[SI-LIST] Re: Noise on BGA core voltage rail
- From: pwelling@xxxxxxxxxxxxxx
- To: Anand.Kuriakose@xxxxxxxxxx, Larry.Smith@xxxxxxx
- Date: Thu, 8 Aug 2002 15:46:26 -0600
Anand,
Have you checked the local probe environment to see if you are inductively
picking up EMI noise from the components around the measurements area? I am
already assuming that you have a very short ground (less than 1/2 inch) from
the scope probe ground to a low impedance ground on the board under test.
Often, we will put ground pads on our boards to minimize the loop. I am also
assuming that there are not alot of traces run between the ground connection
and the test measurement point. This is only one of the reasons why we limit
routing on outside layers of the board.
There is an easy test to see if you are creating measurement error (the
small difference between the 2 measured values - may suggest this) by the
local environment.
That test is to short the oscilloscope probe ground to the oscilloscope
probe tip. Then move the probe near the area you were measuring. You will
then "see" the measurement environment as a single turn loop. If the noise
is there at nearly the same levels, the loop area of the ground is suspect -
or - look at the rest of the measuring environment. The rest of the
measuring environment is made up of the probe body (in some less expensive
probes), probe cable, oscilloscope environment, etc... It sounds funny, but
if you think of a debug station is , you have power supplies with long
cables, power cords, Personal Computers, Display Monitors, keyboard and
mouse cables, etc... I actually walked into a situation once with a high
resolution monitor at a debug station that coupled noise to the oscilloscope
probe cable causing a false reading (CRT card emissions, and Yoke
emissions).
Aside from this possibility, you have received good advice from the LIST
contributors. One thing I wanted to mention is that when we think of
capacitance from the power plane structure, we often consider it high
quality capacitance dominated by capaitance not inductance. As vias
penetrate that plane capacitance structure, the planes become more inductive
(capillary inductive action) the quality of that capacitance degrades. With
high pin count BGAs, like the 1152 pin packages, really perforate the planes
and the buried capacitance suffers. Unfortunately, that is where we need the
plane capacitance for the higher frequency output drivers and core voltages.
Creative device fanout helps, and using micro-vias help that situation, but
are expensive.
Has anyone performed research on how the plane capacitance is degraded by
large BGAs perforations? Both donut style and full package perforations?
Good Luck.
Philip Ross Wellington
Mgr. Signal Integrity & EMI
L-3 Communications CSW
-----Original Message-----
From: ANAND KURIAKOSE [mailto:Anand.Kuriakose@xxxxxxxxxx]
Sent: Thursday, August 08, 2002 11:08 AM
To: Larry Smith
Cc: si-list@xxxxxxxxxxxxx
Subject: [SI-LIST] Re: Noise on BGA core voltage rail
Hi Larry,
The board has 2 power-ground pairs. The spacing b/n the power and
the ground plane is 4 mils. The power planes carry 2.5 V rail (the noisy
rail) along with other volttages on the board.
I have one question.
In addition to having power-ground pairs yeilding low impedances at
high frequencies above 100Mhz (which seems to be the only solution according
to you), what other precautions should be taken during the design or layout
to have low target impedances from DC to around 200Mhz-600Mhz?
Anand.
From: Larry Smith <Larry.Smith@xxxxxxx> on 08/09/2002 12:03 AM
Please respond to Larry Smith <Larry.Smith@xxxxxxx>@SMTP@Exchange
To: si-list@xxxxxxxxxxxxx@SMTP@Exchange, ANAND KURIAKOSE/Apex
Data Inc/01@Apex Data Inc
cc:
Subject: Re: [SI-LIST] Noise on BGA core voltage rail
Anand - It is difficult to do anything about power distribution
noise
at 200 MHz and above by using discreet decoupling capacitors.
Your best ally at high frequency is the PCB power planes. They are
effective at high frequency but may have cavity resonances which
depend
upon the dimensions of the board.
The best way to make the PCB power planes effective is by defining a
stackup that has power/Gnd plane pairs next to each other. The
dielectric thickness between the planes determines the capacitance
and
spreading inductance of the planes. Thinner is better. 4 mils
between
planes is good, 2 mils is better.
Several years ago, it was common to see power and ground planes
separated by 14 mils or so in order to accommodate 2 signal layers
between the planes. With that spacing, the performance of the
decoupling capacitors is limited by the spreading inductance of the
power planes. If you have more than a few dozen ceramic capacitors,
you must use adjacent power planes in the stackup in order to make
them
effective. Otherwise, the impedance of the planes dominates over
the
impedance of the capacitors at high frequency.
regards,
Larry Smith
Sun Microsystems
> Delivered-To: si-list@xxxxxxxxxxxxx
> X-Lotus-FromDomain: APEX DATA INC
> From: Anand.Kuriakose@xxxxxxxxxx
> To: si-list@xxxxxxxxxxxxx
> Date: Thu, 8 Aug 2002 22:06:59 +0630
> Subject: [SI-LIST] Noise on BGA core voltage rail
> Mime-Version: 1.0
> Content-Disposition: inline
> Content-Transfer-Encoding: 8bit
> X-archive-position: 3678
> X-ecartis-version: Ecartis v1.0.0
> X-original-sender: Anand.Kuriakose@xxxxxxxxxx
> X-list: si-list
>
>
>
>
> Hi,
>
> Heres a situation where i have a BGA (chipset with interface to
processor, DDR
> memory and other high speed proprietry buses) with sufficient
decoupling
> sprinkled around the BGA. The decoupling on the core voltage rail
(2.5V, which
> is also the I/O voltage for DDR interface) basically consists of
2 high value
> bulk capacitors, six 1uf caps, ten each of 0.1uF and 0.01uF caps.
I am
noticing
> noise around 150mv of noise during activity on the DDR (using
software
> utilities) and roughly 80-100 mV during almost no activity across
the chip.
> This amplitude is significantly more than the noise noticed at
other high
speed
> chips on the board. Using the FFT function on the DSO, i figured
out that the
> frequencies where it peaks are 200Mhz and integral multiples of
200Mhz.
>
> I tried a couple of things:
>
> 1> Since i am seeing peaks at 200Mhz and its integral multiples,
i thought
> that there could be insufficient high frequency decoupling and
hence i replace
> the 0.1uF caps with 1000pF caps.
> 2> Secondly, fearing that there could be some resonance
happening due the
> different values of caps used, i replaced all the 0.1 uF caps with
0.01uF caps
> (in addition to existing 0.01uF caps).
>
> Both the above strategies failed to reduce the noise. There was no
change in
the
> amplitude of the noise and also the frequencies where peaks were
noticed.
>
> Can somebody out there throw some light on what is lacking in the
strategies
> mentioned above and how to reduce this noise satisfactorily.
>
> Thanx in advance.
> Anand.
>
>
> ------------------------------------------------------------------
> 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 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 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 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:
