How to Implement PCB Design Step by Step Using Eagle

Circuit design is the foundation of electronic engineering, determining circuit performance and functionality. That’s why designers search for PCB design guides to enhance this process. Additionally, choosing design software that suits your project and mastering its use before you start designing is equally crucial. Among the many options, Eagle is a good choice. In this TechSparks article, we’ll briefly introduce you to this software and provide Eagle tutorials to help you with custom PCB design step by step. Let’s get started!

Advanced Reading: Best PCB Design Software List

Step 1: Get to know Eagle Software

Eagle, developed by Autodesk, is a PCB design layout software highly favored by engineers, designers, and students. It offers users a user-friendly layout interface and powerful hardware capabilities, making it widely applicable in various fields, including electronics, telecommunications, and aviation, for creating diverse circuit designs. Eagle PCB comprises the following four basic views:

  • Library View: This view serves as a component information repository containing various types of pre-designed parts. It acts as a starting point for design projects, allowing designers to easily access and incorporate components. Eagle comes with some built-in standard libraries for direct use, and it also supports user customization of components, packages, and other details.
  • Schematic View: Designers can drag and drop components from the library view and arrange them on the schematic canvas to build the entire circuit. This schematic provides a visual representation of the logical structure to help designers understand circuit functionality and perform error checking. Additionally, Eagle software offers annotation features for adding textual labels to highlight important notes.
  • Layout View: Once the schematic design is completed and verified for accuracy, it transitions to PCB layout design. Components configured in the schematic are associated with physical packages during this process. Designers need to consider critical parameters like assembly, heat dissipation, signal transmission, etc., to ensure that the routing does not interfere with the normal operation of the circuit. One advantage of using Eagle for layout design is its automatic routing feature, which reduces design time.
  • Control Panel View: This is the central command center of Eagle software, providing various tools and settings to help designers manage and control various aspects of the design. Here, you can configure design rules, perform multi-layer layout, and generate manufacturing output. Eagle’s highly customizable control panel makes it more user-friendly.

Step 2: Create New File

In this tutorial, TechSparks will use Eagle to create a circuit board to support a virtual ground circuit, ensuring the reliability and safety of the entire electronic system.

virtual ground circuit

At the beginning of the project, you need to create a new file. Launch the software and locate the ‘File’ button in the top menu bar. From the dropdown options, select ‘New’ and ‘Schematic’ to create a new project.

You need to add a frame to this view to define the print boundary and display file information. As shown in the image below, in the sidebar of the design software, find ‘ADD’ and use Eagle’s default component library.

Eagle ADD button

In the dropdown options for ‘Frame,’ locate ‘FRAME_A_L,’ double-click it, and the frame will move with the mouse cursor. Click in the workspace to place it. If you need multiple frames, repeat the process, and you can quickly complete it by pressing the ‘ESC’ key on the keyboard.

Select frame type

Finally, go back to the software’s top menu and find ‘Save As…’ in the ‘File’ dropdown options to name and save your project. This process is very straightforward, much like creating ‘Word’ or ‘Excel’ documents.

Step 3: Design Schematic

Add Components

The purpose here is to add the components your circuit requires to the schematic. You should add whatever your circuit needs. In this example, you need two resistors, one capacitor, and one operational amplifier. Specific steps: “ADD” Button → Find Component → Double-Click.

Place components on Eagle schematic

Adjust Component Position

Components are added to the schematic in symbolic form, and at this stage, they are placed randomly without any connections between them. In the case of a simple circuit like this, where you have a small number of components, it’s manageable. However, in real-world scenarios with numerous components, you should have a layout in mind to position the components logically and prevent crossovers when connecting them.

Cluttered components in schematics

In the Eagle layout software, you can use the left mouse button to drag components and the right mouse button to rotate them. Specific steps: Select the component → Rotate to the specified direction → Drag to the target location → Left-click to place → Repeat the operation.

Change component position

In the illustration, there’s an extra IC1 and a missing operational amplifier. To correct this, select IC1 and press “DELETE” to remove it. When dealing with a large number of components, finding the right one can be challenging. If you know the manufacturer, series, or model of the component you’re looking for, you can quickly search for it using Eagle’s component search function. For example, in the search bar, you can type “741” and then press “Enter.”

Eagle’s component search function

Wiring of Schematic

Now, you need to connect the components in the schematic to form a complete circuit diagram. To do this, find the “NET” button in the toolbar on the left side of Eagle. Specific steps: Use “NET” → Left-click on one end of a symbol → Click again on another symbol → Repeat this process. During the component connection, you can right-click to change the style of the connecting lines.

Connect schematic components

In large and complex circuits, you can make the logical structure and connections clearer by naming and labeling different nets. You can use Eagle’s “NAME” and “LABEL” commands to achieve this. Specific steps: Use “NAME” → Change the name → When renaming, a confirmation pop-up will appear if the name is already in use. Click “Yes” to confirm → Use “LABEL” → Left-click to display.

Component naming

To ensure that essential connections are accessible from outside the PCB for power and other circuit connections, you’ll need to add through-hole pads in the schematic and connect them to nodes using the “NET” command.

Add through-hole pads

Mark Value

The importance of component values for circuit performance is evident, but components are not initially labeled. Therefore, you need to manually mark the values of each component for better understanding and future maintenance. In Eagle, you can use the following commands to achieve this:

  • “VALUE”: Used to mark the value of a specified component.
  • “SMASH”: Allows you to move the component’s name and value while keeping them connected.
  • “REPLACE”: Permits the exchange of equivalent components without deleting the original schematic components.

