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

[sdb@xxxxxxxxxx (Stuart Brorson)]

Hi Vax 9000 --

I looked at your Gerbers using GCPrevue.  It's a very impressive
board, in terms of density.  Also, the horizontal/vertical routing
scheme on different used is very professional looking.  Good job!

Comments:

*  YOu didn't include the top or bottom soldermask layers in your zip
file. One big gotcha is if the soldermask relief (i.e. clearance)
doesn't adequately keep soldermask away from the pins and pads.  We
can't check this if the Gerbers aren't there.  (Not that I want to
make extra work for myself . . . . . .  ) 

*  You might want to back the plane layers away from all board edges by
50 or 100 mils or more.  There are some places where the planes went
right to the end of the board.  Inadequate clearance can lead to
shorts when the panel is broken apart into individual boards.

*  A big gotcha is if your pads aren't adequately larger than the
associated drills.  El-cheapo board houses don't drill exactly on hole
center.  I have used pads at least 20 mils larger than drill
diameters, and this is barely adequate sometimes.  Check this against
the fab drawing (also not in the zip file).

*  I seem to recall that this is a low speed board.  Since there is no
GND or power plane possible with a two layer board, you might be
susceptable to signal integrity problems like crosstalk, particularly
if you are using fast parts.  Make sure your design is robust against
glitches and crosstalk.  This problem becomes more acute as you go to
higher and higher speeds.

Just some thoughts.  I'll bet that others here have other observations
to make.

Stuart






> 
> The .gbr files are posted at
> http://www.geocities.com/mscpscsi/board.zip. Any comment? I am new in
> drawing PCB with gEDA/PCB. Please let me know if I made mistakes.
> Thanks.
> 
> vax, 9000
>