User Tools

Site Tools

pcb_guideline Library Convention

From Kicad Library Convention 0.8 - 19.01.2015

General Rules

  • Writing uses C-style naming with the first letter of each word being capitalized. Ex: “Socket_Strip_Straight_2x06”
  • Every acronym has all of its letters capitalized.
  • Manufacturer name is capitalized as usual. Ex: NEC, Microchip
  • When dimensions are used in part name, they are in millimeters, decimal places separated by a dot, and unit is not capitalized. Ex: “Cap_10x13mm_RM5”
  • Filename is the same as the part name.
  • The order of elements in names must be the same as the enumerations presented in this document.

Symbol Library Names

  • Manufacturer.
  • Category or family of parts. ex: “Capacitors”, “Spartan6”, etc.

General Rules for Symbols

  • Using a 100mil grid, pin ends and origin must lie on grid nodes (IEC-60617).
  • Pin has a length of 100mil or more in increments of 50mil if number needs more space.
  • Origin is placed in the middle of symbol.
  • Black-box components group pins logically, for example by function set, and ports in counter-clockwise position.
  • Whenever possible, inputs are on the left and outputs are on the right.
  • Field text uses a common size of 50mils.
  • The reference field is prefilled with the reference designator of the symbol (IEEE 315-1975).
  • The Value field is prefilled with the object name.

Symbol Names

  • Name of symbol, may be shortened for common components or use reference designator of the symbol (IEEE 315-1975). ex: “Conn_4x2”, “C”, etc.
  • Manufacturer.
  • Part number, including extension for specific footprint. (JEDEC for common devices, ex: 1N4001)
  • Any modification to the original symbol, indicated by appending the reason. Ex: different pin ordering: “Transistor_PNP_Pinswap1”
  • Indication of quantity if symbol is an array. ex: resistor array: “Resistor_x8”

Footprint Library Names

  • Part type (resistor, cap, etc), must be in plural form.
  • Package type (SOIC, SMD, etc).
  • Manufacturer.
  • Part number.

General Rules for Footprints

Footprint tutorial :

  • Follows datasheet recommendation unless intentional variation, for example longer pads for hand soldering.
  • Pad 1 is on the left first, then at the top, except at the top for PLCC (IPC-7351).
  • For through-hole components, footprint anchor is set on pad 1.
  • For surface-mount devices, footprint anchor is placed in the middle with respect to device lead ends. (IPC-7351)
  • Silkscreen is not superposed to pads, its outline is completely visible after board assembly, uses 0.15mm line width and provides a reference mark for pin 1. (IPC-7351)
  • Courtyard line has a width 0.05mm. This line is placed so that its clearance is measured from its center to the edges of pads and body, and its position is rounded on a grid of 0.05mm.
  • Courtyard clearance is 0.25mm except for components smaller than 0603 at 0.15mm, connectors, SMD canned capacitors and crystals at 0.5mm and BGA at 1.0mm. (IPC-7251, IPC-7351B)
  • Cannot be duplicated to match a different pin ordering. This is to be handled in the symbol libraries.
  • Footprint name must match its filename. (.kicad_mod files)
  • The value and reference designator must be placed on silkscreen.

Names for footprints of Surface-Mount Devices (SMD)

  • Specific package feature first, not separated by anything. Ex: “TSSOP”
  • Package name, numbers separated from letters using hyphen. Ex: “SOT-89”
  • Variation of package, separated by another hyphen. Ex: SOT-23 with 5 pins: “SOT-23-5”, Exposed pad under package: “QFP-48-1EP”
  • If it's a manufacturer-specific package, name can be appended, separated by an underscore.
  • Any modification to the original footprint, indicated by appending the reason. Ex: longer pads used to facilitate hand soldering of a QFN component: “QFN-52_HandSoldering”

Names for footprints of common devices, such as resistors, capacitors, etc

  • Name of part, may be shortened for common components. ex: “Cap”, “Socket_Strip”, etc.
  • Dimension, which may include at its end the positioning. Ex: “5x7mm_Horiz”, “1x02_Angled”
  • Pad distance, in the form of an RM rating.
  • Any modification to the original footprint, indicated by appending the reason.

Names for footprints of specific devices

  • Name of part.
  • Part number. Ex: “Oscillator_SI570”
  • Any modification to the original footprint, indicated by appending the reason.
pcb_guideline.txt · Last modified: 2015/02/09 17:03 by sdolt