Re: gEDA-user: non-round PCB pins

[Xtian Xultz <xultz@xxxxxxxxxxxx>]

Sorry for such a dumb question, but I didnt undertood you guys are trying to 
do (my english is really a piece of crap).
As far as I undertood, what you need is to make oblogue drills? To do it, I 
use a command called G85 on the drill file. This is a excellon command to 
make oblongue drills (also called slot). 
The sintax is very simple, is XYG85XY where the first XY are the X and Y 
coordinates of the origin and the last the destination. It is very important 
to use one drill measure to make drill for vias and pins and another to make 
slots, even if they use the same size. Like, if you have pins with 28 mils of 
size and use like T01C0.028, and you want to make a slot with 28 mils too, 
you need to specifie another bit (like T02C0.028) only for the slots. Thats 
because the bit used to drill is different from the bit used to mill. 
Of course, the drill machine must understand the G85 command. My fab uses a 25 
years old drill machine and it undertands well.
I do it mannually in the plated-drill.cnc file. There would be nice to have a 
function to design slots using a line with the size of the line equals to the 
drill size of the slot, I think is not too difficult to implement it.
Here are a reference to the excellon file format:
http://www.excellon.com/applicationengineering/manuals/program.htm

But, what you guys are talking about have nothing to do with what I wroted 
here, please forget all, sorry about that :D


Em Qui 10 Fev 2005 11:29, harry eaton escreveu:
> Most fab shops can route from a gerber file. The trick is to get pcb to
> make a gerber file with only the route path.
> Presently this is somewhat ugly.
>
> What I have done is devote a copper layer to the router. When I'm finished
> with the layout I draw the router tool
> path on this layer. Then I save the design and make the gerber files for
> the board. Next I turn off visibility of
> the router layer and turn on visibility of all pins, vias and silk then
> delete everything visible (easy if nothing is locked).
> Then I print gerbers again (which only prints the router file). I make sure
> to not save the layout with stuff
> deleted.
>
> The reason you need to delete pins and vias is that they appear on every
> layer but you don't want them in the
> router output.
>
> harry
> ----- Original Message -----
> From: "Dan McMahill" <dan@xxxxxxxxxxxx>
> To: <geda-user@xxxxxxxx>
> Sent: Monday, February 07, 2005 8:41 PM
> Subject: Re: gEDA-user: non-round PCB pins
>
> > On Mon, Feb 07, 2005 at 01:54:31PM -0800, Matt Ettus wrote:
> > > I asked my PCB vendor and got this response --
> > >
> > > ====
> > > What CAD do you use for design of the board? Please use mechanical
> > > layer
>
> for
>
> > > layout of the mill-out if you use Protel.  Please uese .mil file if you
>
> use
>
> > > Eagle. Just examples. Thanks.
> > > ====
> > >
> > > How should I do this in PCB?
> >
> > do those layers generate gerber files?
> >
> > Right now there really isn't a way that I know of in PCB to have some
>
> extra
>
> > layer associated with an element.
> >
> > > Thanks,
> > > Matt
> > >
> > >
> > > On Fri, 4 Feb 2005 21:00:01 -0500, Charles Lepple <clepple@xxxxxxxxx>
>
> wrote:
> > > > On Fri, 4 Feb 2005 17:32:36 -0800, Matt Ettus <boyscout@xxxxxxxxx>
>
> wrote:
> > > > > I need to make a PCB footprint for a component which has several
> > > > > "pins" which are actually metal tabs about 1/8" long.  Any ideas
> > > > > how to do this?
> > > >
> > > > Do you want to solder the tabs to plated slots in the board? If so,
> > > > you may want to ask the PCB shop how they would like to see the slot
> > > > represented in the gerber and drill files.
> > > >
> > > > Some places will mill a slot between two drill hits if you call that
> > > > out on the fab drawing, but they may have a minimum size for the
> > > > narrow dimension of the slot.
> > > >
> > > > If you're wave soldering the parts, you could get away with two or
> > > > even one drill hole to fit the width of the tab. This would be a pain
> > > > to rework, though, because of the sheer volume of solder that would
> > > > collect between the tab and the plated sides.
> > > >
> > > > --
> > > > - Charles Lepple
> >
> > --