Issue link: https://iconnect007.uberflip.com/i/1534120
APRIL 2025 I DESIGN007 MAGAZINE 39 to place the via under the solder mask. is keeps the integrity of the solder joint and tents the via (at no extra via fill expense) and reduces resistance. › Vias in SMD pads must be filled with a conductive material. Solder won't stick to a non-conductive surface. Even using a microvia, it is important to have them filled with a conductive material to keep the surface level. Do not count on plating to fill these vias. ey don't plate for that long. (Note: Plating vias shut is a myth. It never happened. at was actually HASL in those holes back in the olden days.) • Copper flooding component pins: Referred to as a solder mask defined (SMD) foot- print. is creates a few assembly issues. › Due to solder mask expansion done at fabrication (for alignment purposes) the "pad" area is now much larger than recommended. e solder can't fill the larger area, and the component pin becomes solder starved. ¤ Make a note to the fabricator and assembler to keep these areas defined "as is" in your design. Add details to your fabri- cation and assembly drawings to identify these areas. › When solder mask is controlled and enough solder is present, be sure the connection to the plane doesn't become a heat sink. Planes draw heat away and will create a quick cooling of the sol- der joint. Ceramic components will oen crack due to the CTE stresses on the component. ¤ Strap into these pins or only flood half the pin to allow the solder to cool prop- erly without creating extra impedance near the pad with typical relief meth- ods. See Figures 2 and 3. • Note on flooding: No more current will enter the component pin from a large cop- per area than what that pin can handle. Adding more copper won't make it better. › A BGA with flooded pins ends up with some of the pins not getting enough solder, the BGA ball doesn't collapse properly, and you can't unsolder it to fix any opens or shorts. FYI: BGAs do not dissipate heat through the pins. Don't flood them. › rough-hole component pins con- nected to GND do not need to con- nect on every layer. If they do not have "relief," they either never get a good sol- der joint or become impossible to both Figure 2: Wrong way: Green denotes solder mask clearance. Figure 3: Right way.