[SI-LIST] Re: 0.8mm BGA routing
- From: "Istvan NOVAK" <istvan.novak@xxxxxxxxxxxxxxxx>
- To: "mediwheel_js" <mediwheel_js@xxxxxxxxxxxxx>,<vincenzo@xxxxxxxxxxxxxx>
- Date: Tue, 30 Dec 2003 11:32:53 -0500
Jack,
The impact of anti-pad on signal routing should not be ignored.
The plane perforation has consequences on both the signal
integrity of traces referencing the perforated plane and on the
power distribution network using the perforated plane.
In my message below I just mentioned the extreme possibility
of completely cutting the plane with anti-pads. In a separate
thread recently, Zhangkun asked about the impact of perforation
on trace signal integrity.
As usual, whether perforation is a problem, it depends on:
both the increase of impedance and increase of crosstalk will
have a time duration equaling the time of flight through the
perforated area. If this time of flight is much less than the
signal transition time, the impact is minimal. For fast edges and
long paths over perforated areas, the impedance increase
will create extra reflections, and crosstalk also goes up.
You can try to compensate for the impedance change either by
narrowing the trace over non-perforated areas, thus increasing
the overall trace impedance (you may need to adjust the termination
values accordingly), or you can try to decrease the trace impedance
over perforated areas by making it wider (this, however, will further
increase the already higher crosstalk and will further limit routing
density).
I hope this helps.
Regards,
Istvan
----- Original Message -----
From: "mediwheel_js" <mediwheel_js@xxxxxxxxxxxxx>
To: <istvan.novak@xxxxxxxxxxxxxxxx>; <vincenzo@xxxxxxxxxxxxxx>
Cc: "Tayyab Jamil" <tayyab@xxxxxxxxxxxxxx>; <si-list@xxxxxxxxxxxxx>
Sent: Monday, December 29, 2003 9:25 PM
Subject: Re: [SI-LIST] Re: 0.8mm BGA routing
> Istvan,
>
> One thing that I did not see mentioned was the anti-pad, and
> its effect on signal routing thru the via array. Should this
> aspect be ignored or is there someway to compensated for
> this???
>
> thanks,
>
> Jack Stone
>
>
> ----- Original Message -----
> From: "Istvan NOVAK" <istvan.novak@xxxxxxxxxxxxxxxx>
> To: <vincenzo@xxxxxxxxxxxxxx>
> Cc: "Tayyab Jamil" <tayyab@xxxxxxxxxxxxxx>; <si-list@xxxxxxxxxxxxx>
> Sent: Monday, December 29, 2003 7:31 AM
> Subject: [SI-LIST] Re: 0.8mm BGA routing
>
>
> > Vincenzo,
> >
> > In addition to what you listed in your mail, you will also need
> > to consider the clearance hole (antipad) around the pad, which
> > may be at least 8 to 10 mils bigger than the pad. Adjacet
> > signal vias would completely perforate the plane.
> >
> > I agree with Lee's comment he made earlier on this thread:
> > 0.8-mm BGA is tough on conventional PCBs with through
> > holes. You may need a build-up process or sequential
> > lamination to get your routing properly.
> >
> > Regards,
> >
> > Istvan Novak
> > SUN Microsystems
> >
> > ----- Original Message -----
> > From: "Vincenzo Kreft-Kerekes" <vincenzo@xxxxxxxxxxxxxx>
> > To: "Tayyab Jamil" <tayyab@xxxxxxxxxxxxxx>
> > Cc: <si-list@xxxxxxxxxxxxx>
> > Sent: Monday, December 29, 2003 9:25 AM
> > Subject: [SI-LIST] Re: 0.8mm BGA routing
> >
> >
> > > Tayyab,
> > >
> > > You're right, I apologize. It looks like you need a 16 mil via pad to
> > route
> > > 5/5 between two vias which in turn makes for a tiny drill hole (8 mil
> > > probably) and all its associated plating problems. Could someone
comment
> > > please? Thanks.
> > >
> > > Regards,
> > > Vincenzo
> > >
> > > -----Original Message-----
> > > From: Tayyab Jamil [mailto:tayyab@xxxxxxxxxxxxxx]
> > > Sent: Monday, December 29, 2003 12:54 AM
> > > To: Vincenzo Kreft-Kerekes
> > > Cc: si-list@xxxxxxxxxxxxx
> > > Subject: RE: [SI-LIST] Re: 0.8mm BGA routing
> > >
> > >
> > > Vincenzo,
> > >
> > > you are perfactly alirght when you mention the space left for pads.
but
> > you
> > > did not talk about the tracks escaping between vias.
> > >
> > > but when i place vias a matrix form, there is only 31.496 mil distance
> > > between the centers of adjacent via pads. keeping via pad of 20 mil
> there
> > is
> > > only 11.496 mil space left between the pads of adjacent vias.
