Re: gEDA-user: Gerber magic numbers
On Sun, May 22, 2011 at 03:00:35PM -0700, Andrew Poelstra wrote: I am cleaning up the unit handling for the gerber exporter, using the guide at http://www.linux-cae.net/PCB/rs274xrevd_e.pdf Things are mostly straightforward, but I am lost as to the /10 factors in /* These are for drills */ #define gerberDrX(pcb, x) ((long) ((x)/10)) #define gerberDrY(pcb, y) ((long) (((pcb)-MaxHeight - (y)))/10) Why are the drill numbers divided by 10, and why are they output with leading zeroes?... The reason for this seems to be that drill layers are output in their own format in .cnc files, which use different units than the .gbr (and do not terminate their lines with *). What is the format of these files? -- Andrew Poelstra Email: asp11 at sfu.ca OR apoelstra at wpsoftware.net Web: http://www.wpsoftware.net/andrew/ ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Gerber magic numbers
On Mon, 23 May 2011 11:09:23 -0700 Andrew Poelstra as...@sfu.ca wrote: On Sun, May 22, 2011 at 03:00:35PM -0700, Andrew Poelstra wrote: I am cleaning up the unit handling for the gerber exporter, using the guide at http://www.linux-cae.net/PCB/rs274xrevd_e.pdf Things are mostly straightforward, but I am lost as to the /10 factors in /* These are for drills */ #define gerberDrX(pcb, x) ((long) ((x)/10)) #define gerberDrY(pcb, y) ((long) (((pcb)-MaxHeight - (y)))/10) Why are the drill numbers divided by 10, and why are they output with leading zeroes?... The reason for this seems to be that drill layers are output in their own format in .cnc files, which use different units than the .gbr (and do not terminate their lines with *). What is the format of these files? The drill files output by pcb's gerber export are NC drill files, commonly called Excellon format. See: http://www.apcircuits.com/resources/information/nc_introduction.html http://en.wikipedia.org/wiki/Excellon_Format Regards, Colin ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Gerber magic numbers
On Sun, 22 May 2011 15:00:35 -0700 Andrew Poelstra as...@sfu.ca wrote: Why are the drill numbers divided by 10, and why are they output with leading zeroes? For the Excellon (NC drill) format: “Maximum m.n format supported is 2.4” [1]. That means that the units are 1/10 mil rather than the pcb-internal 1/100 mil unit. That explains the 1/10 factor. Regards, Colin [1] http://www.apcircuits.com/resources/information/nc_codes.html. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
gEDA-user: Gerber magic numbers
Hey all, I am cleaning up the unit handling for the gerber exporter, using the guide at http://www.linux-cae.net/PCB/rs274xrevd_e.pdf Things are mostly straightforward, but I am lost as to the /10 factors in /**/ /* Utility routines */ /**/ /* These are for films */ #define gerberX(pcb, x) ((double) ((x))) #define gerberY(pcb, y) ((double) (((pcb)-MaxHeight - (y #define gerberXOffset(pcb, x) ((double) ((x))) #define gerberYOffset(pcb, y) ((double) (-(y))) /* These are for drills */ #define gerberDrX(pcb, x) ((long) ((x)/10)) #define gerberDrY(pcb, y) ((long) (((pcb)-MaxHeight - (y)))/10) #define gerberDrXOffset(pcb, x) ((long) ((x)/10)) #define gerberDrYOffset(pcb, y) ((long) (-(y))/10) Why are the drill numbers divided by 10, and why are they output with leading zeroes? Also, these macros are only used in gerber_set_layer, and the output code in this seems indistinguishable from that of set_line (both are X%dY%d\015\012). Could someone knowledgeable about the gerber format and how pcb outputs it help me out here? Thanks. PS: Can I replace the \015\012's all over gerber.c with \r\n's? -- Andrew Poelstra Email: asp11 at sfu.ca OR apoelstra at wpsoftware.net Web: http://www.wpsoftware.net/andrew/ ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
