[PCB_FORUM] Re: 0.5 mm BGA, whew!

Gary:
 
You might try sequential lam for your outers, with microvias from 1-2 and
1-3 on the core outers, then 1-2  and 1-3 on your post-laminated outers.  
 
The results are 1-2, 1-3, 2-3, 2-4.  You can do a stacked 1-2 and 2-4 to get
1-4.  Be sure to check with your vendor about the 2 layer microvias, we have
one vendor who wants the middle layer pad suppressed for these vias, and
another that wants the middle layer pad included.  Different strokes for
different folks :)
 
FWIW, We don't build any microvias into any parts except some of our high
frequency decoupling caps.
-- 
George Patrick
Tektronix, Inc.
Central Engineering, PCB Design Group
P.O. Box 500, M/S 39-512
Beaverton, OR 97077-0001
Phone: 503-627-5272         Fax: 503-627-5587 <http://www.tektronix.com/> 
http://www.tektronix.com     <http://www.pcb-designer.com/>
http://www.pcb-designer.com

It's my opinion, not Tektronix' 

-----Original Message-----
From: Gary MacIndoe [mailto:gary.macindoe@xxxxxxx] 
Sent: Friday, October 29, 2004 12:36
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
Advanced Micro Devices, 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
Advanced Micro Devices, Inc.
Longmont, Colorado

Other related posts: