I am surprised, because I use GC-Prevue with the default values to show the drill and Gerber files without any problem. More exactly, the first time, I tried to use Millimeters, and there I had a difference between drill and Gerber files. So I switched back to Inches and there all was OK. However I only worked on single board, not multiboard.
Regards, Jean-Paul **************** Jean-Paul Gendner 03.88.27.03.44 _____ De : kicad-users@yahoogroups.com [mailto:kicad-us...@yahoogroups.com] De la part de elliomartina Envoyé : lundi 25 janvier 2010 02:06 À : kicad-users@yahoogroups.com Objet : [kicad-users] Viewing KiCad drill files in GC-Preview or Gerbv- Got some strange results I am using KiCad for a few weeks and have designed a few boards ready for production. Following the advise to check the Gerber files, I installed GC-Preview on my Win box and Gerbv on my linux box. Found some tips for the settings to be used when creating the drill files and discovered that most of the settings do not work for viewing them in both viewers. So I started analyzing about what happened when creating the drill files using different options of the settings panel and viewing them As Gerbv did not show anything properly when starting I first tried with GC-preview using the some suggested working settings I found with searching for solutions. I started off with Driil Origin = Auxiliary axis and then trying several Zero formats. All of the comined options except Decimal Format did not work at all to get a good result Mirror X axis should be OFF by default or you never get the drill holes into the board layout, at least I did not get it Here are some messages GC-View showed when importing the dril files: File format: Seen by GC-Preview as: Result: Supress Trailing + 2.4 Aux origin = 3.2/Abs/mm/Trailing Supp/Quad -> size=x10 Supress Leading + 3.2 Aux origin = 4.1/Abs/mm/Leading Supp/Quad-> size=x10 !!!! x10 means that you see the drill holes, but sized 10 times that of the board! I noticed that the format changed not consistently when selecting trailing or leading. Depending on saving the settings in the plot panel, the format displayed either 3.2 and 3.3 or 2.3 and 2.4 when opening the Drill export panel. This is somewhat confusing. So I selected also some settings in this "confusing" modes Supress Leading + 2.3 Aux origin = 3.2/Abs/mm/Leading Supp/Quad-> size=x10 Supress Leading 2.4 Aux origin = 3.3/Abs/mm/Leading Supp/Quad-> size=x10 Absolute origin selection did not work either with these supress options Finally I tried to use the Decimal format option. File format: Seen by GC-Preview as: Result: Decimal Aux origin = 4.1/Abs/mm/Trailing Supp/Quad -> Screen size= OK perfect result Decimal Absolute = 4.3 /Abs/mm/Leading Supp/Quad- size= OK but the drills are placed on negative Y-axis Not mirrored however. So this is not usable with GC-Preview since the absolute Gerber files are placed as the auxiliary ones. With Gerbv the Decimal Auxiliary+Absolute origin options are both working properly for viewing the Gerber files. So far I must conclude that if the drill file's X Y numbers do not have a decimal dot sign viewing in GC-Preview or Gerbv does not work for the Kicads drill files Next to check is what GerbMerge is doing when making a multiboard panel Best regards from Holland, Ellio
