The m4 part library has a higher order of operation over foot print libraries, the TO220-GSD is matching the m4 TO220 not the footprint TO220-GSD
You do not want to use a - in the footprint names, as out m4 setup can't escape the - in footprint names, so I always use underscores _ Alternate option is to disable m4 in gschem2pcb, lots of discussions on disabling m4 libraries in the archives and should be in the wiki too, maybe even in the --help of gschem2pcb Steve On Dec 18, 2009, at 3:16 PM, Larry Battraw wrote: > > Thanks for the suggestions but I actually found a ready-made symbol > from the symbol site and it causes PCB to choke when included in the > schematic. It chokes on the very last line of the definition in the > .pcb file as seen here: > Element(0x00 "" "" "" 50 570 1 100 0x00) > ( > # I have been unable to locate the JEDEC drawing. However, refering > # to [1]http://www.zetex.com/3.0/pdf/TO220.pdf which claims to be > JEDEC > # compliant, I see that the pins are rectangular with dimensions: > # > # 15-40 mils X 16-20 mils which gives a diagonal of > # 21.9 to 44.7 mils > # > # The pin pitch is 90 to 110 mils. > # > # The mounting hole is 139 to 160 mils diameter > Pin(100 800 90 60 "1" 0x101) > Pin(200 800 90 60 "2" 0x01) > Pin(300 800 90 60 "3" 0x01) > # Befestigungsbohrung > Pin(200 130 150 130 "4" 0x01) > # Anschlussdraehte > ElementLine(100 800 100 620 30) > ElementLine(200 800 200 620 30) > ElementLine(300 800 300 620 30) > # Gehaeuse > ElementLine( 0 620 400 620 20) > ElementLine(400 620 400 245 20) > ElementLine(400 245 0 245 20) > ElementLine( 0 245 0 620 20) > # Kuehlfahne mit Kerben > ElementLine( 0 245 400 245 20) > ElementLine(400 245 400 120 20) > ElementLine(400 120 385 120 20) > ElementLine(385 120 385 50 20) > ElementLine(385 50 400 50 20) > ElementLine(400 50 400 10 20) > ElementLine(400 10 0 10 20) > ElementLine( 0 10 0 50 20) > ElementLine( 0 50 15 50 20) > ElementLine( 15 50 15 120 20) > ElementLine( 15 120 0 120 20) > ElementLine( 0 120 0 245 20) > Mark(200 800) > )-GDS(TO220-GDS,S2/Q8,IRFI640G) <<<<<<------ Problem here > I don't know enough about PCB to see what's wrong with this line to > change it, all I know is if I remove it PCB is happy until it hits > the > next instance of the part. Any ideas? > Thanks- > Larry > > On Thu, Dec 17, 2009 at 9:52 PM, Dan McMahill <[2][email protected]> > wrote: > > phil wrote: >> I just use symbols for transistors and for fets that have the pinout > in >> the name: >> >> fet-pmos-3-gds.sym >> pnp-2-cbe.sym >> >> The name of the symbol has the pins in order 1-3, so the p-ch mosfet > is >> gate = , drain = 2, source =3 ... like an insulated to-220 mosfet. >> >> This probably doesn't use the symbols to their full potential but it >> keeps me from getting confused as easily. > > beware that different vendors sometimes put the pin number on > different > physical pins. TO-18's and TO-39's are some example packages > where > I > have seen vendor #1 number them one way and vendor #2 a different > way. > Turns out that the E/B/C to physical location mapping was > identical, > they just mapped 1/2/3 to physical location differently. ugh! > Thats why I use heavy symbols exclusively for things like > transistors. > No need to remember "lets see, was this a cbe transistor" and > "which > vendor numbering". I just say "give me a MMBT3904". > -Dan > > _______________________________________________ > geda-user mailing list > [3][email protected] > [4]http://www.seul.org/cgi-bin/mailman/listinfo/geda-user > > References > > 1. http://www.zetex.com/3.0/pdf/TO220.pdf > 2. mailto:[email protected] > 3. mailto:[email protected] > 4. http://www.seul.org/cgi-bin/mailman/listinfo/geda-user > > > _______________________________________________ > geda-user mailing list > [email protected] > http://www.seul.org/cgi-bin/mailman/listinfo/geda-user _______________________________________________ geda-user mailing list [email protected] http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