> > >
> > > Now if i use 5/5 routing this means i need 5+5+5 = 15 mils total space
> for
> > > routing atleast one track between the pads of adjacent vias, which in
> our
> > > case is only 11.496. Even 4/4 routing scheme does not allow me to
> > > route/escape one track between the pads of adjacent vias.
> > >
> > > I am attaching the rough diagram for reference.
> > >
> > > What you say in this regard?
> > >
> > > Also please let me know the links/documents reffering to the design of
> > BGAs
> > > with 0.8 mm pitch.
> > >
> > > Thanks
> > > Tayyab
> > >
> > > -----Original Message-----
> > > From: Vincenzo Kreft-Kerekes [mailto:vincenzo@xxxxxxxxxxxxxx]
> > > Sent: Friday, December 26, 2003 10:19 PM
> > > To: tayyab@xxxxxxxxxxxxxx
> > > Subject: [SI-LIST] Re: 0.8mm BGA routing
> > >
> > >
> > > Tayyab,
> > >
> > > You place escape vias diagonally in the 0.8 mm raster which means you
> have
> > > 0.8 * sqrt(2) = 1.13 mm (44.5 mil) to work with. If you're using a 20
> mil
> > > via pad and have an etch capable of resolving 5 mil spaces between
> copper
> > > structures then you need a 30 mil zone around your via hole center
(for
> > pad
> > > and clearance) which leaves 44.5 - 30 = 14.5 mil as pad diameter for
the
> > > ball. As was already mentioned, Xilinx has escape diagrams for most if
> not
> > > all of their packages so you can look at what we're talking about,
> Altera
> > > also has a good application note on this topic and both have
recommended
> > > values for the via and etch parameters in these documents.
> > >
> > > Regards,
> > > Vincenzo
> > >
> > > -----Original Message-----
> > > From: si-list-bounce@xxxxxxxxxxxxx
> > > [mailto:si-list-bounce@xxxxxxxxxxxxx]On Behalf Of Tayyab Jamil
> > > Sent: Thursday, December 25, 2003 11:35 PM
> > > To: Stephen Chavez
> > > Cc: si-list@xxxxxxxxxxxxx
> > > Subject: [SI-LIST] Re: 0.8mm BGA routing
> > >
> > >
> > > Hi,
> > >
> > > I could not understand your scheme, for me it is not possible what you
> > > suggest as
> > >
> > > 0.8 mm pitch means there is only about 31 mil distance between via
pads
> of
> > > adjacent pins. 24 mil pad of via leaves only around 7.xx mils space in
> > > between. If we use 5 mil trace this leaves only around 2.xx mils in
> total
> > on
> > > both sides of the trace, means 1.xx mil clearence on each side of
trace.
> > >
> > > What i was thinking of is 18mil via pad and 8mil via hole finished,
and
> > 4mil
> > > trace and 4mil clearnce. This allows one trace to be escaped between
> > > adjacent pades. Any suggestions about this.
> > >
> > >
> > > Please let me know if I am wrong.
> > >
> > > Regards
> > > Tayyab
> > >
> > >
> > > ------------------------------------------------------------------
> > > To unsubscribe from si-list:
> > > si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field
> > >
> > > or to administer your membership from a web page, go to:
> > > //www.freelists.org/webpage/si-list
> > >
> > > For help:
> > > si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
> > >
> > > List technical documents are available at:
> > > http://www.si-list.org
> > >
> > > List archives are viewable at:
> > > //www.freelists.org/archives/si-list
> > > or at our remote archives:
> > > http://groups.yahoo.com/group/si-list/messages
> > > Old (prior to June 6, 2001) list archives are viewable at:
> > > http://www.qsl.net/wb6tpu
> > >
> > >
> >
> > ------------------------------------------------------------------
> > To unsubscribe from si-list:
> > si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field
> >
> > or to administer your membership from a web page, go to:
> > //www.freelists.org/webpage/si-list
> >
> > For help:
> > si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
> >
> > List technical documents are available at:
> > http://www.si-list.org
> >
> > List archives are viewable at:
> > //www.freelists.org/archives/si-list
> > or at our remote archives:
> > http://groups.yahoo.com/group/si-list/messages
> > Old (prior to June 6, 2001) list archives are viewable at:
> > http://www.qsl.net/wb6tpu
> >
> >
>
>
------------------------------------------------------------------
To unsubscribe from si-list:
si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field
or to administer your membership from a web page, go to:
//www.freelists.org/webpage/si-list
For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
List technical documents are available at:
http://www.si-list.org
List archives are viewable at:
//www.freelists.org/archives/si-list
or at our remote archives:
http://groups.yahoo.com/group/si-list/messages
Old (prior to June 6, 2001) list archives are viewable at:
http://www.qsl.net/wb6tpu
Other related posts:
