Why do you need different ones for cap, res, and ind? Matt
On 12/9/05, Dan McMahill <[EMAIL PROTECTED]> wrote: > And just to add to this, there is no single "IPC one". In fact the > ~geda library contains no less than 9 (!) IPC 0603 footprints. These are > > CAPC1608L > CAPC1608N > CAPC1608M > > INDC1608L > INDC1608N > INDC1608M > > RESC1608L > RESC1608N > RESC1608M > > which are for capacitors, inductors, and resistors respectively. the > L/N/M are for least/nominal/most. In addition, there is still just 0603 > in ~geda. 0603 needed repair because the one which was there was not > large enough. That one has been updated to something representitive of > the "N" version. > > As for other versions of 0603 footprints, they're there because no one > has made footprint library maintainence a high priority. > > -Dan > > Steve Meier wrote: > > The IPC footprints have been critisized for being overly large. I > > believe this is true especially for the smaller size components. My > > understanding is that the IPC wants to leave some minimum pad space in > > front and behind (toe and heal) the devices contact. If you then compare > > the IPC recomended foot prints to a device manufacturors recomended foot > > print you will see a consierable size difference. I suspect this might > > very from manufacturor to manufacturor. This is one cause of multiple > > footprints. A second cause is that different assembly techniques may > > suggest variations in the width of the pads. > > > > Is this all really necessary? Propably not. But which one to select? > > > > Steve Meier > > > > > > Matt Ettus wrote: > > > >>I was able to fix this problem by going back to an older PCB CVS. > >> > >>One question -- why are there multiple 0603 footprints? Why wouldn't > >>you want to use the IPC one? All these versions makes for a lot of > >>confusion. > >> > >>Matt > >> > >>On 12/6/05, Stuart Brorson <[EMAIL PROTECTED]> wrote: > >> > >> > >>>>>I recently upgraded to the latest PCB CVS. Now when I run gsch2pcb on > >>>>>an already existing pcb file many of my components get deleted. Also > >>>>>new 0603 caps no longer have silkscreen around them. Is it possible > >>>>>that changes to PCB caused this? I didn't change gsch2pcb. > >>>>> > >>>> > >>>>Yes, latest pcb from cvs does not have silk around the 0603 footprint. > >>>>IPC-7351 seems to indicate no room for silk on 0603. The newer 0603 (or > >>>>preferably the IPC-7351 compliant names for 0603 -- CAPC1608N for > >>>>example) in the ~geda library should be much better from a soldering > >>>>point of view too. The previous one was no good. > >>>> > >>> > >>>A tangential point to this: If you use newlib footprints, John > >>>Luciani's caps have partial silk at the ends of the parts which help > >>>determine the component body size during placement. And (shameless > >>>plug) some time ago I wrote a perl utility called smtgen which > >>>generates footprints for two terminal passives if you give it the > >>>physical parameters like length, width, pad dimensions, etc. You give > >>>it all parameters on the command line, and it writes footprint to > >>>STDOUT. It draws a full rectangle around the part on the silkscreen > >>>layer. I put it on my website for interested parties to use: > >>> > >>>http://www.brorson.com/gEDA/ > >>> > >>>The resulting footprints may or may not be IPC standard (I haven't > >>>paid attention to recommendations for dealing with the silkscreen), > >>>but I have used them and they work. > >>> > >>>Have fun, > >>> > >>>Stuart > >>> > >>> > >> > >> > > > > > >
