Custom footprint tears off board easily

[criznach]

First time poster!  I designed a custom footprint for some SK6812 4020 side emitting RGB LEDs based on the datasheet specifications (attached).  I have built boards and they work fine.  But I've found that the footprints and LEDs are very fragile and can be knocked off far too easily.  The pads are quite small and easily peel off the substrate.  Typically the solder on the well-connected ground pad breaks, and the other 3 pads peel back.  I'm wondering what is typically done to make this type of footprints stronger?  I've thought I could create a larger thermally relieved pad on the "data in" pad, which is at the opposite end as the ground.  Or I could extend the pads length-wise to give them more surface area.  Is this a common problem?

[Philfreeze]

So the problem is that it breaks in the field or in assembly not while soldering or while doing some rework?

We used to have a similar problem a while back in in the solder process, some pads just peeled off for some reason. We later learned it was probably due to thermal shock and backing the pcb a bit longer before going through the solder profile fixed the problem.
My boss also told me once that it is sometimes a good idea to put a via just next to a pad or into the pad for connectors if you want to make the whole thing mechanically stronger, the problem there is that it can lead to the component not sitting flat on the pcb. (and it may lead to the pad sucking away all the solder if it isn't plugged.

[T3sl4co1l]

Three things:

1. Put it in an enclosure so the LEDs aren't being knocked around. (Duh? )

2. Cheap boards give cheap results.  The peel strength may be marginal, or not even meeting IPC spec (see IPC-600).  Likewise poor plating (on the board and components), poor solder or flux, and poor soldering (adequate time*temp at peak soldering temp, assuming reflow).

3. You can always make pads bigger.  IPC recommendations (see IPC-7351) are minimums, though there are some situations where you don't want to go higher, or can't (obviously, you don't have any room to widen a pad into another pad!).

You can also increase connection area around the pad.  Thermals may or may not be important to your design.  You can use wider traces, and more of them.

You can also help anchor pads by putting vias near, or in, them.

Be careful with via-in-pad, as the vias will wick solder.  Not a problem for hand soldering, you'll see how much solder you need.  Use small vias (<= 0.3mm), which are less prone to wicking.  If you are using lead-free solder, that also tends to wick less.  Do not tent the bottom side, that will trap gas.

A typical example is a fully SMT USB connector.  There are several pads in the front, under the metal shell, securing it to the board.  Two or four vias per pad is enough to help, while not hogging too much solder.  The solder joint is also completely blind, no fillets, so there's even some advantage in using up excess solder, letting the connector sit more flush.  The vias also pin the shield to the ground plane, early and often, as it should be.

Tim

[hermit]

Nothing really to add of any value but I'd like to know how these were soldered.  Hand?  Well controlled commercial oven?  Frying pan?

[asmi]

As the most radical measure (if nothing else works) you can just use some glue to glue the part to the PCB. This way it will only tear off with the PCB

[criznach]

The parts have come off from bumping them in casual handling.  They're prototypes, so I've been putting them into different enclosures and taking them in and out of my parts box quite a bit.  They're taller than the pads are wide, so it's easy to put a lot of force on the pins.  They will be in an enclosure, but it's a somewhat open-framed design for aesthetic reasons, so I need them to be a little bit tougher.

Yes, they're pretty cheap boards from JLC.  Soldering technique doesn't seem to change much.  I've pasted and hot air soldered 3 of the 4 I built, but one I put through a reflow oven at the local makerspace using a leaded paste profile. 

I've redesigned my footprints to have larger pads on both outer pins.  I extended all pins up under the solder mask to the full height of the device.  Vias are a good idea, and I may add some of I have enough space.  It would be great if I can add them to the footprint directly, but I'm not sure yet if I can do that in Eagle.

I'm sure glue would help a lot, but I'm trying to optimize these for hand assembly and that would mean a few extra steps.

Thanks everyone!

[Philfreeze]

Never used eagle before but in Altium I would just place a small through hole pad inside the SMD pad as a via.

Maybe you could have a via just in front and just behind the pad so the LED will be held in place by 8 vias. This way you would also ensure that the surface stays flat and you will see how much solder the via wicks. You could also tent them if they are far enough away to prevent the issue entirely.
You would probably have to fan them a bit out so your annular ring doesn't get too small (0.5-0.6mm pad, 0.3mm hole should work) but this way you could tent the vias so you don't have to deal with the wick problem.