I am using some standard 5mm screw terminal blocks for a simple design at low voltages (less than 20V).
The datasheet does not have a standard footprint for the device.
The pin itself has a diameter of 1.3mm, so I was thinking a hole size of 1.5mm, with a solder pad surrounding the hole of 1mm.
There's no real science in choosing these dimensions. What considerations should be given to choosing the pad size? If so, what pad size is best?
Best Answer
According to IPC-7251, IPC-2222 and IPC-2221 standards:
Minimum Hole Size is calculated according to equations below:
Minimum Hole Size = Maximum Lead Diameter + 0.25mm (for Level A of IPC-2222)
Minimum Hole Size = Maximum Lead Diameter + 0.20mm (for Level B of IPC-2222)
Minimum Hole Size = Maximum Lead Diameter + 0.15mm (for Level C of IPC-2222)
note:
Minimum Pad Diameter is calculated according to equations below:
Pad Diameter = Minimum Hole Size + Minimum Annular Ring X 2 + Minimum Fabrication Allowance
Minimum Annular Ring is 0.05mm (50um).
Pad Diameter = Minimum Hole Size + 0.1mm + 0.60mm (for Level A of IPC-2221)
Pad Diameter = Minimum Hole Size + 0.1mm + 0.50mm (for Level B of IPC-2221)
Pad Diameter = Minimum Hole Size + 0.1mm + 0.40mm (for Level C of IPC-2221)
Density Level A is used for General Design Producibility. It is a Preferred Level. Level A is used for the Low component density. In this case, footprint geometry is ‘Maximum’. This method is applied to the most robust producibility.
Density Level B is used for Moderate Design Producibility. It is a Standard Level. Level B conditions are suitable for re?ow, wave, drag or dip soldering. In this case, footprint geometry is ‘Median’. This method provides a robust solder attachment conditions.
Density Level C is used for High Design Producibility. It is a Reduced Level. Level C is used for the High component density. In this case footprint geometry is ‘Minimum’. This method is applied to a hand-held and portable appliances.