From b496cdf984dca96e5b75d9a58306c413ee684b53 Mon Sep 17 00:00:00 2001 From: Oliver Date: Sat, 10 Sep 2016 09:33:20 +1000 Subject: [PATCH] Removed KiCad_Library_Conventiontxt This is a duplicate of the information already on the wiki (https://github.com/KiCad/kicad-library/wiki/Kicad-Library-Convention) it is better to make any changes to the official wiki page as users are already directed there via the contributing.md file --- KiCad_Library_Convention.txt | 162 ----------------------------------- 1 file changed, 162 deletions(-) delete mode 100644 KiCad_Library_Convention.txt diff --git a/KiCad_Library_Convention.txt b/KiCad_Library_Convention.txt deleted file mode 100644 index 0e4ed1ac..00000000 --- a/KiCad_Library_Convention.txt +++ /dev/null @@ -1,162 +0,0 @@ -KiCad Library Convention -======================== -Revision 1.0, November 15th 2015 -Devised by Carl Poirier -With help from members of: -kicad-lib-committers@lists.launchpad.net -kicad-developers@lists.launchpad.net - - -1. General Rules ----------------- - -1.1. Writing uses C-style naming with the first letter of each word being capitalized. Ex: "Socket_Strip_Straight_2x06" -1.2. Every acronym has all of its letters capitalized. -1.3. Manufacturer name is capitalized as usual. Ex: NEC, Microchip -1.4. When dimensions are used in part name, they are in millimeters, decimal places separated by a dot, and unit is not mentioned. Ex: "C_Rect_L13_W4_P10" -1.5. Filename is the same as the part name. -1.6. The order of elements in names must be the same as the enumerations presented in this document. -1.7. Reference fields are prefilled with the reference designator of the part (IEEE 315-1975). - - -2. Symbol Library Names (.lib files) ------------------------------------- - -2.1. Manufacturer. -2.2. Category or family of parts. ex: "Capacitors", "Spartan6", etc. - - -3. General Rules for Symbols ----------------------------- - -3.1. Using a 100mils grid, pin ends and origin must lie on grid nodes (IEC-60617). -3.2. For black-box symbols, pins have a length of 100mils. Large pin numbers can be accommodated by incrementing the width in steps of 50mil. -3.3. Origin is placed in the middle of symbol. -3.4. Black-box components group pins logically, for example by function set, and ports in counter-clockwise position. -3.5. Whenever possible, inputs are on the left and outputs are on the right. -3.6. Field text uses a common size of 50mils. -3.7. The Value field is prefilled with the object name. -3.8. Description and keywords properties contain the relevant information. - - -4. Symbol Names ---------------- - -4.1. Name of symbol, may be shortened for common components or use reference designator of the symbol (IEEE 315-1975). ex: "Conn_4x2", "C", etc. -4.2. Manufacturer. -4.3. Part number, including extension for specific footprint. (JEDEC for common devices, ex: 1N4001) -4.4. Any modification to the original symbol, indicated by appending the reason. Ex: different pin ordering: "Transistor_PNP_Pinswap1" -4.5. Indication of quantity if symbol is an array. ex: resistor array: "Resistor_x8" - - -5. Footprint Library Names (.pretty repositories) -------------------------------------------------- - -5.1. Part type (resistor, cap, etc), must be in plural form. -5.2. Package type (SOIC, SMD, etc). -5.3. Manufacturer. -5.4. Part number. - - -6. General Rules for Footprints -------------------------------- - -6.1. Follows datasheet recommendation unless intentional variation, for example longer pads for hand soldering. -6.2. Pad 1 is on the left first, then at the top, except at the top for PLCC (IPC-7351). -6.3. For through-hole components, footprint anchor is set on pad 1. -6.4. For surface-mount devices, footprint anchor is placed in the middle with respect to device lead ends. (IPC-7351) -6.5. 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) -6.6. 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. -6.7. 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) -6.8. Cannot be duplicated to match a different pin ordering. This is to be handled in the symbol libraries. -6.9. Value and reference have a height of 1mm. - - -7. Names for footprints of Surface-Mount Devices (SMD) ------------------------------------------------------- - -7.1. Specific package feature first, not separated by anything. Ex: "TSSOP" -7.2. Package name, numbers separated from letters using hyphen. Ex: "SOT-89" -7.3. Variation of package, separated by another hyphen. Ex: SOT-23 with 5 pins: "SOT-23-5", Exposed pad under package: "QFP-48-1EP" -7.4. If it's a manufacturer-specific package, name can be appended, separated by an underscore. -7.5. 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" - - -8. Names for footprints of common devices, such as resistors, capacitors, etc ------------------------------------------------------------------------------ - -8.1. Name of part, may be shortened for common components. ex: "Cap", "Socket_Strip", etc. -8.2. Dimension, which may include at its end the positioning. Ex: "5x7mm_Horiz", "1x02_Angled" -8.3. Pad distance, in the form of an RM rating. -8.4. Any modification to the original footprint, indicated by appending the reason. - - -9. Names for footprints of specific devices -------------------------------------------- - -9.1. Name of part. -9.2. Part number. Ex: "Oscillator_SI570" -9.3. Any modification to the original footprint, indicated by appending the reason. - - -10. Footprint properties ------------------------- - -10.1. Footprint name must match its filename. (.kicad_mod files) -10.2. Doc property contains a full description of footprint. -10.3. Keywords are separated by spaces. -10.4. Value is filled with footprint name and is placed on the fabrication layer. -10.5. Attributes is set to the appropriate value, see tooltip for more information. -10.6. All other properties are left to default values. (Move and Place: Free; Auto Place: 0 and 0, Local Clearance Values: 0) -10.7. 3D Shape ".wrl" files are named the same as their footprint and are placed in a folder named the same as the footprint library replacing the ".pretty" with ".3dshapes". - - -Changelog ---------- - - Revision 1.0, November 15th 2015 - 1. Fixed some repetition. - 2. Added rule 3.8 from the checklib scripts. - 3. Tagged as 1.0 for the KiCad 4.0.0 release. - - Revision 0.11, April 6th 2015 - 1. Updated rule 1.4 about dimensions. Units in millimeters are now implicit. - - Revision 0.10, March 1st 2015 - 1. Moved the footprint value property to the fabrication layer - 2. Pin length is enforced only for black-box symbols - 3. Some reorganization has been done. - - Revision 0.9, February 14th 2015 - 1. Added section and rules about footprint properties - 2. Specified the path to 3d models - 3. Moved the reference fields rule to the general section - - Revision 0.8, January 19th 2015 - 1. More thorough rule about courtyard has been split over 6.6 and 6.7. - - Revision 0.7, September 18th 2014 - 1. Added rule 6.6 for courtyard - - Revision 0.6, September 14th 2014 - 1. Specified in 6.9 that value and reference designators must be placed on silkscreen. - - Revision 0.5, August 6th 2014 - 1. Specified in 6.5 that only the outline must be completely visible after assembly. - 2. Rule 3.8 moved from section 1 since it pertains only to symbols. - - Revision 0.4, July 30th 2014 - 1. Completion of convention for symbols. - 2. Rule 6.7 moved from section 1 since it pertains only to footprints. - - Revision 0.3, June 8th 2014 - 1. Specified that pin ordering duplicates are to be handled in symbol libraries. - 2. Specified the rules for footprint silkscreen. - - Revision 0.2, May 19th 2014 - 1. Minor clarifications to few items. - 2. Exposed pad is now considered as a variation of a package, thus separated by hyphen instead of plus sign. - 3. Added 2-level numbering. - - Revision 0.1, May 8th 2014 - 1. Initial Commit