KLC F6.3

Pad requirements for SMD footprints

Surface mount pads have specific requirements for PCB design.

  1. By default, pads for SMD footprints should use only the following layers

    1. F.Cu - Front copper

    2. F.Mask - Front soldermask

    3. F.Paste - Front solderpaste (stencil openings)

  2. If SMD pads are placed on the back of the PCB, then the following layers should be used:

    1. B.Cu - Back copper

    2. B.Mask - Back soldermask

    3. B.Paste - Back solderpaste (stencil openings)

  3. Pads with specific stencil aperture design requirements require special attention (see details below)

Many components (IC packages in particular) have specific design requirements for solderpaste (stencil) design. These requirements are often found in the footprint datasheet or an associated technical document.

Most often, custom stencil openings are required for the exposed pads on large IC packages to reduce the amount of solderpaste that is applied during stencil application.

The image below shows an example stencil design found in a footprint datasheet. The superimposed blue square represents the shape of the exposed copper pad. The green squares are the required openings in the stencil.

Custom stencil openings are accommodated as follows:

  1. Construct copper shape with pad(s) with only copper layers (F.Cu and/or B.Cu) as appropriate. These copper pads should not have the F.Paste or B.Paste layers checked.

  2. Add stencil opening(s) with pad(s) which only use solderpaste layers (F.Paste and/or B.Paste) as required. These pads do not have a pad number.

  3. The solderpaste should cover between 50% and 80% of the soldermask free pad area.

Result: (note: this footprint does not correspond to the example shown above)