How to Create an Effective Circuit Board Diagram

A PCB circuit board diagram/schematic diagram is an organized roadmap to build a circuit board. You can build your circuit diagram using various EDA tools such as Altium Designer, Cadence Allegro, KiCad, Pads, Tinycad, and Express PCB.

These layout design tools enable you to create flawless schematics by keeping an eye on logical and connection errors. As a designer, you must stick to a set of standard design rules to ensure the circuit is machine-readable.

Highlights:

• Auto-grouping is a method of organizing repetitive PCB design blocks
• Follow guidelines for net labeling, off-page connections, and signal flow representation to reduce visual complexity.
• DRC, netlist verification, and a comprehensive BOM enhance design accuracy.

Why do you need a circuit board diagram?

Figure 1: An example of circuit board diagram

A well-organized schematic clearly displays circuit connections. It will help you conceptualize the flow of signals, the interrelation of components, and the overall functionality of the circuit. This visual representation enhances the understanding of the system's architecture and facilitates informed decision-making during the design phase. Further, it can be a great tool to troubleshoot your circuit boards during repairs.

Cramming too much information into a schematic, even if it is technically correct, can sometimes cause confusion.

Guidelines for creating a PCB schematic diagram

Follow these standard schematic guidelines for a successful design.

1. Choose an appropriate page size

Design tools, by default, choose A4 (A3, A2…) page size. However, you can also select a different size based on your requirements.

2. Name the pages in alphabetical order

Name the logical blocks of the schematic using letters like A, B, C, and so on., to separate pages. This allows for orderly arrangement in alphabetical order, as illustrated in the example below:

• A_Block Diagram
• B_Power supply
• C_ MCU interface
• D_Memory interface
• E_ Revision history

This can also be a guide for other designers seeking to comprehend the circuit board diagram. Product-oriented organizations make such protocols and regulations mandatory.

3. Adopt a grid system for reference points

The adoption of a grid system is crucial to accurately establish circuit connections. It provides a guide for routing and component placement. This helps in analyzing specific nets or signal paths within the circuit, simplifying the debugging and verification processes.

4. Add a title block to the page footer

The page title block is a crucial element of the schematic, which is situated in the footer of the page. Add all essential details, including page size, update date, revision, document number, circuit name/function, and a company disclaimer. An example of a title block is provided below.

Figure 2: A page title block in the circuit board diagram

5. Incorporate essential notes/comments on separate sheets

Always include comments about the circuitry on separate sheets or directly on schematic pages. For complex designs, allocate a separate page for notes. Examples of such notes might contain jumper statuses, PCB layout constraints/guidelines, and any specific instructions. A schematic featuring these notes is depicted below.

Figure 3: Schematic with notes and comments

6. Add revision history on the initial/concluding page

The revision history contains alterations made to the design, offering details like the date, a description of the changes, the authors' and reviewers' names, and any accompanying review comments. Typically, the revision history is placed on either the initial or concluding page of the schematic. An illustrative example of a PCB schematic revision history is provided below.

Figure 4: Revision history of a schematic

7. Include the table of contents for the schematic document

The table of contents outlines the topics covered in the schematic document. It helps you quickly find the specific modules within your design. While it can be omitted for smaller and simpler designs, its inclusion proves valuable in larger projects. A sample table of contents is provided below.

Figure 5: Table of contents of a schematic document

8. Use a block diagram to depict design modules and signal flow

A block diagram helps you comprehend the objectives of a design. Here, various design modules and signal flow are clearly depicted. Block diagrams are not necessary for simpler designs but are mostly used for complex projects. Below is an illustration of a schematic block diagram.

Figure 6: Block diagram of a schematic

9. Depict signal flow path using a hierarchical schematic design

A hierarchical design is a must when the project is complex and has numerous modules. The signal flow from one module to another is clearly depicted in the hierarchical diagram, as seen below. Clicking on a module in the hierarchical schematic will take you to a comprehensive view of the chosen module.

Figure 7: Hierarchical schematic design for PCB

10. Use standard component reference designators

Standard reference designators provide a consistent naming convention. This helps you quickly identify components on a PCB. Typically, the IEEE standard is followed to assign designators.

