[PCB_FORUM] Re: .8-MM BGA Geometry
- From: "Richard E Marion" <ricmar@xxxxxxxxxxx>
- To: <icu-pcb-forum@xxxxxxxxxxxxx>
- Date: Wed, 14 Sep 2005 14:24:21 -0400
Thank You Stephen,
I now have a better understanding of 0.8-MM.
The Fear Is Gone.
Appreciatively,
Richard E Marion
169 Little Mill Road Unit 2
Sandown NH 03873-2554
HOME: 603-887-2266
CELL: 603-247-1610
FAX : 603-887-2936
-----Original Message-----
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Feehan, Stephen
Sent: Wednesday, September 14, 2005 11:32 AM
To: 'icu-pcb-forum@xxxxxxxxxxxxx'
Subject: [PCB_FORUM] Re: .8-MM BGA Geometry
Hi Richard,
The top side solder mask for the bga pad is 16 mils, the same as the top.
For the via's
I encroach the solder mask so I use a 12 mil clearance for the top and the
bottom vias
can be 20 mil clearance so its possible to do a flying probe test.
When routing inside the bga area keep in mind that you may need to reduce
the etch
because most fab houses like to have a min. of 4 mils from via to etch
spacing. In my
case the impedance required a 4 mil etch so I only needed to reduce the etch
to 3.75 mils
inside the bga's.
If needed you can reduce the size of the via on inner layer to 19.5 mils.
Regards,
Stephen
Siemens Communications, Inc.
_____
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Richard E Marion
Sent: Wednesday, September 14, 2005 10:29 AM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: .8-MM BGA Geometry
Hello Stephen,
The 20/10 Via keeps "popping up", must be a good choice.
On the 16-Mil BGA Pad, what diameter Soldermask do you recommend?
Thank you for sharing your experience with me.
Sincerely,
Richard E Marion
169 Little Mill Road Unit 2
Sandown NH 03873-2554
HOME: 603-887-2266
CELL: 603-247-1610
FAX : 603-887-2936
-----Original Message-----
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Feehan, Stephen
Sent: Wednesday, September 14, 2005 9:55 AM
To: 'icu-pcb-forum@xxxxxxxxxxxxx'
Subject: [PCB_FORUM] Re: .8-MM BGA Geometry
Richard,
You can start with a 16 mil bga pad and a 20 mil pad / 10 mil drill with a
28 mil
anti pad for the via.
In some designs I use the via in pin technology for all the gnd pins of a
0.8mm bga.
The drill of the micro via is 4 mils and is build into the pad. Typically, I
make sure
Layer 2 is a gnd plane so all the micro vias hit directly into the plane.
Call Merix Corp, they have local reps in MA/NH.
Stephen
Siemens Communications, Inc
_____
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Richard E Marion
Sent: Tuesday, September 13, 2005 6:27 PM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] .8-MM BGA Geometry
Dear Forum,
My Client is utilizing a 0.8-MM SDRAM Package.
The smallest BGA Pitch I have dealt with so far is 1.0-MM.
The Fabrication/Assembly Vendors are yet to be determined.
The PCB "target" construction is 0.062-Inch 14-Layer, three sets of dual
embedded stripline. No Blind/Buried Vias (all Thru Via).
Questions:
1. Any recommendations for local (NH-MA) Fabrication/Assembly Vendors
capable of working with this BGA Geometry?
2. BGA SMT Pad Diameter?
3. BGA SMT Soldermask Diameter?
4. Thru Via Drill?
5. Thru Via Pad Diameter?
6. Alternatively, is Via-In-Pad an option?
7. Any chance of ATE Testing 0.8-MM Pitch?
Thank You,
Richard E Marion
169 Little Mill Road Unit 2
Sandown NH 03873-2554
HOME: 603-887-2266
CELL: 603-247-1610
FAX : 603-887-2936
Other related posts:
