Electronics > PCB/EDA/CAD

SOIC 8 150mil and 208mil in one Footprint

(1/3) > >>


For one of my projects, I want to use a flash memory IC from Winbond (W25Q16JV). This chip is available in multiple packages.
The options with the best availability are SOIC8 150mil and SOIC8 208mil.
Because of the current situation with low availability of semiconductors, I would prefer to have the option to use both SOIC 8 package options.

The difference between 150mil and 208mil is, that the 208mil package is about 1.9mm wider.
I would assume, a footprint with longer pads should serve both packages.
I am a bit concerned, that if using the wider package, there would be solder paste under the package causing issues.

Does anybody have experience with this kind of multi package footprint?
Are there any better options to accommodate both packages?

I don't think it's a problem.. the flux likely gums up underneath, and is a pain to clean.  If it's washable, maybe avoid vias underneath so there's less exposed metal to corrode.  Errant solder balls stuck to the PCB or package, don't really matter, and most will coalesce into the pad.  Somewhat less paste might be used, given the excess pad length, but it also still needs to span most of the length of the pad else there won't be enough flux and spreading ability to tin the whole thing for both components (i.e. don't make a pile at just the heel or toe).  So, probably a bit of negative paste expansion would be the most you'd bother with.

Note that heel can be set to minimum or even somewhat negative, for the narrow body part -- most assemblers are only interested in one fillet, which would be toe in this case, and the heel then is optional.  Note a severely negative heel will emit a "pin on soldermask" error from most DFM tools, which you may or may not wish to honor.

I think pin-on-mask probably doesn't matter too much here, as the radius of the solder blob (meniscus) on the pad should be pretty generous for SOIC, thus even a fairly tilted component should still dip into the blob and make a connection.  (Or if the pin melts first, then that blob onto the pad, whatever.)  I'd be more worried about that for fine pitch (TSSOP etc.?) where the pad width is much less, I think?

I don't think I'd go so far as to halve the joint face area (effectively dimension L, but in the solder joint, from pin tip to pad heel), but you can still see where it takes you with minimal heel or a little under, with respect to body sizes, and tolerances.


You could have the small 150mil SOIC footprint rotated 90 degrees and squeezed within the footprint of the 208 mil SOIC  - you'd just have a few vias to add to make the connections.

I would also consider adding WSON - with a bit of tweaking of the pads you could make it sit in the same footprint as 208mil soic  - see the mockup picture I made in paint to see the relative dimensions

EDIT:  Macronix has an application note with a footprint mixing 209mil 8SOP with WSON  : https://www.macronix.com/Lists/ApplicationNote/Attachments/1886/AN182V1-209mil%208-SOP%20and%206x5mm%208-WSON%20Dual%20Layout%20Guide.pdf

unless I'm mistaken ... SOP and SOIC is same dimensions so maybe check it out.

Is that SON, or DFN (no middle pad)?  The former might be a little awkward, though I think it's just small enough to fit all three (or four even) in the same place.


No problem at all, I've seen this done dozens of times, mostly with SO-16 and SO-16W. Normal practice.


[0] Message Index

[#] Next page

There was an error while thanking
Go to full version