Better surface mount layout question

[mribble]

I'm having low success rates soldering the a SON-10 package with my boost converter on it.  Part here: http://ca.mouser.com/ProductDetail/Texas-Instruments/TPS61200DRCR/?qs=sGAEpiMZZMtY9G8Xaw%2fcnvufCtuHXcIe

Here is my current pcb layout:



I noticed sparkfun uses a similar chip with a different layout.  There part is here: http://www.sparkfun.com/products/10300



The problem I've having is that the ground plane shorts to some of the pins.  I know adjusting the stencil mask might solve this problem, but I'm wondering if the design by sparkfun has advantages.

Does having ground planes on the top and bottom help prevent board flex during soldering?  Also do those 3 vias under the chip help prevent solder overflow?

In general do people see advantages or disadvantages to the layout used by sparkfun?

[daedalus]

Is there some reason you are not following the manufacturers recommended footprint for this part? They have a recommendation for thermal vias and solder paste coverage that you seem to be ignoring.

The vias are there primarily to conduct heat to the ground plane on the bottom of the board. If they are not capped (i dont use eagle, so am not sure), then they will end up wicking some solder paste through when the part is mounted, but this is more of a side effect.

The problem you are having is most likely that you are applying too much solder paste on the central pad. Having a single aperture for this is problematic, you might be better off splitting this into several smaller apertures, and going for a lower fill ratio. The manufacturer recommends a fill ratio of 72%, but you will probably be ok down to 50%. The lower the fill, the less chance of shorts.

[mribble]

Daedalus,

I haven't used parts where stencil coverage mattered in the past so I kind of glazed over that part of the data sheet while reading it.  I am now taking a very close look at their recommendations in this area and taking them into account with the stencil mask.  Thanks!

[KashmirGR]

For best results:
 - Pad dimensions should follow pin dimension + 0.25-0.75mm toe
 - Soldermask between pads (1:1 with pad, PCB vendor to open.  Do not gang relieve).
 - Solderpaste should be 1:1 with pad, but can be slightly smaller (If you are going to do smaller, use less Y, and leave X 1:1).
 - Solderpaste for exposed pad should be 1:1, with 0.25mm cross pattern (4 solder regions) if pad is greater than 4mmx4mm
 - No PTH in pad, microvia okay.
 - For exposed pad, if you are using PTH via, cap on opposite side.  It is better if you can keep these around the edge and seperate with soldermask from the soldered pad area

Generally speaking, manufacturer recommended footprints will follow the above guidelines.