Library Conventions | KiCad EDA

Version 3.0.45

Library maintainer rules & guidelines

F3.4 SMD IC package naming conventions

The following footprint naming conventions should be used as examples for naming SMD IC package footprints.

If you do not find an appropriate convention that matches a particular footprint type, either contact the KiCad library team or try to match a convention set by existing library components.

In the entries below, variable fields are denoted as follows:

- Fixed fields
- Mandatory fields
- Optional fields

Gullwing Packages

The format below provides a guide for naming Gullwing IC packages.

Examples:

  • SOIC

  • SOP

  • QFP

  • J-Lead

[PKG]-[Pin count]-[EP Qty]EP_[X]x[Y]x[Z]_P[Pitch]_[Modifiers]_[Options]
  • PKG - Package name
  • Pin count - Number of (unique) pins
  • EP Qty - Number of exposed pads under the device (if greater than zero) (Optional)
  • X - Major dimension of part on x axis
  • Y - Major dimension of part on y axis
  • Z - Major dimension of part on z axis (Optional)
  • Pitch - Lead pitch
  • Modifiers - Footprint modifiers (Optional)
  • Options - Extra footprint options (Optional)

Example:

SOIC-16[-][1][EP][_][3.9][x][9.9mm][_][P][1.27mm]

Notes:

  1. [PKG] - refers to the name most commonly used in the industry. Generally this implies JEDEC naming but some other standard may be used as required.

  2. [Pin count] - the number of uniquely numbered pads (excluding any exposed pads under the device)

  3. [Modifiers] - may vary for individual IC footprint types. Includes:

    • Clearance

    • Lead size

    • Pad size

    • Exposed pad size

    • Soldermask expansion

No-Lead Packages

Examples:

  • DFN

  • QFN

  • LCC

[PKG]-[Pincount]-[EP Qty]EP_[X]x[Y]x[Z]_P[Pitch]_[Modifiers]_[Options]
  • PKG - Package name
  • Pincount - Number of (unique) pins
  • EP Qty - Number of exposed pads under the device (if greater than zero) (Optional)
  • X - Major dimension of part on x axis
  • Y - Major dimension of part on y axis
  • Z - Major dimension of part on z axis (Optional)
  • Pitch - Lead pitch
  • Modifiers - Footprint modifiers (Optional)
  • Options - Extra footprint options (Optional)

Example:

DFN-12[-][1][EP][_][4][x][4][x][0.9mm][_][P][0.5mm]

Notes:

  1. The lead length is the nominal lead length for which the footprint is designed

  2. Optionally the nominal lead width can also be provided

Ball Grid Array Packages

[PKG]-[Pincount]_[X]x[Y]x[Z]_Layout[Columns]x[Rows]_P[Pitch X]x[Pitch Y]_Ball[Ball]_Pad[Pad]_[NSMD/SMD]_[Modifiers]_[Options]
  • PKG - Package name
  • Pincount - Number of (unique) pins
  • X - Major dimension of part on x axis
  • Y - Major dimension of part on y axis
  • Z - Major dimension of part on z axis (Optional)
  • Columns - Number of ball columns
  • Rows - Number of ball rows
  • Pitch X - Ball pitch in x direction
  • Pitch Y - Ball pitch in y direction (if different from x direction (Optional)
  • Ball - Ball diameter
  • Pad - Pad diameter
  • NSMD/SMD - Solder Mask Defined or Non Solder Mask Defined
  • Modifiers - Footprint modifiers (Optional)
  • Options - Extra footprint options (Optional)

Example:

BGA-24[_][3.2][x][4.4mm][_][Layout][3][x][4][_][P][0.5mm][_][Ball][0.25mm][_][Pad][0.2mm][_][NSMD]

Notes:

  1. For BGA simply providing the pin count is not sufficient. It is also necessary to provide the number of [Columns] (x direction) and [Rows] (y direction).

  2. Some BGA packages have different pitch in x and y directions. If this is the case then both [Pitch] dimensions need to be provided

  3. The [Ball] diameter for which the footprint is designed needs to be provided

  4. [NSMD/SMD]

    • NSMD means the footprint is designed for non solder mask defined (mask cutout is larger than copper pad)

    • SMD means the footprint is designed for solder mask defined (mask cutout is smaller than copper pad)


Edit on GitLab