Re: gEDA-user: Finished drawing two sided board in PCB. Any comment?

[sdb@xxxxxxxxxx (Stuart Brorson)]

Hi Vax 9000,

So I looked at your Gerbers again after you posted the whole set.
Overall I am very impressed.  I suspect that this is not your first
board!

Some comments:

*  Some people asked to see the PCB file.  That is fine, since you can
look at how the DRCs were set up, and run the DRC checker.  However, I
think it better to inspect the Gerbers since this is what the
manufacturer will see.  Ideally, you would run Valor or CAM350
against the Gerbers since it would automatically pick up manufacturing
problems.   These are not open-source tools, however!  :-(

*  As far as I could tell, you did a great job with all manufacturing
tolerances.  I checked your design against the tolerances listed on
the Advanced Circuits webpage:

http://www.4pcb.com/fast_design_quote_online_pcbs_tolerances.htm

Solder mask and solder paste look fine to me.   However, did you check
the drill diameters against your PGA and DIP pin diameters?  I don't
recall a typical pin diameter; your drill diameters are .029.  Is this
enough? 

*  Finally, your fab drawing shows the outline of the board extending
waaaaay below the actual edge of the board.  You may want to examine
this yourself.  PCB autogenerates the fab drawing based upon the
active drawing area you used when laying out the board.  I suspect
that you extended the drawing area down when you were working.  

The problem is that your board is not a simple rectangle.  I suspect
that you actually want to route out along the silkscreen outline of
the board.  The problem is that PCB has autogenerated your board
outline in the fab drawing assuming that it is the rectanglular
drawing area.   PCB developers: this is a misfeature, IMHO.  

In commerical tools, you would have a separate layer calling out the
board outline.  For PCB, you probably need to put a manual instruction
somewhere for the fab house to route the boad along the silkscreen
outline.  Maybe you can draw your desired outline on a new, separate
Gerber layer?  Alternately, you can make a mechanical drawing of the
desired board outline, and include it with your design materials.
Don't forget to make it *totally* clear where the holes and outline of
the board lie w.r.t. the positions of the features in teh Gerbers.  If
you can speak to an engineer at the fab house in person, that would
help you clarify exactly what board outline you want.  Otherwise, if
the fab house operates "open loop" (like many of the el-cheapo places
do) then you will get back a rectangular board which you will have to
rework yourself.

Others, any opinions about how to create complex board outlines in
PCB?

Stuart