[SI-LIST] Re: 6 layers stackup
- From: steve weir <weirsi@xxxxxxxxxx>
- To: Scott McMorrow <scott@xxxxxxxxxxxxx>
- Date: Mon, 25 Feb 2008 13:47:32 -0800
Scott, Lee's metric is for a single via. He divides that by the total
number of vias. So for example, an 0402 with two vias he would factor
at 35pH / 2 or 17.5pH / mil. It's a little low versus the theoretical
value of 21pH / mil for 10mil drills on 1mm pitch, but is in the ballpark.
Best Regards,
Steve.
Scott McMorrow wrote:
> Lee,
>
> That depends on your via size, spacing and where the planes are
> located w.r.t. the capacitor. The via pair inductance is:
>
> Lmounting vias - 5.08 pH/mil x 2 x H x ln(2S/D)
>
> as reported by Howard Johnson from a closed form solution.
>
> where
>
> H is the length of the vias in the plane cavities
> S is the center to center via separation
> D is the via diameter
>
> If we use 10 mil vias at a 30 mil spacing, then our inductance is
>
> 18.2 pH/mil
>
> If we use 15 mil vias at 40 mil spacing, our inductance is:
>
> 17pH/mil
>
> To get your number of 35 pH/mil, we would need to use 10 mil vias and
> space them approximately 150 mils apart. So, to start with, your
> approximate via inductance is high by a factor of 2 to 1.
>
> 15 to 20 pH is a much better number for vias on well-mounted
> capacitors. So, if we place the planes at 3 mil and 7 mil below the
> surface of the board where the capacitors are mounted, the via
> inductance is 140 pH. Certainly this is less than the inductance of
> an 0402 capacitor, which is approximately 450 pH. A so-called "magic
> capacitor", with an inductance of 120 pH would most necessarily
> provide a significant reduction in total mounted inductance. Last I
> checked
> 120 + 140 is much less than 450 + 140. In addition, those "magic
> capacitors" take advantage of mutual inductance coupling between the
> vias, while using more vias, by a factor of about 4:1 (5 pH/mil vs. 20
> pH/mil). In which case the inductance for the "magic capacitor"
> solution is:
>
> 120 pH + 35 pH = 155 pH
>
> Last time I measured this and simulated this
>
> 155 pH is << than 590 pH, or about 3.8:1 difference.
>
> Since the ratio of vias used for an X2Y capacitor vs an 0402 is 6:2 or
> 3:1. The via inductance efficiency ratio is;
>
> 1.27:1
>
> That is, an X2Y capacitor is at least 1.27 times more efficient in
> using vias than an 0402 capacitor.
>
> This has been confirmed multiple times by measurements and by
> electromagnetic simulation.
>
> Now, I do agree that the further down you reach into the cavity, the
> less benefit that you get. However, the via efficiency ratio of
> "magic capacitors" continue to be significantly better than
> conventional MLCC capacitors, no matter where the planes are placed in
> the stack.
>
>
> regards,
>
> Scott
>
>
> Scott McMorrow
> Teraspeed Consulting Group LLC
> 121 North River Drive
> Narragansett, RI 02882
> (401) 284-1827 Business
> (401) 284-1840 Fax
>
> http://www.teraspeed.com
>
> Teraspeed® is the registered service mark of
> Teraspeed Consulting Group LLC
>
>
>
> Lee Ritchey wrote:
>> I disagree that ultralow inductance capacitors perform significantly better
>> that standard two leaded capacitors such as 0402 and 0603 due to the added
>> inductance associated with the mounting pads and mounting vias. This has
>> been supported many times by physical measurements on real PCBs and is
>> documented in my book, "Right the First Time, A Practical Handbook on High
>> Speed PCB and Systetm Design" as well as in several other sources.
>>
>> I am mystified at how it can be claimed that this is not so when the
>> inductance of the vias connecting capacitors to the associated planes
>> averages something like 35 pH per mil of length- no matter what kind of
>> magical capacitor they are connected to. It is especially true when one is
>> speaking of a six layer PCB that has planes 20-40 mils below the surface.
>> That is 0.7 nH to 1.4 nH per lead. Even if the capacitor has 0.1 nH
>> inductance as an IDC capacitor is said to have, the total inductance is
>> driven up near 1 nH. How can any capacitor make this go away?
