The CAT4104 LED driver symbol
A symbol is how a part looks in the schematic: a box with named, numbered pins. We create our own library, then draw the CAT4104 symbol.
- Datasheets
- Symbols & footprints
- Schematic
- PCB layout
- Files & order
KiCad needs two drawings for every part: a symbol for the schematic and a footprint for the board. Our LED driver isn't in KiCad's library, so we draw both ourselves. This lesson is the symbol, made from the pin table we read in lesson 1.3. The footprint follows in 2.2, and in chapter 3 we use the symbol in the schematic.
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
1Create your symbol library
All our own parts go into one library, so every future project can use them too.
- KiCad → Symbol Editor → File → New Library → Global
- Name it something general, e.g.
steppeschool_library
2New symbol and the 50 mil grid
A clean grid now means no warnings later, when we wire the schematic.
- Select the library → File → New Symbol → name
CAT4104→ OK - Preferences → Preferences → Symbol Editor → Grids:
50 mil
3Draw the body
The body is just a box. Its only job is to make the symbol easy to read.
- Draw a rectangle for the body, press
Esc, select it - In its properties, fill it with a colour (something between red and yellow)
4Add the pins from the datasheet
The pins are what matter: each one becomes a connection in the schematic.
- One pin by hand to see the dialog: name
LED1, number1 - Open the Pin Table → press + until there are 8 rows
- Copy the Name column from the datasheet (Table 5), select the Name column in the Pin Table, paste. Same for the numbers
5Electrical types
The pin types let KiCad check our wiring in chapter 3.
- LED1–LED4:
Output· EN/PWM, RSET:Input· VIN, GND:Power input
6Place the pins by function
Good pin placement keeps the schematic in chapter 3 clean and easy to follow.
- Outputs LED1–LED4 on the right (rotate with
R) - Inputs EN/PWM and RSET on the left, VIN on top, GND at the bottom
- Resize the body so it fits the pins
7Symbol properties, then save
The properties carry what you and the factory need later: the datasheet, the manufacturer and the part number.
- Right-click → Symbol Properties: Reference
U, Footprint: later (lesson 2.2) - Datasheet: browse to the PDF you downloaded · Description:
Constant Current LED Driver· Keywords:LED driver - Add a field
Manufacturer=onsemi→ OK → File → Save
Check & troubleshoot
What you should see
- The library
steppeschool_libraryhas a symbolCAT4104 - Eight pins: LED1–LED4 (1–4) on the right as outputs, EN/PWM (6) and RSET (8) on the left as inputs, VIN (7) on top and GND (5) at the bottom as power inputs
- The pins sit on the 50 mil grid
If it doesn't work
- Lots of "pin off grid" warnings: the grid was smaller than 50 mil. Set it to 50 mil and move the pins again
- Pasting into the Pin Table fills only one cell: select the whole column first, then paste
- Can't select a column in the PDF: many PDF readers select a column with
Alt+ drag; otherwise type the names, there are only eight
Good to know
- Why by function and not by position? Inputs on the left, outputs on the right, power on top and ground at the bottom makes the schematic easy to read and the wires short
- A global library can be used in all your projects, not only this one