KiCad PCB Design· Live
Home / Chapter 2 / 2.1

The CAT4104 LED driver symbol

Lesson 2.1 · KiCad · free

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.

In this lesson · 7 steps
  1. Create your symbol library
  2. New symbol and the 50 mil grid
  3. Draw the body
  4. Add the pins from the datasheet
  5. Electrical types
  6. Place the pins by function
  7. Symbol properties, then save

1Create your symbol library

  1. KiCad → Symbol Editor → File → New Library → Global
  2. Name it something general, e.g. steppeschool_library

2New symbol and the 50 mil grid

  1. Select the library → File → New Symbol → name CAT4104 → OK
  2. Preferences → Preferences → Symbol Editor → Grids: 50 mil
Why?
The grid is where the pins snap. Pins must be on a 50 mil grid in KiCad, or the schematic check fills up with warnings. Set it once, it saves a lot of time later.

3Draw the body

  1. Draw a rectangle for the body, press Esc, select it
  2. In its properties, fill it with a colour (something between red and yellow)

4Add the pins from the datasheet

  1. One pin by hand to see the dialog: name LED1, number 1
  2. Open the Pin Table → press + until there are 8 rows
  3. Copy the Name column from the datasheet (Table 5), select the Name column in the Pin Table, paste. Same for the numbers
Why?
Typing pins one by one is slow. In the Pin Table we add eight rows, then paste the Name column and the Number column straight from the datasheet's pin table. Ten seconds for all of them.

5Electrical types

  1. LED1–LED4: Output · EN/PWM, RSET: Input · VIN, GND: Power input
Why?
The electrical type tells KiCad's checker what each pin does, so it can warn us later, e.g. when a power pin has no power.

6Place the pins by function

  1. Outputs LED1–LED4 on the right (rotate with R)
  2. Inputs EN/PWM and RSET on the left, VIN on top, GND at the bottom
  3. Resize the body so it fits the pins
Why?
A common mistake is to copy the pin positions from the chip drawing. In a schematic symbol we place pins by function: inputs left, outputs right, supply on top, ground at the bottom.

7Symbol properties, then save

  1. Right-click → Symbol Properties: Reference U, Footprint: later (lesson 2.2)
  2. Datasheet: browse to the PDF you downloaded · Description: Constant Current LED Driver · Keywords: LED driver
  3. Add a field Manufacturer = onsemi → OK → File → Save
Why?
A link to the datasheet lets you open it from the schematic later, which is very handy. Keep the datasheets in their own folder next to the project.
Check & troubleshoot

What you should see

  • The library steppeschool_library has a symbol CAT4104
  • 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

Next: Lesson 2.2: the footprint of the CAT4104, from the package drawing in the datasheet.