Mark component values in Eagle

Detect and Convert

After completing the schematic design, use the “ERC” command to check the circuit. This is a tool or function used to inspect the schematic for electrical rule errors or issues. If any problems are detected, a warning window will pop up. Once you’ve confirmed the design is correct, click on the “BOARD” in the toolbar to switch to the PCB window. When prompted to create the board, click “Yes.”

Schematic to PCB

Step 4: PCB Layout


People who are not familiar with circuits might confuse or not fully understand the concepts of a schematic diagram and PCB layout. Let’s provide a simple explanation:

A schematic diagram represents the logical representation of an electronic design, displaying the various components in the circuit and how they are connected.

PCB layout, on the other hand, pertains to the placement of components on the PCB, the paths of connecting lines, and the spacing and arrangement of components.

Converted design drawing

Component Placement

The layout view shown in the above image represents the initial configuration after the switch. It is located in the bottom-left corner of the board. To simplify operations, move it to the center of the outline frame. There’s no need to worry about disarray during the relocation, as the connections are already in place. Furthermore, you can use the “RATSNEST” feature to tidy up and reestablish connections via the shortest routes between components. The result is illustrated in the following image.

Eagle Component Placement

Routing Traces

Traces are the conductive copper pathways on a PCB that establish connections between various components. The process of placing traces on the board closely resembles using the “NET “command in the schematic. To begin, select the “ROUTE” command and left-click on a component pad. Components that share the same node will be highlighted, and the trace will take the place of the previous airwire as it’s set in place. To change the direction of the trace, simply left-click in an empty area to end a segment, and then proceed by routing in a different direction. When you need to finish a trace, left-click on another pad connected to the same node.

If you wish to adjust the routing style, right-click to modify the route’s bend style. By default, for through-hole components, the bottom layer serves as the trace layer. You can switch this to the top layer with a center-click or through the drop-down menu. However, for this board, it’s recommended to keep all traces on the bottom layer. If there’s an unwanted or incorrect trace, you can easily remove it using the “RIPUP” command. Follow the routing process as depicted. We’ve intentionally left one connection incomplete to illustrate how nodes are highlighted when you’re placing a trace.

Eagle Routing Traces

Adjust and Confirm

Select the “GROUP” command and left-click and drag a box around all of the components. Select MOVE, right-click on any component and select MOVE: GROUP. Move the entire group to the bottom left corner of the outline box.

Employ “SMASH” and “MOVE” commands to reposition the values associated with R1, R2, and U1 outside of their respective component outlines. This adjustment ensures these values remain visible even after the components are soldered onto the board.

Modify the dimensions of the outline box by using the MOVE command on the corners or by right-clicking on a segment. Opt for the “Properties” option and adjust the “To” and “From” coordinates. It’s advisable to size the box just slightly larger than the space occupied by the components. A box size of 1.5″ by 1.5″ is often suitable.

Select the Properties button and adjust

To confirm the manufacturability of the board layout, run a design rule check (DRC). Select DRC and load the “default.dru” file, then click on “Check.”

Keep in mind that DRC tolerances, such as minimum trace width and clearance between traces and components, can vary between manufacturers. Using the default DRC may result in numerous errors. If the DRC specifies a minimum clearance of 12 mils, but the manufacturer can work with clearances as narrow as 8 mils, you can either disregard these DRC errors or adjust the DRC clearance parameters accordingly.

DRC detection PCB design

Step 5: Generate Gerber

To bridge the gap between theory and the final product, you must generate manufacturing files, with Gerber files being a universal standard that encompasses various details like components, traces, and solder pads. You can directly create Gerber files using Eagle. Specific steps: Select “File” → “Open” → “Job” and open the “” file.

It’s important to note that Eagle does not offer a built-in feature for viewing Gerber files. Therefore, you may need to utilize third-party software for this purpose.

Related Articles:

KiCad PCB Design Step-by-Step Tutorial for Beginners

How to Design PCB in Altium

You Might Be Interested

A Comprehensive Guide to PCB Reverse Engineering
PCB Reverse Engineering Guide

PCB reverse engineering, also known as cloning or copy, is essentially the process of extracting the original information from electronic products’ circuit boards through various

what is design rule check
What is Design Rule Check in PCB Projects?

Discover the crucial role of Design Rule Check (DRC) tools in modern PCB design with our comprehensive guide. Learn how DRC ensures precision, enhances production quality, and prevents costly errors, helping you deliver top-notch products. Optimize your design process and meet advanced manufacturing standards effortlessly!

pcb for iot
Everything You Want to Know About PCB in the IoT

Designing IoT PCBs comes with challenges such as ensuring high-speed data transmission, compact layouts, and energy efficiency. Leveraging advanced technologies like flexible and HDI PCBs helps meet these demands, enabling reliable and efficient IoT devices.

What is Microvia in PCB?

Microvias are small holes in PCBs facilitating high-density interconnections. Their reliability is challenged by complex thermo-mechanical environments, requiring careful design and manufacturing. Techniques like mechanical and laser processing are used to create them, advancing PCB technology.

tented vias
Tented Vias in PCB

The article emphasizes the significance of tenting PCB vias to shield them from external factors, enhancing signal integrity and assembly processes, particularly in high-speed and SMT applications. It discusses design considerations and manufacturing techniques involving materials like solder resist ink and dry film.

buried via hole
What Are Buried Vias in PCB and Their Purpose

Buried vias enhance signal efficiency in multilayer PCBs, crucial for high-density interconnects. Despite added costs, they play a vital role in advanced electronic devices, optimizing circuit performance. Designed for multilayer PCBs, they address the demand for high circuit density in various applications. Manufacturing involves intricate processes like laser drilling and precise layer stacking.

Scroll to Top