[SI-LIST] Re: Decoupling of digital power i PCB's, how do we avoid pole peaks in the impedance, how far up in frequency do we need low impedance

  • From: "Lars Juul" <write2larsj@xxxxxxxxx>
  • To: si-list@xxxxxxxxxxxxx
  • Date: Mon, 20 Aug 2007 08:28:55 +0200

Hej Peter,
A brief comment on your last statement:
>It looks like I am back in the old days where we build a prototype and then
started to find the correct components values?

Even though you can literally spend 100K's of $$$ on simulation tools that
can extract your board layout and simulate your decoupling network, you
always have to make the call whether it's

a) cheaper and faster to build a few prototypes, building your own set of
decoupling design rules based on your already good understanding of linear
systems.

or

b) preferable to come up with a simulation flow where the results are
correllated to the boards you produce, enabling you to quickly verify your
layout.

Either way, you need to build a knowledge base of do's and don'ts and that
experience doesn't come for free.

a) is the choice if you're focusing mostly at perfecting one product at a
time, and if you or your test and measurement folks are experienced, able to
effectively pinpoint the defects of a design.

b) is the choice if you have a steady flow of new designs coming enabling
you to constantly correllate your results and have fewer redesigns. The
initial matching of simulation and measurements can be a painful, lengthy
affair, though.

My point is, the EDA folks will always try to convince you that using their
tools you'll always have hole-in-one designs, but for me prototyping remains
as the most secure way of ensuring your board works.

And I'd rather put my money on something that works in the lab rather than
in a simulator.
But again, that's just my ?0.02.

Best regards,
Lars

2007/8/20, istvan novak <Istvan.Novak@xxxxxxx>:
>
> Peter,
>
> A few quick answers/observations:
>
> 1) How far down the IC needs low impedance?
> The core power distribution circuit from the chip's perspective is
> probably OK with a high
> impedance at 900MHz; the package and/or silicon has to take care of that
> frequency range.
> SI and EMI may suffer though; if you happen to route signal traces
> referencing this core
> plane, the signal may suffer too much.  Similarly, dependent on the PCB
> and system
> constructions, the resonance may create EMI problem.
>
> 2) Higher ESR capacitors; do they exist?
> In ceramic MLCCs, they start to appear on the market.  You can look at
> the DesignCon
> 2007 presentations at http://home.att.net/~istvan.novak/papers.html
>
> 3) How many of you do power impedance analyses during design?
> Well, at large OEMs we have to do at least some sort of analysis,
> sometimes very detailed
> designs and validations.
>
> In general, the problem you notice is the resonance between the
> inductances of the bypass
> capacitors resonating with the static capacitance of the planes.  There
> are a few ways of
> helping it:
> - you can make the static capacitance lower (this pushes out the
> resonance frequency).
> You can lower the capacitance by placing the power/ground planes further
> away, but
> this also increases the plane inductance; this is not your first
> choice.  You can. however,
> make the plane shape as small as possible (with some boundary area
> left), this will
> minimise capacitance.
> - as you pointed out, you can increase the ESR of parts.  This does not
> change the
> resonance frequency, but reduces the peak.  Dependent on what
> mid-frequency
> impedance you need, you can simply use R-C components with low-inductance
> layout, or you can consider the high-ESR MLCCs.
> - finally, a brute force solution, not requiring special part is to
> overwhelm the inductance
> of the plane.  If cumulatively your capacitors present an inductance,
> which is about 1%
> of the plane inductance, the resonance peak is mostly gone.  To achieve
> this, you can
> place the power/ground planes close to the surface, so that via
> inductance is less, or
> can use multiple vias for each capacitor, use low-inductance capacitors,
> like reverse
> geometry, X2Y or multi-terminal capacitors.
>
> Regards,
>
> Istvan Novak
> SUN Microsystems
>
>
> Peter Sørensen wrote:
>
> >At present I am trying to analyse and fix the impedance of my digital =
> >power
> >supplies in our new PCB construction.
> >This turns out to be more complex than most digital designers think.
> >I have read a number articles and a book so far, but I have not found =
> >the
> >solution. It just made me able to do simulation in a spreadsheet and
> >visualize the problem.
> >
> >Modern SMD capacitors have low ESR =3D high Q. They also have some =
> >inductance,
> >but do not forget the VIA inductance which often is bigger than the
> >component itself. Traces are totally forbidden in my world due to
> >inductance. Large caps like 1210 get one via on each side of the pad.
> >These stray inductors combined with the capacity generates zeros and =
> >poles.
> >The zero's are great they reduce the impedance to the ESR value plus
> >resistance in VIA's, equal to a very low impedance at some frequencies.
> >Using many capacitors increases the frequency area with a low impedance.
> >Power Planes places close to GND planes are great, they makes capacity =
> >with
> >zero inductance for any frequency that matters, but they only works at =
> >high
> >frequencies especially if you have small planes.
> >
> >I have made some simulations showing that with a small power plane of 2
> >square inch (a core voltage use by one BGA) I get a huge pole at
> >900MHz. The impedance is above 0.05 ohms from 100MHz and up 3 GHz. The
> >question is how far down do IC's need a low impedance.
> >At 3 GHz is does not matter, at this frequency only decoupling in =
> >silicium
> >will work due to inductance in package etc.
> >But what about the 100MHz, I believe a low impedance must be provided =
> >for
> >many IC's up to about 300MHz or even more.
> >Eg. This core is running at 400MHz and I would like a low impedance in =
> >that
> >range.
> >The IC's supplier do not specify supply impedance, many have PCB layout
> >guidelines but often they can not be copied.
> >For this one I used one 1210 100uF and an array of twenty 0402 220nF. =
> >Adding
> >more caps would help but there is not room.
> >The simulation result also depends on what you estimate your via's
> >inductance and resistante to be.
> >
> >What really would help would be capacitors with higher ESR =3D low Q. =
> >They
> >would lower the poles impedance and raise the zero impedance.
> >Do they exist?
> >Properly not, I have not beeen able to find them.
> >
> >Using leaded components is not an option, they may have lower Q but they
> >will also have more inductance and use more space etc.
> >
> >Combining two or more values of array caps in 0402 house like 220nF+ =
> >10nF
> >does not help much and generate a new pole between the two zero's, this =
> >poel
> >is lower but also at a lower and more critical frequency.
> >
> >To me it looks impossible to garantee a low impedance of below 0.05 ohms
> =
> >or
> >better at the intire frequency range of interest.
> >
> >I belive the reason that most digital designs still works is that the =
> >poles
> >do not match the load frequencies in most applications.
> >I believe most designers still do as usual and then cross their fingers =
> >and
> >hope they do not have any poles at critical frequencies.
> >How many of you do power impedance analyses during design?
> >
> >It looks like I am back in the old days where we build a prototype and =
> >then
> >started to find the correct components values?
> >
> >Best regards
> >Peter S=F8rensen
> >
> >
> >
> >
>
> ------------------------------------------------------------------
> 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.net
>
> 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.net

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:

  1. Home
  2. si-list
  3. Archive
  4. 08-2007