Re: gEDA-user: Next step questions

[DJ Delorie <dj@xxxxxxxxxxx>]

> Well, my PCB arrived in the mail a short while ago.  I soldered in
> the components, and everything works beautifully.

Yay!  Mine's in fab now.

> 1. Is it possible when autorouting traces in PCB to have some
> automatically set to one set of thicknesses, drill hole sizes,
> etc. and others automatically set to another set of thicknesses,
> drill hole sizes, etc?  Or must I always select traces by hand to be
> autorouted to a specific set of thicknesses, drill hole sizes, etc?

In theory, you can assign route styles to nets, but I've never done
it, nor do I know if it works.

> 2. I noticed in examining the PCB design after autorouting that
> extra "nubbins" occasionally appeared on traces.

Have you tried the optimizer?  It's intended to clean up after the
autorouter.

> 3. In my next PCB, I need to add surface mount components.  I've
> noticed that some part data sheets spec out the pad sizes, but many
> don't--they just spec out the part feet.  Are there good general
> rules for making SMT pads?  Generally, what should the space be
> *between* the pads?

For many parts, if they're a "standard" footprint, PCB has a standard
footprint for them.  For example, 0603's, SSOPs, TQFPs, etc.  If in
doubt, the specs I've seen normally have something like 60% of the
pitch for the width of the pad, and 40% for the space between them.
If you need to route traces between pads, set the space according to
your design rules (i.e. 6 mil rules, space at least 18 mil).

Also, make sure the footprint doesn't exceed your line/space rules,
and think about your mask up front - if there may be enough space to
have mask between pads, make sure you leave it.  FABs spec how far the
mask should be from the copper, and how thin the mask can be, add
those up to get a minimum space.  If it's too small, you won't have a
mask anyway, so you can ignore that part.

If you really have to make things up, this is what I do (refer to
http://www.gedasymbols.org/user/dj_delorie/tools/dilpad.html):

* space between rows of pads (G) is the minimum package body width.

* total width (PXL) is the maximum width lead-tip to lead-tip, plus 20
  mil (I allow 10 mil on each side for hand soldering if needed).

* pad width (PW) is the same or slightly more than the lead width
  (LW).  This makes the space between (PG) anywhere from 50% to 100%
  of the available space.


_______________________________________________
geda-user mailing list
geda-user@xxxxxxxxxxxxxx
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user