[SI-LIST] Re: AW: Vias on decoupling pads
- From: Larry Smith <Larry.Smith@xxxxxxx>
- To: Sol.Tatlow@xxxxxxxxxxxxxxx
- Date: Tue, 06 Apr 2004 08:41:30 -0700
Sol, Chris - Micro vias in pads can be a very important technology for
reduction of capacitor mounting inductance. But as you indicate,
there is certainly a cost associated with this. My understanding is
that most of the cost is in the setup for micro vias, not in the vias
themselves. Once you decide to put one blind via on a board surface
for any reason, you might as well use a lot of them because the "per
unit" cost is very small once you have paid the setup charge. With
that line of reasoning, you might as well fill up each decoupling cap
pad with as many micro vias as will reasonably fit in order to further
reduce the mounting inductance. It is practical to get blind vias in
pads down to layers 2 and 3 if those are your power and ground plane
levels.
I also would like to see more information on filled vias in pads. I
understand that the technology is available to do this, but once
again, I believe it will be a cost/performance trade-off. Again, once
you use filled vias in a BGA pattern and have the technology on the
board, you might as well use it for the capacitor pads also because
the incremental cost is small.
Several years ago, we determined that you could successfully solder
capacitors on pads that had through hole vias as long as the pads were
for 0805 size caps or larger, and the board was .056 inches thick or
smaller. But now our boards are thicker than that and most of our
caps are smaller than that so this is not as useful as it once was.
regards,
Larry Smith
Sun Microsystems
Sol Tatlow wrote:
>
> Hi Chris,
>
> >Is it ok to put vias actually on the pads of
> >a ceramic decoupling cap in terms of manufacture?
> >Do other people do this?
>
> yes, you CAN do this, BUT it can require technologies
> (micro-via or via-plugging techniques) that are
> otherwise not needed - this can make the PCB more
> expensive, as well as extending delivery times, plus
> can limit your choice of PCB manufacturers: it is NOT
> simply a case of placing normal vias in pads at the
> layout stage and end of story (solder paste disappears
> into the holes=3Dbad/no joints, solder paste application
> difficulties on other side, etc.).
>
> Obviously, via-in-pad CAN give you the best technical
> result/performance with very small decoupling caps,
> where there is no space to put the vias for the
> individual pads BETWEEN the pads (0603 and smaller),
> and in the case of micro-vias allows the placement
> of caps directly under full matrix BGAs where it might
> otherwise not be possible (good against 'bounce'),
> but needs to be weighed against cost requirements.
>
> On a more detailed level, before you use something like
> micro-vias, you perhaps also need to do analysis
> (comparison) of the impedances of the various
> possibilities of connecting the pads to the planes,
> since micro-vias are (obviously!) small. Plus, micro-
> vias (normally) only connect between neighbouring
> layers - stacking is possible, but EXPENSIVE! - which
> means they are perhaps ok for GND (L1-L2) but not
> for PWR (L1-Lx).
>
> Plugging is yet another different story, with different
> methods and (plugging) materials.
>
> If you want more info, let me know, and I can give
> you more info on manfg. techniques that will help
> you evaluate the pros and cons.
>
> Hope this helps!
> ____________________________________
> Sol Tatlow, M.Eng. (Oxon)
> ProDesign Electronic & CAD Layout GmbH
> Product Developer
> Albert-Mayer-Str. 16
> D-83052 Bruckmuehl
> Phone: +49 (0) 8062-808-302
> Fax: +49 (0) 8062-808-333
> Mailto:sol.tatlow@xxxxxxxxxxxxxxxxxxxx
> www.prodesign-europe.com
> ____________________________________=20
>
> -----Urspr=FCngliche Nachricht-----
> Von: Chris Chalmers [mailto:cchalmers@xxxxxxxxxxx]=20
> Gesendet: Dienstag, 6. April 2004 12:48
> An: si-list@xxxxxxxxxxxxx
> Betreff: [SI-LIST] Vias on decoupling pads
>
> ------------------------------------------------------------------
> To unsubscribe from si-list:
> si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field
>
> or to administer your membership from a web page, go to:
> //www.freelists.org/webpage/si-list
>
> For help:
> si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
>
> List FAQ wiki page is located at:
> http://si-list.org/wiki/wiki.pl
>
> List technical documents are available at:
> http://www.si-list.org
>
> List archives are viewable at:
> //www.freelists.org/archives/si-list
> or at our remote archives:
> http://groups.yahoo.com/group/si-list/messages
> Old (prior to June 6, 2001) list archives are viewable at:
> http://www.qsl.net/wb6tpu
>
------------------------------------------------------------------
To unsubscribe from si-list:
si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field
or to administer your membership from a web page, go to:
//www.freelists.org/webpage/si-list
For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
List FAQ wiki page is located at:
http://si-list.org/wiki/wiki.pl
List technical documents are available at:
http://www.si-list.org
List archives are viewable at:
//www.freelists.org/archives/si-list
or at our remote archives:
http://groups.yahoo.com/group/si-list/messages
Old (prior to June 6, 2001) list archives are viewable at:
http://www.qsl.net/wb6tpu
Other related posts:
