Re: gEDA-user: Newbie fab Qs

[DJ Delorie <dj@xxxxxxxxxxx>]

> I'm happily using gschem & PCB to design my board, and now I'm actually
> thinking about fabricating it :)  For a 2-layer board, PCB Express requires
> the following Gerber files: 

For a given board.pcb . . .

> Top & Bottom - positive polarity 

This is the normal gerber output from pcb.  Use Export->Gerber.  Look
for board.front.gbr and board.back.gbr (front is the "component" side,
back is the "solder" side).

> Aperture/Dcode file (if not RS274X) 

We are RS274X.

> Excellon Drill file 

board.plated-drill.cnc

> Drill Tool list (if not embedded within NC Drill file) 

It's embedded.

> Soldermask Top & Bottom - positive polarity 

board.frontmask.gbr
board.backmask.gbr

> Silkscreen 1 or 2 sides - positive polarity 

board.frontsilk.gbr
board.backsilk.gbr

> Super newbie question: how do I generate these files?

File->Export->Gerber

> And what is RS274X?

The newer gerber file format.  The older one, RS274D, didn't include
the aperture definitions (i.e. pen shape/size).

> And do you have any tricks/pitfalls recommendations for generating these
> files? 

Gerber output is pretty dummy-proof.  Just push the button and send
them the files.  The only pitfalls are (1) swapping gerbers (usually
your fault for tagging them wrong), or (2) if the fab misinterprets
the polarity (rare, they usually can tell when it's wrong).

Some fabs want dos-compatible file names, and may suggest names.  Just
rename the file if needed.

Include a README.TXT that says what each file is for, if the fab
doesn't include a web interface for defining them (4pcb does).
There's no standard for naming the various gerber files, so each fab
has some technique for letting you tell them which is which.

Some fabs, like pcb-pool, prefer encapsulated formats (like orcad or
eagle files).  I use gc-preview to encapsulate them, which just means
reading in the gerbers, tagging them for purpose, and writing out a
single project file.


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