KLC S5.2 Footprint-Filters Question: Exposed Pad

[cpresser]

Can anybody please clarify why we don't include the EP size in the Footprint-Filter? @KiCad/librarians

From KLC S5.2

Neither the size of the exposed pad nor the size of the mask cutout are included.

But this contradicts

They should be designed to result in no false suggestions.

---

I am currently working on KiCad/kicad-symbols#2336. The contributor did not add the EP-Size to the filter, which matches the rule.
But that will lead to false suggestions. If the user selects the wrong EP-Size for the footprint proper reflow-soldering is not ensured.

[chschlue]

I think its so the filter matches SMD variants which are named EP<actual copper dimensions>_Mask<exposed copper dimensions>, but I can't make any real sense of this rule either.

I'd really love to hear the actual reason we have it on the books.

[evanshultz]

We made the EP size a user choice. By default, a symbol is assigned the footprint with a thermal pad size that we believe is correct. But the user may choose some other footprint for their specific board. If the outer pads aren't correct there could be soldering issues, but changing the thermal pad size doesn't guarantee soldering issues depending on the assembly process.

This flexibility comes from something like using a trailing asterisk on the FP filter so that a user could utilize just the symbol libs and use their own footprint libs. It's flexibility. A user might have variations of our footprints to suit their process or philosophy, and the FP filter allows leeway to choose alternate footprints which may be seen as less than ideal. Using an alternate EP size is one of those options. It's easy to think of many others, like a different body size in box caps if the lead pitch matches or different lead pitch on an axial resistor. The user may use our footprint library as a starter for their own footprints, or create their own footprints from scratch but use our symbol library since KiCad gives the flexibility of having an interface between symbols and footprints.

If the manufacturer gives a footprint then we will use the thermal pad size given, with the EP_size_overwrite parameter in the generator script. But if there is no guidance we use the thermal pin size for the pad size. (Personally, I would ignore the thermal pad size in all cases since we really have no reason to believe any manufacturer knows what they're doing in this regard. Trust me, it's shocking how little many of them know.)

Some odd package designs, like the TI ones mentioned above with a smaller mask cutout, were noticed after we'd already started the policy above and fit into it. But that wasn't the impetus. I believe @Ratfink was the one who pointed that out, but I could be wrong and I didn't find the history anywhere with a quick search. The term "ep size" in the footprints' Issues page turns up some discussions which I'm sure are relevant but I didn't read each thread. Rene may recall more.

This ultimately all comes from IPC not giving a recommendation on how to size the thermal pad and not finding any authoritative source for this. I recall a TI paper with results of reflow soldering various footprints, but it wasn't to the level of the IPC docs. So we are otherwise using IPC rules for the land pattern but there aren't any rules (we found) for the thermal pad size.

It just now occurs to me that IPC has a land pattern calculator software which we could perhaps use and see what comes out. I think it's free but I don't recall. Regardless, leaving off the EP size means we specify a default footprint in which we have high confidence will work in most assembly applications but also gives flexibility to users if they want to forge their own path.