The CAT4104 footprint, layers and the 3D model
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.
- Datasheets
- Symbols & footprints
- Schematic
- PCB layout
- Files & order
The symbol says what the chip does; the footprint says where it sits on the board. We build it from the package drawing in the datasheet, check it with a 3D model, then link it to the symbol from 2.1. In chapter 4 these pads are exactly what we route the copper tracks to.
Datasheets
- CAT4104VP2-GT3 (onsemi), LED driver · TDFN-8; the datasheet link is on the product page
Want the ready symbol and footprint?
The full course includes the Steppeschool KiCad library: every symbol, footprint and 3D model from this course, plus the whole project (schematic, PCB, Gerbers). Members download it from the Project Files lesson on the course page. Not a member yet? Get the full course (from $5).
In this lesson · 7 steps
1New footprint library
Footprints get their own library, next to the symbols.
- KiCad → Footprint Editor → File → New Library → Global → name it, e.g.
steppeschool_library - The new library appears in the list on the left
2Footprint Wizard: start from SOIC
The wizard draws regular rows of pads for us, so we start from the closest package.
- File → Create Footprint… (Footprint Wizard) → SOIC
3Enter the datasheet dimensions
If one number is wrong here, the chip won't fit on the board. Take every value straight from the datasheet.
- Pad count
8· pad pitch0.5mm · pad width0.3mm · pad length0.68mm - Row spacing
2.72mm → keep the rest → Export footprint to editor
4The layers
Before going on, we learn what the layers mean. They come back in every PCB lesson.
- Open a pad's properties: it is on
F.Cu,F.PasteandF.Mask
5Add the thermal pad and rename
The pad under the chip carries heat and ground. Without it, the chip runs hot.
- Add a pad: number
9, size1.56×1.45mm, at the centre - Rename the footprint
TDFN8→ save
6Attach the 3D model
The 3D model lets us check the footprint by eye, and later see the whole board in 3D.
- Download the STEP file from the product page (Digi-Key: EDA/CAD Models) or Ultra Librarian. Keep all STEP files in one folder
- Footprint Properties → 3D Models → add the
.stepfile → rotation Z-90°until it sits on the pads → OK → save
7Link footprint and symbol
Linking makes the symbol and the footprint one part. The PCB editor uses this link in chapter 4.
- Symbol Editor → CAT4104 → Symbol Properties → Footprint: choose
TDFN8from your library - Add a field
Part Number=CAT4104VP2-GT3 - Add pin
9for the thermal pad (Power input) → save. Pin and pad numbers must match
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)