[SI-LIST] Re: Power plane coupling
- From: "Larry Smith" <LSMITH@xxxxxxxxxx>
- To: "steve weir" <weirsi@xxxxxxxxxx>, <christopher.mcgrath@xxxxxxxxx>, <ludovic.levieil@xxxxxxxxxxx>, <si-list@xxxxxxxxxxxxx>
- Date: Tue, 25 Oct 2005 13:59:14 -0700
Chris - As you and Steve have mentioned, the best side of the board for
placement of decoupling capacitors is a function of inductance. There
are three important inductances involved, each of which play a different
roll.
1) The capacitors are attached to the PCB with a mounting inductance
that is closely related to the via length from the cap pads to the
power/ground plane pair. The mounting inductance is an important factor
in determining the resonant frequency and Q of the mounted capacitor.
For this reason, you want the power/ground plane pair to be as close as
possible to the front or back surface of the PCB. In the stackup under
discussion in this thread, that would be layers 2, 3, 4 and 5 (or N-1
through N-4 where N is the number of layers). I like to use a matrix of
different valued capacitors, each with a similar mounting inductance, to
establish a low and flat impedance from about 1MHz to 100MHz for a bank
of capacitors attached in this way.
2) The power/ground plane pair is the conduit that carries power from
the bank of capacitors (above) to the vicinity of the load. Istvan
mentioned the value of thin power plane dielectric (Vcc to Gnd) to
maximize plane capacitance. Thin dielectric also has superior
inductance properties because the power plane spreading inductance is
proportional to the dielectric thickness. The second important
inductance in our problem is the horizontal power plane spreading
inductance.
3) Charge that is stored in the capacitors flows vertically through the
mounting inductance, horizontally through the plane spreading inductance
and once again goes vertical in the vicinity of the load. A
checkerboard pattern of power and ground vias is often used underneath a
load (i.e. BGA package) to form a low inductance path from the power
planes to the power consumer. This is the third inductance in our
problem.
These three inductances should be closely balanced in the power
distribution system because any one of them can dominate. I have seen
cases where hundreds of power/ground vias underneath the BGA load have
far less parallel inductance than the horizontal power plane spreading
inductance, even when the vias carried current all the way from the
backside of the board. Thin power plane dielectric could be very
valuable for this system. But if there are not very many power and
ground vias in the BGA pattern, there is no point in using thin power
plane dielectric.
The sum of inductances 2 and 3 gives a series inductance for the bank of
decoupling capacitors mounted on the board and gives an upper limit to
the number of decoupling capacitors that are useful. The equivalent
inductance of all the parallel decoupling capacitors should be
calculated (mounting inductance divided by the number of caps). In a
well designed power distribution system, about 1/3 of the inductance
should be allocated to the BGA vias, 1/3 for the power planes and 1/3
for the parallel mounting inductances. If one of these three
inductances significantly dominates, it establishes the performance of
the PDS and there is no point in putting additional cost into the other
two inductances.
So, to answer your question on which side of the board to place the
caps, you need to look at the three inductances of the system.
Regards,
Larry Smith
Altera Corporation=20
-----Original Message-----
From: steve weir [mailto:weirsi@xxxxxxxxxx]=20
Sent: Friday, October 21, 2005 4:11 PM
To: christopher.mcgrath@xxxxxxxxx; Larry Smith;
ludovic.levieil@xxxxxxxxxxx; si-list@xxxxxxxxxxxxx
Subject: Re: [SI-LIST] Re: Power plane coupling
Chris,
You always want to think in terms of minimizing demon inductance. So,
first=20
we want to put the plane(s) that support our lowest impedance
requirements=20
closest to the device they feed. Not every plane can be in the top of
the=20
stack, so this will compromise some supplies.
The placement of capacitors should also be selected to minimize the
total=20
inductance between the caps and the devices they serve. For a plane=20
towards the bottom of the board, this means the caps go on the bottom.
We=20
are already burned by the long vias from the device to a plane near the=20
opposite side of the board. If we place the caps on the same side as
the=20
part, then the attachment vias for the caps will be just as long, a very
bad thing.
Spreading inductance is another issue. It is part of the price we pay
for=20
the reality that it is essentially impossible to put discrete caps of
any=20
size right on the die pads. The further we move away in any axis, the=20
higher a penalty we pay. The natural log behavior of spreading
inductance=20
and resistance is such that once we are in for a dime, we might as well
be=20
in for a dollar.
Regards,
Steve.
At 01:32 PM 10/21/2005 -0700, Mcgrath, Christopher wrote:
>Larry,
>
>I have a related question that popped into my head when I read your
>response.
>
>If you expand this example so that there were a number of layers
between
>VCC1 and VCC2 which included both ground and signal layers so that the
>thickness of the board begins to become significant with respect to the
>placement of decoupling capacitors, is the preferred location for
>decoupling of a device placed on the top side of the PCB on the top
side
>or bottom side of the board IF the voltage being decoupled is VCC2.
