Hello Peter.
> I'm getting a problem with a module i imported from Eagle, its a TO66
> package
> power transistor. It all looks fine, in the layout, I had to add pads to
> it, but
> in the PCB layout program I can not connect any tracks to it, although the
> ratsnest indicates its connected and all looks fine there.
Mmmmh. Importing from Eagle needs some corrections, i think.
I did this at the module editor.
1) ">Name" from Eagle gots the Value at kicad. So i changed the Value to
TO-66_Housing.
2) The Reference at Kicad was somehow "3". I changed it to "T" for Transistor,
but perhaps you may like "Q" or "V" or something else, but i guess not "3". ;-)
3) I removed the old ">Value" from Eagle complete, because the complement Value
at Kicad is already set. See at 1).
4) The Pads. For through hole pads, you have to aktivate some layers.
At least copper top, copper bottom, soldermask top and soldermask bottom.
5) The left flange hole was as pad named "TO66". I changed it to "3" like the
right flange hole. This is important, because Kicad does the correspondence
between schematic and layout byt corresponding pin numbers at the schematic and
pad numbers at the layout.
Giving the same names to different pads means to connect them electrically,
like it should be for flange holes.
I put the corrected footprind at the attachment as TO-66_RevB.emp, but i have
to say, that i did NOT test it. Also i did NOT check the geometrie. But i
think, it will work now.
If not, look for corresponding pin and pad numbers!
Also i think, that it is not nice, that the silkscreen lines are crossing the
pads. Some people perhaps will get trouble from this. But i think, it is a
minor problem.
Good luck and best regards: Bernd Wiebus alias dl1eic
--
GMX DSL SOMMER-SPECIAL: Surf & Phone Flat 16.000 für nur 19,99 ¿/mtl.!*
http://portal.gmx.net/de/go/dsl
