Re: gEDA-user: Error, too many apertures needed for Gerber file

[Pete <pete@xxxxxxxxxxxxxxxxxxxxxxxxxxxx>]

Hi

Thanks DJ, Stuart and Dan for the prompt and very helpful answer's.
For the sake of closing this thread informatively Ive documented what I 
did to cause and solve the problem.
> We added a global aperture cache to work around some problems with
> certain fabs.  The table has 256 entries.  Your board has 315 unique
> apertures (that means, 315 total of line widths, pad widths, pin
> diameters, etc).
>
> If you want a work-around, just edit globalconst to change this:
>
> #define GBX_MAXAPERTURECOUNT	256
>
> To have a larger number.  Of course, this assumes that your fab
> supports that many apertures.
>
>   
Heres what I did to change the constant:

1. Downloaded and uncompressed pcb-20080202.tar.gz from sourceforge.net
2. Read the readme and INSTALL files
3. ran ./configure
4. Checked the resulting output for any missing packages
5. Used Synaptic Package Manager (Debian) to download and install 
anything that was missing
6. Found #define GBX_MAXAPERTURECOUNT in globalconst.h and changed it 
from 256 to 1000
7. ran make
8. Changed to superuser (su)
9. ran make install
10. Prayed to my god
11. Ran PCB, loaded the file and Exported to gerber, shouted with joy.

> Since an aperture is usually associated with a pin or pad definition,
> it's likely that your footprints use many different pad diameters,
> ring radii, hole sizes, etc.  Accordingly, you can also address your
> problem by editing all your footprints and harmonising the pin and
> pad definitions.
>
> Shameless plug for gerbv:  Take a look at your Gerbers in gerbv, and
> use the window available under the "analysis" menu item to look at all
> the apertures you have defined.  I'll bet you have lots of slightly
> different, but similarly-sized apertures.
>
I think I got myself into this problem by the way I use PCB. Three 
specific things I do (a lot) are:
1. I fill in any small gaps in a copper surface by drawing a line and 
then resize it to fill the gap.
2. I manually increase the size of thru hole pads, where possible, to 
maximize the size of each pad.
3. I manually tweak track sizes, solder mask gaps and text size etc.

All of the above actions would create a lot of unique apertures.

> Without looking at the code to see the implications of this, perhaps 
> this is a good thing to be an export time option.  Something like a 
> boolean for limited or unlimited apertures.
>
After increasing the GBX_MAXAPERTURECOUNT to 1000, I created a 400x250mm 
panel which contained 8 different circuits and resulted in 724 unique 
apertures.
Ive sent this PCB off to my PCB manufacturer and they had no problem 
dealing with it.
Therefore, I agree with Dan's suggestion that the number of apertures 
should be an export time option.


Thanks again
I hope this helps someone sometime!

Pete




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