kicad-developers team mailing list archive

[Milan Horák <konference@...>]

Hallo,

let's look on the specs, no offense:

> Author: Vesa Solonen 6.10.2008
> License: GFDL
>
>
> Schematic symbol guidelines
>
> -The main dimensional unit (DU) is tied to resistor symbol width. The 
> width includes outline line thickness and keepout.

Resistor symbol dimensions are defined in IEC-617-4 (EN 60617-4) width 
is 2.5mm, which is approx. 1/10", which is 100 mils. IMO it is measured 
from one line axe to another. The height is defined 7.5mm, which is 
approx. 3/10", which is 300 mils. It is called an M like module.

> -There must be at least one DU spacing between pins or any other 
symbol >feature, like corner. Excluding symbols with width less than 2*DU.

Spacing between pins is defined also in IEC-617-4 (EN 60617-4) as 2*M so 
it is 5mm, which is approx. 2/10", which is 200 mils.

> -Resistors: length 2.2*DU, pins 3*DU

see above, pins are M/2

> -Capacitors: plates 0.5*DU apart center to center, plates width 
> 1,25*DU, plates thickness Thick, pins 2*DU. Positive plate in Bold 
> outline.

Plates defined as M/2 center to center, width 2*M, positive marked with 
"+" one M wide, one M high, placed one M left and one M up from center.

> -Transistors: outline ring diameter 2*DU, base-beam length 1.33*DU in 
> Thick, emitter arrow in Bold.
> 	Pins in C(0.5, 1.5), E(0.5, -1.5), B(-1.5, 0) positions taking 
> outline ring centre as origin.

Transistor is defined without circle (except transistor with one 
electrode connected to the envelope - in this case circle diameter is 4*M).

Base beam is 2*M.

That is said in IEC-617-5 (EN 60617-5).

Milan

Vesa Solonen napsal(a):
> What's the policy for official libraries? I'd like to enhance them a bit
> and also would like to know wether we can agree on 'official' library
> style. The style part is probably the most difficult task and my ultimate
> goal is to look after possibilities to make dynamically styled schematic
> library. I think one of the finest examples is ATMEGA8 symbol, but the
> whole library lacks coherency.
>
> For some examples please look at:
> http://users.tkk.fi/~vsolonen/kicad/ <http://users.tkk.fi/~vsolonen/kicad/>
>
> How to get dynamic styling? Some ideas will be found in
> Symbol_guidelines.txt document and the real implementation would need
> adding style tag to the library graphic primitives and support to the
> parser. I think the better way of getting there is devising SVG import
> system for symbols and just leaving the pin object definitions to kicad
> library editor. That way complex gui etc for graphics manipulation would
> be external to Kicad (Any good svg editor, like Inkscape). Full blown
> internal svg-support might be too heavy with very complex schematics,
> would it? At least it would be a whole lot of work.
>
> I might try writing an svg importer in python some time...
>
> SVG import would be really fine way for adding custom logos to layouts.
>
> -Vesa