Hi,
I am making a footprint for the Nexperia BC847QAS:
Is uses a DFN1010B-6 (SOT1216) package, and the footprint in the datasheet shows the paste area (“solder paste”) being bigger than the pad (“solder land plus solder paste”) itself.
Can this be right?
I think it’s a error in the datasheet (simple mistake in the legend of figure 12 in the datasheet). Compare with a similar part with DFN1010B-6 case (see attached pdf for PMDXB550UNE).
Note that I personally would add two pads (7+8) on the bottom, or at least a copper-rule-out area at the bottom. Running traces under this case only isolated by the pcb stop mask would be too risky for me.
PMDXB550UNE.pdf (720.3 KB)
Thank you,
I only checked similar datasheets, which all seem to have the same typo:
Yes, I actually used a footprint generated with easyeda2kicad as a starting point, which already includes pads 7 and 8.
Well all three of your datasheets are from Nexperia so at least they are consistent in-house. 
I don’t use so small footprints but as in datasheet they don’t suggest these pads I would be afraid whether paste put under this element will lead to shorts. When the element is attracted by surface tension, the paste beneath it will be pushed around.
Yes, this can be right.
It is not very common, but sometimes the aperture in the soldermaks is made bigger then the pad, and this is a valid technique to get more solder paste on a pad. During reflow, the solder will wick onto the pad. You can quite easily find examples on this on youtube for home soldering. For example when manually putting paste on a SOIC footprint, a “sausage” of paste is laid over a row of pads, and as long as the amount of solder per pad is correct, there are no (or very few) solder bridges after reflow.
It also looks plausible to do this with this part, because the pads are very small. Making the pads wider is not an option, because when pads are close together this increases the chance of solder bridges. Making the pads longer is possible, but would also pull the solder away from the place it needs to be, and extending the pads further from the IC may also increase the chance for solder bridges.
But also, you can not take the suggestion for the solder mask in the datasheet too seriously. The thickness of the stencil has a large influence on the amount of paste, and grain size of the solder is also important, especially with such small pads. And neither are mentioned in the datasheet. It is also nearly impossible (and very expensive) to make real sharp corners in the soldermask. Often they are cut with a laser, and this will result in rounded corners with at least the radius of the laser beam. Therefore IPC recommends rounded corners for solder paste apertures. With a specified and thus known radius, the aperture size is better defined, and thus the paste deposit becomes more consistent (for example when ordering stencils from different manufacturers). Rounded corners also help with paste release, and thus further increase consistency.
Another problem I spot is with the solder mask apertures. The datasheet suggest a with of 0.3mm for the solder mask, and with a 0.35mm pitch for the pads this results in 50um wide ridges on the soldermask, and that is probably too thin for most manufacturers.
Because I believe mf_ibfeew’s answer is not correct, I untick it as the solution. If you do prefer his answer, you can set it again and I won’t interfere anymore.
Thanks for the additional information.
I already changed all pads to 25% rounded corners.
Looking at the datasheet for the package itself (https://assets.nexperia.com/documents/package-information/SOT1216.pdf), it seems like the footprint was changed at some point (Issue date: 14-07-28 17-03-31), with the newer version having bigger paste area than pad area. This also matches the footprint dates of the other datasheets, with the older ones having footprint issue date 14-07-28 and the newer ones 17-03-31.
I guess this should go into the PCB’s board setup settings anyways. I assume there is no problem if the solder mask expansion is smaller than suggested if the manufacturer supports it.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.