Newbie needs help making footprint for LED

I’m a complete newbie working with Kicad. The last PCB I made was in 1993.
Picking up the hobby again now I’m retired.
I’m developing a PCB containing OSRAM LED’s: KWDPLS32.EC
Since there is no footprint in the Kicad library, I have to make it myself.
This is what I made so far, two pads.

But in the data sheet there is much more: what is ment by that “Cu area”? And how do I incorporate it in the footprint? On which layer?
And what is the green hatched “solder resist”? Is it a solder mask?
All new to me, some help very welcome.

Hello! This is a fairly complex footprint. Let me try to explain what is intended:

The “Cu Area” is showing the regions that the footprint is meant to be attached to. They are suggesting it be attached to a massive copper pour on both sides for heatsinking purposes. You don’t need to worry about that here, and you can’t add it to the footprint as the dimensions are not specified, but you should consider it in layout when you use the part. The “solder resist” is the inverse of your solder mask openings - because it matches the pads, if you enable the F.Mask layer in your footprint pads that will be fine. The stencil is the equivalent of the F.Paste layer - because this doesn’t quite match the pad sizes, you will need to make a pad of type “SMD Aperture” set to the F.Paste layer for those three elements.

In addition, your footprint is missing a Fab layer (showing the dimensions of the part and the pin 1 indicator corner), a courtyard layer (0.25mm from all exposed copper, 0.25mm from edge of part, whichever is closer) and a silkscreen layer.


Cu area is the area where the copper on the PCB should be placed. Think about it as the landing pads for the contacts. The “foot print” in the context of the datasheet represents the contacts of the LED.
Solder resist is indeed the solder mask. It indicates the area in which NO solder mask should be placed.

1 Like

This is probably not relevant unless OP is mass manufacturing something. Stencils are typically a little bit smaller than pads and many standard prototype manufacturers like JLC or Aisler or whatever will automatically decrease the size of stencil holes. So I wouldn’t worry about that here. (Edit: I didn’t noticed the gap on the right pad. In that case it might be necessary to set a custom shape if soldering using stencils is desired, otherwise the right pad could get too much solder paste)

The footprint looks fine as is if the missing layers (courtyard, fab and silkscreen) are added.

1 Like

I see that while I was looking at the datasheet, you already added the same picure and kliment also answered. But still, here is a bit bigger footprint suggestion from the datasheet with readable numbers:

As has already been mentioned LED’s need a heatsink. This LED’ operating parameters are 120mA and 3V, which is 360mW, and it can even go up to 180mA and 3.35V, which is 603mW


As a rule of thumb only around 30% of that energy is converted to light, and the other 70% has to be dissipated as heat. The life expectancy of LED’s goes down dramatically with higher temperatures. Dissipating 400mW in such a small package leads to a quite big temperature rise and the plastic housing of the LED itself is a relatively good heat insulator, which would make the LED even hotter.

Copper is a very good heat conductor, and the metal pins of the LED itself also conduct heat pretty well. Therefore it is expected that PCB itself is being used as a heatsink to keep the LED cool.

Also, have a good look at the two graphs I posted. On the left graph you can see that the forward voltage over the LED goes up for higher currents, on the right graph you can see that the luminous flux does not increase lineairly with higher currents, but bows a bit downward. The combination of these two resulst in a quite big efficiency loss at high currents. Running LED’s at a lower current is highly recommended. Both for higher efficiency, and for the lower temperature of the LED, which results in a longer lifetime.

1 Like

To make it even clearer – add zones around it with “solid” connections to these pads, and make them as large as possible, and add zones below it to other layers and stitch the zones on different layers together with vias. Whatever helps conducting the heat away from the component. Actually even other surrounding components, including external wires attached to nearby connectors, can work as coolers, but it of course requires some cool air around the system.

On the other hand soldering manually with an iron may become difficult or impossible when the heat is conducted away from the pads.

The “Cu areas” are for illustrative purposes, they are in no way “must calculate the dimensions and use areas identical to the image”.


Hi all, thanks everyone for the replies. Sorry I didn’t react any earlier, I’ve been a few days off…
I tried to work further on the footprint. Since there will be 20 LED’s on the board, and the board will sit in a confined space, I added copper on the front of the pcb and on the back. On the front I drew a solder mask, but I doubt I did it the right way. Can I post the footprint file on this forum? So someone can review it.
In the meantime I drew a 3D step file too. Since I was a mechanic in the past, that suits me better :slight_smile:

Led_Stoel_Evelien.kicad_mod (3.3 KB)

Yes, you can just drag a file from a file manager. Or use the upload button of the forum’s text editor.

Thx, I attached it to my post.

If you have 20 high power leds in a confined area, you might need to be quite careful with thermal management. Copper pours will help to reduce local hotspots but you might have trouble sinking sufficient heat from the board without planning for a suitable heat sink or adequate air flow. One thing worth considering is using a aluminium backed board either for all of your circuit or at least for the leds. This would help with heat management which otherwise might cause problems and possible premature failure. Most pcb fabs offer aluminium cores at very reasonable prices. There are some design and manufacturing constraints to consider when using these (SMD only - no THT components, reflow only).


this could be an option (I also added solder resist layer EDIT: moved F.Silks to F.Fab layer)
KWDPLS32EC6H6J4C8E1-kSU-v6.kicad_mod (7.2 KB)

led-kv6.kicad_pcb (9.4 KB)

KW DPLS32.EC.step (78.3 KB)


Make sure the silkscreen has enough clearance to the pads and it usually shouldn’t be below the component body of SMD components as that can raise the components and increase the likelihood of problems. It looks like some of the silkscreen should maybe be moved to the fab layer.

1 Like

Silkscreen is normally cut by mask layer during production. For lazy fab, there is an option in kicad to produce gerber cutting this layer.

When the silkscreen overlaps with the openings, we will follow the principle of openings first. In another word, we will ignore the silkscreen and make the openings on the boards only.

1 Like

You are right, this should be moved in Fab layer for SMD components


Right, but it’s still better to intentionally design the visible shape, rather than relying on error correction by the software or even worse by your manufacturer, which is way less predictable.

1 Like

I agree with Jonathan. Why draw silkscreen where it will not be printed if the purpose of the silkscreen is to be printed? The option to remove it from maskless areas is good for preventing accidents.


it is useful in 3d viewer to check model alignment, and it is simply removed by manufacturer under production. Still it could be problematic having it under SMD part…

1 Like

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.