Issue link: https://iconnect007.uberflip.com/i/1529118
20 DESIGN007 MAGAZINE I NOVEMBER 2024 • Avoid using less than 3-mil trace or space without checking with the PCB fabricator. Less than 3-mil trace or space is oen con- sidered an advanced capability for most fabricators and will affect yields and costs. • Do not design silkscreen (legend) text less than 40 mils in height and 4 mils in width. It can become illegible and/or difficult to produce. • Most 0.8 mm pitch BGAs will not meet Class 3 via requirements using through- hole technology. e annular rings are not wide enough for Class 3, unless laser drill- ing is used. • 3-mil webbing must always be maintained between component pads, otherwise use gang mask. • Exotic colored solder-masks typically have different properties and higher/greater manufacturing tolerances (up to ±5 mils vs. the standard ±2 mils). • Always pull the solder mask greater than 10 mils from the board outline. • Solder-mask is typically about 0.7 mils thick. • Fabricators will typically increase all sol- der-mask features 2 mils over pad size if given to them at 1:1 scale. • PCBs are etched by dielectric core layer pairs. Try to balance the copper weight on the stackup between dielectric cores when possible, to ensure consistent copper etch- ing. icker copper weight takes longer to etch, so a mismatch can cause problems if one side is thinner. • Try to evenly distribute copper over as much surface area on all layers of a PCB as possible. Add GND backfill if possible. is practice allows the fabricator to only etch away a smaller percent of copper vol- ume, resulting in more consistent etch and final copper thickness. It also helps main- tain board rigidity and coplanar lamination press. • Outer layers and vias will also plate more uniformly if copper is evenly distributed and balanced over the entire surface of the PCB. If there are areas absent/void of cop- per, the fabricator will typically add thiev- ing at their discretion. Assembly • Place all through-hole component types on same side of board. is minimizes assembly profile and cost. • Keep all heavy/tall components on the same side of the PCB. is prevents them from falling off during reflow. • Don't use via-in-pad for BGA pads, even if filling vias with epoxy and planarizing. ere are still bumps and depressions that can cause assembly issues. • Use placement courtyards to keep proper distance between components for assem- bly pick-and-place machines. is will avoid DFM issues. • Do not place short components in between two much taller components. is can prevent proper solder reflow and hinder rework.