# Why would metal from a pad be *underneath* the solder mask in a footprint specification?

One of TI's new regulators has a rather unusual footprint, with several pads (7-13 in this instance) requiring that the pad metal extend under the solder mask.

This is in contrast to the usual case where the solder mark starts some distance outside the pad, as is the case of pads 1-6, 14 and 15 in this instance.

What would be the purpose of having a footprint designed like this? My guess would be heat dissipation, but it would be far more common to have a centre pad in this instance.

• I don't think it makes sense for heat dissipation. My guess would be for manufacturing this gives more consistent results. – PlasmaHH Sep 5 '16 at 11:30
• Is there something to do with registration going on here: that the actual pattern produced may vary as the mask and metal don't line up exactly, or the mask openings produced are slightly larger than specced? – pjc50 Sep 5 '16 at 14:21
• Anything that moves away from an unaccessible center pad is great though. – Passerby Sep 5 '16 at 21:26

There are two ways of defining the "active" area of a surface mount footprint: SMD and NSMD - that is Solder Mask Defined and Non-Solder Mask Defined.

It is unusual to see both in one footprint, but certainly not impossible.

SMD pads effectively have a raised lip around the edge of the pad. This at times can have an advantage over NSMD pads for a couple of reasons:

1. It can create an insulating seal around the pads reducing the possibility of solder bridges forming during re-flow
2. It increases the mechanical strength of the pad since the mask helps hold it down
3. It limits the surface tension pull-down of the component on large pads

Looking at the current rating of the internal switches (3.6A) and the device pinout, the use of soldermask defined and non-soldermask defined pads seems to be correlated with one thing: the high-current paths. Control/status/feedback are all NSMD and referenced to the NSMD GND pad. The input, output, and inductor pads are referenced to PGND and are SMD. I conjecture that since pads 7 to 13 are on high-current paths, the footprint recommendation designer expected the pads to be connected to wide, heavy traces that could consume additional paste if NSMD pads were used. Thus, these pads are intended to have SMD openings to ensure consistent copper land sizes.
With the switched inductor being on connected using the other side of the circuit board, the enlarged copper area to hold the vias for L1 and L2 would likely reduce the success rate for soldering those pads because the paste would spread over a larger copper area than desired. Thus, SMD openings for these pads contains the flowing solder and could reduce the defect rate for this component.