[SI-LIST] Re: PDN Question
- From: "Traa, Boris" <boris.traa@xxxxxxxxxxx>
- To: "Han, Guobing" <han.guobing@xxxxxxxxx>, Istvan Novak <istvan.novak@xxxxxxx>
- Date: Thu, 19 Aug 2010 11:09:41 +0200
Dear Guobing,
If you want to use the formule f=1/2/pi/sqrt((Lloop+ESL)*C) you should know how
the ESL is defined, determined and measured. If the circumstances in your
application (e.q. the distance between the capacitor and the ground plane)
differ from the ESL measurement set up than the use of your formula is doubtful.
In addition I think that in case the thickness of the capacitor is not
negligible to its ground plane distance the capacitor cannot be substituted by
only one capacitance with one series inductance. In my opinion the capacitor
will contain many LC circuits in parallel with different values for these L's
and C's while these L's and C's might be frequency dependent too.
Kind regards
Boris Traa
System design engineer EMC
It's the currents that make circuits work or fail.
Philips Applied Technologies/EMC center
Room 2.020
High Tech Campus 26
5656AE Eindhoven, The Netherlands
Tel: ++ 31 40 27 43766
Fax: ++ 31 40 27 42224
E-mail: boris.traa@xxxxxxxxxxx
-----Original Message-----
From: si-list-bounce@xxxxxxxxxxxxx [mailto:si-list-bounce@xxxxxxxxxxxxx] On
Behalf Of Han, Guobing
Sent: 2010 Aug 19 10:36 AM
To: Istvan Novak
Cc: Joel Brown; si-list@xxxxxxxxxxxxx
Subject: [SI-LIST] Re: PDN Question
Hi Joel,
The effective frequency provided is from the formula
f=1/2/pi/sqrt(ESL*C) . However,in practical, the loop inductance is
greater than ESL and so dominate the real resonant frequency.
Thus, the formula should be modified by
f=1/2/pi/sqrt((Lloop+ESL)*C) . Please change the 100nF to 10nF, 1nF,
even 0.1nF may help to your designs.
Thanks,
Guobing
2010/4/8, Istvan Novak <istvan.novak@xxxxxxx>:
> Hi Joel,
>
> These are the usual dilemmas in many designs.
>
> Just a few quick comments:
> - if you need to lower the cumulative inductance from your capacitors,
> you can consider
> using multiple vias per pad. Downside: with your planes in the middle of
> the stack, more
> vias will block more routing unless you do backdrilling or sequential
> lamination.
> - the bottom side of the board is not necessarily useless for
> low-inductance PDN.
> Consider the case when a consumer has multiple power/ground vias
> (typical for FPGA core).
> The multiple vias can connect to the surface effectively, so if you had
> your power plane
> closer to the bottom, it could still be connected with relatively low
> inductance to the
> package on the top side and you could bypass it with fewer caps on the
> bottom.
> Alternately you could leave the planes in the middle and see if you can
> add bypass
> capacitors directly across the power/ground pins on the bottom. This
> will depend on
> many factors, but it is becoming more widely available.
> - your asymmetrical stackup may work well if the board is small or if
> the assembly
> can live with some warpage. I would not do this on large boards, because
> the copper
> utilization is very different on signal versus power layers.
>
> Regards,
>
> Istvan Novak
> Oracle-Sun
>
> Joel Brown wrote:
>> Currently I am using the Altera PDN tool for Stratix III.
>> With the values I entered the target impedance is 0.012 ohms.
>>
>> There is also Feffective of 59 MHz.
>>
>> The users manual states that using PCB capacitors for PDN
>>
>> decoupling beyond their effective frequency range brings little
>> improvement
>> to PDN
>>
>> performance and raises the bill of materials (BOM) cost.
>>
>>
>>
>> So my first question would be why is it ok to not provide bypassing beyond
>> this Feffective frequency?
>>
>> I do realize that it may not be possible to do this which what I think is
>> what Altera is saying.
>>
>> But what will prevent the noise voltage from exceeding limits above this
>> frequency?
>>
>> I do know that Altera has internal bypass capacitors on these parts but
>> there is no information on their characteristics.
>>
>>
>>
>> Most of our board designs use power planes in the center of the board.
