On Wed, 29 Jun 2011 23:41:06 +0200 Kai-Martin Knaak <k...@lilalaser.de> 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@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user