USB Charger: Footprint Creation and Board Setup

Introduction

With your completed schematic from last week's lab, you can start the design of the physical board!

This week, you will prepare your component footprints and prepare the board layout for part placement and routing.

Footprint Creation

Before starting a board layout, there must be component footprints that can be associated with your schematic. To get checked off for this lab, we would like to see a project library filled with:

Make some footprints for your parts!

For the components you create, we recommend adding the parts to a project library, just like for your schematic symbols.

Note: Do NOT add standard passives to your library (i.e. external capacitors, resistors for ICs). DO add the passive if it has a special shape (i.e., a high wattage resistor).

Something to think about: Why might, in a collaborative environment, using project libraries instead of global libraries be a good idea?

  1. Open up your footprint editor from the KiCad home window:
  1. Create a new footprint Library by doing File → New Library. Make sure to select "Project" in the library table window.

Note how the footprint library is saved. A folder with a custom extension!

  1. Create a new footprint for one of the parts you have chosen and add it to the footprint library you had just created (KiCad will prompt you if you try saving).

We suggest that you try to use the footprint generator ("Create Footprint...") for 1 part, just to know it exists. Make sure to double check the footprint it creates though!

  1. The process for creating footprints is broken down as so:
    1. Place and dimension component pads
    2. Draw important silkscreen
    3. Draw component courtyard region
    4. Anything else: assembly data, 3D model

You should have the component's datasheet open to the page on its physical dimensions for whatever component package you have chosen to use before starting.
We highly suggest watching Digikey's Footprint Creation Tutorial. Start from 5:51. Parts 5 and 6 of the intro to KiCad series are also recommended watches for this lab. (And the entire series is a good walkthrough of the KiCad/PCB design process. Note however, that the video tutorial was made using an older version of KiCad, and thus certain features have been changed since then.)

We do not recommend remaking standard packages that already exist in the default footprint libraries generally, but you should do it this lab for practice.

Use pre-existing parts!

In addition to creating footprints yourself from component datasheets, you may also find component footprints (as well as symbols, or even entire part libraries such as the Digikey KiCad component library) online. There are a multitude of tools at your disposal: feel free to use any of them but make sure to always double check any footprint found online.

How to import KiCad footprints

  1. Download the footprints (must be for KiCad v4+) and uncompress them if needed.
  2. File → Import Footprint from KiCad File. Select the .kicad_mod footprint file that you would like to use.
  3. Double check the imported footprint.
  4. Save the footprint to your project footprint library.

How to import KiCad footprint libraries

You shouldn't need to do this for this lab, but you might as well know.

  1. File → Add Library (its like, the "New Library" symbol but with a plus + sign)
  2. Select the footprint library folder.
  3. Add the library either to the Project or Global library table.
  4. Money

Board Layout Setup

Now that you have your component footprints, it is time to associate your schematic symbols with those footprints then move on to getting all those parts into the layout editor!

Assigning Footprints to Schematic Symbols

These instructions were pulled straight from the introduction lab! Just be sure to associate the symbols to footprints from your just-created project footprint library.

  1. Go to "Tools → Assign Footprints". Note that it may take a while to open.
  1. Pick the first unassigned footprint from A. If you want to assign multiple components with the same footprint, select multiple components using SHIFT-select.

  2. In B, select the component library from which you want to select your footprint. For example, for standard capacitors, you would probably choose either libraries "Capacitor_SMD" (surface-mount capacitors) or "Capacitor_THT (through-hole capacitors).

  3. Activate the footprint filters in C. Filter by the library "L" and the number of pins "#". You can further narrow down your search by adding keywords in the text box to the right.

  4. Select the appropriate footprint in D. Press E to preview selected footprints. Make sure to double-click on the footprint in the right panel assign it.

  5. Repeat these steps until all footprints are assigned. Feel free to use standard passive footprints from the global libraries for your passives.

  6. Press "OK" to save and dismiss the window.

Moving from Schematic to Layout

Also pulled straight from the intro lab!

Inside the schematic layout editor, go to Tools → Update PCB From Schematic. This should open up the Pcbnew window and a popup window. Click 'Update PCB'

If you've done everything correctly so far, there should be no errors in the "Update PCB from schematic" window, as shown above. Click somewhere in the PCB layout editor window to place down all the imported footprints.

Basic Layout Environment Setup

Let's do some basic environment setup before actually getting started.

  1. Make sure you're using the Modern Toolset. Preferences → Modern Toolset (Accelerated).

  2. Also make sure you are set up to use inches. Press the "in" button in the left sidebar. (Why the inferior imperial measurement system? Hopefully Mr. Hymel has given you some indication of why)

  3. Set a grid size. Just a warning you may need to change this around for the next part of lab.

  4. Get to the board setup window by File → Board Setup. Set Preset Layer Groupings to "Two layers, parts on front" in the 'Layers' page (default screen that the Board Setup should open with).

Board Outline

(Not needed for checkoff, but you should start this if you have the time this lab)


The tech club mechanical team has dropped the basic board outline for you PCB designers. Note the mechanical requirement:

Draw the board outline in the PCB editor on the Edge.cuts layer. Note that all dimensions are in inches.

dimensions are in inches

Checkoff

Submit a screenshot of your parts in the PCB layout editor (after the "Moving from Schematic to Layout" section) as part of the BCourses checkoff submission.

What we are checking in the checkoff:

  1. Project footprint library
    1. At least 3 self made footprints
    2. Other components seem to match the datasheets
    3. No unnecessary passives in the library
  2. Properly assigned footprints (from your new library)
  3. PCB with the parts imported

You do not need to have completed the board outline to get checked off. Though, it will need to be completed by the time the next lab is checked off.