Buck inductor land pattern?

[cupoftea]

Hi,
The 74477820 inductor by wurth has a simple footprint in the datasheet

https://www.we-online.com/components/products/datasheet/74477820.pdf

..but in the board we got sent, the footprint is as in the attached...ie, matching the
bottom metalwork, or so it seems.
Which pad pattern is best here?
Its being used in a 20V to 5V Buck

 

[Easy peasy]

If your soldering processes are up to it - and you don't have a L<->R error - then the extant copper should be fine

 

[FvM]

If you look sharp a component side view, only rectangular pads are touching the PCB. Extra copper most likely won't solder. Post #1 landing pattern looks inappropriate to me.

 

[mtwieg]

Absolu

..but in the board we got sent

Send it back.

I'm guessing you contracted out board/footprint design. Looks like somebody went to a lot of trouble to ignore the manufacturer recommendation. That person has probably never seen an inductor in person before.

IMO something like this would have me looking for another contractor.

 

[cupoftea]

Thanks, i guess the issue of the post #1 land pattern is all the solder paste slopping about on that big (raised) pad which isnt even soldered in?
The recomended pads do look uneccesarily small.....could be bigger and give more copper pour cooling effect?

 

[mtwieg]

The recomended pads do look uneccesarily small.....could be bigger and give more copper pour cooling effect?

Maybe, but that extra copper should not be part of the footprint itself. Should be left to the board designer to add extra copper shapes as they see fit. The soldermask openings should not be expanded beyond the manufacturer's recommendations.

 

[marce]

Nope use the Wurth define4d footprint, if extra copper is needed, then add it during the design cycle, you will then get a solder mask defined pad... Never seen a footprint like the one shown and would kick the ass on any so called PCB designer who presented one like that to me...
On the mounting layer, there should be NO copper under the inductor apart from the pads...
All that copper is connected to the high di/dt loop, so will cause EMC and signal integrity issues...

 

[cupoftea]

Thanks, that sounds good, though the customer just tells me that the big "diagonal" pad shape of the top post actually solders to the metal on the inductor anyway, even though it is slightly raised, and says its got good heatsinking properties to do it like that....because the actual soldering of that bottom metalwork to the PCB copper offers best heatsinking. IMHO, i tend to agree that the recomended pad with any extra copper done with solder mask over it sounds better.
They have been doing it like the top post for years and not had problems so they say.

 

[cupoftea]

Thanks, and as you rightly purport, high di/dt tracks need low loop area, high dv/dt tracks need low copper area.

 

[FvM]

customer just tells me that the big "diagonal" pad shape of the top post actually solders to the metal on the inductor anyway, even though it is slightly raised

It's raised 0.20 mm according to .stp model and can't solder completely unless you use extra thick solder stencil, hardly compatible with other components on the PCA.