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
[EMAIL PROTECTED]
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
