From: Lum Wee Mei ([email protected])
Date: Mon Oct 25 1999 - 19:32:52 PDT
If I have a 400-balls BGA on a 12 layers board, can I use blind-via of 0.3mm diameter as via-in-pads on the BGA. How deep can my blind-via goes before there can be assembly problems like those mentioned in some of the earlier
discussions?
Regards.
Matt Kaufmann wrote:
> 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)
> [email protected]
>
> > -----Original Message-----
> > From: [email protected]
> > [mailto:[email protected]]On Behalf Of Dave Hoover
> > Sent: Thursday, October 14, 1999 8:22 AM
> > To: '[email protected]'
> > 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:[email protected]]
> > Sent: Thursday, October 14, 1999 5:02 AM
> > To: [email protected]
> > 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
> > [email protected] <mailto:[email protected]>
> > tel 972-9-7751239
> > Fax 972-9-7751212
> >
> > **** To unsubscribe from si-list: send e-mail to
> > [email protected]. 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 [email protected]. 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 [email protected]. 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 ****
This archive was generated by hypermail 2b29 : Tue Feb 29 2000 - 11:39:19 PST