[PCB_FORUM] Re: 0.5 mm BGA, whew!

From: "richard moffat" <richard.moffat@xxxxxxxxxxxxxxxxxxx>
To: <icu-pcb-forum@xxxxxxxxxxxxx>
Date: Wed, 03 Nov 2004 10:53:38 +1300
Hi

Just out of interest, what was the field solver / calculator you used
for this?

>>> Blake.Moore@xxxxxxxxxx 3/11/2004 10:24:22 a.m. >>>
Feed back info on this question was good, also consider how you would
connect pin to pin if pwr is on an outer layer?
You wouldn't want the pwr on the outer top or bottom, because then it
would limit your ability to run etch for the pin to pin net
connections.

10 layer Stack-up                            Line/Space

Signal--        Top layer 50 ohms single ended = 19 mils
Top layer 100 ohms differential = 15 mils / 15 mils

Plane------------GND----------------------------

Signal--        Inner Layer 50 ohms single ended = 10 mils
Inner layer 100 ohms differential = 10 mils / 20 mils

Plane-----------GND-------------------------------------------

Plane-----------PWR------------------------------------------

Plane-----------PWR------------------------------------------

Plane-----------GND------------------------------------------

Signal--        Inner Layer 50 ohms single ended = 10 mils
Inner layer 100 ohms differential = 10 mils / 20 mils

Plane-----------GND------------------------------------------

Signal--        Bottom layer 50 ohms single ended = 19 mils
Bottom layer 100 ohms differential = 15 mils / 15 mils 
------------------------------------------------------------------------
--

-----Original Message-----
From: Kevin McCowan [mailto:kmccowan@xxxxxxxxxxxxxx] 
Sent: Tuesday, November 02, 2004 3:47 PM
To: icu-pcb-forum@xxxxxxxxxxxxx 
Subject: [PCB_FORUM] Re: 0.5 mm BGA, whew!

WOW! A post that is actually on topic!
Not that it wasn't fun or anything.

I distribute power and ground based on needing a signal layer next to
a
solid plane. Your stackup should be built around the performance you
need not "should it be in the middle" type parameters. Many things
drive
the stackup and all should be considered.

Kevin McCowan
Sr. PCB Designer
TSI Telsys

Tom Robinson wrote:
> Is it better the have the pwr & gnd in the middle of the board?
>  
> tr :)
>  
> 
>     -----Original Message-----
>     *From:* Gary MacIndoe [mailto:gary.macindoe@xxxxxxx] 
>     *Sent:* Friday, October 29, 2004 3:36 PM
>     *To:* icu-pcb-forum@xxxxxxxxxxxxx 
>     *Subject:* [PCB_FORUM] Re: 0.5 mm BGA, whew!
> 
>     Natalie,
>      
>     Thanks for the reply!
>      
>     1)  Are you saying the through hole micro vias built into the
pads
>     are stacked, right?
>      
>     3)  Yes I'm still using mils, been doing it this way for 16
years.

>     Allegro handles the round off quite well (to the tenth of a mil,
>     which is to 1/10,00 of an inch).
>      
>     4)  I'm just comfortable with mils.  Have not designed/post
>     processed at all in mm.
>      
>     5)  As far as I know micro vias (laser drilled) can only be 1-2
or
>     1-3.  I would still need to get to layer 4, since I believe I
will
>     need three routing layers, all of which need to reference to a
plane
>     (Top-route, L2-gnd, L3-route, L4-route, L5-pwr, Bottom).  How do
you
>     mean "have a micro via in pad set for 1-4"?  Are you saying
stacked
>     micro vias?
>      
>     Thanks again for your help.
> 
>     Gary E. MacIndoe
>     PCB Design Engineer
>     *A*dvanced *M*icro *D*evices, Inc.
>     Longmont, Colorado
> 
>         -----Original Message-----
>         *From:* Degennaro, Natalie N
[mailto:natalie.n.degennaro@xxxxxxxxx] 
>         *Sent:* Friday, October 29, 2004 10:59 AM
>         *To:* icu-pcb-forum@xxxxxxxxxxxxx 
>         *Subject:* [PCB_FORUM] Re: 0.5 mm BGA, whew!
> 
>         Gary,
> 
>          
> 
>         1)       We use micro vias in pad (built into padstack used,
and
>         are through hole).
> 
>         2)       Decide ahead of time and build them into the
symbol.
>         Otherwise "replace padstack" for when you do know what
layers
>         you need to connect to. That will get you out of the DRC
>         quandary. You can use the blind/buried via wizard to
generate
>         them automatically.
> 
>         3)       Why are you still using a .brd in mils? Your parts
are
>         dictating that you need to switch to millimeters (like we
have).
>         Or is this just a personal thing? (LOL). Parts built in
>         millimeters and then read into a mils .brd will have round
off.
> 
>         4)       Why do this?
> 
>         5)       Why not have a micro via in pad set for 1-4, in
your
>         example? Your three mv's are going to connect anyway, if
they
>         are at same center.
> 
>          
> 
>         It doesn't have to be as hard as you think. Just change the
way
>         you think and try something new (LOL). It can be fun!
> 
>          
> 
>         Natalie
> 
>          
> 
>         
>
----------------------------------------------------------------------
> --
> 
>         *From:* Gary MacIndoe [mailto:gary.macindoe@xxxxxxx] 
>         *Sent:* Friday, October 29, 2004 9:06 AM
>         *To:* Allegro Forum
>         *Subject:* [PCB_FORUM] 0.5 mm BGA, whew!
> 
>          
> 
>         All,
> 
>          
> 
>         Well, it seems to be a slow day on the Forum, so I'll
through
>         out a relatively involved set of questions!
> 
>          
> 
>         We are looking into using a 0.5 mm BGA in a very dense
design,
>         so big time HDI practices will come into play: micro vias
(MVs),
>         probably even stacked micro vias (SMVs), in order to fan out
on
>         several layers.
> 
>          
> 
>         -  would you use the micro vias in pad or not?  Why?  Build
them
>         into the symbol?
> 
>          
> 
>         -  how can you have the micro vias built into the symbol if
you
>         don't know which balls will go down to which layer?
> 
>          
> 
>         -  I will make the 0.5 mm BGA Allegro symbol with the
drawing
>         units set to Millimeters, but would like to keep the design
>         database set to Mils.  Is this the way most of you have done
it?
> 
>          
> 
>         -  if the symbol is set to Millimeters and the design set to
>         Mils, this makes dropping the micro vias (in pad or not)
after
>         the BGA symbol is placed in the design tricky.  Any other
way
to
>         get around this?
> 
>          
> 
>         -  So, setting up blind/buried micro vias should be the same
as
>         any blind/buried via.  How about SMVs?  If you have a micro
via
>         set up for layers 1-2, 2-3, 3-4, etc., how do you avoid the
DRCs
>         when you stack them (same X,Y)?
> 
>          
> 
>         My head is about spinning trying to comprehend all of this
micro
>         via/stacked micro via stuff!
> 
>          
> 
>         Any help from someone that has already used a 0.5 mm BGA on
a
>         very dense design with stacked micro vias would be greatly
>         appreciated!!
> 
>          
> 
>         Thanks in advance,
> 
>         Gary E. MacIndoe
>         PCB Design Engineer
>         **A**dvanced **M**icro **D**evices, Inc.
>         Longmont, Colorado
> 
>          
> 
> This message and any file transmitted with it may contain
confidential

> information and is exempt from disclosure under applicable law. The 
> information contained in this message and any file transmitted with
it

> is transmitted in this form based on a reasonable expectation of 
> privacy. Any disclosure, distribution, copying or use of the 
> information by anyone other than the intended recipient, regardless
of

> address or routing, is strictly prohibited. If you have received this

> message in error, please advise the sender by immediate reply and 
> delete the original message. Personal messages express views solely
of

> the sender and are not attributable to Biodex Medical Systems, Inc.
> 
-----------------------------------------------------------
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
//www.freelists.org. Our list name is icu-pcb-forum or go to
//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
//www.freelists.org. Our list name is icu-pcb-forum
or go to //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 
-----------------------------------------------------------

NOTICE: This message contains privileged and confidential
information intended only for the use of the addressee
named above. If you are not the intended recipient of
this message you are hereby notified that you must not
disseminate, copy or take any action in reliance on it.
If you have received this message in error please
notify Allied Telesyn Research Ltd immediately.
Any views expressed in this message are those of the
individual sender, except where the sender has the
authority to issue and specifically states them to
be the views of Allied Telesyn Research.
-----------------------------------------------------------
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
//www.freelists.org. Our list name is icu-pcb-forum
or go to //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
-----------------------------------------------------------
[PCB_FORUM] Re: 0.5 mm BGA, whew!

Other related posts:
