Footprints and parts

A symbol says "this is a resistor". A footprint says "solder it onto these two rectangles of copper, 1.6 mm apart". The schematic knows nothing about size, so before the board can exist every symbol must be matched to a real, purchasable part and the correct land pattern for it. This is the step where most first boards go wrong, so we slow down here.

What a footprint contains

A footprint is the physical drawing of a part on the board. It includes:

• Pads: the exposed copper where the leads or terminals are soldered. Each pad has a number that matches a symbol pin.
• Silkscreen outline: a line showing where the body sits, with a pin 1 mark.
• Courtyard: an invisible keep-out rectangle. DRC complains if two courtyards overlap, which is how KiCad stops you placing parts too close to pick up with tweezers.
• Solder paste and mask openings: generated automatically from the pads.
• 3D model: used only for the viewer in lesson 5.

The pad shapes are larger than the part's terminals on purpose. A bit of extra copper at each end forms a solder fillet, which is the little meniscus that holds the part mechanically and makes the joint easy to inspect.

SMD or through-hole

Use SMD for almost everything: resistors, capacitors, LEDs, the regulator and the module. Use through-hole where mechanical strength matters, such as the 2.54 mm pin headers. Our USB-C connector is a hybrid: small SMD signal pins plus through-hole shield tabs that survive being plugged and unplugged hundreds of times.

Choosing 0603 or 0805

Passive parts are named by size code. The code is a number like 0603, where the first two digits are length and the last two are width in hundredths of an inch. The metric version uses tenths of a millimetre, so 0603 imperial equals 1608 metric. KiCad footprint names look like R_0603_1608Metric and show both.

Why choose 0603 for this project? It is small enough to keep the board at 40 mm by 25 mm, large enough to place with tweezers, and every fab and distributor stocks it in huge quantities, so it is cheap and rarely out of stock. Choose 0805 if you want an easier first solder job or need the extra power rating. Use 0402 only when space is truly short and you have assembly service. Also check capacitors: a 10 µF ceramic in 0603 is available, but its real capacitance drops sharply under DC bias (a 10 µF 6.3 V part may give 5 µF at 3.3 V), so for bulk capacitors pick a higher voltage rating, 16 V or more, or a larger package.

Assigning footprints in KiCad

In the Schematic Editor, open Tools > Assign Footprints. The left pane lists libraries, the middle lists symbols, and the right pane lists footprints. Select the 10 kΩ resistor symbol, then double-click Resistor_SMD:R_0603_1608Metric. You can select several identical parts at once. Alternatively double-click any symbol and fill its Footprint field.

For common parts the standard library has what you need. For the ESP32-C3-MINI-1 and the USB-C connector, look in the libraries RF_Module and Connector_USB, or download the manufacturer footprint. If you cannot find one, you can draw it yourself in the Footprint Editor, which is how everyone creates parts that are missing.

Reading a datasheet land pattern

Never trust a footprint blindly, especially one from the internet. Open the datasheet of the part and find the section called "Recommended PCB footprint", "Land pattern" or "Recommended PCB layout". You are checking five things:

1. Pitch: distance between pad centres, for example 0.5 mm for the USB-C signal pins.
2. Pad size: width and length of each pad.
3. Pad count and numbering: pin 1 location and which pad is which.
4. Mounting holes: size and position of any through-hole shield or mounting pegs.
5. Keep-out areas: the ESP32-C3-MINI-1 datasheet shows an area under the antenna where no copper may exist.

Print the footprint at 1:1 scale and place the real part on the paper. If the pads line up, you are safe. This simple trick has saved many first boards.

BOM and part numbers

A Bill of Materials (BOM) is the list of every part with value, footprint and quantity. To order, you also need an exact manufacturer or distributor part number. LCSC part numbers start with the letter C followed by digits; Digi-Key and Mouser have their own formats. JLCPCB's assembly service uses LCSC numbers because it stocks parts from that catalogue.

In the Schematic Editor, Tools > Edit Symbol Fields lets you add a column named LCSC and paste a part number for each unique value. Export the BOM with File > Fabrication Outputs > BOM... in KiCad 8 and 9. When you pick a part, check three things on the distributor site: the package matches your footprint, stock is available in quantity, and the part is not marked obsolete. Always verify part numbers on the site itself, because numbers change and a wrong one is easy to type.