nRF52840 aQFN footprint

[Daisy.hung]

We used the nRF52840 in some projects, but there are still some problems with the short bridge at the IC during production. 

So we want to leave the blank layout of the unused IO pins.

We still need help from Nordic, do you have any concern or recommend for this? 

[Martin Sivertsen]

Hi,

The size of the pads around the perimeter of the nRF52840 aQFN is 0.275 mm (as you mentioned), and the inner row of pads have blind vias with a hole size of 0.150 mm (which is filled and capped) and a via pad size of 0.350 mm, the only part of the reference layout that has through hole vias is the center pad.

The distance between the center of the pads around the perimeter is 0.500 mm, with a solder mask opening of 0.375 mm around the pads, that leaves a 0.125 mm sliver of solder mask between the pads to act as a solder barrier.

Increasing the solder mask opening to 0.450 mm leaves only a 0.050 mm sliver of solder mask between the pads, if any at all as PCB manufacturers also have minimum solder mask sliver values, this leaves your design very open for solder brides and shorts. Please check if this is the case on your design.

Best regards,

Martin S.

[Daisy.hung]

As your mentioned, the blind vias with a hole size 0.15mm and with pad size 0.35mm, if keep mask increasing open to 0.45mm, so the distance between two pads also leave 0.04mm, or I have an misunderstanding 

[Martin Sivertsen]

Hello,

The solder mask opening is 0.375 on all the pads, both the ones with a blind via and those without.
Here is a picture from Altium Designer to show what it looks like:

Note that the vias in the pads should be filled and capped so they won't have a visible hole on the finished board, like this:

Best regards,

Martin S.