1 - Introduction

With your components selected, it’s time to design symbols and footprints so you can use them in your schematic and PCB layout. If you recall from the project setup portion of the bootcamp, Altium requires 2 libraries in order for you to use your components in your PCB design. There’s the schematic symbol library to store symbols representing components and their parameters in order to place them in your schematic. Then there’s the PCB footprint library which stores footprints for the physical layout of the components to use in your PCB layout. This section will go over how to use the provided library files you have to add your components and use them in your PCB design.

2 - Reusing a Schematic Symbol

It’s not always necessary to create a new symbol from scratch for each component. Especially for generic chip resistors and chip capacitors, it’s much faster to simply reuse existing components and just modify them to fit the new component parameters. In the provided schematic symbol library, you’re given a sample 10k resistor (size 0603) and 1uF capacitor (size 0805) for you to use. If you selected resistors or capacitors with different values or of different sizes, you can reuse the provided symbols to add your resistors and capacitors more quickly.

Open the schematic symbol library in Altium. A SCH Library pane should open up on the left, but if it didn’t, manually open it by clicking Panels > SCH Library from the bottom left. You should see the 2 sample components provided for you.

Open

To reuse a symbol, simply select it in the SCH Library pane and copy it (either Ctrl + C or right click > Copy), then paste it (Ctrl + V or right click > Paste). A duplicate should appear that you can then replace with your own component. To do so, you’ll need to adjust the component’s Parameters, which is covered in section 4.

3 - Adding a New Schematic Symbol

For the LDO component you selected, you’ll need to create a new symbol from scratch to represent the component and its required connections. Start by clicking Add in the SCH Library pane, then paste the manufacturer’s part number for the LDO you selected in the Design Item ID field and click OK. Before starting your symbol design, be sure your Grid is set to 100mil. You can see your current grid in the bottom right of the screen, and toggle it between 10mil, 50mil, and 100mil by pressing G on your keyboard.

Start by placing a decently sized rectangle in the design grid by clicking Place > Rectangle, clicking once to place the rectangle and clicking a second time to define the size. Then place each of the pins for your LDO on the rectangle. Do so by clicking Place > Pin, or clicking the Place Pin button from the hotbar at the top, then clicking to drop a pin in the design grid. Place a pin down for each pin on the LDO you selected.

Once you’ve placed your pins, you’ll need to adjust each pins properties to match the LDO you selected. To do so, you’ll have to go to the LDO’s datasheet and find the section that details all the pins and their functions. This will typically be titled something like Pin Configurations and Functions, and can be found easily in the table of contents. Click on each pin and, in the Properties pane, set the Designator and Name to match the pin numbers and names given in the datasheet exactly.

Once all the pins are configured properly, move and orient them so that they are placed on the left and right sides of the rectangle with the names inside the rectangle. It’s also good practice to place the pins such that you have:

• GND pin(s) at the bottom right

• Input power pin(s) at the top left

• Output power pin(s) at the top right

• Any other input and output pins on the left and right sides respectively

When you’re done, your symbol should look something like this:

Open

Don’t forget to also set the Properties and Parameters for the component itself, as explained in the next section.

4 - Setting Properties and Parameters for a Component

Every component must have the proper properties and parameters set in order to identify it. These are found in the Properties pane on the right. With your component selected, go to the Properties pane and adjust the following properties using the values provided on the Digi-Key page or datasheet:

• Design Item ID: Put the manufacturer part number here

• Designator: Put the proper designator based on the type of component (i.e. R? for resistor, C? for capacitor, U? for an IC, etc.). If you’re unsure which letter to use, see Reference designator - Wikipedia

• Description: Copy the description from Digi-Key

Now go to the Parameters table and click Show More to see all the parameters currently attached to the component. If you’re reusing a component, simply replace the value for each row with the appropriate value from the Digi-Key page or the component’s datasheet. If you’re making a symbol from scratch, manually add each of the following parameters via Add… > Parameter:

• Manufacturer 1

• Manufacturer Part Number 1

• Supplier 1

• Supplier Part Number 1

• Value (if resistor or capacitor)

• Power Rating (if resistor)

• Voltage Rating (if capacitor)

The last thing you’ll need to do is link a footprint to your component. You’ll notice that the sample components already have the right footprint linked to them in the footprint table at the bottom of the screen. If you’re creating a new symbol from scratch, you’ll need to click Add Footprint > Browse… to select the right footprint from the footprint library. If you’re reusing a symbol and need to change the footprint, first select the existing footprint and click Remove, then add the correct footprint.

5 - Adding a New Footprint

The provided footprint library does not have all the footprints you’ll need to complete the bootcamp. Specifically, you’ll need to make a footprint for your LDO and connectors. To make a new footprint, open your footprint library and in the PCB Library pane, click Add. It should open a new footprint titled PCBCOMPONENT_1. Click Edit and put the name of the footprint you’re making. You can either take the name given in the Package/Case field on the Digi-Key page, or make your own descriptive name if one isn’t given.

To actually make the footprint, follow the guidelines here, under the Within the Footprint Editor section: Schematic Symbol and Footprint Guidelines. If you’re confused about anything or get stuck, send a message on the WARG Discord to get help from one of the current electrical team members.

Note: That page also has guidelines for creating schematic symbols. However, those guidelines are for using WARG’s cloud-based libraries, which you won’t have access to until you complete the bootcamp. As such, please follow the guidelines provided on this page for creating your schematic symbols, since the bootcamp makes use of file-based libraries instead of cloud-based libraries.

After making your new footprint, be sure to save the footprint library so that you can link your schematic symbol(s) to that footprint.

Congrats on making it this far! Once you’ve got your components all ready, you can move on to starting your schematic.