[Author Prev][Author Next][Thread Prev][Thread Next][Author Index][Thread Index]

Re: gEDA-user: Gerber files

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@xxxxxxxxxxxxxx
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user