I've sent stuff to PCB Express using PCB, and it always comes out
like a champ.
Note that the 'board.plated-drill.cnc' is only the plated drill
holes, and does not include any holes you have that are unplated. I
usually open up 'board.unplated-drill.cnc' and copy over any holes
(and drills) into the plated file and stick that into the file
archive to send to them. I don't know if it would mess anything up
to just cat the two files together, I haven't tried it.
Keep an eye out for specials from PCB Express too, they tend to have
free express days off and on.
-Steve
On Jan 3, 2007, at 9:46 PM, DJ Delorie wrote:
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@moria.seul.org
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
_______________________________________________
geda-user mailing list
geda-user@moria.seul.org
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
