Estimated reading time: 6 minutes

Elementary, Mr. Watson: The Anatomy of Your PCB Component, Part 2

At the start of my series on the anatomy of a component, I noted that the component has two major divisions. The first is information that consists of name, description, parametric information, sourcing (part choices), and the datasheet (Figure 1). Next, the component comprises a symbol, PCB footprint, 3D model, and simulation models.

I then gave the example of the dissection of the frog, with the analogy that every part has a purpose. In the same way, each part of our component has a distinct purpose in our PCB design, including our models.

Schematic Symbol
The first model is the schematic symbol. As we all know, a schematic symbol is a pictogram representing various electrical and electronic devices or functions. A glance at some of the symbol's standards, such as IPC-2612-1, IEC 60617, or ANSI standard Y32, shows that it is a vast study area—fortunately, with industry-wide standards.

Simple vs. Complex Component Symbols
Most libraries I've seen consist of discrete and straightforward components. The schematic symbols used are only a few pins, simple representations, such as resistors, capacitors, inductors, transistors, and diodes. These types of simple symbols are created once and used multiple times. There are also complex symbols. These are the reverse: often single-use symbols tied to a specific component with hundreds or even thousands of connections. With such complexity comes the need for organization and best practices.

Schematic Symbol Best Practices
When constructing your schematic symbols, it's essential to have accuracy, consistency, and quality. But more importantly, remember that the symbols are the building blocks for everything else in your design. It is often said that if your schematic design were a novel, the symbols would be the words. This could not be more accurate. The quality and clarity of your schematic are based on the precision and structure of your symbols. Got a messed-up schematic? Most likely, you've got messed-up symbols. So, start with your end-objective in mind to have good schematic design practices and place those same principles in your symbols. Our goal is to have a clean schematic that is clear, understandable, and easy to follow. There is a certain quality to an exemplary schematic that always amazes me. When you can quickly identify the power, ground connections, and the flow of the circuit from left to right, top to bottom, there is uniqueness and beauty to reading a schematic like that of a fine novel.

Keep in mind how you want your final schematic to look. The same thoughtful steps should be put into your symbols. Many times, symbols are arbitrarily thrown together. One of the worst things I've seen is when someone copies the position of the pins on the component precisely as they are on the footprint. I know this may come as a shock to some, but the IC designers were not thinking of you as a PCB designer, the flow of the circuit, or the routing of the PCB when they laid out the silicon chip inside that IC. They were making the fastest route to get connections to the outside world.

Divide and Conquer
The first best practice is to divide and conquer your symbols. Learn in detail the breakdown of every component you use; for example, ATMEGA2560-16AU Atmel microcontroller with 256 KB in-system programmable flash, 8-bit. The datasheet classifies and shows the purpose of each pin. You see the organization of the 11 ports of 8-bits (except Port PG). Then have the reset circuit. You then have the connections to the crystal and the power and ground. When building this symbol, do not organize the pins of the component numerically. That may be the physical layout of the IC silicon die but not the electronic operations. Instead, order the pins based on their grouping and purpose. Doing so can easily make the required connections to the same ports, control lines, power, ground, etc. That allows more flexibility when creating your schematic.

Most EDA design software allows you to create various parts connected to a single component. It allows you to take components and break them into smaller, manageable pieces. Of course, we would do that on a large pin count component. Still, it should also happen with even small and low pin count components; when a component has the same functionality, you can easily separate and break it into manageable parts. This practice will open much more flexibility and help create a clear and readable schematic.

One of the most critical parts of your schematic symbol is the "pins." These will be where the connections are made for your circuits and ultimately into your PCB design. Pay attention to several details. Have a set standard and follow that standard. All components should have the same pin length and characteristics. It was drilled into me as a young PCB designer: grid, grid, grid, and that the layout of your schematic begins with the symbol. All pins should be on a 100-mil (25 mm) grid. One of the biggest mistakes new designers make is ignoring their grid settings. By keeping the symbol pins on a large grid, you then place those components on the grid and finish it by making the connections on the grid. That process assures that you make all connections. Many times, it is easy to miss an off-grid pin and connection. To the naked eye it looks fine, but you miss it, and don't realize it until your circuit doesn't work.

You should distinguish each pin with both a pin identifier and name. The name should include the full name according to the datasheet. Don't take shortcuts on the naming of your pins. With many complex components, pin identification gets rather elaborate. But identifying the pin by its "full name" helps the development, debugging, and troubleshooting process down the road. Of course, that does take more time to create your symbol, but the return on your investment is enormous.

Figure 4: Similar components can lead to problems unless they're identified by their full names.

A moment ago, I purposely said to use a pin identifier rather than a pin number. I have left the best for last, and it’s probably the most controversial. When we look at the footprint model, it is vital to have the symbol pin identifiers match the pins of the footprint. A common practice, especially with some components, is not to use numbers at all but rather pin identifiers, especially for components such as diodes, transistors, MOSFETs, etc.

Figure 5: In a footprint model, be sure your symbol pin identifiers match the pins of the footprint.

For example, with an ordinary diode, you identify the pins as anode (A) and cathode (K) or MOSFETs as gate (G), drain (D), and source (S). The transistor with base (B), collector (C) and emitter (E). Of course, having an alpha or numeric pin identifier has pros and cons. But I have used both systems and have seen that using alpha allows for more standardization of the footprints. We will take a deeper look into this with the footprint models.

John Watson, CID, is a customer success manager at Altium.

Download The Printed Circuit Designer’s Guide to… Design for Manufacturing. You can also view other titles in our full I-007eBooks library.