PCB Technologies: PCB Design Tutorial

 A printed circuit board (PCB) serves as the foundational structure for assembling and connecting components in electronic devices. It encompasses mechanical, electrical, and occasionally thermal elements, making it a crucial element in most products. This technology, originating from the era of linking vacuum tubes, has evolved into a contemporary and cost-effective method for constructing electronic systems that demand electrical interconnections between components. Despite its historical roots, PCBs continue to play a central role in modern electronic hardware, facilitating the interconnection of the latest high-performance integrated circuits. In essence, circuit boards form the core of electronic hardware products.


Due to historical conventions, the term used for an unpopulated circuit board, devoid of any components, is either a printed circuit board (PCB) or a printed wiring board (PWB). Once components are affixed to it, the assembly is then termed a printed circuit assembly (PCA). The illustration below provides examples of both PCBs and PCAs showing the distinction between the terms printed circuit boards and printed circuit assemblies. 


PCB Physical Design

A printed circuit board (PCB) is constructed by layering conductors made of copper foil and dielectric materials. The number of layers in a PCB is determined by the count of metal layers, irrespective of their specific functions. The simplest PCB consists of one conductor layer on a dielectric substrate, while a more common configuration includes two layers.

The progression of board layers typically occurs in increments of two layers. The subsequent stack-up involves a 4-layer board, followed by a 6-layer board, and so forth. This pattern stems from the manufacturing process, where pairs of layers are laminated together to create multilayer boards.

Each dielectric layer is crafted from a glass weave yarn saturated with an epoxy dielectric, essentially forming a structure similar to fiberglass. The prevalent dielectric material used is known as FR-4 which is notation for Fire Retardant style #4

The image depicted below illustrates a sliced view of a signal line, copper planes, and the fiberglass dielectric situated between them. Although the illustration features three metal layers, it is important to note that this represents only a portion of the complete board stack-up. Additional metal layers are present above these layers in the stack.

PCB Physical Design

Vias Technologies

Using various layers for signals, power, and ground in a circuit board necessitates the establishment of electrical connections between these layers through vias. Vias are categorized into three common types based on their manufacturing process and the connections they facilitate. The diagram below provides visual representations of these three via types.


visual representations of via types
The most prevalent type of via used in circuit boards is the through-hole or plated through-hole (PTH) via. If there's a need to prevent a specific layer from connecting to the PTH via, a clearance hole can be added on that layer where the drill passes through. In most routing tools, this is automatically handled based on net names, and the clearance hole in the plane layer is sometimes called an antipad.

When connecting two inner layers, like two ground planes, using a through-hole via, it's essential to ensure there are no traces on the top or bottom layers where the drill passes through the board. This configuration results in a through-hole via that exclusively connects the inner layers.

The protruding portion of the plated through-hole barrel that extends beyond the last connected layer is termed a stub. In high-frequency boards with signals operating above 10 Gbps, via stubs can pose a significant signal integrity issue. However, for boards operating at 5 Gbps and below, via stubs are seldom a performance concern and can be disregarded.

The text refers to a 4-layer board constructed with through-hole vias, and an illustrative example is provided in the accompanying figure below.

 In this illustration, all the Plated Through Hole (PTH) vias drilled in the circuit board penetrate completely through the board. The specifications and measurements of the PTH are integral to the design of the via pad stack. Unless there is a compelling reason to deviate, the features should adhere to the following criteria:

  • Drill diameter: 13 mils (resulting in a finished, plated hole diameter of 10.2 mils).
  • Capture pad diameter surrounding the via on any layer with a connection: 25 mils (comprising a 6 mil copper annulus around the 13 mil drill diameter).
  • Clearance annulus on a copper plane with no connection: 6 mils.

During the process of plating the via holes, it is necessary to have capture pads on both the top and bottom layers of the via hole. The purpose of the capture pad is to provide a larger target for the drill, compensating for registration tolerances. On layers where there are no connections to be established through the via, the inclusion of a capture pad is unnecessary. Removing these non-functional capture pads is considered a good practice.

For cost-effectiveness, the annulus of the capture should not be narrower than 6 mils. Consequently, the outer diameter of the capture pad is calculated as 13 mils (drill diameter) + 6 mils (clearance annulus) + 6 mils (capture annulus) = 25 mils.

The narrowest clearance between copper features in this scenario is 6 mils, and the closest spacing between vias is 31 mils. A recommended via-to-via pitch is 35 mils, leaving 10 mils as the spacing between the edges of the via pads. A buried via typically connects only between two adjacent layers and is drilled and plated when the 2-layer core is patterned, adding to the overall board cost. The advantage of a buried via is that it doesn't obstruct routing channels above and below it, which can be beneficial in very dense boards.

However, most low-cost fabrication shops, like JLCpcb.com, do not offer buried vias. On the other hand, a blind via is drilled from the top of the board to a controlled depth during the same process as through-hole vias. This creates a small, blind hole from the top or bottom of the board, stopping on a lower layer. Plating the inside of the hole is challenging, especially if the aspect ratio is greater than 1 to 1, requiring special chemistry to address air bubbles and ensure proper plating fluid contact.

The value of a blind via lies in its ability to be placed inside a pad, providing a low inductance contact to the layer below without blocking routing channels on other layers. Unlike through-hole vias in pads, blind vias do not compromise solder joint quality during automated assembly. Blind vias are commonly used for via-in-pad applications, particularly for decoupling capacitors where low loop inductance connections are crucial. They don't wick solder from a pad and thus do not pose assembly problems, making them suitable for via-in-pad connections.

However, via-in-pad is not an option for many low-cost fabrication shops due to the need for specialized plating chemistry and drilling processes.

 See next:

Post a Comment

Previous Post Next Post