Olimex advice - adjusting drill sizes

Update: 18th June 2009

I don't think I can recommend olimex any longer. I used them between 2005 and early 2009, and over that time they've got less and less reliable. It is now very difficult to place orders with emails seemingly often getting lost, and the orders seem to be getting slower / taking longer and longer to be handled. The PCBs are unfortunately also not the best; incidences of tracks lif$ through hole plating coming out during rework are significantly higher with the$ I've had from Olimex than those from other manufacturers.

I'm currently using European Circuits. So far, their service and responsiveness is far above that of olimex, the boards are higher quality and the prices seem comparable.

Here's a procedure you can use for adjusting your drill sizes in an existing design done using 'Eagle' - I use it to make the drills 0.1mm bigger as Olimex require the drill sizes you give to be before plating, whereas the standard Eagle libraries give the sizes required after plating.

1. Open eagle and load your design
2. Go to the schematic view (important: this won't work if you do it from the board view)
3. Select 'File' -> 'Run'
4. Select the 'exp-project-lbr.ulp' from c:\Program Files\EAGLE-4.15\ulp\.
5. Click 'open'
6. Ensure 'multiple libraries' is selected
7. Click 'Collect data' (takes a little while to run)
8. When 'Collect finish' appears, you will have a <your-filename;>.scr in c:\Program Files\EAGLE-4.15\ulp\project\<your-project>.
9. The file contains a script to recreate the eagle libraries - included a lot of lines that look like 'Change Drill 1016.000000;' - this means a 10mm drill, and you can now go through this file and change the drills.

   I use a perl script:

   #!/usr/bin/perl -w
   
   while (<>)
   {
       if (/^Change Drill (.*);/)
       {
           my $origdrill = $1;
           my $drill;
           
           $drill = int(($origdrill + 50)/100)*100 + 100;
           # special case - use 3.3mm where we'd use a 3.4mm
           $drill = 3300 if ($drill == 3400);
           $drill = "$drill.000000";
           # print STDERR "Drill $origdrill $drill\n";
           s/\Q$origdrill\E/$drill/
       }
       print;
   }
   

   The above script will output a file with the drill sizes all changes to be 0.1mm bigger, except for any 3.3mm drills which will be left alone.

10. Now go back to eagle select 'File' -> 'Script', select the script file you just changed and click 'Open'
11. The script will now create new lbr files using your new drill sizes.
12. Now go to the Eagle control panel
13. Select 'Options' -> 'Directories'
14. Change the 'Libraries' directory to be your project directory, which is where the new .lbr files have been created.
15. Go to the board view
16. Select 'Library' -> 'Update all'.
17. After a short delay, you should get a message advising you that the board has changed and you should rerun the DRC.
18. Rerun the DRC and check your board.