kicad-developers team mailing list archive

[jp charras <jp.charras@xxxxxxxxxx>]

Le 23/12/2013 15:10, Lionel Sainte Cluque a écrit :
> Dear all,
> 
> I'm not a native english speaker so please excuse my approximate english
> writting.
> 
> I used to be an happy GEDA/PCB user and I recently switched to KICAD.
> I'm happy with that choice (I still maintain old projects under PCB
> which is old fashioned, but works).
> 
> My professional activity includes a very wide range of actions, from
> design engineer to CAM operator and board assembly.
> 
> As a CAM operator I daily face designs produced by different CAD
> software. As my pcb manufacturing prices are low and my company is
> young, my clients are DIYs students and small companies. Free (in terms
> of money) software is common amongst my clients.
> 
> I can appreciate the differences between CAM files produced by different
> tools. By now I was glad to work with kicad files as it was prefectly
> state of the art :
> Power planes are not vector filled polygon but rasters
> Round / rectangle and oblong pads are "flashed" rather that drawn (means
> it is described in the apertures list and then inserted in the gerber
> file with a single set of coordinates).
> 
> 
> In the most recent builds of Kicad it seems that soldermask generation
> changed. Soldermask used to consist of flashes and now it consists in
> raster polygons. The problem is that a raster polygon is a kind of
> drawing and lacks the information required for a pad. The two main
> drawbacks are :
>   * The shape and size of the soldemask feature can not be easily
> modified. This is an important issue as we (too) often have to modify it
> as designers take great care of the copper and little care of the
> soldermask. Now with kicad designers I just don't use their soldermask.
> I generate a new one from the copper layer by copying and enlarging pads
> ans use the user soldermask layer for the controls.
>   * Alignement of soldermask and copper can not be done by center
> alignement of pads as there are no pads in the soldermask. For similar
> reasons it is not possible for my flying probes editor to use the
> soldermask to control what is a pad and what is not.
> 
> There are probably positive reasons to use raster polygons in
> soldermask, and I would be glad to hear it, but from the manufacturer's
> point of view it is a regression.
> 
> Would it be possible to have the minutes of the debate prior to that
> change in order for me to understand the motivations?
> 
> I hope this email is not too direct, I really like Kicad and I am very
> FOSS oriented. I am glad to use a software of this quality and I hope I
> can contribute to develop and promote it.
> 
> Sincerely yours.
> 
> Lionel SAINTE CLUQUE
> adresse:
> 1, rue Paul de KOCK
> 92500 Rueil Malmaison
> Téléphone +33 (0)6 18 04 20 75
> 

Solder mask is generated by using polygons when the user sets the min
width value > 0.
Because the actual solder mask is the negative image of the pads, the
full solder mask should be created (and the actual shape is a polygon)
to find areas smaller than this value and remove them.
Recreating the right (negative) solder mask (which is no more the
negative pad area) is made from the polygonal solder mask shape.
To create the solder masks from the pads using flashed pad shapes, just
use 0 as min width value to generate these solder masks.

-- 
Jean-Pierre CHARRAS