LED symbol and footprint
Now the LED, a Würth Elektronik 158301265A (white, 1206). Its datasheet says 2.8 V and 65 mA, which suits our 5 V board.
- Datasheets
- Symbols & footprints
- Schematic
- PCB layout
- Files & order
Same job as the driver, smaller part: symbol, footprint, 3D model and link, this time for the LEDs. With only two pads, we place them by hand, which is how you'll make most small parts.
Datasheets
- 158301265A (Würth Elektronik), white LED 1206 · datasheet and 3D model on the product page
Want the ready LED 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 · 6 steps
1Read the LED datasheet
As always, we start from the datasheet: its land pattern gives the pad sizes.
- Dimensions, recommended land pattern and schematic: forward voltage 2.8 V, current 65 mA
2New symbol
A simple two-pin symbol: anode and cathode.
- Symbol Editor → select your library → New Symbol → name
158301265A, default referenceLED - Two pins, both Power input:
C(cathode, pin 1) andA(anode, pin 2), as in the datasheet - Draw the diode with lines, plus two small arrows for the light
3Symbol properties
These fields go into the BOM in chapter 5, so the factory buys exactly this LED.
- Datasheet: browse to the PDF · Description: from the distributor page (e.g.
LED Lighting - White, Cool 6500K … 2.8V 65mA 120° 1206) - Fields
Manufacturer=Würth Elektronik,Part Number=158301265A, KeywordsLED→ OK → save
4Footprint: two pads by hand
For two pads, placing them by hand is faster than any wizard.
- Footprint Editor → your library → New Footprint
- Pad 1:
1.8×1mm at x =-1.1· Pad 2:1×1mm at x =0.7
5Polarity arrow and courtyard
The arrow shows the LED's direction on the real board; the courtyard reserves its space.
- On
F.Silkscreen, draw an arrow from anode to cathode, the way the current flows - Pick
F.Courtyard→ draw a rectangle around the part - Rename the footprint
158301265A→ save
63D model and link
With the 3D model and the link, the LED is ready for the schematic.
- Download the STEP file (e.g. from Component Search Engine) → Footprint Properties → 3D Models → add it → offset X
-0.4mm → OK → save - Symbol Editor → LED symbol → Footprint:
158301265A→ save
Check & troubleshoot
What you should see
- Symbol
158301265A, referenceLED, pins 1 = C (cathode) and 2 = A (anode) - Footprint: pad 1 is 1.8 × 1 mm, pad 2 is 1 × 1 mm, 0.4 mm gap
- A courtyard rectangle on
F.Courtyardaround the part - The 3D model sits on the pads
If it doesn't work
- LED lights the wrong way round later: check which pad is the cathode in the datasheet and that pin and pad numbers match
- Can't draw on the courtyard: pick the
F.Courtyardlayer in the layer list first - No 3D model on the distributor site: try Component Search Engine (free account)
Good to know
- Pad positions: we put the origin in the middle of the gap. The gap is 0.4 mm, so each pad starts 0.2 mm from the centre; a 1 mm pad then has its centre at 0.2 + 0.5 = 0.7 mm
- The courtyard is the space a part needs. Before ordering, KiCad checks that no two courtyards overlap, because two parts can't sit in the same place