RE: [SI-LIST] : micro BGA SI vrs PCB consideration

Dave Hoover (dhoover@mccurdy.com)
Thu, 14 Oct 1999 10:29:10 -0700

True. You can terminate (not so sure this is the right word)
the microvia at lyr 2 or lyr 3 as long as the correct
aspect ratio is maintained (as previously discussed). Through
hole vias are very hard to process as via-in-pad and I agree
with Matt...don't go there.

Dave
-----Original Message-----
From: Matt Kaufmann [mailto:matt@silicon-spice.com]
Sent: Thursday, October 14, 1999 9:45 AM
To: si-list@silab.eng.sun.com
Subject: RE: [SI-LIST] : micro BGA SI vrs PCB consideration

Be careful when you talk about via-in-pad. Yes, a microvia is technically a
via-in-pad and would be acceptable (and probably advisable for fine pitch
parts (<1 mm)) but via-in-pad can also denote a drilled via in the center of
the BGA pad which is a big no-no since the via can wick solder away from the
joint (a microvia will not have this problem since the via is terminated at
the second layer).

Matt

Matt Kaufmann
Senior Packaging Engineer
Silicon Spice Inc.
415 East Middlefield Road
Mountain View, CA 94043-4005
650-567-7824
408-806-9680 (cell/pager)
650-940-7770 (fax)
matt@silicon-spice.com

> -----Original Message-----
> From: owner-si-list@silab.eng.sun.com
> [mailto:owner-si-list@silab.eng.sun.com]On Behalf Of Dave Hoover
> Sent: Thursday, October 14, 1999 8:22 AM
> To: 'si-list@silab.eng.sun.com'
> Subject: RE: [SI-LIST] : micro BGA SI vrs PCB consideration
>
>
> You can use that stack-up from a PCB fab standpoint.
> The microvias can go to layer 2 (or layer 3 or 4).
> The real issue is the following:
> 1) The microvia needs to be <=.7:1 Aspect Ratio.
> This is to guarantee the plated hole quality. (+/- 3 sigma)
> 2) The depth of the microvia needs to be evaluated from an
> assembly approach. For example, for via-in-pad will
> the microvia create a huge bubble during reflow? If so
> does the solder void violate the 20% max rule?
>
> I agree that for CSP (<.8mm pitch grid array packages) that
> microvia is the best approach. It allows more rout channels
> for signals.
>
> You can have signals on the outerlayers also. Via-in-pad
> provides more room for that. You can even have a plane
> on layer 2 with a signal on 3 to have the plane act as an
> EMI shield. (Get noisy clocks under a plane) like...
>
> sig (c/s)
> pln
> sig
> ...
>
> There are MANY reasons I've seen for MicroVias. Here's just
> a few.
> 1) Fine Pitch BGA. (Like CSP, FPBGA, DSP. Pitch's less that 1.0mm)
> 2) Via-in-pad. (To free up real estate under the BGA's so termination
> resistors and caps can be mounted as close as possible to the device)
> 3) Dropping a noisy clock/signal below a plane (to lyr 3) for EMI/EMC
> reasons.
> 4) Providing distributed plane capacitance right at the solder ball
> (no lead inductance which can degrade electrical performance on
> high speed devices)
> 5) Separating Logic types on the PCB on one side only with something
> else on the other. With microvias you could leave the planes intact
> with no clearances or "swiss cheese" effect.
> (i.e., Analog, Digital, RF, Control, or Microwave)
> 6) Connecting directly to planes for heat dissipation (or pwr)
> without "swiss cheesing" the plane(s).
>
> That's just a few. It looks like when the PCB (or substrate) get's
> greater than 130 Holes per square inch, then microvias (or
> buried/blind vias) are necessary.
>
> Common PCB types using microvia are:
>
> Portable Consumer Products
> like GPS, PDA, camcorders, PCS, and Cellular Phones.
>
> Interposer/Adapter Boards
> like BGA to CSP, QFP to BGA, CSP to BGA (The skys the limit here)
>
> Organic Chip Carrier Packages (FlipChip, PBGA, MCM-L)
> like CSP or microBGA
>
> Wireless Products
> like Wireless Base stations
>
> Memory Modules
> like SIMM
>
> Computer Networking Cards
> like PCI, Compact PCI, Mother Boards
>
> What have I forgot?
>
> Dave
> -----Original Message-----
> From: Ilan Adar [mailto:ilan.adar@seabridge.co.il]
> Sent: Thursday, October 14, 1999 5:02 AM
> To: si-list@silab.eng.sun.com
> Subject: [SI-LIST] : micro BGA SI vrs PCB consideration
>
>
> hallo
>
> We run into some problems when using micro BGA.
>
> We used PTH vias between the micro BGA pads and this leads us to
> low yield in the manufacturing .
>
> the PCB people tell us that we must use micro via technology, but this
> requires us
> to change the PCB stack to :
> CS
> SIG
> SIG
> GND
> ..
> ..
> ..
> ..
>
> can I use such a stackup ? or is there a mother solution to micro BGA PCB
> layout.
>
> thanks very much
>
> Ilan Adar
> Ilan.adar@seabridge.co.il <mailto:Ilan.adar@seabridge.co.il>
> tel 972-9-7751239
> Fax 972-9-7751212
>
> **** To unsubscribe from si-list: send e-mail to
> majordomo@silab.eng.sun.com. In the BODY of message put:
> UNSUBSCRIBE si-list, for more help, put HELP. si-list archives
> are accessible at http://www.qsl.net/wb6tpu/si-list ****
>
>

**** To unsubscribe from si-list: send e-mail to
majordomo@silab.eng.sun.com. In the BODY of message put: UNSUBSCRIBE
si-list, for more help, put HELP. si-list archives are accessible at
http://www.qsl.net/wb6tpu/si-list ****

**** To unsubscribe from si-list: send e-mail to majordomo@silab.eng.sun.com. In the BODY of message put: UNSUBSCRIBE si-list, for more help, put HELP. si-list archives are accessible at http://www.qsl.net/wb6tpu/si-list ****