headers
Bokkyu Choi | 1 Jul 2011 04:39
Picon

Re: [SI-LIST] Re: 答复: [SI-LIST] Crosstalk and Overshoot/Undershoot

The polarityof the FEXT is related with the capacitive & inductive coupling. 
If the inductive coupling is larger than the capacitive coupling then FEXT is negative. 
If the capacitive coupling is same as the inductive coupling the FEXT is minimized. 

나의 iPhone에서 보냄

2011. 6. 30. 오후 11:23 Scott McMorrow <scott@...> 작성:

> Shaopeng brings up a good point.  However, I'd like to add a bit more 
> clarity
> 
> FEXT (Far End Crosstalk) and NEXT (Near End Crosstalk) are what we 
> measure in an interconnect system.  They depend on both the coupling 
> coefficients of the interconnect, the directionality of the aggressor, 
> the topology of the interconnect, and any mismatches in the sections of 
> the lines, or the termination at all ends.
> 
> Forward Crosstalk and Reverse Crosstalk define the wave fronts that 
> propagate on perfectly matched uniform sections of the interconnect.  
> Forward crosstalk has the opposite polarity of the aggressor pulse.  
> Reverse Crosstalk has the same polarity of the aggressor pulse.
> 
> Measured FEXT may not be the opposite polarity of the aggressor pulse.  
> It is the instantaneous sum of all propagated Forward Crosstalk, and all 
> reflected Reverse Crosstalk on the interconnect from all possible 
> aggressors.  If reflected Reverse Crosstalk is dominant, then measured 
> FEXT can have the same polarity as the aggressor pulse.  Everything 
> depends on the interconnect system.
> 
>
(Continue reading)

Permalink | Reply | 0 comments |
headers
Newbie Pugal | 1 Jul 2011 05:58
Picon
Favicon

Re: [SI-LIST] Re: 答复: [SI-LIST] Crosstalk and Overshoot/Undershoot

Hi All,
Thanks for all the replies. Now one question on the tools and crosstalk measurement. Does the simulation
tools gives us the overall crosstalk values due to FEXT and NEXT? Or else provides the values separately
and which one to worry most. I know that if there is a impedance mismatch at the near end NEXT will reflect
back to receiver on victim lines right, but how long the generated  crosstalk remains in its peak value?

What are all the boundary conditions need to be followed for crosstalk simulations?

Thanks
Pugal

________________________________
From: Scott McMorrow <scott@...>
To: si-list@...
Sent: Thursday, 30 June 2011 7:53 PM
Subject: [SI-LIST] Re: 答复: [SI-LIST] Crosstalk and Overshoot/Undershoot

Shaopeng brings up a good point.  However, I'd like to add a bit more 
clarity

FEXT (Far End Crosstalk) and NEXT (Near End Crosstalk) are what we 
measure in an interconnect system.  They depend on both the coupling 
coefficients of the interconnect, the directionality of the aggressor, 
the topology of the interconnect, and any mismatches in the sections of 
the lines, or the termination at all ends.

Forward Crosstalk and Reverse Crosstalk define the wave fronts that 
propagate on perfectly matched uniform sections of the interconnect.  
Forward crosstalk has the opposite polarity of the aggressor pulse.  
Reverse Crosstalk has the same polarity of the aggressor pulse.
(Continue reading)

Permalink | Reply | 1 comment |
headers
Paramjeet Singh | 1 Jul 2011 06:16
Picon

Help regarding SI setup

Hi All,
I am new to Signal Integrity, and am interested on doing SI analysis using
the simulation tools.
I have the extracted package as well as the extracted I/O's of my chip.
I  do not have the board models with me as such.

Currently I am creating the ring structure using the I/O's for the critical
signals (only signals of DDR interface) in the same order as they are in the
actual chip.
I am establishing the connectivity between the I/O and package node.

Can someone let me know:
1)  what all things we need to check in the simulation runs for the signals.
2) Also what all are the critical signals for DDR1 I need to look for.
3) What is the stimulus methodology I need to follow
4) Do I need to run for every signal individually in the simulation keeping
it static and toggling the other signals.

Can someone share with me the setup criteria to be followed.

Thanks
Paramjeet Singh

------------------------------------------------------------------
To unsubscribe from si-list:
si-list-request@... with 'unsubscribe' in the Subject field

or to administer your membership from a web page, go to:
http://www.freelists.org/webpage/si-list
(Continue reading)

Permalink | Reply | 1 comment |
headers
Shao, Peng | 1 Jul 2011 07:11
Favicon

答复: [SI-LIST] Help regarding SI setup

Singh,
Please do not expect to hug an elephant, of course not to try to hug four elephants(your 4 questions) once a time.
For your case:
1 Pick up anyone of the signals in your design. Simulate and Study the result.
2 Changing the Trace Length/Terminator/Buffer Model, any factors you may change, compare the different
result and think about it.
3 Study the DDR specification, try to understand what is DDRx. Then you will know which signals should be
simulation and the timing relationship between these signal.
4 Different stimulus means different response. So, it depends on what kind of characters you want to investigate.
BTW: Hyperlynx from MentorGraphics is a good tools, with a lot of design wizards and kits, whick can guide
you to finish your job quickly in the right direction.
And the customer training held by MentorGraphics covers all the topics you are interested in. 

