Re: gEDA-user: Two questions about pcb.

[Xtian Xultz <xultz@ig.com.br>]

Em Qui 30 Set 2004 20:25, harry eaton escreveu:
> > 1)  I need to make a drilled hole without copper in a layout (see the
> >     part at
>
> http://rocky.digikey.com/scripts/ProductInfo.dll?Site=US&V=102&M=SJ-3524NG
>
> >     )  Can I do this in pcb by making a via with holesize=viasize?  Or
> >     is the board house gonna complain?
>
> You want to turn the via  into a pure hole, by typing Ctrl-H (H for hole)
> with the cursor over the via. That way it doesn't have a copper annulus
> and it appears in the fab drawing as unplated and in the "unplated" drill
> file.
>
> > 2)  How do I make a pcb that is not rectangular in pcb?  That is, I need
> >     to tell the board maker how to route the outside of the pcb.
>
> You need to make one of your layers a route layer. Name the layer "route"
> or "outline" and make sure it's in it's own group. Then draw a 10 mil path
> of lines/arcs
> for the board outline. The fab drawing will then show the center line of
> the path
> as the board outline. It's up to you to make sure all your stuff fits
> properly inside.
> You really should make a gerber file that has only the route too, but at
> the moment
> this isn't automatic because the gerber for that group will show all the
> pin and via
> pads too. To make this gerber file do this:
> (1) save your design
> (2) turn off the route layer so it's not visible, but make all other
> visible (3) do a "select all"
> (4) remove selected
> (5) print the gerber files
> (6) quit pcb *WITHOUT SAVING CHANGES*
> (7) change the name of the gerber file having the route output to something
> like "myroute.gbr"
> so it won't be overwritten
> (8) launch pcb and re-load your design.
> (9) print the gerbers normally
> (10) chuck the new gerber cooresponding to the route layer ('cause it has
> pads in it)
>
If he makes the step  5, make a undo (U key), make the step 7 and jump to step 
9 it does not work (I didnt test if the undo works after a print command)