nRF52840 aQFN footprint

RE: nRF52840 aQFN footprint

Martin Sivertsen — Mon, 01 Nov 2021 08:04:40 GMT

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.

RE: nRF52840 aQFN footprint

Daisy.hung — Mon, 01 Nov 2021 01:42:23 GMT

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

RE: nRF52840 aQFN footprint

Martin Sivertsen — Fri, 29 Oct 2021 17:55:11 GMT

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.

RE: nRF52840 aQFN footprint

Daisy.hung — Fri, 29 Oct 2021 01:52:32 GMT

Yes, our layout had follow this guidelines, expect for through hole via pad, the design rule require 0.61mm, it is very big size if the two adjacent holes, so we modify the through hole pad size to 0.4mm, and keep mask 0.05mm larger than pad. other normal pad size use 0.275mm and mask open 0.375mm.

RE: nRF52840 aQFN footprint

Martin Sivertsen — Wed, 27 Oct 2021 09:15:40 GMT

Hi,

Removing unused GPIO pads from the PCB layout should not be an issue as long as they are not critical to the function of the nRF52840.

But you shouldn't get shorts under the IC, what size holes are you using for the paste mask?

You can find dimensions and guidelines in the application note nAN40 - Circuit Board Guidelines for aQFN Package here: https://infocenter.nordicsemi.com/topic/nan_040/APP/nan_040/nan40_intro.html?cp=16_1

Here is an excerpt that is relevant to your issue:

The application note also contains guidelines on what type of solder paste to use and the reflow profile to ensure good results.

I hope you find this information helpful.

Best regards,

Martin S.