bolay.co 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.

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.

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”

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.

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”

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.