For signal layers, we use a 12mil drill with a 25mil pad. This allows up to
5/5 within the BGA field.
The 12 mil drill into 0.062 thick board also saves money. Shop will charge
you extra for vias they have to mask or plug. See IPC-2222 Sec. 9.2.2.3
page 19 for the rules of thumb. Aspect ratio of 6:1 or less when you can is
always good.
We haven't done any BGA on 0.093 thick board here. However, aspect ratio
becomes a factor. I have found that shop will charge you extra because of
that phenomenon.
At any rate, if you need to go smaller with the vias, use 0.025mil pad on
the plane layers which will give you better thermal relief definition. I
have found that shop will charge you extra NRE when they have to redefine
thermals.
I've successfully used 0.025mil pads on plane layers all the way down to
0.75mm BGA. That uncommon pitch, seen only on a very few SRAMs, required
8mil drill and 18mil pad with 0.1mm/0.1mm routing within the BGA field on
the signal layers.
See my message dated 10/11/2006 titled "Maximum drill size for vias in
0.75mm BGA fanout" for details on what I went through. On that same board I
used the 12mil drill and 25mil pad for the 1mm BGA as recommended above.
Thanks and Best Regards,
----------------------------
Gary M. Koven, C.I.D.
Dynazign, Inc.
Charlotte, NC, USA
Veteran of the Marsh School
-----Original Message-----
From: DesignerCouncil [mailto:[log in to unmask]] On Behalf Of Carol
Chapman
Sent: Tuesday, May 15, 2007 9:46 AM
To: [log in to unmask]
Subject: Re: [DC] Via Specification
We've used an 8mil drill with a 19mil pad. This allows us to route 4/4
within the BGA field.
Carol Chapman, CID+
PG ECAD Design, Sr. Analyst
MS RR5-38
Dell, Inc
501 Dell Way
Round Rock, TX 78682
512-728-4494
-----Original Message-----
From: DesignerCouncil [mailto:[log in to unmask]] On Behalf Of
Brionez, Gregory
Sent: Tuesday, May 15, 2007 6:07 AM
To: [log in to unmask]
Subject: [DC] Via Specification
Karl - I know you are lurking.
I need to specify a via for a 1mm BGA. We use to do these a lot at
Tellabs.
My gray matter deceives me.
Anyone please let me know what you are using for .063, .093 thick PCBs.
Thank for all replies.
Paul Brionez - CID +
[log in to unmask]
PCB Designer
PH: 847-673-2718 x1394
FAX: 847-673-9789
DIVISION: Electronic/Systems
MPC Products Corporation
<http://www.mpcproducts.com/> ISO 9001 Certified Skokie, IL USA
***************************************************************
This message and any attachment are confidential and may be privileged
or otherwise protected from disclosure. If you are not the intended
recipient, you must not copy this message or attachment or disclose the
contents to any other person. If you have received this in error,
please email the sender or telephone in the United States at (847)
673-8300 and delete this message and any attachment from your system.
For further information about MPC Products Corporation please see our
web- site at http://www.mpcproducts.com or refer to any MPC Products
Corporation office.
***************************************************************
------------------------------------------------------------------------
---------
DesignerCouncil Mail List provided as a free service by IPC using
LISTSERV 1.8d To unsubscribe, send a message to [log in to unmask] with
following text in the BODY (NOT the subject field): SIGNOFF
DesignerCouncil.
To temporarily stop/(restart) delivery of DesignerCouncil send: SET
DesignerCouncil NOMAIL/(MAIL) Search previous postings at: www.ipc.org >
On-Line Resources & Databases > E-mail Archives Please visit IPC web
site http://www.ipc.org/contentpage.asp?Pageid=4.3.16 for additional
information, or contact Keach Sasamori at [log in to unmask] or 847-615-7100
ext.2815
------------------------------------------------------------------------
---------
----------------------------------------------------------------------------
-----
DesignerCouncil Mail List provided as a free service by IPC using LISTSERV
1.8d
To unsubscribe, send a message to [log in to unmask] with following text in
the BODY (NOT the subject field): SIGNOFF DesignerCouncil.
To temporarily stop/(restart) delivery of DesignerCouncil send: SET
DesignerCouncil NOMAIL/(MAIL)
Search previous postings at: www.ipc.org > On-Line Resources & Databases >
E-mail Archives
Please visit IPC web site http://www.ipc.org/contentpage.asp?Pageid=4.3.16
for additional information, or contact Keach Sasamori at [log in to unmask] or
847-615-7100 ext.2815
----------------------------------------------------------------------------
-----
---------------------------------------------------------------------------------
DesignerCouncil Mail List provided as a free service by IPC using LISTSERV 1.8d
To unsubscribe, send a message to [log in to unmask] with following text in
the BODY (NOT the subject field): SIGNOFF DesignerCouncil.
To temporarily stop/(restart) delivery of DesignerCouncil send: SET DesignerCouncil NOMAIL/(MAIL)
Search previous postings at: www.ipc.org > On-Line Resources & Databases > E-mail Archives
Please visit IPC web site http://www.ipc.org/contentpage.asp?Pageid=4.3.16 for additional information, or contact Keach Sasamori at [log in to unmask] or 847-615-7100 ext.2815
---------------------------------------------------------------------------------
|