>>
>> It is time to stop pretending that there are magic capacitors out there.
>>
>> Lee Ritchey
>> Speeding Edge.
>>
>>
>>
>>> [Original Message]
>>> From: steve weir <weirsi@xxxxxxxxxx>
>>> To: QU Perry <Perry.Qu@xxxxxxxxxxxxxxxxxx>
>>> Cc: <si-list@xxxxxxxxxxxxx>
>>> Date: 2/25/2008 11:52:30 AM
>>> Subject: [SI-LIST] Re: 6 layers stackup
>>>
>>> Perry, the discussion has been limited to 4/6 layer boards with a single
>>> symmetric power cavity. The Z axis inductance for an IC or bypass cap
>>> to the cavity depends on the distance to the center of the cavity. With
>>> a single, symmetric cavity, that is going to be half the board
>>> thickness. This is not to be confused with higher layer count boards
>>> where we can place at least one modestly thin cavity near the IC /
>>> capacitor mounting surface. In all cases, the cavity spreading
>>> inductance becomes a limiting factor in PDN impedance. Cavity impedance
>>> varies directly with cavity height.
>>>
>>> In the case of any almost thickness PCB, the via attachment structure is
>>> a significant, if not dominant contributor to the mounted capacitor
>>> inductance, that is the inductance as seen at that attachment point at
>>> the planes. Capacitors like X2Y(r)'s, and IDC(r)'s when properly
>>> attached yield much lower inductance than discrete caps. This is
>>> readily modeled in any number of tools, and confirmed by properly
>>> constructed experiments. So low inductance caps still work, whether or
>>> not you have a thin cavity, and whether or not the cavity is adjacent to
>>> the caps.
>>>
>>> We are talking about two different resonances. The resonance that you
>>> are referring to are the half-wave modes. I am talking about the
>>> parallel resonance between the bypass network and the power cavity.
>>> This is the beast that eats most people's lunch. It is a matter of
>>> capacitance per unit area of the cavity which depends directly on
>>> height, and the area / unit inductance of the bypass network.
>>>
>>> Best Regards,
>>>
>>>
>>> Steve.
>>>
>>> QU Perry wrote:
>>>
>>>> Steve:
>>>>
>>>> My understanding on the impact of thinner power cavity is mainly the
>>>> reduction of spread inductance, such that any added benefit of IDC/X2Y
>>>> placed at the peripheral of BGA will not be compromised by the planes..
>>>> In most applications however, we rely heavily on the decoupling caps
>>>> (0402) directly placed underneath BGAs, and in those cases, I would
>>>> think thickness of power cavity is not important as the total inductance
>>>> looking into PCB from BGA pads to the planes and to the decoupling caps
>>>> don't change. Your thoughts ?
>>>>
>>>> I'm also not clear when you say parallel resonance frequency is driven
>>>> by thickness. Comparing Z dimension vs. X/Y for a normal power plane/PCB
>>>> thickness, I would say the resonance frequency is mainly determined by
>>>> how big the plane is not how thick the cavity ?
>>>>
>>>> Thanks
>>>>
>>>> Perry
>>>>
>>>> =======================================
>>>>
>>>> Perry Qu
>>>>
>>>> Design & Qualification, Alcatel-Lucent Canada Inc.
>>>>
>>>> 600 March Road, Ottawa ON, K2K 2E6, Canada
>>>>
>>>> DID: 613-7846720 Fax: 613-5993642
>>>>
>>>> Email: perry.qu@xxxxxxxxxxxxxxxxxx
>>>>
>>>> =======================================
>>>>
>>>>
>>>>
>>>>
>>>>
>>>>> -----Original Message-----
>>>>> From: si-list-bounce@xxxxxxxxxxxxx
>>>>> [mailto:si-list-bounce@xxxxxxxxxxxxx] On Behalf Of steve weir
>>>>> Sent: Saturday, February 23, 2008 6:44 PM
>>>>> To: DAVID CUTHBERT
>>>>> Cc: Fernando Yuitiro Mori; si-list@xxxxxxxxxxxxx
>>>>> Subject: [SI-LIST] Re: 6 layers stackup
>>>>>
>>>>> Dave, Fernando my $0.02 on 4/6 layer stack-ups with a single
>>>>> symmetric power cavity:
>>>>>
>>>>> 1) The Z-axis inductance seen at the IC solder pads to the
>>>>> power cavity is pretty much fixed by:
>>>>>
>>>>> a. The total thickness of the PCB.
>>>>> b. The pin-out of the IC.
>>>>> c. The via drill diameter.
>>>>>
>>>>> 2) Similarly the Z-axis inductance seen between the bypass
>>>>> caps and the power cavity is fixed by:
>>>>>
>>>>> a. The total thickness of the PCB.
>>>>> b. The type of bypass capacitors used.
>>>>> c. The via pattern used w/ the bypass caps.
>>>>> d. The via drill diameter.
>>>>> e. The areal density of the bypass caps used.
>>>>>
>>>>> b/c/d Determine the mounted inductance of each cap. X2Y(r)'s
>>>>> and IDC(r)'s yield the best results. In all cases the via
>>>>> pattern used makes a big difference in the number of caps
>>>>> used and the behavior at parallel resonance. In my mind it
>>>>> is a lot better to floor plan bypass caps w/ optimal via
>>>>> patterns up front, than to have the PCB designer try to fit
>>>>> them in later.
>>>>>
>>>>> 3) As the power cavity is made thinner, six notable things happen:
>>>>>
>>>>> a. The horizontal spreading inductance of the planes falls.
>>>>> The extremes for six layer 0.062" stack-ups can be almost
>>>>> 10:1 going from a
>>>>> 4 mil to a 38 mil power core.
>>>>> b. The high frequency impedance of the power system comes
>>>>> down. On the bad side one will be in PCB wave effects at
>>>>> lower frequencies. Detuning w/ discretes takes about the
>>>>> same number of parts independent of the cavity thickness.
>>>>> Tolerances are more forgiving for the thinner cavity.
>>>>> c. The parallel resonant frequency of the power system comes
>>>>> down as the square root of the power cavity thickness.
>>>>> Typical resonant frequencies typically vary over a 300MHz to
>>>>> 1.5GHz range depending on bypass scheme over the 4mil to
>>>>> 38mil cavity thicknesses.
>>>>> d. The Q of the parallel resonance goes up. On the good
>>>>> side, higher Qs
>>>>> are generally easier to detune. The bad side is that the natural
>>>>> magnitude of Zpeak is fairly independent of the cavity
>>>>> thickness, now it is much more likely to be where there is
>>>>> more signal energy. The moral here is: detune the resonance.
>>>>> e. Above and below the resonant frequency noise attenuation improves..
>>>>> f. The asymmetry between outer and inner routing layers in a
>>>>> 6 layer stack-up become more pronounced and routing density
>>>>> can suffer severely. Maintaining 50Ohms and/or acceptable
>>>>> cross talk values on outer layers more than about 10 mils
>>>>> from an image plane demands some rather wide traces and
>>>>> routing pitches.
>>>>>
>>>>> 4) An S1 G S2 S3 P S4 stack-up works best when the highest
>>>>> speed signals can be broken out and routed completely on S1.
>>>>> Otherwise S1 P S2 S3 G
>>>>> S4 is usually better breaking out high speed signals on layer
>>>>> S4 first and layer S3 second, minimizing via stubs. In
>>>>> either case prioritizing the traces with the most high speed
>>>>> energy to the routing layer(s) adjacent an image plane
>>>>> connected to the dominant coupling rail in the IC will help
>>>>> reduce demands on the PDN. That rail is usually ground.
>>>>>
>>>>> Best Regards,
>>>>>
>>>>> Steve.
>>>>>
>>>>>
>>>>> DAVID CUTHBERT wrote:
>>>>>
>>>>>
>>>>>> Fernando,
>>>>>> The S1 S2 G P S3 S4 stackup can provide excellent power plane
>>>>>> performance at the expense of S1 and S4. Routing S1 and S4
>>>>>>
>>>>>>
>>>>> mostly at
>>>>>
>>>>>
>>>>>> right angles to S2 and
>>>>>> S3 can greatly reduce the crosstalk. And using narrow traces to
>>>>>> maintain the Z0 of S1 and S4 will take care of the Z0.
>>>>>>
>>>>>> I often use S1 G S2 - S3 P S4 for 6-layer boards. The
>>>>>>
>>>>>>
>>>>> signal traces
>>>>>
>>>>>
>>>>>> are nicely isolated with a 62 mil board having spacing like so:
>>>>>> 10 mils, 5 mils, 22 mils, 5 mils, 10 mils. The tradeoff is that the
>>>>>> power plane Z0 is about 2X that of a board having 10 mils
>>>>>>
>>>>>>
>>>>> between each
>>>>>
>>>>>
>>>>>> layer. The power plane Z0 is still quite low with an inductance of
>>>>>> about 200 pH per square. Contrast this to an S1-G via inductance of
>>>>>> about 300 pH and the plane Z does not dominate things.
>>>>>>
>>>>>> Dave Cuthbert
>>>>>> NARTE Certified EMC Engineer
>>>>>> Consulting, SI, EMC, power electronics, analog of all kinds
>>>>>>
>>>>>>
>>>>>> On Wed, Feb 20, 2008 at 2:17 PM, Fernando Yuitiro Mori
>>>>>> <mori@xxxxxxxxxxxxx>
>>>>>> wrote:
>>>>>>
>>>>>>
>>>>>>
>>>>>>
>>>>>>> Hi,
>>>>>>> I normally use S1 S2 G P S3 S4 for the 6 layers stackup. I
>>>>>>>
>>>>>>>
>>>>> need the 4
>>>>>
>>>>>
>>>>>>> layer with 60 ohms, so there are some problem if I use S1
>>>>>>>
>>>>>>>
>>>>> G S2 S3 P S4?
>>>>>
>>>>>
>>>>>>> Regards,
>>>>>>>
>>>>>>> Fernando Mori
>>>>>>> ------------------------------------------------------------------
>>>>>>> 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
>>>>>>
>>>>>>
>>>>>>
>>>>>>
>>>>>>
>>>>>>
>>>>> --
>>>>> Steve Weir
>>>>> Teraspeed Consulting Group LLC
>>>>> 121 North River Drive
>>>>> Narragansett, RI 02882
>>>>>
>>>>> California office
>>>>> (408) 884-3985 Business
>>>>> (707) 780-1951 Fax
>>>>>
>>>>> Main office
>>>>> (401) 284-1827 Business
>>>>> (401) 284-1840 Fax
>>>>>
>>>>> Oregon office
>>>>> (503) 430-1065 Business
>>>>> (503) 430-1285 Fax
>>>>>
>>>>> http://www.teraspeed.com
>>>>> This e-mail contains proprietary and confidential
>>>>> intellectual property of Teraspeed Consulting Group LLC
>>>>> --------------------------------------------------------------
>>>>> ----------------------------------------
>>>>> Teraspeed(R) is the registered service mark of Teraspeed
>>>>> Consulting Group LLC
>>>>>
>>>>> ------------------------------------------------------------------
>>>>> 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
>>>>>
>>>>>
>>>>>
>>>>>
>>>>>
>>>>
>>>>
>>> --
>>> Steve Weir
>>> Teraspeed Consulting Group LLC
>>> 121 North River Drive
>>> Narragansett, RI 02882
>>>
>>> California office
>>> (408) 884-3985 Business
>>> (707) 780-1951 Fax
>>>
>>> Main office
>>> (401) 284-1827 Business
>>> (401) 284-1840 Fax
>>>
>>> Oregon office
>>> (503) 430-1065 Business
>>> (503) 430-1285 Fax
>>>
>>> http://www.teraspeed.com
>>> This e-mail contains proprietary and confidential intellectual property
>>>
>> of Teraspeed Consulting Group LLC
>>
>> ----------------------------------------------------------------------------
>> --------------------------
>>
>>> Teraspeed(R) is the registered service mark of Teraspeed Consulting Group
>>>
>> LLC
>>
>>> ------------------------------------------------------------------
>>> 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
>>
>>
>>
>>
--
Steve Weir
Teraspeed Consulting Group LLC
121 North River Drive
Narragansett, RI 02882
California office
(408) 884-3985 Business
(707) 780-1951 Fax
Main office
(401) 284-1827 Business
(401) 284-1840 Fax
Oregon office
(503) 430-1065 Business
(503) 430-1285 Fax
http://www.teraspeed.com
This e-mail contains proprietary and confidential intellectual property of
Teraspeed Consulting Group LLC
------------------------------------------------------------------------------------------------------
Teraspeed(R) is the registered service mark of Teraspeed Consulting Group LLC
------------------------------------------------------------------
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:
