Re: gEDA-user: latest PCB w/gsch2pcb deletes parts?

[Matt Ettus <boyscout@xxxxxxxxx>]

Why do you need different ones for cap, res, and ind?

Matt

On 12/9/05, Dan McMahill <dan@xxxxxxxxxxxx> 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 <sdb@xxxxxxxxxx> 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
> >>>
> >>>
> >>
> >>
> >
> >
>
>