The names of the common electronic components and their reference designators are displayed in the table below. Always designate a component with a capital letter.

11. Use standard library symbols for components

The schematic diagram contains various kinds of components. Transistors, diodes, logic gates, processor ICs, FPGAs, and op-amps are a few examples of active components.

Passive devices include parts like transformers, inductors, and capacitors. Create a new symbol only if that component is missing in the standard library.

Resistors

As seen here, there are two ways to represent resistors. Designers need to be careful to maintain the uniformity of the symbols they utilize.

Figure 8: Resistor symbols

The unit of resistance is Ohm, represented by the symbol 'Ω.' Occasionally, the symbol 'Ω' may be substituted with the letter 'E.' Always maintain consistent unit representation throughout the design. Input all required data about components into the design tool. This eases the creation of BOM for your design.

Polarized and non-polarized capacitors

Positive and negative terminals are found on capacitors. A mistake in placing capacitors can lead to an explosion.

The capacitor symbols from the IEEE standards are displayed in the graphic below.

Figure 9: Polarized and nonpolarized capacitors

Make sure that the pin numbers allocated to the symbols precisely correspond with the footprint arrangement.

Transistors

A semiconductor device with three terminals (emitter, collector, and base) is called a transistor. Always refer to the manufacturer’s datasheet when allocating pins in the layout footprint.

Always include a component description when the symbols are created. This will be helpful in the future when you have to replace the part. The BOM is easier to read when these details are included. The transistor symbol's description fields are fully filled in the two images below.

Figure 10: Transistor description

Figure 11: Component symbol description(Image credit: Altium)

Op-amp

It is crucial to build the op-amp symbol in accordance with IEEE guidelines. Many designers frequently draw the op-amp to suit their needs, which sometimes loses readability.

Figure 12: Op-amp symbol

Always have the input pins on the left and all of the output pins on the right when creating a symbol. Likewise, the top and bottom pins can be used for power and ground, respectively.

From the image above:

• Input: 2 and 3
• Output: 6
• Power and ground: 7 and 4, respectively

As a PCB designer, you should exercise caution when flipping or changing the symbol's orientation. It's likely that the positive and negative terminals will move positions when we do this. If the wiring isn't adjusted after flipping symbols, it can cause misalignments between the schematic and physical connections, risking incorrect functionality or circuit failure. Therefore, it is important to carefully compare each symbol with the datasheet provided by the manufacturer.

Heterogeneous schematic symbol

Heterogeneous components are complex devices such as FPGA, memory, and microprocessors. Numerous pin types, including data lines, inputs/outputs, address lines, control lines, and power lines, are present in these components. It is expected that manufacturers produce several UxA, UxB, UxC, and UxD components in one package in order to maintain readability and clarity.

Certain pins on components can serve multiple functions, and this versatility is typically indicated on the symbol itself, along with specific details presented outside the symbol. Consider pin AA5 shown below, which is designated for various purposes such as GPIO.6, CLKOK, PWM, or T3. Further, the external notes situated at the connection point indicate the current function of the pin – for instance, the notation "GPIO6" outside the symbol indicates its present function.

Below is an illustration of a heterogeneous schematic symbol for a component.

Figure 13: Heterogeneous schematic symbol of a component

--

Below are the ground pin and power symbols.

Figure 14: Power and ground symbols

Since there may be negative voltages on the board, it is usually a good idea to express voltages with a "+" sign. When representing the voltage levels and their respective sections inside the silicon, designers should adhere to a uniform and consistent convention. +3.3V_IO, +3.3V_DG, +3.3V_AN +1.8V_Core, +1.2V_LVCore, +2.5_Vref, etc. are a few examples.

In the same way, the board may have a variety of grounds. Below is a display of the symbols.

Figure 15: Different types of ground symbols

12. Minimize unnecessary net connections for improved clarity

Every junction formed by two wires sharing an electrical connection requires the presence of a junction dot. This is a common procedure in all circuit board schematic designs. However, most schematic design software applications omit the junction dot when a wire is directly connected to a pin or terminal on a component.

Figure 16: Net connection in a PCB schematic design

Net labeling conventions

The primary goal of a schematic is to enhance the circuit's clarity. Minimize unnecessary net connections, a common occurrence when representing an integrated circuit (IC) symbol on a schematic.

Instead of cluttering the diagram with numerous interconnecting lines, designers assign a net name to a specific pin, linking it to a corresponding pin on another device. Further, understand that connecting pins with the same name reduces the visual complexity of the schematic and improves readability. This strategy is particularly useful when the net is connected to three or more locations.

The image below illustrates a series of named nets.

Figure 17: Net labeling convention

Guidelines for net labeling

When nets are directly connected on the same page to another IC, net naming is unnecessary. You can adhere to these straightforward rules when labeling nets.

• Signal names should be in uppercase and positioned just above the net.
• Opt for concise names, ideally with a maximum of 4 letters.
• Indicate active low or high signals using an upper bar. A pin with an upper bar is interpreted as an active low pin.
• Remove open nets or unconnected connections.

Off-page connections

For improved readability, designers typically name nets in the schematic. While this is effective for connections on the same page, when a net needs to link to a pin on a different page, the use of an off-page connector symbol becomes necessary.

Signal flow representations

On a schematic page, the signal flow is typically from the left to the right side. The power and ground connections will be placed on the top or bottom side of the page. You should adhere to this convention and position components accordingly.

13. Ensure legibility when illustrating component placements

Efficient component placement in a schematic is essential as it guides the layout engineer in placing the components suitably. The schematic on the left illustrates a parallel connection of capacitors, and it's evident that the readability is not optimal.

Figure 18: Parallel connection of capacitors in a schematic

Enhancing the connection, as illustrated below, achieves improved readability.

Figure 19: Preferred parallel connection of capacitors in a PCB schematic

14. Place components linked to the crystal in close proximity

The PCB circuit board diagram typically features crystal placement, as illustrated below. Position components connected to the crystal in close proximity due to the potential for high-frequency signals. In general, if the design requires two components to be placed in close proximity, they should be depicted accordingly (e.g., shunt and series terminations).

Figure 20: Crystal placement in a schematic

15. Utilize DRC to evaluate the logical and physical integrity of the design

CAD software embeds an intelligent feature known as Design Rule Check, which assesses both the logical and physical integrity of a design. This entails ongoing checks against all enabled design rules as the design progresses.

16. Verify the nets manually to mitigate design errors

Upon completing the schematic design, the system generates a netlist, which is ready for import into the layout. The .net is the most common file extension for netlist. Further, to mitigate design errors, it is advisable to manually verify the nets.

17. Import components from the library to generate a complete BOM

CAD system currently offers a crucial capability in the form of BOM generation. As a result, designers generate or import components from the library, providing all the necessary inputs in the tools to generate a complete and sufficient BOM. Further, enter the Manufacturing Part Number (MPN), packaging, vendor name, vendor part number, and other information into the BOM. As a recommended practice, provide all essential data during the creation of the symbol.

Checklist for an error-free schematic

• Pin numbering and labels: Verify pin numbering and labels for each component in accordance with the datasheets.
• Polarity check: Conduct a polarity check for all polarized components.
• Avoid overlapping labels and pin numbers: Check for any overlapping labels and pin numbers that may cause confusion.
• Transistor pin verification: Validate the base, collector, and emitter pins of all transistors against the datasheet, schematic symbol, and footprint package.
• Component details: Verify the component's value, reference designators, and correct location.
• Schematic symbol descriptions: Ensure that schematic symbol descriptions are present, including details like Manufacturing Part Number (MPN), vendor name, vendor part number, etc.
• Off-page connectors: Check for the presence and accuracy of off-page connectors, especially when connecting to components on different pages.
• Inter-sheet references: Look for inter-sheet references to guarantee seamless connectivity across different schematic pages.
• Decoupling capacitor checks: Perform decoupling capacitor checks for all ICs, considering ground pin separation based on signal types (analog, digital, signal, ground).
• BOM verification: Conduct checks on the bill of materials to ensure accuracy in quantity, part numbers, and, essentially, package types.

By rigorously conducting these checks, you can significantly enhance the reliability and accuracy of the schematic design. Please let us know in the comments section if you require any assistance in creating your circuit diagram.

If you have any further inquiries or if you require additional information regarding schematics, feel free to let us know in the comments.