[PCB_FORUM] Re: BGA Fanout / Filled vias

Mark:
 
We typically do a secondary soldermask "via cap" on fine pitch BGA vias
so there is NO copper showing on the via.  The secondary soldermasking
operation typically will not have as much "slump" and does not run as
far into the via holes as a single soldermask that is tenting the vias.
 
Your mileage may vary, as others have said check with your board fab and
assembler to verify what they really want.
 
-- 
George Patrick
Tektronix, Inc.
Central Engineering, Engineering Design Services
P.O. Box 500, M/S 39-512
Beaverton, OR 97077-0001
* 503-627-5272 (voice)     * 503-627-5587 (fax)
<http://www.tektronix.com/> 
http://www.tektronix.com     <http://www.pcb-designer.com/>
http://www.pcb-designer.com
 
"Off-Grid and Proud of it!"

-----Original Message-----
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Gerry Meier
Sent: Thursday, February 16, 2006 07:15
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: BGA Fanout / Filled vias


Mark,
 
I would  definitely ask my CM. If he says yes then I would do a via plug
and the entire via would be covered with mask. I don't know how much
soldermask dam you have if it's at least 5 mils you may be OK. Be sure
to specify your via encroahment and or plugging etc in your pcb notes or
requirement doc to your fabricator.
 
One other thing if your pad is 18 mil dia and your soldermask opening is
14 mil dia you only have a 2 mil encroachment. The requirement I have is
for a min of 3 mil encroachment. In my scenario a min soldermask opening
diameter would be 12 mil dia. So also check if the 2 mil is OK
 
regards,
Gerry
 

Gerry Meier

Sr. PCB Designer

Freedom CAD Services, Inc.

Voice: (603) 864-1300 x1350

AL Voice: (256) 417-6944

Email: gerry.meier@xxxxxxxxxxxxxx

Visit us at www.freedomcad.com <http://www.freedomcad.com/> 

 

  _____  

From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Mark Salberg
Sent: Thursday, February 16, 2006 8:53 AM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: BGA Fanout / Filled vias


Yes Gerry,
That is what I consider "copper to copper".
On my 1mm BGA, I have 11.8mil. (18mil BGA pad, 18mil via encroached to
14mil)

Now, on my .75mm BGA using the same via: 6.5mil ball pad to encroached
via

 Should this drive me to filling or tenting the vias?

Thanks for all the great responses!
Mark

Gerry Meier wrote:


Mark,
 
I am not sure what you are asking "is this atrue statement' ?
 
If the soldermask is encroached on the via the copper to copper is the
bga pad to the encroachment area.
There should also be a min 5 mil soldermask dam.
 
 
 
 

Gerry Meier

Sr. PCB Designer

Freedom CAD Services, Inc.

Voice: (603) 864-1300 x1350

AL Voice: (256) 417-6944

Email: gerry.meier@xxxxxxxxxxxxxx

Visit us at www.freedomcad.com <http://www.freedomcad.com/> 

 

  _____  

From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Mark Salberg
Sent: Thursday, February 16, 2006 8:03 AM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: BGA Fanout / Filled vias


On my 1mm BGA, I have an 18mil BGA pad and (18mil via pad, encroached to
14mil with a 8mil hole).
BGA pad (not mask) to via encroachment = 11.8mil.

However, the assembler specified "copper to copper" which would be
"airgap" pad to via measurement.
Copper to copper / airgap = 9.8mil.
The via encroachment to ball copper pad (not larger mask) sounds like
what they should spec.

Is this a correct statement?

Looks like he may be in the "Ball-park" with the filled vias for .8mm
and below pitch BGA's.
On my .75mm BGA I have: 6.5mil ball pad to encroached via.
airgap = 4.5mil. (same for mask to encroached mask on via) = 4.5mil.

Our thought was that if there is a soldermask dam, then there should be
no paste wicking in the via.
But with 10mil min airgap, they must be filled and possibly tented.

When you epoxy fill the vias, do you also tent the vias with mask?


Gerry Meier wrote:


 

Mark,



If you encroach your vias you would measure from pin to encroachment

area. This should give you enough Pin to Via/Encroachment (copper to

copper) clearance for your Assembler. The formula I have used is for a

min 3 mil encroachment is Formula: Pad size diameter - Soldermask

opening diameter > or = to 6 mils. But Soldermask opening diameter is

not < the drill size (nominal hole size + 3 mils). Sample: 18 mil pad -

11 mil soldermask opening = 7 mil + 9.8 = 16.8 pad to via/encroachment

(copper to copper).



This may also work for the .75mm BGA however some Assembler's or CM's

require BGA's with an .8mm pitch or smaller have their vies plugged

under the BGA's.



Hope this helps,

Gerry



Gerry Meier

Sr. PCB Designer

Freedom CAD Services, Inc.

Voice: (603) 864-1300 x1350

AL Voice: (256) 417-6944

Email: gerry.meier@xxxxxxxxxxxxxx

Visit us at www.freedomcad.com



-----Original Message-----

From: icu-pcb-forum-bounce@xxxxxxxxxxxxx

[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Mark Salberg

Sent: Thursday, February 16, 2006 3:25 AM

To: Cadence User Group

Subject: [PCB_FORUM] BGA Fanout / Filled vias



Hello all,

What BGA Ball pad to via clearance is needed for BGA fanout?

Our Assembly house is telling us that we need 10 mil copper to copper

(15mil preferred).

On 1mm BGA's using an 18mil via with 8mil drill gets us 9.8mil via to

pad.

On our .75mm BGA this via gets us 4mil via to pad. Which also breaks the

soldermask dam.



Is epoxy filled and tented vias our best or only option at this point?



Thanks for any input.

Mark





________________________________________________________________________

_____

Scanned by IBM Email Security Management Services powered by

MessageLabs. For more information please visit http://www.ers.ibm.com

________________________________________________________________________

_____

-----------------------------------------------------------

To subscribe/unsubscribe: 

        Send a message to icu-pcb-forum-request@xxxxxxxxxxxxx

        with a subject of subscribe or unsubscribe



To view the archives of this list please login at

http://www.freelists.org. Our list name is icu-pcb-forum or go to

http://www.freelists.org/archives/icu-pcb-forum/



Problems or Questions:

        Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx



Want to post a job listing ?  DON'T DO IT HERE!  

Better yet, join our jobs listing forum.



SUBSCRIBE:  icu-jobs-forum-subscribe@xxxxxxxxxx

POST:       icu-jobs-forum@xxxxxxxxxx

-----------------------------------------------------------

-----------------------------------------------------------

To subscribe/unsubscribe: 

        Send a message to icu-pcb-forum-request@xxxxxxxxxxxxx

        with a subject of subscribe or unsubscribe



To view the archives of this list please login at

http://www.freelists.org. Our list name is icu-pcb-forum

or go to http://www.freelists.org/archives/icu-pcb-forum/



Problems or Questions:

        Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx



Want to post a job listing ?  DON'T DO IT HERE!  

Better yet, join our jobs listing forum.



SUBSCRIBE:  icu-jobs-forum-subscribe@xxxxxxxxxx

POST:       icu-jobs-forum@xxxxxxxxxx

-----------------------------------------------------------



________________________________________________________________________
_____

Scanned by IBM Email Security Management Services powered by
MessageLabs. For more information please visit http://www.ers.ibm.com

________________________________________________________________________
_____



  


________________________________________________________________________
_____
Scanned by IBM Email Security Management Services powered by
MessageLabs. For more information please visit http://www.ers.ibm.com
________________________________________________________________________
_____

________________________________________________________________________
_____
Scanned by IBM Email Security Management Services powered by
MessageLabs. For more information please visit http://www.ers.ibm.com
________________________________________________________________________
_____



This correspondence and any attachments are considered confidential. If
you are not the intended recipient, please notify Freedom CAD Services,
Inc. immediately by either replying to this message or by sending an
email to operations@xxxxxxxxxxxxxx; please destroy all copies of this
message and any attachments. Thank you. 

JPEG image

Other related posts: