Did I create this complex LED footprint correctly?

I’m working on a project using Samsung LED’s and their Datasheet has a recommended footprint that I was trying to replicate since there are no built in footprints for 5630 or 5730 LED’s. It looks decent in the footprint viewer but then looks a little odd when adding in PCB editor. I’m fairly new to all this so just want to make sure I did a good job.

LED_5630 Footprint File

Samsung LM561B Plus Datasheet

How does it look at the Gerber level? That’s the true test.

It looks fine except for a couple little things. The lines your are seeing show netpad clearances. Your version of KiCad doesn’t handle clearances of combination pads gracefully. It’s not the end of the world, but if it bugs you, you can try a nightly build. Now they have rounded corners for the offset.

I don’t think you need to use a Nightly Build to have KiCAD recognize overlapping pads as a single, large, pad. Try adjusting the dimensions and locations of your pads to get more overlap, and see if those white “air wires” go away. (Or, add yet another pad to the assembly of pads. Specify it so that it has generous overlap with the other pads, and thus serves only to “tie them together” into a complex pad shape.)


This did not work but I did what hermit suggested and generated the gerber files and it looked great. I’m not going to worry about it for now, hopefully it’ll be fixed in future versions.

You wouldn’t see anything on Gerber files unless you have a copper zone or a track next to the pad. You don’t really need Gerbers for that either. Just put your footprint in the middle of a copper zone, re-flow it and see if it bothers you enough to tinker with it any further

Really? If you you overlap several pads KiCad will treat it as a single pad? Since when?

Since I picked up KiCAD and started using it, over 2 years ago. Look at
Pad Holes Under SMT for Heatsinking . . .
The TO-220 footprint attached to that post may be a better example than the DPAK illustration.


p.s. (Added) - Here’s another example: Single pad with two holes possible?

Try using the atch footprint in place of yours. If it still doesn’t do the job completely, post another screenshot and I’ll make it work for you. Or, use Footprint Editor to study what I did and give it a try on your own.


LED_5630_Alt1.kicad_mod (1.2 KB)

I’ll try it. Looks much cleaner than mine. Thanks!

Not that it matters, but you are mistaken. Overlapping pads with the same pad number doesn’t create a “single, large pad”, it just creates multiple pads that overlap with the same net assigned to every single one of them at the board level. The example discussed in this thread clearly demonstrates it. Had it been like you said, you wouldn’t have been having separate clearances outlines for each pad included.

[quote=“ArtG, post:11, topic:9341”]
. . . The example discussed in this thread clearly demonstrates it . . . . [/quote]
The example shown in the original post by @Blake does not demonstrate overlapping pads. The footprint is composed of pads carefully butted up against each other. I wouldn’t expect even incidental overlap due to numerical roundoff, since the footprint appears to have been created in metric units. We have not yet seen a screenshot using a footprint with overlapping pads, such as the one I composed and posted for him to try.

You seem to have grasped the intent of my statement (below), so the communication wasn’t entirely ineffective. Can you suggest a concise alternative wording that addresses the user’s question in this thread?

[quote=“dchisholm, post:4, topic:9341”]
I don’t think you need to use a Nightly Build to have KiCAD recognize overlapping pads as a single, large, pad. . . . [/quote]


With KiCad 5 polygon pads will be added which supports such shapes out of the box

1 Like

I would venture a guess that we are talking about two different things. My point was that no matter what combination of the overlap you use, the current version of the KiCad will treat each pad as an individual pad. The original post demonstrates that because you can see individual pad net clearances. Here is another example where two pads with the same number fully overlap.

As you can see they haven’t magically merge into a single pad.
If you are talking about passing DRC check and consequently not having extra rat’s nest lines, that has nothing to do with KiCad treating overlapping pads as a single pad. It has everything to do with two pads making physical (copper) connection, which can be true not only for two overlapping pad, but also for two pads belonging to two separate footprints and connected with a track. I hope you wouldn’t say that in such a case KiCad would treat them as a single, large pad?

This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.