Create the Hierarchical Sheets

Before reading further, you can watch the companion video that demonstrates how to create and structure a hierarchical schematic in KiCad. In it, I show how to set up a clear schematic hierarchy for the LattePanda Mu Carrier project, including how to name and organize each subsystem.

Introduction

In this guide, we will set up a multi-sheet schematic structure in KiCad for the LattePanda Mu Carrier board.
The hierarchical approach allows you to organize complex designs into logical and functional blocks, making your schematic easier to navigate, understand, and modify.

Rather than fitting the entire design into a single schematic sheet, which quickly becomes cluttered and error-prone, you will divide the project into smaller functional sub-circuits—each implemented in its own sheet.
This mirrors the method used in professional PCB design and directly follows the structure of the official LattePanda Mu Carrier reference design.

Benefits of Hierarchical Design

A multi-sheet schematic offers several advantages beyond simple organization. It improves collaboration when multiple engineers work on the same project, simplifies debugging and testing, and allows for reusable circuit modules that can be easily adapted to future designs.

Each hierarchical sheet focuses on a particular subsystem, such as power management, USB connectivity, Ethernet, GPIO headers, or fan control.
This approach also helps during the PCB layout stage, where each schematic sheet can correspond to a well-defined physical region on the board.

This modular organization mirrors how professional compute-module carrier boards are designed, allowing for clear separation of logic, power, and signal domains.

Creating the Root and Sub-Sheets in KiCad

Begin by opening your project’s schematic in KiCad.
The first step is to adjust the sheet size to A2, as the design requires substantial space for all the subsystems.
Open File → Page Settings, and under “Paper Size,” select A2. Update the issue date and revision number, marking this as Revision 1.

An offer from our sponsor

To create hierarchical sheets, use the Hierarchical Sheet Tool (or press S on your keyboard).
Draw a sheet box on your main schematic and name it according to the subsystem—for example, LattePanda_Module.
For the file name, use the same name as the sheet, but replace spaces with underscores (e.g., LattePanda_Module.kicad_sch).

Repeat this process for each subsystem listed above. The schematic hierarchy will automatically populate in the Hierarchy Navigator, showing each sub-sheet under the root schematic.

Adding Mounting Holes and Fiducials

In the root sheet, include four mounting holes to provide mechanical stability when the board is installed in an enclosure.
You can find these in the KiCad symbol library under “MountingHole.” Add a GND symbol to each one to ensure they are grounded.

Additionally, include two fiducials. Fiducials are small copper reference markers used by automated optical inspection (AOI) and pick-and-place machines to align the PCB during assembly.
Place these markers in opposite corners of the board for accurate camera calibration during manufacturing.

Annotation Strategy

Once the symbols are placed, use manual annotation for most of the schematic symbols rather than KiCad’s automatic annotation feature.
Manual annotation ensures that reference designators (like R1, C1, J1, etc.) remain consistent with those in the LattePanda reference design.
Maintaining alignment with the reference design makes debugging and comparison easier and avoids mismatched component numbering during schematic updates.

Final Check

After creating all sheets and symbols, verify that the hierarchy tree in KiCad shows each sub-sheet correctly linked to the root schematic.
Confirm that file names match the sheet names exactly and that all connections between the root and sub-sheets are properly represented.

At this point, your schematic project will have a solid structure ready for component placement and interconnection.
In the next step, we will begin implementing the sub-circuits, starting with the LattePanda Module sheet, which forms the foundation for the entire carrier board design.

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.