kicad-developers team mailing list archive

[Wayne Stambaugh <stambaughw@xxxxxxxxxxx>]

On 5/1/2014 2:47 PM, Carl Poirier wrote:
>> 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.

5. Use a common field text size of ???.

My preference is 50mils but no matter what field text size you choose,
please revise all of the existing symbols accordingly.  As of right now,
symbol field text sizes are all over the map which makes for some ugly
looking schematics.

Thanks,

Wayne

> 
> 
> 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
> <l.marcantonio@xxxxxxxxxxxx <mailto:l.marcantonio@xxxxxxxxxxxx>> 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     : kicad-developers@xxxxxxxxxxxxxxxxxxx
>     <mailto:kicad-developers@xxxxxxxxxxxxxxxxxxx>
>     Unsubscribe : https://launchpad.net/~kicad-developers
>     More help   : https://help.launchpad.net/ListHelp
> 
> 
> 
> 
> On Tue, Apr 29, 2014 at 4:22 AM, Lorenzo Marcantonio
> <l.marcantonio@xxxxxxxxxxxx <mailto:l.marcantonio@xxxxxxxxxxxx>> 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     : kicad-developers@xxxxxxxxxxxxxxxxxxx
>     <mailto:kicad-developers@xxxxxxxxxxxxxxxxxxx>
>     Unsubscribe : https://launchpad.net/~kicad-developers
>     More help   : https://help.launchpad.net/ListHelp
> 
> 
> 
> 
> _______________________________________________
> Mailing list: https://launchpad.net/~kicad-developers
> Post to     : kicad-developers@xxxxxxxxxxxxxxxxxxx
> Unsubscribe : https://launchpad.net/~kicad-developers
> More help   : https://help.launchpad.net/ListHelp
>