible along the board edge. What if you could only cut material from specific layers in the interior of the board? This would enable inset components or complete embedding of components in a PCB.

If you plan to include these kinds of cavity structures in a PCB, they need to be specified correctly such that cavities can be fabricated without defects or damage to other features in the PCB. This guide outlines how cavities are used and specified in rigid PCBs, as well as how deliverables can be formatted to include cavity specifications.

Why Are Embedded Cavities Used?

There are several reasons an embedded cavity might be used in a PCBA. Some ideas include embedding components internally in the PCB, inset components on the top/bottom layers, embedding heat sinks for high-power components, and unique applications in RF design. If you want to use an embedded cavity in your PCB, then there are certain design standards to follow, as well as industry standards that define DFM requirements.

IPC Standards for Embedded Cavities

Like most other aspects of PCB design and manufacturing, there are IPC standards that apply to embedded cavities placed in a PCB. The relevant standard describing fabrication of cavities in a PCB is the IPC-6012F standard. There are three types of cavities specified in this standard:

• Type 1: A cavity with no metalization on the wall or floors
• Type 2: A cavity with some metalization on either the wall or floors (not both)
• Type 3: A cavity with metalization on the floor and walls

Metalization is applied selectively by etching the lower/upper layers, which allows formation of mounting pads for embedded components. If plating along the wall is needed (Type 2 or Type 3), then the manufacturer will need to have wall plating specified and the plating will be applied in a standard process. If the entire cavity will be filled with metal (copper coin), then a Type 3 cavity will need to be specified in the final manufacturing deliverables (see below).

How to Specify Embedded Cavities for a PCB

When specifying an embedded cavity for a PCB, the intended location, shape, and type of cavity need to be specified in three sets of files:

• In the native design files in a mechanical layer
• In the Gerbers/ODB++ files
• In the fabrication drawing

PCB Layout Files and Fab Files

An embedded cavity outline can be drawn in a mechanical layer. It’s best to use arcs to draw out the cavity just to illustrate the intended shape of the cavity (see below). Because the actual cavity outline does not sit in a signal layer, it

Type 1 and Type 2 cavities: After placing the outline, you can create a keepout in the upper and lower copper layers with the same shape as your cavity. For Type 2 cavities, this of course assumes that the cavity will not be plated on the floor of the cavity. Next, create a clearance rule between the keepout and copper on the upper and lower layers; the clearance should be the same as what would be used along the board edge (typically at least 8-10 mils).

Type 3 cavities: For these cavities, a keepout is not needed on the upper and lower layes; the layers that form the floor and ceiling of the cavity can be etched as normal.

Once these features are placed in the PCB layout, the mechanical layer containing the cavity outline should be included in the Gerber/ODB++ export. The mechanical layer can also be exported as a DXF for use in a fabrication drawing or layer prints.

Fabrication Drawing

The fabrication drawing should show the routing path, tooling parameters (drill diameter), and finished cavity outline. Fabrication drawings should include fabrication notes, so make sure to specify the IPC-6012F cavity type in your fabrication notes. You can include a note similar to the following:

Replace X, Y, and Z with the top/bottom layers and the cavity type respectively. This is similar to the kind of fabrication note that would be included to specify board cutouts.

During an initial review of the PCB before fabrication, the CAM team at the fabrication house will need to check the placement of the embedded cavity and the presence of topper against the cavity Type defined in IPC-6012F. Make sure your design documentation is consistent across your mechanical layers in your Gerbers/ODB++ package, your fabrication drawing, and your native design files.

Whether you want to place a board cutout or an embedded cavity in your PCB layout, you can implement these best practices into your designs with the complete set of CAD tools in OrCAD from Cadence. Only Cadence offers a comprehensive set of circuit, IC, and PCB design tools for any application and any level of complexity.

Subscribe to our newsletter for the latest updates. If you’re looking to learn more about how Cadence has the solution for you, talk to our team of experts.