Which is the "best" footprint for SOD-523?

I revised a few manufacturers for suggested SOD-523 (small SMT diode) footprint, and the result is really confusing(…)
If you take as an example a BAT54X or similar (say a Zener like the MM5Z series) every mfr has a totally different opinion on the correct pad layout. The component itself has a body roughly in a metric 1608 size (same box of a 0603 resistor), however the terminals are thinner, so to prevent floating during reflow it’s reasonable that pads are thinner.
What’s unclear to me is why someone like Fairchild (now ON) draws a total length of 2.8 mm, see Fairchild BAT54X
As a comparison, that same part from ON Semiconductor has a total length of 1.8 mm, and that’s shorter of 1 mm: a huge amount on a 1.6 mm body length! :open_mouth:
As a comparison, Vishay is still on short(er) pads, ST is on quite long pads.
Doesn’t even look like they’re suggesting longer pads for manual soldering (which would be reasonable).

I’ve seen some footprints from consulting designers, working on other circuits where I followed the project, using that same Fairchild long-pads footprint, but I suspect they just chose what they had ready at hand.

I’d like to see some review and opinion on this. If I solder the Fairchild part on the ON Semi footprint I wouldn’t expect troubles, but… then why different?

Maybe to increase the thermal conductive zone?
Depending on what the application design engineer decides (measurements based, experience based, guess based, etc.) they suggest a minimum land pattern to stay within the specs for power dissipation and thermal resistance.
In the case of the Fairchild and ONsemi examples they both dissipate 200mW and seem to have similar thermal resistances of about 500 degC/W on FR4 - each for their respective land pattern.
No guarantee what happens with those values when you mount the Fairchild unit on the ONsemi land pattern.

Personally I use land patterns that leave enough bare pad surface to solder them cleanly without those diodes goofing around on too big pads and then there is more pad/copper underneath the soldermask for heat dissipation. Overall the device then looks more like the respective sized SMD resistor body. But then I don’t work in mission critical areas and have no idea what kind of process would need to be established to confirm that this is even useful.
Example for the bigger SOD323:

PS: some fabs have problems with that and will expose the whole copper pad, which then naturally causes the diode to goof around and become misaligned during reflowing. :angry:

Yes, that about thermal a point I didn’t list. Although the pad itself, with these tiny dimensions, won’t give any appreciable benefit – unless you connect it to a flooded larger area. Moreover, the operating conditions can’t push it over the 200 mW, rated for the minimal pad.

Just to be picky :wink: I checked the Fairchild BAT54H, which hey it’s SOD-323 :grin:
Surprise: pads are small almost as ON part! So same device, same dissipation (and everything makes me suspect has the same die inside), smaller pads…
Again, can’t believe it’s a thermal reason – note: the ON part has also an higher RthetaJA, that would require larger pads, smaller won’t suffice

Manufacturer’s “recommended” land patterns are just a guide. They are usually the recommended minimum land pattern, unless otherwise specified, required to meet the specifications given in the datasheet. You will notice on the Fairchild datasheet it states “Land pattern recommendation is based on IPC7351A standard SOD1609X65M”.

The thermal resistance specified is based on the “recommended” land pattern and therefore you would expect the On-Semi one to be slighter higher. No surprise there.

As I said, the manufacturer’s recommended land pattern is just a guide, you are free to change it, but too much larger or too much smaller and you run the risk of having manufacturability issues as Joan_Sparky has pointed out. It is usually best to stick with the IPC7351 standard if there is one, or use the next closest one.

If you are pushing a component anywhere near it’s rated power dissipation and are concerned about the thermal resistance then more copper is better. One way to address this is to use wider traces connecting to the pads for a short distance and then neck them down to the preferred width. This adds copper without affecting manufacturability.

It would be nice if KiCAD had better support for necking, tapering from one size to another rather than abruptly changing.


The “BAT54” is a pretty good indication that it is the same die. Different package, different land pattern, different specifications. You will notice the only difference in the specifications, other than package, is the thermal resistance and the peak forward surge current. Both of which are likely due to the difference in the size of the leads.


[quote=“1.21Gigawatts, post:4, topic:4179, full:true”]
You will notice on the Fairchild datasheet it states “Land pattern recommendation is based on IPC7351A standard SOD1609X65M”.[/quote]
Good point, in the rush I didn’t read it.

Not being a professional in PCB design, I can’t access IPC-7351A. I found at most an older(?) IPC-7351 document, and at first look is the short form of an encyclopedia :hushed:

An interesting reference is that IPC-7351B is supported by a calculator software, by an IPC third part.
This is somewhat easier to use, and if you can stand the obsessive ads in the “lite” edition you can get some pad measures, compliant to IPC-7351B. There’s even a KiCAD 4.0.1 compatible version (to output directly the libraries), for just :dizzy_face: half a grand.

Making long chatter short, yes: IPC-7351B suggests quite elongated pads

1 Like

I made a board with several SOD-323, using a 0.45Wx0.59L pad and had many dry joints.
I have just redone the board with the pads 0.6x0.6mm, going longer would have modified tracking too much, but at least the joint should be stronger