Re: gEDA-user: Anybody had luck with QFN64 at PCBExpress et al?

["Steven Michalske" <smichalske@xxxxxxxxx>]

I used rounded and square pads on my QFN designs,  The boards were
made at Sierra proto express.  They may not be the cheapest,  but they
can do bards with 1 mil traces.

I did not have the boards assembled, I hand soldered them,  not on a
hot plate or other oven like methods.

Drag soldering the QFN is not a difficult process,  it just takes a
bit of time to line up the pins to the pads 2 dimensionally.  solder
paste probably would have helped.

The thermal pad on the backs of QFN and friends, I put in one or two
untented vias, they serve two purposes, I can now hand solder through
them, and they thermally connect the thermal pad to the copper on the
opposite side.


Best of luck on you boards!

Steve

On Feb 2, 2008 11:55 AM, Jeffrey Baker <jwbaker@xxxxxxxxx> wrote:
> On Feb 2, 2008 11:41 AM, joe tarantino <joeft@xxxxxxxxxxxxx> wrote:
>
> >
> >
> >
> >
> >
> >
> > On Feb 2, 2008 11:23 AM, Jeffrey Baker <jwbaker@xxxxxxxxx> wrote:
> >
> > >
> > >
> > >
> > > Nearly every major part I need for my latest project is packaged in a
> QFN (or LFCSP as they call it over at Analog Devices).  I'm worried because
> the parts have round leads and Sunstone, the PCB prototype shop, says they
> can't make radiused SMD pads.  Has anyone run into trouble with this, or are
> square pads OK?
> > >
> > > Generally speaking the .5mm-pitch QFN seems to be on the edge of or
> beyond the capabilities of a proto shop like Sunstone, but Sunstone has the
> best tolerances I've been able to find.
> > >
> >
>
> >
> >
> > >
> > >
> > >
> > >
> >
> >
> > I have had one of the Sunstone shops build boards with QFN32 and QFN48 as
> I recall.  Results were pretty good.  They had square-ended pads.
>
>
> DId you draw them that way, or did you draw them rounded?
>
>
> >
> >
> >
> > -Be careful of solder resist "floaters" due to the little pieces between
> the leads.  Best bet is to remove all resist between pads.
>
> Interesting.  Manufacturers seem to disagree on this point.  Freescale says
> remove solder mask between pins.  Intersil says keep it.  Sunstone can do
> .005" solder mask web so it's just barely possible to have it either way.
> You don't worry about solder bridges without solder mask?
>
> >
> >
> >
> > -You may want to check your gerber files to see how much solder paste will
> be applied and check with Sunstone to see if it is sufficient (or too much).
> >
> > Does your pad have a large heat sink pad on the back?  If so, you must
> carefully construct this pad in the footprint (possibly out of multiple
> squares).  Again, check the paste layer.
> >
>
> Oh yes, the dreaded exposed pad.  I appreciate the thermal properties of
> this package.  However I find drawing it to be a huge nuisance.  I drew the
> stencil layer with an array of rectangles of the same size as the SMD pads
> (.30mmx.65mm) separated by .13mm.  It seems like that should give a decent
> coverage without leaving the part high-centered.
>
> Thanks for the tips!
>
>
>
> _______________________________________________
> geda-user mailing list
> geda-user@xxxxxxxxxxxxxx
> http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
>
>


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