I use a lot of TSSOP package and I get a lot of solder briding between the pins.
Investigating, currenlty, e.g. for TSSOP14, the pin width is 0.45, while the pitch is 0.65, meaning only 0.2mm clearance, where no solder mask is placed.
I’m using solder paste applied by a stencil and machine placed parts.
Following analogs footprint manual, that 0.45 fits exactly.
I’m thinking to follow on semi recommendations on page 13 with 0.36 to avoid solder bridges.
What are you experiences?
Both of the packages seem to have the exact same dimensions including tolerances. So my guess is analog and on used different standards and or different manufacturing parameters to derive the footprint.
We are currently in the process to convert all official footprints for standard packages away from using manufacturer suggestions for exactly this reason. We now directly use IPC-7351B for calculating the land pattern via our script https://github.com/pointhi/kicad-footprint-generator/tree/master/scripts/Packages/Package_Gullwing__QFP_SOIC_SO You can try and generate the footprint using the script and see what it would do.
The thing to keep in mind is that ipc suggests different fillet sizes depending on if the pitch is larger than 0.625 or smaller than that. So one reason for the difference could be that on used the smaller than 0.625 rules while analog correctly used the one for larger than that.
I verified with a colleague who uses eagle today.
He uses 0.35mm width and the results of his PCBs look fine.
0,5mm pitch is critical but works fine if you use correct stencil and printing parameters. For Gerber output, I narrow the pads (edit Gerber aperture) to about 80%. Pad size of about 0,45mm becomes 0,36mm width (what is equal with recommendations above). Stencils above 120um do not work any more. If you can choose direction, use spatula movement in parallel to the pads long side. Its also critical to have correct temperature and consistence of solder paste must not stick at the stencil edge if you lift up the stencil. Just do some more experiments and you will master this matter nearly perfect. To clarify this again: Stencil aperture needs to be smaller than copper pad size what avoids too much material causing the shorts. This is not possible with pool manufacturers stencil-include offers what do not accept separate Gerber for stencils.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.