> I was hoping for some convention like this to array soon since I'm making new components for every project and I would love them to follow the KiCad convention so they can be contributed. Carl, could you please upload a document with those conventions that are already decided? Like naming, perhaps.
I do think we are better to make official what we have now, and then continue from there. I have corrected the few points discussed previously with Lorenzo, so the following should be good to go. Are there any other concerns? I would like to commit this in the root of kicad-library directly, in the form of a text file. General Rules: 1. Writing uses C-style naming with the first letter of each word being capitalized. Ex: "Socket_Strip_Straight_2x06" 2. Every acronym has all of its letters capitalized. 3. Manufacturer name is capitalized as usual. Ex: NEC, Microchip 4. Component name must match its filename 5. When dimensions are used in part name, they are in millimeters and unit is not capitalized. Ex: "Cap_10x13mm_RM5" 6. Filename is the same as the part name Symbols: 1. Using a 100mil grid, pin ends and origin must lie on grid nodes (IEC-60617) 2. Pin must have a length of 100mil or more in increments of 50mil if number needs more space 3. Black-box components group pins logically, for example by function set, and ports in counter-clockwise position. 4. Whenever possible, inputs are on the left and outputs are on the right. Footprint Library Names: 1. Part type (resistor, cap, etc), must be in plural form 2. Package type (SOIC, SMD, etc) 3. Manufacturer 4. Part number Footprints: 1. Follows datasheet recommendation unless intentional variation, for example longer pads for hand soldering 2. Pad 1 must be on the left first, then at the top, except at the top for PLCC. (IPC-7351) 3. For through-hole components, origin is set on pad 1. 4. For surface-mount devices, origin is placed in the middle with respect to device lead ends. (IPC-7351) Names for footprints of Surface-Mount Devices (SMD): 1. Specific package feature first, not separated by anything. 2. Package name, numbers separated from letters using hyphen Ex: "SOT-89" 3. Pin number is expanded with '+' sign for extra pads to package, with acronym for type of pad. Ex: Exposed pad under QFP: "QFP-48+1EP" 4. Variation of package, separated by another hyphen. Ex: "SOT-23-5" 5. If it's a manufacturer-specific package, name can be appended, separated by an underscore. 6. Any modification to the original footprint, indicated by appending the reason. Ex: longer pads are used to facilitate hand soldering of a QFN component: "QFN-52_HandSoldering" Names for footprints of common devices, such as resistors, capacitors, etc: 1. Name of part, may be shortened for common components. ex: "Cap", "Socket_Strip", etc. 2. Dimension, which may include at its end the positioning. Ex: "TO-220_Horiz", "1x02_Angled" 3. Pad distance, in the form of an RM rating. 4. Any modification to the original footprint, indicated by appending the reason. Names for footprints of specific devices: 1. Name of part. 2. Part number. Ex: "Oscillator_SI570" 4. Any modification to the original footprint, indicated by appending the reason. On Tue, Apr 29, 2014 at 4:22 AM, Lorenzo Marcantonio < [email protected]> wrote: > On Tue, Apr 29, 2014 at 10:14:41AM +0200, Mariusz Radzimirski wrote: > > As most of symbols have pins created using grid 100 (2x50), it is > reasonable > > to use grid 100 when drawing wires on schematic. > > It's a one-liner. Actually TWO lines. One in sch_screen.cpp and one > wherever the ID_POPUP values are defined. However care should be taken, > read the comment at the begin of the definition. > > > BTW, I think there should be possibility to use user defined grid size in > > Eeschema instead of predefined few grid sizes. It would solve the > problem. > > Seems overkill to me, especially in the view of the future LU stuff. > > -- > Lorenzo Marcantonio > Logos Srl > > _______________________________________________ > Mailing list: https://launchpad.net/~kicad-developers > Post to : [email protected] > Unsubscribe : https://launchpad.net/~kicad-developers > More help : https://help.launchpad.net/ListHelp > On Tue, Apr 29, 2014 at 4:22 AM, Lorenzo Marcantonio < [email protected]> wrote: > On Tue, Apr 29, 2014 at 10:14:41AM +0200, Mariusz Radzimirski wrote: > > As most of symbols have pins created using grid 100 (2x50), it is > reasonable > > to use grid 100 when drawing wires on schematic. > > It's a one-liner. Actually TWO lines. One in sch_screen.cpp and one > wherever the ID_POPUP values are defined. However care should be taken, > read the comment at the begin of the definition. > > > BTW, I think there should be possibility to use user defined grid size in > > Eeschema instead of predefined few grid sizes. It would solve the > problem. > > Seems overkill to me, especially in the view of the future LU stuff. > > -- > Lorenzo Marcantonio > Logos Srl > > _______________________________________________ > Mailing list: https://launchpad.net/~kicad-developers > Post to : [email protected] > Unsubscribe : https://launchpad.net/~kicad-developers > More help : https://help.launchpad.net/ListHelp >
_______________________________________________ Mailing list: https://launchpad.net/~kicad-developers Post to : [email protected] Unsubscribe : https://launchpad.net/~kicad-developers More help : https://help.launchpad.net/ListHelp
