KiCad PCB Design· Live
Home / Chapter 2 / 2.2

The CAT4104 footprint, layers and the 3D model

Lesson 2.2 · KiCad · free

A footprint is the pattern of copper pads the part is soldered on. We make the CAT4104's TDFN-8 footprint with the Footprint Wizard and the numbers from the datasheet, then add the thermal pad, attach a 3D model to check it, and link the footprint to the symbol.

In this lesson · 7 steps
  1. New footprint library
  2. Footprint Wizard: start from SOIC
  3. Enter the datasheet dimensions
  4. The layers
  5. Add the thermal pad and rename
  6. Attach the 3D model
  7. Link footprint and symbol

1New footprint library

  1. KiCad → Footprint Editor → File → New Library → Global → name it, e.g. steppeschool_library
  2. The new library appears in the list on the left

2Footprint Wizard: start from SOIC

  1. File → Create Footprint… (Footprint Wizard) → SOIC
Why?
The Wizard can't know every package. We pick the closest one, SOIC, enter our numbers and fix the rest by hand.

3Enter the datasheet dimensions

  1. Pad count 8 · pad pitch 0.5 mm · pad width 0.3 mm · pad length 0.68 mm
  2. Row spacing 2.72 mm → keep the rest → Export footprint to editor
Why?
Row spacing is from the centre of one pad row to the centre of the other. The drawing gives 3.4 mm outside to outside, so we subtract one pad length: 3.4 − 0.68 = 2.72 mm.

4The layers

  1. Open a pad's properties: it is on F.Cu, F.Paste and F.Mask
Why?
Everything on a PCB is a layer. Copper becomes real pads and tracks. Silkscreen is the white print: outlines and the pin 1 dot. The solder mask covers the board (it gives the colour) except the pads, and stops solder bridges. Paste marks where solder goes; it makes the stencil. F. is the front, B. the back.

5Add the thermal pad and rename

  1. Add a pad: number 9, size 1.56 × 1.45 mm, at the centre
  2. Rename the footprint TDFN8 → save
Why?
The chip has a pad underneath (the TAB) that carries heat into the board. The datasheet connects it to GND.

6Attach the 3D model

  1. Download the STEP file from the product page (Digi-Key: EDA/CAD Models) or Ultra Librarian. Keep all STEP files in one folder
  2. Footprint Properties → 3D Models → add the .step file → rotation Z -90° until it sits on the pads → OK → save
Why?
The 3D model is also a free check: if the pads are wrong, the model won't sit on them.

7Link footprint and symbol

  1. Symbol Editor → CAT4104 → Symbol Properties → Footprint: choose TDFN8 from your library
  2. Add a field Part Number = CAT4104VP2-GT3
  3. Add pin 9 for the thermal pad (Power input) → save. Pin and pad numbers must match
Why?
The full part number tells the factory exactly which part to buy. "CAT4104" alone is not enough: the letters at the end choose the package and the packing.
Check & troubleshoot

What you should see

  • Eight pads 0.3 × 0.68 mm, 0.5 mm apart, two rows 2.72 mm apart (centre to centre)
  • A thermal pad 9, 1.56 × 1.45 mm, in the middle
  • The 3D model sits exactly on the pads
  • The symbol has a pin 9 (thermal pad) and its Footprint field points to TDFN8

If it doesn't work

  • 3D model next to the pads or turned: change the rotation and offset in Footprint Properties → 3D Models. Ours needs -90° around Z
  • The 3D model doesn't match the pads at all: a pad size or pitch is wrong. Check the numbers against the datasheet again
  • Pad 9 not connected on the board later: the symbol needs a pin 9 too. Pin and pad numbers must match

Good to know

  • Two ways to make a footprint: place each pad by hand (fine for 2–3 pads), or the Wizard for regular packages. There is no TDFN in the Wizard, so we start from SOIC and edit it
  • Why not download ready symbols and footprints? You can, but a mistake there breaks the whole board, and you don't control the style. We draw our own and only download the 3D model
  • Where to find 3D models: the distributor's product page (Digi-Key: "EDA/CAD Models"), Ultra Librarian or Component Search Engine (free account)

Next: Lesson 2.3: the same for the LED, this time placing the pads by hand.