Re: gEDA-user: Remove solder mask from polygons

[Colin D Bennett <colin@xxxxxxxxxxx>]

On Wed, 29 Jun 2011 23:41:06 +0200
Kai-Martin Knaak <kmk@xxxxxxxxxxxx> wrote:

> George Boudreau wrote:
> 
> > I am working on a micro-stripline layout and the presence of the
> > soldermask on portions of the board will cause problems. With
> > gEDA/pcb micro-stripline work is a drafting task consisting of
> > numerous polygons. Is there a method/switch that will allow me to
> > remove blocks of the solder mask. This exposed copper will be gold
> > plated.
> 
> Two hacks:
> 
> 1) Select the tracks to be gold plated. 
> 
> 2) Cut the selection to buffer
> 
> 3) Do convert_buffer_to_element from the buffer menu
> 
> 4) Paste the result. This is formally a footprint. Tracks will
> behave like SMD tracks. That is, they will be cleared from solder
> mask
> 
> 5) You can increase solder mask clearance as needed with the [k]
> key when soldermask is active. Alternatively, you can use the 
> ChangeClearSize() action. See 
> http://pcb.gpleda.org/pcb-cvs/pcb.html#index-ChangeClearSize_0028_0029-548
> 
> Drawback number one: gsch2pcb will remove the footprint on its next
> run. This can be fixed, if you make the micro-strip a real footprint
> and add a micro-strip symbol to the to the schematic. 

Actually gsch2pcb won't remove a footprint that has no name, so this
drawback does not apply: just don't name the micro-strip "element" on
the board.


> Drawback number two: This works only with tracks vias and rectangles. 
> No arcs, no text, no arbitrary polygons.
> 
> 
> The second hack can uncover any object: 
> 
> 1) Draw a line (with "new_lines_clear_polygons" activated).
> 
> 2) Cover th track with a polygon. 
> 
> 3) Convert to footprint and paste as before
> 
> 4) Save.
> 
> 5) Open the file with a text editor
> 
> 6) Locate the pad definition. It will be the last line in its layer
> section. 
> 
> 7) Set the thickness to zero (third parameter).  
> 
> 8) Reload the layout. The zero thickness pad will stand out in the
> polygon.
> 
> 9) Set mask clearance as before.
> 
> 10) Export gerbers.
> Make sure, your fab does not barf on zero thickness lines. I put 
> a comment in the README that tells them, this is no error and they
> can safely remove zero thickness lines. If you want to be double 
> sure, you can use the edit abilities of gerbv to remove the line
> yourself. 
> 
> I use this second hack to achieve text with exposed copper. The shiny
> HAL surface makes for good readability.

That's an interesting trick; I'll have to try it sometime.

Regards,
Colin


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