Conventional thru-hole vias--where and how to use them.
Examining the makeup and use of blind, buried, and microvias.
Organizing the vias in your PCB design.
Thru-hole and microvias in a 3D view of PCB routing
Circuit boards can contain thousands of traces, pads, and holes to conduct signals and power between component pins. As a circuit board layout designer, your job is to organize and design these elements to connect them correctly without allowing them to come into contact with other signal or power nets. To do this requires routing the traces through the circuit board design and transitioning them between layers with small holes known as vias.
While using a via would seem to be a straightforward operation, there can be many different types of vias in use on your design. Each of these vias may have different rules associated with them, and your job as a designer is to keep them all organized and apply the correct rules for each in the CAD system. Here is some more information on PCB via design rules and how you need to work with them to guarantee the performance and manufacturability of your circuit board.
Conventional Thru-Hole Vias: Where and How to Use Them
Since the first two-layer circuit boards went into mass production, the standard plated thru-hole via has become a staple in PCB design. These vias are drilled all the way through the board at whatever size is required, allowing traces or metal fills to connect to them on any of the board layers. Thru-hole vias are used for various purposes, including:
- Regular routing: Thru-hole vias are the standard method of transitioning a signal trace running on one board layer to another.
- Escape routing: Surface mount components usually need their pins to immediately connect to a via for routing on the internal layers of a multi-layer circuit board. These escape or fan-out vias are usually routed before the other traces in the design. Escape vias should be placed in a defined pattern to allow for the maximum amount of routing channels beneath them on the internal layers of the board.
- Power routing: Vias are also used to connect components to power or ground planes or traces. Most power vias are larger than regular routing vias to accommodate the greater current they are conducting.
Thru-hole vias are also used for special use or unique circumstances on a circuit board, including the following:
- Thermal vias: For components that run hot, a thru-hole via is often embedded in a large central ground pad to dissipate the heat through the ground planes of the board. These vias are essential in preventing a build-up of heat from causing component failures throughout the other parts on the circuit board.
- Stitching vias: These vias provide multiple connections for high-current circuits conducted by multiple power traces running on different layers of the board. Stitching vias will also help with the thermal dissipation of these circuits and lower the inductance of the connections.
- Fencing vias: When multiple ground vias are placed around the perimeter of sensitive circuitry, they will create a faraday cage effect. This style of routing will help to suppress potential EMI problems from affecting circuitry.
- Ground transfer vias: In high-speed designs, ground transfer vias are used to preserve the signal return path between multiple ground plane layers when the signal routing transitions between layers.
- Via-in-pad: Vias can be placed in the pads of dense surface mount components such as ball grid array (BGA) packages. This helps resolve spacing problems but can be difficult for fabricators when using a mechanical drill in a standard thru-hole via. Microvias are a better solution.
As with a plated thru-hole for axial leaded components, the thru-hole via requires a pad on every board layer that is large enough for the drill being used but small enough to not take up too much space. Thru-hole vias will also need a standard anti-pad on the plane layers of the board, sized appropriately for their drill diameter. The metal ring around a thru-hole via on the outer board layers is known as the annular ring. Annular rings are one of the main determiners of the reliability level of the board. A class 1 board allows the ring to be broken by the drilled hole, while class 2 requires the hole and the ring to be tangent. Class 3 boards have the highest reliability rating of all, and the annular ring must not be thinner than 5 mils at any point around the hole.
Another key design rule of thru-hole vias is choosing via sizes according to the aspect ratio of the drilled hole in relationship to the thickness of the board. Mechanical drills are limited in how deep they can be reliably drilled, and the aspect ratio determines that limit. Typically, circuit board fabrication shops prefer an aspect ratio of no more than 10:1, meaning that in a 62 mill thick board, the smallest size that can be reliably drilled is 6 mils.
If a thru-hole via connects a high-speed signal on the first two layers of a 12 layer board, the majority of the unused via barrel may act as an antenna and create signal integrity problems. To counter this, many fabricators will back drill the unused portion of the via. Back drilling requires specific instructions and data from the designer to indicate which vias barrels should be removed. However, back drilling does increase fabrication costs, and it is often better to use microvias or blind and buried vias to improve the performance of the board.
Lastly, thru-hole vias can be covered or filled if necessary, but like back drilling, this operation requires specific instructions for the fabricator from the PCB designer:
- Tented or covered: Solder mask is used to cover the via without actually filling it, but care must be taken to avoid creating air pockets in the barrel that can outgas when heated during soldering. Usually, a small hole is left in the center of the via tent to allow heated air to escape. Tenting helps the vias be closer to the surface mount land patterns without the solder flowing down the hole.
