[Date Prev][Date Next][Thread Prev][Thread Next][Date Index][Thread Index]
Re: gEDA-user: Gerber files
I have used Sunstone (PCB Express) for all of my boards. See my
additions to Dan's comments ---
On 4/12/07, Dan McMahill <dan@mcmahill.net> wrote:
> Craig Niederberger wrote:
> > Hi Gurus, in using Sunstone to fab, they ask for these files:
> > Layer 1
> > Layer 2
> > Top soldermask
> > Bottom soldermask
> > Top silkscreen
> > Excellon Format Drill file
> > Tool Size Report
> > Aperture for 274D Format
> > Outline Layer
> >
> > My pcb Gerber export produced the following files:
> > bike.back.gbr bike.fab.gbr bike.frontmask.gbr bike.frontsilk.gbr
> > bike.backmask.gbr bike.front.gbr bike.frontpaste.gbr
> > bike.plated-drill.cnc
> >
> > It seems to me that these are the assignments:
> > Layer 1: bike.front.gbr
> > Layer 2: bike.back.gbr
> > Top soldermask: bike.frontmask.gbr
> > Bottom soldermask: bike.backmask.gbr
> > Top silkscreen: bike.frontsilk.gbr
> > Excellon Format Drill file: bike.plated-drill.cnc
>
> yes.
>
> > But what would these files be:
> > Tool Size Report
>
> they're looking for a file which maps tool number to drill diameter for
> the Excellon format drill file. In the case of the files generated by
> PCB, the drill size is embedded in the .cnc file. Near the top, you
> probably have lines like:
>
> T11C0.020
> T17C0.040
> etc.
>
> Those specify drill sizes for T11 and T17.
This is the drill/tool file that they are looking for.
> > Aperture for 274D Format
>
> not needed. RS-274-D had the aperture list as its own file (very error
> prone). RS-274-X (what pcb generates) embeds the aperture list.
>
> > Outline Layer
For an outline Sunstone expects a continuous line around the perimeter of the
board on one of the PCB layers (maybe the top layer). I usually do
this by drawing a one mil trace on the top layer. There is probaby a
way to do this by merging the top layer and an outline layer.
>
>
> > bike.fab.gbr
>
> some times known as the "drill drawing". Shows a picture of the board
> with locations of all drill holes, and a list of the drill sizes.
>
> > bike.frontpaste.gbr
>
> used for making a solderpaste stencil. Only needed if you have having
> the board populated in a factory environment.
These are not needed to fabricate the PCB.
(* jcl *)
--
http://www.luciani.org
_______________________________________________
geda-user mailing list
geda-user@moria.seul.org
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user