How to make a footprint for this IR LED



I am trying to use On Pg 5 , I see the footprint. Does that have to be on copper? Do I have to specify any soldermask or is it automatically specfied in kicad?

Not plotting the ECO layer in Gerber

We have to design everything like actual pad size, silk screen area, component edges etc…



KiCAD creates a soldermask layer based on the board outline, any copper fill zones, and pads defined in the copper layers. At worst you need to specify a value for the “soldermask swell” or “mask pullback” parameter. This soldermask layer created by KiCAD is typically quite reasonable and effective as long as you have simple, commonplace, pads in the solder layers.

This component does not have simple, commonplace, pads in the solder layers. You will have to explicitly draft this component’s soldermask layer, and modify parameters for this component’s pads. (And do much the same thing for the solderpaste layer, if it is needed.)

I suggest that you make an honest attempt to draft a footprint for this component, post that footprint here, and ask for comments. If it appears that your effort was sincere and rational, the responses will be respectful, forthright, and helpful. “Initiative” is a highly admired quality around here.



I started making the footprint but I have a couple of questions. The one on Pg 6 shows two dotted lines for copper. Should the entire thing be filled with copper or just the specific one like I have attached?


Copper only - deselect Paste/Mask
Paste or Mask - choose None for Copper


I’ve been gone all day and @Joan_Sparky beat me out for seeing & responding to this post.

This part dissipates a LOT of power, and the suggested footprint includes some “extra” copper to help control the heat. Osram really should have discussed this in the datasheet, and included suggestions for ways to improve the circuit board’s thermal design.

If you have difficulty following the suggestions from @Joan_Sparky , search this Forum and/or the KiCAD footprint libraries for examples of footprints for medium- or high-power packages such as TO-220, or DPAK. While the dimensions are very different from your footprint, I know that some of these footprints were assembled using the same techniques you’ll use for this LED footprint.



So the extra copper is for power dissipation bit is covered by soldermask?


I will take a look at those and get back if I have questions.


Yes, the more the better.
I guess the datasheet will mention somewhere what this pad design is able to manage in regards to K/W or somesuch…
If you can do bigger and involve vias to the backside you’ll have more fun with that LED as it runs cooler.
Think of the copper as a heatsink…
In those outer non-soldering copper pad sections, vias to the backside would be good.
You also might want to look into 35u copper instead of the normal 16 or what it is.
Also check if there is mentioning of aluminium core there which is a different ballgame again.


Your pretty quick. I will do so.


I’m just ‘still awake’ and the browser keeps notifying me if someone replies… I should be in bed already. :sleeping:


Yes. The effect of the soldermask is a matter for opinions and debates. You would think the soldermask inhibits heat exchange but the degradation is minimal. Having soldermask over heatsink copper saves plating chemicals, inhibits corrosion, and reduces inadvertent contact with system voltages.

The exception is where a metallic heatsink will be installed. There you will leave off the soldermask to improve thermal contact between the heatsink and the heat-conducting copper.



Thanks. It makes sense now