Istvan,
after having worked for a PCB manufacturer for 20 years, let me tell you a
secret: there are better PCB shops and worse PCB shops.
All the higher end PCB shops by now understand, that changing the material
or the glass style or the copper roughness will have a significant impact,
even if they find the impedance to be correct at the back end of the line
(impedance testing still being the only "SI-test" at the final PCB for most
boards).
Quite a few of the higher end PCB shops have invested in insertion loss
testing like SET2DIL or SPP or VNA.
It is always a good thing, to talk with your PCB shop before they launch
your boards into production. By doing this, you can pick a stackup with
materials, that they actually have on stock and that suit your needs (nobody
can stock every flavor of material available). They can then also
understand, what is important for you (is it mainly cost, as very often, so
you pick the cheapest solution, or do you have requirements for a particular
glass style, copper roughness,...).
So bottom line, if your purchasing department is selecting the cheapest
vendor, I would double check each time. But if you are using the same
vendor(s) over a longer period of time, it is possible to build up a
relationship, were understanding between both parties can easily prevent
what you described.
Best regards,
alex
----------------------------------------------------------------------------------------------------------------------------------------
Alexander Ippich
Senior Signal Integrity Engineer
OEM Marketing Europe
Tel: +49 7457 / 605 70 79
Cell.: +49 170 / 63 68 571
e-mail: alexander.ippich@xxxxxxxxxxxxxxx
web: www.isola-group.com
-----Ursprüngliche Nachricht-----
Von: si-list-bounce@xxxxxxxxxxxxx [mailto:si-list-bounce@xxxxxxxxxxxxx] Im
Auftrag von Istvan Nagy
Gesendet: April 15, 2015 05:55 AM
An: leeritchey@xxxxxxxxxxxxx; istvan.novak@xxxxxxxxxxx; weirsi@xxxxxxxxxx;
si-list@xxxxxxxxxxxxx
Betreff: [SI-LIST] Re: 答复: Re: ??: Re: Why is my PCB loss so high?
Hi all,
Let me add my comments.
I always specify the exact material, exact glass style and copper roughness
type, but even after that I have to face these in almost every project:
- at several points in the project I will have to remind the fab that "by
the way use the material I specified". Otherwise some fabs simply ignore
this (or any other inconvenient) part of my manufacturing specs.
- they act puzzled to how come a hardware designer is telling them what
material to use, they thought it was their private business.
- some cases they tell me they are going to use "B" material, even though I
specified "A". Then I have to try to stop the manufacturing process.
I guess they are used to not getting tight specs, that when they get such
then they try to ignore it.
Regards,
Istvan Nagy
Fortinet
-----Original Message-----
From: Lee
Sent: Tuesday, April 14, 2015 9:08 AM
To: istvan.novak@xxxxxxxxxxx ; weirsi@xxxxxxxxxx ; si-list@xxxxxxxxxxxxx
Subject: [SI-LIST] Re: 答复: Re: ??: Re: Why is my PCB loss so high?
Istvan,
Not a problem. It is my experience that most companies do not specify what
they want built with enough precision to be sure that what comes in the
receiving dock is what they expected.
We have a habit as an industry of allowing fabricators to change materials,
weaves and such to achieve the lowest price and we don't know what is in the
actual PCB when we receive it. I have seen this over and over with papers
submitted to track 5 of DesignCon and the authors are mystified as to why
simulations don't match measurements.
My experience is that when a PCB is properly specified, there are very few
variations from lot to lot and vendor to vendor.
Lee
-----Original Message-----
From: Istvan Novak
Sent: Monday, April 13, 2015 9:09 PM
To: Lee ; weirsi@xxxxxxxxxx ; si-list@xxxxxxxxxxxxx
Subject: [SI-LIST] Re: 答复: Re: ??: Re: Why is my PCB loss so high?
Lee,
First I want to mention that I did not mean to pick on Isola, just the first
post referenced it. I want to acknowledge that laminate vendors have come a
long way to provide more data for the users. And yes, good laminates have
fairly consistent and repeatable electrical parameters for a given
construction, even with the anisotropy of reinforced materials. Plus it is
also clear that the lamination process itself may contribute significantly
to the final values we see in our PCBs. With all that having said, when it
comes to the SI design process, the simulation tools need numbers and
numbers need tolerance range. The range may be tight based on experience,
but without datasheet guarantee one has to wonder if once in a while a
bigger outlier may slip through...
Best regards,
Istvan
On 4/10/2015 10:15 AM, Lee wrote:
I don’t know what data sheets others have, but those I have for Isola
laminates have very detailed dk values for every combination of glass
weave style and resin content from 100 MHz to 10 GHz. I get very
precise impedance calculation results when I use that data. The
FR408HR data on the Isola web site has this level of detail. Same for
their other materials. Don't know about this for Nelco and Panasonic.
My guess is that many engineers and fabricators are operating with
very old materials data, not the most current. I know fabricators
that assume a DK that suits their equation based calculation methods!
Equations in the 21st century!
Good data is out there. Insist on it! That is how you get good results.
By the way, at the frequencies we are all dealing with now, the 2 GHz
value of DK is what you should be using. You will note that above 2
GHz, the DK is essentially constant for all materials we are likely to
use in multilayer PCBs. Nice break! Also, for a given glass to resin
ratio, the DK does not vary significantly from lot to lot. Obviously,
if you allow the fabricator to change your stackup this will not be
true.
Lee
-----Original Message----- From: Istvan Novak
Sent: Friday, April 10, 2015 5:30 AM
To: weirsi@xxxxxxxxxx ; si-list@xxxxxxxxxxxxx
Subject: [SI-LIST] Re: 答复: Re: ??: Re: Why is my PCB loss so high?
Steve,
Having worked with Scott, Al and Yuriy (and with FR408HR as well), I
fully agree with your assessment about the quality of their work.
Terry's e-mail, however, brings up something worth discussing. When
we have a product to design for volume applications, we cant assume
that every single board will go through the thorough testing and
validation to confirm the performance down to the last piece of data
we have to use in our simulations. The design eventually has to be
based on a paper trail of specifications. And since we cant test to
this detail every piece, the paper trail in the design somehow has to
consider the corner cases, the extremes. And this is where with all
the great improvements in the details of the laminate data sheets, the
specifications still do not have sufficient information. If you pull
up the FR408HR data sheet from the Isola website, you see for instance
Dk and Df values listed at 0.1, 1, 2, 5 and 10 GHz, but other then the
0.1GHz data point, all others are only typical; no range is given.
Until a range is guaranteed for the user, these questions will keep
popping up.
Regards,
Istvan Novak
Oracle
On 4/10/2015 12:40 AM, steve weir wrote:
Getting the measurements and models right is very important if you
are going to vary anything, which is pretty hard to avoid. In this,
Wild River and Simberian as well as others have done excellent work
towards obtaining pristine de-embedded measurements and accurately
derived parameter coefficients. They got there by doing a lot of time
consuming good work and constant error checking and refinement.
Being paranoid, I tend to trust very little: especially myself.
Because of the very careful and rigorous processes used, I trust Wild
River's measurements and the coefficient extractions performed using
Simbeor. If you are getting different results from the same or
similar materials you owe it to yourself to carefully double check
your extraction methodology and practices. Don't make yourself a victim
of Finnegan's Finagling Factor.
Steve.
On 4/9/2015 7:51 PM, pcb_layup wrote:
Hi Yuriy,
We used the same stackup and cross-section to compare different
base-material's performance.
Yes, different cross-section will get different data. But the
measured data (measured lots of data from mass-produced boards )
tell me that the normally 4mil trace with 85 ohm and RTF copper
designed cross-section which is hard to reach 0.35db/inch@4G for
FR408HR,even for I-SPEED. So I just want to suggest don't
over-optimistic on loss budget design.
Best regards,
Terry Ho
-----邮件原件-----
发件人: si-list-bounce@xxxxxxxxxxxxx
[mailto:si-list-bounce@xxxxxxxxxxxxx]
代表 Yuriy Shlepnev
发送时间: 2015年4月10日 5:34
收件人: pcb_layup@xxxxxxx; al@xxxxxxxxxxxxxxxxx; 'si-list'
抄送: 'Tom Dagostino'; 'Joel Brown'; 'Scott McMorrow'
主题: [SI-LIST] Re: ??: Re: Why is my PCB loss so high?
Terry,
It looks like you are lumping dielectric and conductor losses into
the dielectric loss by increasing the dissipation factor. It may be
suitable only in case if you use exactly the same cross-section as
used on the test board. Change of cross-section may cause
substantial difference in the loss estimation if losses from
conductor roughness were not properly separated in the model. See
more on that at app notes #2012_02 and #2013_01 (paper from
DesignCon 2012) at http://www.simberian.com/AppNotes.php
Considering FR408, in another "Lessons learned..." project with
smaller traces in FR408HR we have observed total losses from 0.3 to
0.35 dB/inch - see details in DesignCon 2013 paper available as
#2014_01 at http://www.simberian.com/AppNotes.php We used accurate
analysis with GMS-parameters that eliminates the reflection
completely.
Best regards,
Yuriy
Yuriy Shlepnev, Ph.D.
President, Simberian Inc.
3030 S Torrey Pines Dr. Las Vegas, NV 89146, USA Office
+1-702-876-2882; Fax
+1-702-482-7903 Cell +1-206-409-2368; Virtual +1-408-627-7706
Skype: shlepnev
www.simberian.com
Simbeor – Accurate, Fast, Easy and Affordable Electromagnetic Signal
Integrity Software
2010 and 2011 DesignVision Award Winner
-----Original Message-----
From: si-list-bounce@xxxxxxxxxxxxx
[mailto:si-list-bounce@xxxxxxxxxxxxx] On Behalf Of pcb_layup
Sent: Wednesday, April 8, 2015 6:39 PM
To: shlepnev@xxxxxxxxxxxxx; al@xxxxxxxxxxxxxxxxx; 'si-list'
Cc: 'Tom Dagostino'; 'Joel Brown'; 'Scott McMorrow'
Subject: [SI-LIST] ??: Re: Why is my PCB loss so high?
Hi Joel,
I would like share some data simulated IS408HR for reference.
IS408HR: Stripline, VLP copper foil, DF=0.0101@1G; Simulation：
-0.448db/inch@3G.
IS408HR: Microstrip with SM coated, HTE copper foil, DF=0.0101@1G;
Simulation：：-0.404db/inch@3G.
Personally I think IS408HR cannot reach -0.25~-0.3db/inch level.
Because
comparing the ISOLA more high-end I-Speed DF=0.0068@1G, I got the
measured data about: -0.45db/inch@4G (Strip:VLP and microstrip HTE).
The data came from mass-produced TV boards follow Intel's 16L
Insertion Loss test board design, also did measurement correlation
with third-party.
Best regards,
Terry Ho
-----邮件原件-----
发件人: si-list-bounce@xxxxxxxxxxxxx
[mailto:si-list-bounce@xxxxxxxxxxxxx]
代表 Yuriy Shlepnev
发送时间: 2015年4月9日 1:01
收件人: al@xxxxxxxxxxxxxxxxx; 'si-list'
抄送: 'Tom Dagostino'; 'Joel Brown'; 'Scott McMorrow'
主题: [SI-LIST] Re: Why is my PCB loss so high?
Joel,
To be more specific, here are the data we have observed on Wild
River's
CMP-28 channel modeling platform made of FR408HR (see description at
the "Sink or Swim at 28 Gbps" app note available at
http://www.simberian.com/AppNotes.php, or complete description of
Simbeor Kit for CMP-28 platform at
http://www.simberian.com/Presentations/CMP-28_Simbeor_Kit_Guide.pdf):
Models identified with GMS-parameters (very similar to SPP):
FR408HR model: Wideband Debye, Dk=3.815 (3.66 in spreadsheet),
LT=0.0117 @ 1
GHz; Conductor roughness model for strip: Modified Hammerstad,
SR=0.4 um,
RF=2; Conductor roughness model for micro-strip: Modified
Hammerstad, SR=0.4 um, RF=3.5; SR is RMS value of surface roughness
and RF is the roughness factor.
As you can see the identified FR408HR parameters are close to
identified and published by Isola. Small increase in the Dk is due
to the anisotropy - Isola uses Berezkin's method that identifies out
of plane value of Dk with wide strip resonator. For narrow strips we
observe larger Dk because of in plane values are typically larger
due to layered structure of the laminate.
As you can see, attenuation for both strip and micro-strip is about
0.25
dB/inch at 3 GHz; It is a little larger for the common mode in
microstrip - about 0.268 dB/inch. Those are numbers identified with
GMS-parameters by removing reflection completely.
Let's see what can possibly increase the insertion loss from 0.3 to
0.76 or
even 1.4 dB/inch, as you observed it.
1. Reflection: Let's assume you have 5 inch t-line segment and 0.3*5
insertion loss expected without the reflections. If you observed
0.7*5 dB
insertion loss, the reflection loss should be about 5.8 dB at 3 GHz
- pretty
bad connector or launch. It is even less possible to have 1.4*5 -
the reflection loss should be 2.9 dB (half of the energy reflected).
You definitely should notice that.
2. Roughness: The skin depth at 3 GHz in copper is about 1.2 um. To
have losses losses doubled the strips and planes must have RMS
roughness value close or larger than skin depth and roughness factor
larger than 2 (mushroom-like surface). This is possible.
3. Plating for microstrips: Nickel-gold plating can substantially
increase the losses at 3 GHz (nickel produces resonance around 2.5
GHz). In this paper
https://www.researchgate.net/publication/238524042_Nickel_characteri
zation_f
or_interconnect_analysis we observed increase in the attenuation
from 1 dB/inch to 1.64 dB/inch, though for different dielectric and
packaging interconnect. It would be very interesting, if it is
nickel in your case.
4. Combination of different factors. The best way to go is to
eliminate one contributor at a time.
Best regards,
Yuriy
Yuriy Shlepnev, Ph.D.
President, Simberian Inc.
3030 S Torrey Pines Dr. Las Vegas, NV 89146, USA Office
+1-702-876-2882; Fax
+1-702-482-7903 Cell +1-206-409-2368; Virtual +1-408-627-7706
Skype: shlepnev
www.simberian.com
Simbeor - Accurate, Fast, Easy and Affordable Electromagnetic Signal
Integrity Software
2010 and 2011 DesignVision Award Winner
-----Original Message-----
From: si-list-bounce@xxxxxxxxxxxxx
[mailto:si-list-bounce@xxxxxxxxxxxxx] On Behalf Of Alfred P. Neves
Sent: Wednesday, April 8, 2015 8:30 AM
To: si-list
Cc: Tom Dagostino; Joel Brown; Scott McMorrow
Subject: [SI-LIST] Re: Why is my PCB loss so high?
Our Channel Modeling platform used for SERDES testing, ISI-32 is
constructed
with FR408HR and the loss dB/inch/GHz as calculated by Simbeor, and
ADS is
close to the Isola published loss numbers for loss tangent. This
platform
includes multiple microstrip and stripline lengths from approximately
3inches to 50inches for creating ISI in several inch increments.
We have
found the Isola published data to provide reasonably good accuracy
for their
materials. TomБ-?s point is important in that return loss vectorially
subtracts from insertion loss, so a good launch design is important,
even if
your using fancy de-embedding or loss extraction schemes.
For ADS we used measure-modeled based de-embedding, for Simbeor we
used GMS
parameters. Simbeor uses line segments, in ADS we used lines and
Beatty
standards. The ADS approach is described on Keysight/WRT Tutorial
we did
last DesignCon and is on our website, 32Gbpsec Test Fixture Design, and
Simbeor has numerous app notes on GMS method.
Our measurements were validated using a good S-parameter work flow,
checking
for passivity, causality, with a validated calibration using Stepped
impedance standard and precision wideband terminators, along with short
THRU. We pass our S-parameters through Simbeor for our post
measurement
work flow.
- Al
Products for the Signal Integrity Practitioner
Alfred P. Neves
Chief Technologist
Office: 503-679-2429
www.wildrivertech.com
On Apr 7, 2015, at 5:44 PM, Scott McMorrow <scott@xxxxxxxxxxxxx>wrote:
wrote:
to follow on, stripline or microstrip? are you deembedding the traces
to remove fixturing from the loss measurement.
Scott McMorrow
Consultant - R&D
16 Stormy Brook Rd
Falmouth, ME 04105
(401) 284-1827 Business
http://www.teraspeed.com
On Tue, Apr 7, 2015 at 5:13 PM, Tom Dagostino <tom@xxxxxxxxxxxxxxxxx>
boards?Joel
What is your test method? How are you connecting to the board? What
test equipment are you using? Are you measuring the same net on both
inch.Tom Dagostino
Teraspeed Labs
9999 SW Wilshire Street
Suite 102
Portland, OR 97225
tom@xxxxxxxxxxxxxxxxx
www.teraspeedlabs.com
971-279-5325 office
503-430-1065 cell
-----Original Message-----
From: si-list-bounce@xxxxxxxxxxxxx
[mailto:si-list-bounce@xxxxxxxxxxxxx]
On
Behalf Of Joel Brown
Sent: Tuesday, April 07, 2015 2:01 PM
To: SI-List
Subject: [SI-LIST] Why is my PCB loss so high?
We have had several boards made from Isola FR408HR.
My understanding is that at 3 GHz loss should be about 0.3 db / inch.
On one board I am measuring about 0.76 db / inch, on another 1.4 db /
------------------------------------------------------------------What can account for this?------------------------------------------------------------------
Thanks
------------------------------------------------------------------
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 forum is accessible at:
http://tech.groups.yahoo.com/group/si-list
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
------------------------------------------------------------------
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 forum is accessible at:
http://tech.groups.yahoo.com/group/si-list
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
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 forum is accessible at:
http://tech.groups.yahoo.com/group/si-list
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
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 forum is accessible at:
http://tech.groups.yahoo.com/group/si-list
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
------------------------------------------------------------------
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 forum is accessible at:
http://tech.groups.yahoo.com/group/si-list
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
------------------------------------------------------------------
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 forum is accessible at:
http://tech.groups.yahoo.com/group/si-list
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
------------------------------------------------------------------
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 forum is accessible at:
http://tech.groups.yahoo.com/group/si-list
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
------------------------------------------------------------------
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 forum is accessible at:
http://tech.groups.yahoo.com/group/si-list
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
------------------------------------------------------------------
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 forum is accessible at:
http://tech.groups.yahoo.com/group/si-list
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
