Size of exposed pads


I have looked a bit into exposed pad sizes for the official library. To me it seems most footprints suggested by manufacturers suggest to use the nominal size of the “slug” for the exposed pad.
This seems odd to me as it does not take into account any tolerances (neither the tolerances of the part it self nor the tolerances of the manufacturing process.)
If i use the IPC calculations with 0 (or even with slightly negative) fillet i get a result that would be nearer to the maximum size of the “slug”.

The only thing i can find in IPC standards is a mention that the exposed pad should not be too large. And with too large they mean there should be at least 0.2mm clearance between the outer pads and the exposed pad.

Just to be clear: this is talking about the size of the exposed copper. (So the size of copper if a non soldermask defined pad is used and the size of the area free of mask if a soldermask defined pad is used.)
It is clear to me that the paste layer needs special handling.

With “slug” i mean the large metal pad on the bottom of such parts. (I chose this word as it differentiates from the word pad that is used to describe the PCB side)


I happened to have open (TI general instructions), it says only that “The dimensions of the thermal pad on the PCB should be equal to the exposed pad on the QFN/SON.” It doesn’t tell why. I could imagine one reason: the exposed pad is so large compared to other pads that the adhesion caused by it may be relatively high. Therefore it may give better self alignment if it’s accurate. But that’s just a guess.


Thanks for this information. Your reasoning makes sense.


and in the case of TI and most others they give detailed dimensions for their footprints/parts.

most of the time no need to guesstimate or use rules of thumb etc


For older datasheets their suggestion is most likely a bit out of date (will be based on older ipc standards)
So if one has access to ipc standards i would guess this is the better way to go.


you could compare them and see if they differ significantly.

rarely have production problems due to footprints from datasheets, but the other way around is common.
You also must take into account if the EMS has manipulated the paste-mask (forbidden)

A run of least 3000 units per year to start to discuss ppm fault levels, and that is only the production aspect, one should also consider the long-term reliability, something the EMS will not care about, as long as it goes trough final test EMS is happy.
We do very detailed solder analysis from time to time,


What does EMS stand for?


Electronic Manufacturing Site

Flextronics etc


I also asume you know your solder screen thickness.
and that you make sure its laser-cut.

And I assume you specify the solder-paste to be used, at least some basic data, alloy, granularity etc.


As i am researching for the official lib we can not really know this sort of thing. We are aware that our footprints might not fit the manufacturing constrains of every user.
So we try to walk a middle ground (as the suggestion for paste is that you split it and have a coverage of between 50 to 80% we aim for somewhere near the middle of this range.)


ok fair enough

i just say that for us that work with this daily, footprints is not a black-magic secret sauce magic filled with rules and other bits and pieces.

soldering is a physical process under laws of nature.

I have problem with about 1 footprint out of 200, so I just fix it and wait until next problematic footprint 200 footprints later down the road and fix that also.

its not a big problem


Yea that is what i gathered from reading different blog posts and from my own experiences. I just want to learn as much as possible (from more experienced people) such that we can provide the best footprints we can under the limitations for the official library.


I would recommend that you define a stencil thickness of 0.1mm (most common) for the public library.

if not already done.

its a fundamental parameter that directly affects the solder-volume.

otherwise you have a 2 dimensional heap of solder and that is no solder at all.


Yes, you can’t make it smaller as that violates clearances, and one hopes the number they spec is actually already a tolerance-max (tho that sort of metal will be very precise anyway).
If you make it larger, you lose some position control, and the other step taken to help self-align is to reduce the paste on the slug, so the part tends to not ‘float on the slug’, but rather ‘floats on the pins’.
Importantly, it avoids one row of pins not quite wetting by floating on/just above the flux.


This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.