Re: gEDA-user: Gerber files

[Dan McMahill <dan-atMUNGEDmcmahill_dot_net>]

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.

Try telling them that the tools are embedded.  If they don't like that, 
copy the section from INCH,TZ to % inclusive.

> 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


> 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.


-Dan



_______________________________________________
geda-user mailing list
geda-user@moria.seul.org
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user