--- In [email protected], "Jean-Paul Gendner" <jean-paul.gend...@...> wrote:
> I have tested that the generated Kicad drill file is an ASCII > file. > And it's indeed an excellon drill file... > The second file I have sent begins as follows: > M48 > INCH,TZ > T1C0.031 > T2C0.039 > T3C0.040 > T4C0.120 > % That's the header with unit and tool definition... > G05 This is the 'now start drilling stuff' > T1 This means 'pick tool 1' (as defined before) > X7000Y-1500 > X7000Y-1700 These are the hole locations. It's a perfectly fine excellon drill tape to me... > However, I get now from eurocircuits the error message: GERBER > drillmaps are NOT supported. Drillmaps??? first the drill tape is in excellon format, not gerber; second the 'drill map' is *another thing* and it's used by the operator to verify that the drill file was loaded correctly, it isn't used to fabricate the board! > May any one give me information on how I may generate a non > Gerber drill file with Kicad? Kicad only creates excellon drill files; it can also generate a drill map in various formats (ps, hpgl and gerber). The drill file is the .drl one, the map is the -drl.ps or -drl.pho or whatever, but the one needed to drill the board is only the .drl (which you correctly sent). Also, I've read the eurocircuits guidelines... it says: Artwork: Gerber RS-274X (Extended gerber with embedded apertures) ==> The .pho files from kicad are of this type Drilling: Excellon (1 or 2) + appropriate tool list (ideally embedded) ==> The .drl file is an excellon 2 with embedded tool list. The external tool list is given in the drill report file All the files are ASCII ones, no EIA or EBCDIC stuff... *maybe* but only maybe if you're under Linux they could have unix line terminations instead of DOS ones (a 'file' command would confirm this). Maybe it's this their problem? (gencad files often don't load with unix terminators)
