Layout – Board Outline and Import Components

Before reading further, you can watch the companion video where I demonstrate how to import all schematic components into the layout editor and define the rectangular board outline for the LattePanda Mu Carrier.

Introduction

With the schematic complete and the design rules configured, the next step is to move into the layout editor and begin defining the physical structure of the PCB.
In this stage, you will import all footprints from the schematic, create the board outline, and confirm that the overall mechanical design accommodates all major connectors, components, and mounting points.

An offer from our sponsor

For the LattePanda Mu Carrier, the design goal is to create a compact, rectangular board that balances functionality with manufacturability. The layout must allow easy access to external connectors, avoid mechanical conflicts, and provide adequate spacing for silkscreen labels, graphics, and mounting holes.

Planning the Board Dimensions

Before drawing the outline, it is essential to determine the target board size. The LattePanda Mu Carrier prototype was designed with the following practical considerations:

• Keep connectors as close as possible to the LattePanda Mu compute module’s interface connector to minimize trace length.
• Ensure connector accessibility so that USB, HDMI, and power plugs fit without interference.
• Maintain enough clearance between connectors to avoid mechanical strain or cable obstruction.
• Position the M.2 slots symmetrically on opposite sides of the LattePanda Mu module connector for structural balance and signal routing convenience.

These constraints resulted in a final prototype board size of 164.25 mm × 98.5 mm, providing sufficient space for all I/O connectors, mounting holes, and power circuitry while maintaining a manageable footprint.

Creating the Board Outline in KiCad

1. Open the PCB Layout Editor and select the Edge Cuts layer.
2. Use the Rectangle Graphic Tool to draw the outer boundary of the board.
3. Adjust the grid spacing (for example, 0.05 mm) for precise control when setting the board size.
4. Draw a rectangle with dimensions of approximately 164.25 mm by 98.5 mm.
5. Center the board outline using the origin (set by pressing the space bar) and the drag handles.

Once the rectangular shape is drawn, the board outline can be enhanced for aesthetics and manufacturability. KiCad provides built-in corner shaping tools to round or chamfer the board edges:

Rounded corners not only improve the board’s appearance but also reduce mechanical stress concentration during fabrication and assembly.

After adjusting the corners, lock the outline to prevent accidental modification during later stages of routing.

Setting Page and Revision Properties

Before importing components, open the Page Properties dialog.
Set the following project details:

• Page size: A4 (sufficient for compact boards)
• Revision: 2 (if the prototype version was Revision 1)
• Title and author fields: Update with project identifiers and revision notes

This ensures that all exported fabrication and documentation files carry correct metadata.

Importing Components from the Schematic

Once the outline and metadata are set, import the components from the schematic into the layout editor.
Use Tools → Update PCB from Schematic (F8) to synchronize the design.

If any schematic symbols are missing footprints, KiCad will display a warning list.
Copy the list of missing footprints and assign them manually in the schematic editor before re-importing.
It’s common for early versions of a design to lack footprint assignments for certain connectors, mounting holes, or passive components.

After successful import, all components appear in the layout workspace, typically grouped near the board origin and connected by thin ratnest lines that represent logical net connections.

You can temporarily hide these ratnests to focus on component organization and placement before beginning routing.

Preparing for Next Steps

At this stage, your layout environment should include:

• A correctly dimensioned and labeled board outline on the Edge Cuts layer
• All schematic components successfully imported and visible
• Properly set project metadata and revision number

The next phase will involve organizing and positioning these components logically—starting with large mechanical items such as connectors, M.2 sockets, and mounting holes—followed by power circuits and smaller supporting components.

This systematic approach establishes the physical foundation for a clean, manufacturable, and high-performance PCB layout.

By the end of this stage, you’ll have a complete board outline and component library import—the foundation for designing the full LattePanda Mu Carrier PCB layout.

Ready for the next tutorial in this series? Here's the next one, or choose an alternative from the list of articles in the side bar. There's also lots of interesting article in our Blog. where you can read about off-grid communication technologies, electronics test equipment, course updates, and much more.