- Conductive fills: An epoxy resin combined with a metal substance such as gold, silver, or copper is used to fill the via. This fill helps increase the current capacity of the via and dissipate the heat, but it is expensive.
- Non-conductive fills: This fill protects the vias, eliminating the need for a surface finish, but otherwise does not help with heat dissipation or current capacity. Typically, this fill is done with solder mask or other similar materials.
Next, we’ll look at the PCB via design rules governing blind and buried vias in a circuit board.
A 3D view of vias and their routed traces in a CAD system
PCB Via Design Rules for Blind and Buried Vias
To help create more routing room on the circuit board, fabricators came up with a method of restricting the number of layers in a circuit board that a thru-hole via would penetrate. These vias are known as blind or buried, but designers need to be aware that they cost more to process than a standard thru-hole via.
A blind via starts on an outer layer of a circuit board and only penetrates partway through the layer stackup of the board. Blind vias have the same drill size limitations as thru-hole vias because they are mechanically drilled, but they allow additional routing channels below or above the via in the board layer stackup. This capability gives blind vias a definite advantage compared to thru-hole vias that are back drilled, as the thru-hole via won’t allow routing below or above it due to the barrel of the via.
Blind vias are built up sequentially, meaning that the layer pairs are drilled and plated before being bonded together. Blind vias are not cost-effective due to the extra steps necessary in the fabrication process to build them, but their use may be required for signal integrity or electrical performance reasons. PCB designers should exercise caution with blind vias and only use them when required and after working out the fabrication details with their manufacturer.
Buried vias are mechanically drilled vias just as blind vias are, but they start and stop on internal layers of the board without going to the surface. These vias are also very useful for printed circuit boards with dense routing, allowing for routing channels to be used both above and below the via. However, like blind vias, a buried via is also expensive, and unless their use allows a significant reduction in a board’s layer count, you are unlikely to realize a lower price by using them.
The better alternative to mechanically drilled blind and buried vias is to use a laser-drilled microvia.
A detailed view of the physical makeup of a microvia
De-Mystifying the Microvia in PCB Design
Microvias are those holes that are less than 6 mils in diameter and are usually drilled with a laser. These vias typically span only one layer due to their size but can be used on both external and internal circuit board layers. Microvias can be used in many scenarios that a thru-hole via can’t due to their small size, but those capabilities come at a much higher fabrication cost. Here are some of the other PCB via design rules associated with microvias that designers need to be aware of:
- Aspect ratio: Due to their small size, microvias are very difficult to plate down into the hole, and the best practice is to keep their diameter larger than their depth.
- Pad size: With their smaller hole diameter, PCB designers can use a much smaller pad size, down to 12 mils, giving them more routing channels.
- Filled: Microvias are also typically filled and plated, making them flush with other metal objects. This fill makes the microvia ideal for via-in-pad applications.
Microvias are versatile in how they can be used in PCB layout, making them essential for high-density designs. Without microvias placed in the small pads of high-density BGAs, these large pin-count processor and memory devices wouldn’t be able to be routed. Microvias can also be used in combination with other types of vias. Not only can microvias be stacked on each other, but they can be stacked with buried or blind vias as well.
Now that we’ve looked at the different types of vias available for PCB routing along with their design rules, let’s look at how a PCB designer can control these vias within their design.
The Edit Via List in Cadence Allegro’s PCB Editor
Organizing Vias in Your PCB Design
Before you can control the vias in your design, you first have to install the vias in your PCB CAD database. You can do this by either constructing the via object yourself or pulling it in from another source. Most CAD systems give you tools and features for building your vias, such as the padstack editor available in Cadence Allegro. Once the via is built, it can then be saved into your corporate libraries, where you can access it for future designs.
With the vias now built and available for use, you can choose which via to work with from a list as shown in the picture above. Tools like this visually show how the via is constructed, so you know exactly what you are working with. In Cadence Allegro’s Constraint Editor, you can then assign the appropriate vias to individual nets or net classes for routing the board. The PCB via design rules allow the designer to manage the different vias that will be used in the design without having to manually change vias for each new net. Once set up correctly, the design rules will automatically select the correct via for the net being routed, easing the designer’s workload.
For more information on PCB layout and design, take a look at this E-book from Cadence.
If you’re looking to learn more about how Cadence has the solution for you, talk to our team of experts.