Re: gEDA-user: Removing soldermask over traces/polygons in PCB?

[Steve Meier <smeier@xxxxxxxxxxxxxxxxxxx>]

Diagonal pads can be made but you have to do a simple modification to
the pcb code.

in create.c comment out the following lines //

Then you can do diagonal pads. I understand why they are discouraged but
being able to rotate a conector 45 degrees was critical for one board!

Steve Meier

P.S. This is why I love open source... If you don't like the rules...
you can change them.

/*
---------------------------------------------------------------------------
 * creates a new pad in an element
 */
PadTypePtr
CreateNewPad (ElementTypePtr Element,
	      Location X1, Location Y1, Location X2, Location Y2,
	      BDimension Thickness, BDimension Clearance, BDimension Mask,
	      char *Name, char *Number, int Flags)
{
  PadTypePtr pad = GetPadMemory (Element);

  /* copy values */
 // if (X1 != X2 && Y1 != Y2)
 //  {
 //    Message ("Diagonal pads are forbidden!\n");
 //    return NULL;
 //  }
//  pad->Point1.X = MIN (X1, X2);	/* works since either X1 == X2 or Y1
== Y2 */
//  pad->Point1.Y = MIN (Y1, Y2);
//  pad->Point2.X = MAX (X1, X2);
//  pad->Point2.Y = MAX (Y1, Y2);
  pad->Thickness = Thickness;
  pad->Clearance = Clearance;
  pad->Mask = Mask;
  pad->Name = MyStrdup (Name, "CreateNewPad()");
  pad->Number = MyStrdup (Number, "CreateNewPad()");
  pad->Flags = Flags & ~WARNFLAG;
  pad->ID = ID++;
  pad->Element = Element;
  return (pad);
}




On Wed, 2005-01-19 at 10:20, Xtian Xultz wrote:
> Em Qua 19 Jan 2005 15:03, Steve Meier escreveu:
> > Do you really want bare copper or would bare copper with the surface
> > finish be ok? If so create one or more "devices", with land patterns, to
> > represent the exposed contacts. Then place these phony devices on the
> > board. I like to put them in the schematic, perhaps connected to a
> > ground plane, as well.
> 
> Well, there is a problem because I cant make device with land pattern in the 
> diagonal orientation, so the line must be made with horizontal or vertical 
> lines only. And there is a problem, because that kind of lines is to conduct 
> high levels of currents, and using only 90 degrees curves makes the 
> inductance be indreased, and of course the line becomes longer. And its a 
> boring process, because I must represent every piece of land pattern in the 
> schematic (because of the netlist) and must create every piece too. Its not a 
> solution.
> 
> I made a suggestion on the pcb site, without answer, I dont know how difficult 
> is it to implement, to made a way to edit the solder mask with lines and 
> poligons, using some boolean operations. Like, enabling the show of the 
> soldermask, when selecting the line command, the line will erase the 
> soldermask where I draw it. To make it perfect, the soldermask must be drawn 
> with transparency, these function is in the PCB configuration file for the 
> layers.
> 
> >
> > Steve Meier
> >
> > On Wed, 2005-01-19 at 03:26, Xtian Xultz wrote:
> > > Em Qua 19 Jan 2005 01:13, Randall Nortman escreveu:
> > > > I would like to create areas of bare copper, with no soldermask.  In
> > > > particular, I'd like to create grounded guard bands around the edges
> > > > of my board to protect against ESD during handling of the board.  To
> > > > see what I'm trying to do, have a look at the last two slides of:
> > > >
> > > >   http://www.cae.wisc.edu/~benedict/pcbpres.pdf
> > > >
> > > > As far as I can tell, only pads seem to clear the soldermask.  Is it
> > > > possible to get PCB to clear the soldermask over a trace or polygon?
> > > >
> > > > Thanks,
> > > >
> > > > Randall Nortman
> > >
> > > AFAIK, no. I sometimes do it to increase the current capability of a
> > > trace. To do it, I use the postscript output, convert it to .sk with
> > > pstoedit and opens it with sketch, and there I edit the way I want (and
> > > place some logos, figures, and stuff). And then export to .ps and send to
> > > my fab.