Re: gEDA-user: add Logo to silkscreen in pcb, exactly how to insert the EPS?

[Mark Rages <markrages@xxxxxxxxx>]

On Tue, Jul 21, 2009 at 2:39 AM, andrew
whyte<aw@xxxxxxxxxxxxxxxxxxxxxxxx> wrote:
> Apologies if this post is a little late.  I realise that others have
> answered this, but I have some more info, and more questions...
>
> I have used pstoedit to creat pcb logos in the silk screen,   I made
> my logo into a black and white only version using inkscape(I also had
> to convert the whole think to a single-shape/few-shapes using the
> menu: Path>>Object to path, and the Path>>union functions - and reduce
> the number of vertices to something that made a reasonably sized
> file), then I exported to ps then ran:
>
>> pstoedit -xscale 0.25 -yscale 0.25 -f pcb ./paramita-logo-BW-hi-res.ps ./logo-output.pcb
>
> at the command line.  This makes a layout file,  then I converted this
> to a symbol as usual.   I have a logo .sym file that I drop into each
> schematic, then the footprint automatically appears on the pcb in the
> silk layer when I run xgsch2pcb.
>
> The only think that I sometimes would like, would be to be able to
> convert the solid shapes on the ps into solid areas of silk/copper.
> pstoedit seems to make shapes into outlines, and outlines into double
> lines.  Has anyone ever solved this one?  Is there a simple way to
> move shapes from one layer to another within pcb (eg. silk -> copper)
> Would I be best scripting my own svg-pcb converter?
>

If you use the "pcbfill" format to pstoedit, it will convert to
polygons on the silk layer.  You will probably find the -ssp option
useful as well.

Here's the relevant Makefile snippet, where I was drawing (pretty
font) text and logos in the file text.svg:

text.ps: text.svg
	inkscape text.svg -p '> text.ps'

text.pcb: text.ps
	pstoedit -flat 0.02 -ssp -dt -f pcbfill text.ps text.pcb

I usually cut and paste from the pstoedit output to my board in a text editor.

Note that polygons aren't allowed in element/footprint files.

You can move polygons from one layer to another within pcb.

Regards,
Mark
markrages@gmail
-- 
Mark Rages, Engineer
Midwest Telecine LLC
markrages@xxxxxxxxxxxxxxxxxxx


_______________________________________________
geda-user mailing list
geda-user@xxxxxxxxxxxxxx
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user