tztz
/
KicadLib
1
0
Fork 0
Code Issues Pull Requests Releases Wiki Activity

Merge pull request #686 from SchrodingersGat/remove_klc.txt 

Removed KiCad_Library_Convention.txt
This commit is contained in:
CarlPoirier 2016-09-09 21:34:10 -04:00 committed by GitHub
parent 0d35ffb12c b496cdf984
commit 7ad7ce3e8d
1 changed files with 0 additions and 162 deletions
Show Stats Download Patch File Download Diff File Expand all files Collapse all files

162
KiCad_Library_Convention.txt
View File

@ -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