Your First PCB in Flux: Complete Design Walkthrough

Get started with Flux by designing a complete PCB from start to finish in one streamlined tutorial.

Overview

This quick-start guide takes you through the full process of creating a PCB in Flux, step by step. In just one session, you'll design a drop-in replacement for the LM3671 buck-boost converter, covering project creation, schematic design, layout, routing, and export for manufacturing.

1. Project Setup

• Create Project: Open the Flux UI and create a new project.

• Identify & Describe: Rename your project at the top left and add a description to help other users and the Co-pilot AI understand the project's purpose.

• Set Permissions: Adjust permissions in the advanced menu for public viewing. To collaborate, add specific users and grant them "editing access."

• Reference Materials: Use the "C" shortcut to leave a comment on the canvas. You can paste links or embed images (like a reference schematic from a data sheet) using markdown for easy reference without switching tabs.

• AI Interaction: To interact with the AI within the design space, use the Co-pilot handle inside a comment to invoke it

2. Schematic Design

• Add Parts: Drag and drop parts from the Library (public or private) onto the canvas.

• Configure Passives: For generic components like capacitors, specify the footprint (e.g., 0603) and enter known values in the properties menu.

• Arrange Components: Use the bracket keys to rotate parts and use the alignment guides for a clean layout.

• Wiring/Tracing:

  • Click the dots (terminals) on components to start a trace.

  • Place Ground and Power terminals and rename them (e.g., VIN) to create electrical connections through portals.

  • Press "F" while tracing to change the trace elbow style.

3. PCB Layout & Setup

• Enter PCB Mode: Click the PCB tab at the top of the interface.

• Define Board Shape: Click on the layout object and enter dimensions in the toolbar (e.g., 0.4 x 0.6 inches).

• Add Corner Radii: Specify corner radius values (e.g., 0.1, 0.1, 0, 0) to round specific corners of the board.

• Layer Configuration: Change the stack-up from the default to a two-layer stack-up in the layout object properties. If the stack-up rule is not visible, manually add it to the layout object.

• Configure Design Rules: Create a "New Rule Set" to manage the visibility of designators and values. Set the "enabled" property to "false" and use an "important" flag to ensure these rules override default settings.

4. Component Placement & Routing

• Placement Strategy: Minimize airwire distance and crossovers. Follow heuristics like keeping decoupling capacitors near supply pins to reduce parasitic inductance and keeping high-frequency signals separated.

• Set Trace Widths:

  • Press "W" to cycle through active trace widths.

  • For specific power requirements (e.g., 1.2 amps), add a "Preferred Trace Widths" rule by going to the net container.

    • e.g. Include values for 200 micrometers (specifically to match the small pins of the BGA package), 10 mil, and 15 mil

• Routing & Vias:

  • Start routing by clicking touch points

  • To switch layers, right-click while routing to spawn a via at that exact location

5. Silk Screen & Aesthetics

• Add Logos: Create a "Silk Line" object in the layout and use an "Asset Rule" to link an uploaded SVG from the Asset Manager. Adjust the scale property (e.g., 0.001) as needed.

• Labels: Add text objects for pin labels and adjust font sizes through the properties menu.

• 3D Inspection: Use the 3D viewer to verify component placement and silk screen labels before finalizing.

6. Manufacturing Preparation & Export

• Copper Fills: Ensure copper fills are enabled (default). You can toggle their visibility for easier routing, but they must be on for export.

• BOM Enrichment (Object Search):

  • To update the Bill of Materials, use the object search to find specific components (e.g. search “10 Micro”)

  • Add Manufacturer Part Numbers (MPN) to components. You can bulk-update similar parts (like all 10µF capacitors) by right-clicking and using "Copy Special -> Properties" then pasting (Ctrl+V) onto other selected components.

• Export Files: Click the Flux logo and navigate to Export to download:

  1. Gerber files.

  2. Bill of Materials (BOM).

  3. Pick and Place (Centroid) file.

• Ordering: Upload these three files to your preferred manufacturer to complete the fabrication process.

Next Steps

If you’re ready for a more advanced, multidisciplinary challenge, dive into our "ON AIR" board series, a multi-part tutorial that evolves the concepts you just learned into a professional-grade design.

In this series, we build a Wi-Fi-connected sign featuring an ESP32, USB-C power, and digital intensity control. You will learn how to transition from simple circuits to complex system-level design by creating reusable modules and utilizing professional collaboration tools

To see our detailed breakdown of each stage, check out the in-depth sections (linked below):

• Project Setup: An introduction to the profile page and the different ways of reusing other user's work

• Schematic Design: How the schematic editor works and finding parts in the library

• PCB Layout & Routing: How the PCB editor works and best practices for component placement

• Export & Manufacturing: Getting your design ready for manufacturing and understanding required output files