Hello David P.,

> How do you use this.  I can't even figure out how to do the CAM
processing.
> Can you outline the steps you take.  For example, which output device do I
use -
> my guess: Gerber_auto_23.

    it's a bit dificult but after you have it done it right once it appears
to be more logical.

    Are you using Eagle4.08r2? I think 3.55 does the same way, but can't
remember the details. Anyway, I hardly have to deal with the CAM processor,
because the board house does all these work for me.

    First, open the CAM Processor. You can do this choosing CAM Processor
from the file menu of schematics or board.

    Then, file\open\job\ and choose one of the predefined job files. To a
quick start, choose one of the "ger???.cam".

    You'll see various tabs on the top of the window workspace. Each tab is
a file that will be generated, like one .cmp file for the component side
solder mask (with top, pads and vias layers), one .plc file for the silk
screen mask (with dimension, tplace, tnames and tvalues layers) etc.

    In the bottom of the workspace you have buttoms to add and delete files.
You can do as many as you want. You can have top (component side) solder
mask, bottom solder mask, top silk, bottom silk, top stop mask, bottom stop
mask etc.

    For each tab (section), you can give section name (description), user
prompt (something it will ask to continue), offsets (live at 0), file
extension (the defaults are ok) etc.

    You have an option where you tell each section the device that will be
used (file output format).

    On the "Style" checkbox group you have various options for making the
file "upside-down", "mirrored" etc. Live the "optimize" and the "pos.coord"
checked. The defaults are usually ok.

    The drill file is a bit more complex. You have to create a drill rack
file. It's like a file where the size of the drills disponible at the PCB
plant. A file can contain something like:

            T01 0.012in
            T02 0.024in
            T03 0.032in
            T04 0.036in
            T05 0.040in
            T06 0.044in
            T07 0.080in
            T08 0.125in

    You can generate this file for your board using the "drillcfg.ulp" user
language program. Run it from the Board application. If you don't have many
drills disponible at the same time on the plant, you can reduce the number
of hole sizes editing the ???.drl file prior to generating your gerber
output:

            T01 0.012in
            T02 0.024in
            T03 0.036in
            T04 0.036in
            T05 0.044in
            T06 0.044in
            T07 0.080in
            T08 0.125in

    But then you'll have to play with the tolerance values.

    Hope this got you started. If not, ask. :)

    Best regards,

    Brusque

-----------------------------------
Edson Brusque
Research and Development
C.I.Tronics Lighting Designers Ltda
Blumenau  -  SC  -  Brazil
www.citronics.com.br
Say NO to HTML mail
-----------------------------------

--
http://www.piclist.com hint: The PICList is archived three different
ways.  See http://www.piclist.com/#archives for details.