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

[Steve Meier <smeier@xxxxxxxxxxxxxxxxxxx>]

ohhh i am asleep at the keyboard... that was diagonal not horizontal..
where is the coffee machine?

Steve M.

On Wed, 2005-01-19 at 12:58, Steve Meier wrote:
> opps.... you also have to add
> 
> 
>   pad->Point1.X = X1;
>   pad->Point1.Y = Y1;
>   pad->Point2.X = X2;
>   pad->Point2.Y = Y2;
> 
> 
> Then you get horizontal pads...
> 
> Steve M.
> 
> 
> 
> On Wed, 2005-01-19 at 12:46, Steve Meier wrote:
> > 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.
> > 
>