Re: gEDA-user: Remove solder mask from polygons

[Kai-Martin Knaak <kmk@xxxxxxxxxxxx>]

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. 

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.

---<)kaimartin(>---
-- 
Kai-Martin Knaak
Email: kmk@xxxxxxxxxxxxxxx
Ãffentlicher PGP-SchlÃssel:
http://pool.sks-keyservers.net:11371/pks/lookup?search=0x6C0B9F53



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