HOPE Lab 1: Light-Sensor Schematic

In this KiCad activity, you will draw the schematic for a PCB of an LED light sensor. You may find our short write-up on KiCad schematics, the reading for this week, a helpful reference. We also recommend using a mouse for all labs as it will make navigation and component placement much easier.

Getting Started

  1. Launch KiCad. You should be greated with the main project manager window.

  2. Make a new project by File -> New -> Project or by using the keyboard shortcut Ctrl-N. Pick reasonable project name (i.e. light sensor) and a safe place to save your project directory (a folder will be created to house all your KiCad project files)

    You won't be able use KiCad (or any other PCB ECAD for that matter) as a comprehesive PCB ECAD unless you're working under the context of a project, so make sure to do this step!

Schematic Capture

Open the 'Schematic layout editor', aka the 'Eeschema' app, and replicate the KiCad schematic shown below:

Light sensor schematic
  1. The first thing we want to do in the schematic is add the components: resistors, op-amps, etc.

    Interested in why the op-amps come as these separate units of one part? Take a look at page 18 of the LMC6482's datasheet to get some idea of why the component would be set up this way.

Choose part search
  1. Continue by placing the following parts to match the completed reference schematic:

    • two capacitors ('C')

    • a LED part symbol ('LED')

    • a potentiometer part symbol ('R_POT')

    • a 1×3 connector part symbol ('CONN_01x03') - should be listed as generic

Go to Help -> List Hotkeys... or press Ctrl+F1 (Win) to open up KiCad's built-in keyboard shortcuts cheat sheet! Note that the middle mouse can be used to drag your view in both the schematic and layout editor. This will help alleviate the headache of trying to scroll around both.

  1. Wire up your components! Repeat until the schematic is fully captured.

    • Drag placed wires by hovering over them and pressing 'g'. Delete segments
      by pressing 'Backspace' or 'Del', or right click the wire for more options.

    • To create a wire that does not connect to a component on one end
      (floating wire), double click where you want the wire to end. Floating wires will be useful for components that will need power or ground labels later.

    • To add labels (the 'Vout' label shown above), press 'l' and type in the
      name of your label. Labels connect two or more nodes together without
      actually drawing the wire on screen. They are basically magic wire tunnels
      linked by name.

    • Note that these wires do not stay snapped to component pins. If you move or rotate a component, its seemingly connected wires will not follow.

Wiring components
  1. Now add power symbols to your schematic. For this step, it may be easier to duplicate a component instead of adding multiple of the same component. To do this, hover your cursor over the component you want copied and press 'c'.

  2. Assign component values to components. The easiest way to find this menu is to double-click the component. You can also find it in the 'Properties' section of the right-click menu. In the 'Text' field, type the appropriate value. Omit units (F for farads, H for Henries, etc.).

  3. Annotate your schematic (assign a unique and appropriate identifier to each component). You can do this in the same menu as above, or automatically by using Tools → Annotate Schematic → Annotate.

    Feel free to use these interface menus to learn more about KiCAD's functions, or even for this entire first lab. However, we do recommend learning how to use the keyboard shortcuts, as doing so will speed up your work in future projects considerably. Also, you'll look much cooler.

  1. Run the Electrical Rules Checker (ERC) and ensure there are no errors. If there are, fix the listed errors in your schematic and run the ERC again, until it is error free.


Show an instructor:

  1. completed, neat schematic
  2. ERC error free