gEDA-user: Newbie fab Qs

[Steven Ball]

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 at moria.seul.org
> http://www.seul.org/cgi-bin/mailman/listinfo/geda-user