[PCB_FORUM] Re: .4 mm pitch bga's
- From: PETER PIETRANGELO <peter_pietrangelo@xxxxxxxxxxxxx>
- To: icu-pcb-forum@xxxxxxxxxxxxx
- Date: Wed, 1 Nov 2006 16:02:35 -0800 (PST)
What is high volume to you? Everything we do is 500K-2M / month. Is yours a
cell phone board? I have seen some that are using stacked micro vias so they
can do .100mm via size. There is a board shop in Asia doing .100mm mechanical
drill in volume.
Gino Papelera <da.papelera@xxxxxxxxx> wrote: Peter,
Thank You for the info. We will be using 10 layers with stacked microvias. 4
layers will be internal planes.
This product will be high volume. Minimum linewidth is .075mm.
regards,
Gino
On 10/30/06, Peter <peter_pietrangelo@xxxxxxxxxxxxx> wrote: We do
.300mm pad .150mm drill on 6 layer .5mm thick BT. That is 500K/month qty. We
have also done .250mm pad and .100mm micro via in pad. Also stacked vias.
Obviously there is increased cost and lead times as well. Is it a high volume
product?
Peter
---------------------------------
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx [mailto:
icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of sjchar3@xxxxxxxxxxxx
Sent: Monday, October 30, 2006 7:23 AM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: .4 mm pitch bga's
We usually call the board house and ask them if they can do it. The
smallest we've gone is .5mm pad with .3 mm drill. The BGA was a 7x7 array but
the ic used only the two outside rows. We used via in pad, now I need to write
up a paper on how i did the board. Anyone seen good documentation on this
subject (BGAs, Microvias)?
Thanks Sam
-----Original Message-----
From: rmora@xxxxxxxxxxxxxxxxxxxx
To: icu-pcb-forum@xxxxxxxxxxxxx
Sent: Fri, 27 Oct 2006 9:39 AM
Subject: [PCB_FORUM] Re: .4 mm pitch bga's
Gino,
Wow, where will it end.
We use a .25mm pad with a .1mm hole and that's pushing it. But our application
is a high volume product.
What is the BGA pad size you are using?
Are you using stacked vias?
Are the BGA pads masked defined or etch defined.
These will all have an impact on the via pad, trace space numbers.
Are you under filling the BGA?
For the very dense designs we use ALIVH technology in an 8 layer stack up.
This allows us to put a via in pad and route directly down to any layer.
Ron
At 10:06 AM 10/27/2006 -0500, you wrote:
Everyone,
What's your recommendation for microvia sizes, line and spacing for routing
.4mm bga's?
I saw a technotes using .065mm line and space between 0.2mm pad/0.1 drill
micro via. Anyone using these in their designs?
regards,
Gino
---------------------------------
size=2 width="100%" align=center>
Check Out the new free AIM(R) Mail -- 2 GB of storage and industry-leading
spam and email virus protection.
Other related posts:
