gEDA-user: PCB gerber export problem - update

[Tomaz Solc <tomaz.solc@xxxxxxxxxx>]

Hi

After spending a couple of hours with our PCB manufacturing staff I 
found a solution to my problem. I'll try to explain, but please keep in 
mind that my knowledge of the gerber format is limited to what I 
learned today...

This time I used the latest CVS version of PCB to export my layout to 
the gerber format (I first had to fix polygons that were displayed 
differently in the 20060822 snapshot, but that will be subject of 
another mail). The problem appeared when we tried to import these files 
into CircuitCAM. If we imported just one layer (for example solder or 
component copper layer) everything looked fine. But as soon as the 
second layer was imported the previously imported layer got mangled - 
line widths were wrong, random rectangles appeared, pin disappeared, 
etc.

We traced the problem to aperture definitions in gerber files. For 
example, the solder layer has these definitions:

%ADD11C,0.0200*%
%ADD12C,0.0600*%
%ADD13C,0.0300*%
...

On the other hand the component layer has these:

%ADD11C,0.0300*%
%ADD12C,0.0200*%
%ADD13C,0.0150*%
...

You can see that D11 for example is defined differently in each file. 
The problem we were having was caused because CircuitCAM updated D11 
aperture for the first layer from the second layer we imported. It 
looks like aperture definitions are shared between layers in this 
software. The obvious solution was to rename apertures so that each 
layer has it's own set and names are shared. A simple 'sed' script took 
care of that (for example replacing D1x with D7x in one file).

Now, GCPrevue has no problems with shared aperture names. Neither has 
gerbv, so obviously this is a problem specific to CircuitCAM. On the 
other hand people at the laboratory never saw this kind of a problem 
before (and they assured me they go through  gerber files produced by a 
lot of strange software).

I'm guessing that it would be a simple change to fix aperture naming in 
PCB - it seems that most of the other PCB software out there takes care 
not to share names. I'm prepared to make a patch if you agree that it 
would be a good thing to fix this.

Best regards
Tomaz



_______________________________________________
geda-user mailing list
geda-user@xxxxxxxxxxxxxx
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user