>>
>> Here is an example stackup:
>>
>>
>>
>> Layer 1: Component side / Signals
>>
>> Layer 2: Ground Plane
>>
>> Layer 3: Signal 1
>>
>> Layer 4: Signal 2
>>
>> Layer 5: Ground Plane
>>
>> Layer 6: Power Plane
>>
>> Layer 7: Power Plane
>>
>> Layer 8: Ground Plane
>>
>> Layer 9: Signal 3
>>
>> Layer 10: Signal 4
>>
>> Layer 11: Ground Plane
>>
>> Layer 12: Solder side / Signals
>>
>>
>>
>> We do this to reduce layer count and so the split power planes are
>> surrounded by solid ground planes.
>>
>> In trying to achieve 0.012 ohm target impedance out to 59 MHz I found that
>> I
>> reached a point of diminishing returns and no matter how many bypass caps
>> I
>> used I could not really get there even with X2Y caps. By playing around I
>> found that reducing the inductance by moving the power planes closer to
>> the
>> top layer I could achieve the target impedance. But this would mean a
>> different stackup:
>>
>>
>>
>> Layer 1: Component side / Signals
>>
>> Layer 2: Ground Plane
>>
>> Layer 3: Power Plane
>>
>> Layer 4: Power Plane
>>
>> Layer 5: Ground Plane
>>
>> Layer 6: Signal 1
>>
>> Layer 7: Ground Plane
>>
>> Layer 8: Signal 2
>>
>> Layer 9: Signal 3
>>
>> Layer 10: Ground Plane
>>
>> Layer 11: Signal 4
>>
>> Layer 12: Ground Plane
>>
>> Layer 13: Power Plane
>>
>> Layer 14: Power Plane
>>
>> Layer 15: Ground Plane
>>
>> Layer 16: Solder side / Signals
>>
>>
>>
>> Now the board has gone from 12 layers to 16 layers and the power planes on
>> layers 13 and 14 are of no use for high frequency bypassing.
>>
>>
>>
>> My next question would be is it possible to use a slightly asymmetrical
>> stack up like this:
>>
>>
>>
>> Layer 1: Component side / Signals
>>
>> Layer 2: Ground Plane
>>
>> Layer 3: Power Plane
>>
>> Layer 4: Power Plane
>>
>> Layer 5: Ground Plane
>>
>> Layer 6: Signal 1
>>
>> Layer 7: Signal 2
>>
>> Layer 8: Ground Plane
>>
>> Layer 9: Signal 3
>>
>> Layer 10: Signal 4
>>
>> Layer 11: Ground Plane
>>
>> Layer 12: Solder side / Signals
>>
>>
>>
>> The copper weight of the power planes would be ½ oz to match Signal layers
>> 9
>> and 10.
>>
>> Would this be manufacturable? Would any special technology be required?
>>
>> I keep hearing that boards with asymmetrical stack ups will warp too much.
>>
>>
>>
>> Thanks - Joel
>>
>>
>>
>>
>>
>>
>>
>>
>>
>>
>>
>>
>>
>>
>>
>>
>>
>>
>>
>>
>>
>>
>>
>>
>>
>>
>>
>>
>>
>>
>>
>>
>>
>>
>
> ------------------------------------------------------------------
> 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
>
> Old (prior to June 6, 2001) list archives are viewable at:
> http://www.qsl.net/wb6tpu
>
>
>
--
Thanks,
- Robin (Han, Guobing)
TEL: 86-21-61094805
MSN: han_guobing@xxxxxxxxxxx
------------------------------------------------------------------
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
Old (prior to June 6, 2001) list archives are viewable at:
http://www.qsl.net/wb6tpu
The information contained in this message may be confidential and legally
protected under applicable law. The message is intended solely for the
addressee(s). If you are not the intended recipient, you are hereby notified
that any use, forwarding, dissemination, or reproduction of this message is
strictly prohibited and may be unlawful. If you are not the intended recipient,
please contact the sender by return e-mail and destroy all copies of the
original message.
------------------------------------------------------------------
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
Old (prior to June 6, 2001) list archives are viewable at:
http://www.qsl.net/wb6tpu
Other related posts:
