Soldermask Expansion on DFN Footprints

Recently I've spent some time redesigning the PCB I had made to test out the MCP9808 temperature sensor from Microchip.  I'm satisfied I can solder the small footprint DFN packages without too much hassle.  This then allows me to remove the large footprint components and arrange the board the way I want, so that it satisfies some mechanical constraints.  I basically want to water proof the board and provide strain relief for the cables.

In the process of redesigning the board, I tidied up the footprints and thought it would be a good opportunity to talk about solder mask expansion.  Solder mask on a PCB is there for a couple of reasons, it provides the underlying traces some protection from the environment, but what I'm mainly interested in is its ability to prevent bridges between pins during soldering.  In an ideal world you'd design the solder mask so that it only exposes parts of the board that you want to solder, but due to inaccuracies in manufacturing you need to make the holes in the solder mask slightly larger than needed to account for things like misalignment and shrinkage.  This means that even if there are alignment issues, the whole of the pad is still exposed.  The amount that the openings are increased is called the solder mask expansion.

Typically you'd want an expansion of 5 mil to be safe, but in certain instances you have to have a smaller amount.  For example the DFN component below has no expansion.  The red line indicates the space between pads, 0.2 mm, and the green line indicates the pad width 0.3 mm.  The black area is solder mask, and the light green areas are pads.

DFN Footprint - No solder-mask expansion

In the image below, after a 5mil (blue line) solder mask expansion is applied, all of the solder mask between the pads disappears, which is a valid way of doing things called a gang solder mask, but it's not what I'm after.  I'm experimenting and trying to figure out the pros and cons of different methods.  The dull green area is bare board, the black area is solder mask, and the light green areas are pads.

DFN Footprint - 5 mil solder-mask expansion

To make sure that there's solder mask between the pads, the expansion needs to be decreased.   When doing this, another requirement needs to be met, the minimum-solder mask web.  If the slivers of solder-mask between pads are too thin they'll lift off and cause problems during manufacturing.  A safe minimum value for this parameter would be 5 mil.  This means that the solder-mask expansion in the diagram below has to be smaller than about 1.4 mil (blue line) to allow the black section of soldermask in between the pads to be wider than 5 mil.

DFN Footprint - 1.4 mil solder-mask expansion

Using a solder mask expansion of 1.4 mil is less than optimal.  Ideally an expansion of 5 mil would be better.  Ultimately it all depends on the capabilities of the board manufacturer.  If there is good alignment of the solder mask with the copper layer it doesn't really matter.  I'm considering doing two runs of the board, one with an expansion of 5 mil and one with an expansion of of 1.4 mil, the boards don't cost a lot, so it's a cheap way to learn and get some experience.