>
>At issue is whether it is better to place the decoupling capacitor
>closer to the voltage it is decoupling or closer to the device that is
>actually receiving the power.
>
>I believe that the path with the least inductance and maximum
>effectiveness would be to place the decoupling capacitor on the top
side
>of the board right next to the device. While the spreading inductance
>should be very similar in both cases, the loop inductance would be
>slightly less when the cap is placed on the top of the board. =3D20
>
>Any thoughts?
>
>Thanks,
>Chris
>
>=3D20
>
> >-----Original Message-----
> >From: si-list-bounce@xxxxxxxxxxxxx
>[mailto:si-list-bounce@xxxxxxxxxxxxx] On
> >Behalf Of Larry Smith
> >Sent: Friday, October 21, 2005 12:05 PM
> >To: ludovic.levieil@xxxxxxxxxxx; si-list@xxxxxxxxxxxxx
> >Subject: [SI-LIST] Re: Power plane coupling
> >
> >Ludovic - I like this power plane stackup sequence, particularly if
it
> >is on the top or bottom surface of the PCB.
> >
> >The power planes will be highly coupled to ground by discrete
>decoupling
> >capacitors mounted on the surface of the board. There are probably
> >100's of uF that are trying to maintain a constant voltage between
VCC1
> >and Gnd, also between VCC2 and Gnd. But the internal plane to plane
> >capacitance is on the order of 1nF, not much compared to the external
> >capacitance. At 100MHz, the 1 nF plane-to-plane impedance is about
> >1/(2*pi*100e+6*1e-9) =3D3D3D 1.59 Ohms. This is not strong compared =
to
=3D
>the
> >impedance of the PDS which is probably in the mOhms. The impedance
> >division insures that there will not be substantial noise coupled
from
> >one power plane to the other in this stackup. But as Istvan has
> >commented in another note on this thread, this might not be best for
a
> >sensitive analog supply or PLL circuitry. Further filtering should
be
> >used for those supplies.
> >
> >Noise above 100 MHz usually gets onto a power plane because of
> >transmission line return current. I like your stackup because the
>power
> >planes are surrounded by Gnd planes. You have an opportunity for
> >transmission lines to reference only ground planes throughout the
rest
> >of the stackup. This keeps the return current noise off the power
> >planes and the power plane noise off the transmission lines. Skin
> >effect in solid ground planes greatly attenuates magnetic fields from
> >penetrating through the planes at 1 MHz and above.
> >
> >Noise below 100 MHz is usually caused by current transients from the
> >loads. A well designed PDS will be below target impedance from some
> >corner frequency (50 to 100 MHz) all the way down to DC. The noise
> >coupled between power planes below this corner frequency is
diminished
> >because the impedance of the plane-to-plane capacitance diminishes at
> >lower frequency. This stackup puts you well on the way towards good
> >power and signal integrity in your product.
> >
> >Regards,
> >Larry Smith
> >Altera Corporation
> >(Sun Microsystems was very good for me, but it was time to move on.)
> >
> >-----Original Message-----
> >From: si-list-bounce@xxxxxxxxxxxxx
>[mailto:si-list-bounce@xxxxxxxxxxxxx]
> >On Behalf Of Ludovic Levieil
> >Sent: Thursday, October 20, 2005 1:12 AM
> >To: si-list@xxxxxxxxxxxxx
> >Subject: [SI-LIST] Power plane coupling
> >
> >Hello All,
> >In my current board design I have the following stack up:
> >
> > .......
> >---------------- GND (solid plane)
> >------ ----- --- VCC1 (splitted plane)
> >--- ----- ------ VCC2 (splitted plane)
> >---------------- GND (solid plane)
> > .......
> >
> >4 mils separate GND and VCC planes
> >5 mils separate VCC1 and VCC2 planes
> >
> >Both VCC planes are splitted in different power domains and I am
> >wondering=3D3D20
> >:
> > - if having two coupled VCC planes is good/acceptable
when=3D3D20
> >thinking about noise ??
> > - if there is a problem in having one power domain on on
>plane=3D3D20
> >overlapping at least two power domains on the other plane ??
> >
> >Thanks
> >
> >Ludovic Levieil=3D3D20
> >
> >------------------------------------------------------------------
> >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 FAQ wiki page is located at:
> > http://si-list.org/wiki/wiki.pl?Si-List_FAQ
> >
> >List technical documents are available at:
> > http://www.si-list.org
> >
> >List archives are viewable at: =3D3D20
> > //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
> > =3D3D20
> >
> >
> >
> >------------------------------------------------------------------
> >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 FAQ wiki page is located at:
> > http://si-list.org/wiki/wiki.pl?Si-List_FAQ
> >
> >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 FAQ wiki page is located at:
> http://si-list.org/wiki/wiki.pl?Si-List_FAQ
>
>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 FAQ wiki page is located at:
http://si-list.org/wiki/wiki.pl?Si-List_FAQ
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:
