kicad-developers team mailing list archive

[Carl Poirier <carl.poirier.2@xxxxxxxxx>]

> 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 <
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
> 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> 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
> Unsubscribe : https://launchpad.net/~kicad-developers
> More help   : https://help.launchpad.net/ListHelp
>