How would you design this pad layout?

[knotlogic]

I'm trying to layout the pads for a Yuji 5730 package LED, but I have my doubts about their recommended solder pad layout (page 5 of the linked datasheet).

For one, they don't seem to describe any reference point between the package dimensions and the solder pad layout.  That isn't so bad I guess, but if I assume the gap between the terminals is centered with the gap between the pads I get the result in my attachment.  (The grid spacing is 0.5 mm per div.)

That asymmetric layout really bugs me, should it really be that "lopsided"?

Also, the solder pad seems unusually wide to me.  It's 2.8 mm wide for a tab that's listed as being 2.05 mm at its widest.  I can understand if they mean to have a large copper area for heat sinking, but should there be that much of a margin in the solder pad?

Oh, and that's all not counting the fact that I still haven't found any mention in the datasheet of which is anode and which is cathode.  I've just made a guess at it in my initial layout, but I'll test that myself later.  Just to be sure.

How would you guys layout the solder pads for this?

[lordium]

I would just go with the datasheet (or add EVEN MORE copper, for thermal reason). The LED itself is wider than the pad so it should cover it all even if it's 2.8 mm wide.

You can see the third last page for anode/cathode direction, there should be a mark in the corner to indicate.

[SiliconWizard]

I see no reason not to follow the datasheet's suggested land pattern.
Actually, a lot of power SMD diodes also have asymetrical pads.

As lordium said, there is a "polarity mark" indicating the cathode, which corresponds to the larger pad. Seems to be some sort of convention for SMD diodes. All the power SMD diodes I've used that had asymetrical pads had the cathode at the larger pad (such as those with POWERMITE packages).

[knotlogic]

I would just go with the datasheet (or add EVEN MORE copper, for thermal reason). The LED itself is wider than the pad so it should cover it all even if it's 2.8 mm wide.

I'm not worried about that part, I plan to place the LED pads on large thermal planes anyway.  It's the unmasked areas that I'm concerned about.

You can see the third last page for anode/cathode direction, there should be a mark in the corner to indicate.

Thanks!  That was driving me nuts.

I see no reason not to follow the datasheet's suggested land pattern.
Actually, a lot of power SMD diodes also have asymetrical pads.

I'm worried the large fillet on the cathode side and surface tension might pull the LED across, with a risk of shorting the device anode to the cathode pad.

The larger cathode pads on other devices is why I guessed at that being the cathode on this one.  The 5730 package might actually be a standard size too, but I've only seen one other manufacturer using it and their terminals and land pattern are different.

[SiliconWizard]

I'm worried the large fillet on the cathode side and surface tension might pull the LED across

Quite frankly, I doubt that because the thermal masses on the diode are probably adapted to this, but in doubt, I think you should ask your PCB assembly service. They are experienced with those issues and will be the ones who will deal with your design in the end (they usually don't like bad yields, so they should be happy to help).

IME, this is good practice to check your layout with your usual assembly service before having your PCB manufactured.

[knotlogic]

Thanks for the advice, but I don't have one.  This going to be for my own use, so PCBs from whichever budget service I can find, and self-assembly with a hot air station.  Guess I'll just have to try my luck.

[SiliconWizard]

Oh, I see!

If it's not for automated assembly, I would seriously not bother. I may even enlarge the pads further so they become actually accessible when the LED is positioned, so I can actually solder it with a soldering iron instead of an hot air station.

[T3sl4co1l]

Look up IPC-7351 (the old version is free, and you can find the proposed revisions for A and B for free as well; or just look a little harder for the full, current version).  The pad area is an LGA style joint, with ~no height (it's not a BGA), so has ~zero fillet.  The leads are flat, so can have side and toe fillets.

Starting with the datasheet footprint: I wouldn't make it so wide, 2.1 instead of 2.8mm.  The pad gap is alright, but the recommended 0.5mm isn't really any harder to manage.  I might use 0.6mm.  The width will give more than adequate side fillet, and the overall length will give more than enough toe fillet, fine if you ever need to hand solder it, too.

Connecting: via-in-pad is alright for a pad this size.  Use small (<= 0.3mm i.d.) vias, maybe 4-8 of them.  Around the edge: eh, direct connect to pour is alright too.  Keep in mind, the more copper you have heatsinking it, the harder reflow will be, and the more preheat the board will need.

Tim

[knotlogic]

Thanks Tim!  I'll see if I can dig up an older copy of IPC-7351.