Shaopeng
AE Consultant   Mentor Graphics Electronic Technology Co., Ltd.
Tel:  +86-10 - 5930 4050
Cell:  +86-136 1105 7707
Fax:  +86-10-6808 0319
E-mail: peng_shao@... 
Address: RM1512, CanWay Building, No.66 NanLiShi Lu, Beijing, China 100045

-----邮件原件-----
发件人: si-list-bounce@...
[mailto:si-list-bounce@...] 代表 Paramjeet Singh
发送时间: 2011年7月1日 12:17
收件人: si-list@...
主题: [SI-LIST] Help regarding SI setup

Hi All,
I am new to Signal Integrity, and am interested on doing SI analysis using
(Continue reading)

Permalink | Reply | 0 comments |
headers
Shao, Peng | 1 Jul 2011 07:18
Favicon

答复: [SI-LIST] Re: [SI-LIST] Re: 答复: [SI-LIST] Crosstalk and Overshoot/Undershoot

Pugal,
Basically, yes. The simulation tools can tell you the overall corsstalk and reflections.
But by setting up the special and right environment, you may get the FEXT and NEXT separately from
simulation tools. 
For the pure Xtalk, the duration of NEXT and the amplitude of FEXT is proportion to the couple length.
But in practice, Xtalk always mixed with reflections. So, you need to do different simulation by modifying
the terminator scheme and trace length to study each factors of Xtalk and reflections. 

Shaopeng
AE Consultant   Mentor Graphics Electronic Technology Co., Ltd.
 Tel:  +86-10 - 5930 4050
Cell:  +86-136 1105 7707
Fax:  +86-10-6808 0319
E-mail: peng_shao@... 
 Address: RM1512, CanWay Building, No.66 NanLiShi Lu, Beijing, China 100045

-----邮件原件-----
发件人: si-list-bounce@...
[mailto:si-list-bounce@...] 代表 Newbie Pugal
发送时间: 2011年7月1日 11:58
收件人: Scott McMorrow; si-list@...
主题: [SI-LIST] Re: [SI-LIST] Re: 答复: [SI-LIST] Crosstalk and Overshoot/Undershoot

Hi All,
Thanks for all the replies. Now one question on the tools and crosstalk measurement. Does the simulation
tools gives us the overall crosstalk values due to FEXT and NEXT? Or else provides the values separately
and which one to worry most. I know that if there is a impedance mismatch at the near end NEXT will reflect
back to receiver on victim lines right, but how long the generated  crosstalk remains in its peak value?

What are all the boundary conditions need to be followed for crosstalk simulations?
(Continue reading)

Permalink | Reply | 0 comments |
headers
Jayasuryan KG | 1 Jul 2011 10:04
Picon
Favicon

Re: Differential Pair - Impedance Question

Dear Rohit,

Thanks for the detailed reply. Is there any tool to make sure that the 
impedance of the individual trace is 45 Ohm and it is 90 Ohm (no mutual 
coupling) when it will be differential?
How can we make sure it is meeting the our requirement in manufacturing too. 
Impedance coupons are the only way or do we have any other solution(s)?

Best Regards,
Jayasuryan

-----Original Message----- 
From: Rohit MISHRA
Sent: Thursday, June 30, 2011 7:06 PM
To: si-list@...
Cc: suryan_tvm@...
Subject: RE: [SI-LIST] Re: Differential Pair - Impedance Question

Jayasuryan,

When you talk about "45 Ohm impedance for individual", you are talking about 
characteristic impedance(Z0) of individual or single ended line which is 
intrinsic to that line only and can't be changed by changing differential 
impedance actually it is other way around, once you have set the 
characteristic impedance of your single ended line then differential 
impedance between two lines depends on characteristic impedance(Z0) of lines 
and mutual coupling between them.

So if characteristic impedance of single ended line (D+ & D-) is Z0 and 
coupling coefficient between them is k then
(Continue reading)

Permalink | Reply | 4 comments |
headers
steve weir | 1 Jul 2011 10:20

Re: Differential Pair - Impedance Question

Use a field solver.

Steve.
On 7/1/2011 1:04 AM, Jayasuryan KG wrote:
> Dear Rohit,
>
> Thanks for the detailed reply. Is there any tool to make sure that the
> impedance of the individual trace is 45 Ohm and it is 90 Ohm (no mutual
> coupling) when it will be differential?
> How can we make sure it is meeting the our requirement in manufacturing too.
> Impedance coupons are the only way or do we have any other solution(s)?
>
> Best Regards,
> Jayasuryan
>
> -----Original Message-----
> From: Rohit MISHRA
> Sent: Thursday, June 30, 2011 7:06 PM
> To: si-list@...
> Cc: suryan_tvm@...
> Subject: RE: [SI-LIST] Re: Differential Pair - Impedance Question
>
> Jayasuryan,
>
> When you talk about "45 Ohm impedance for individual", you are talking about
> characteristic impedance(Z0) of individual or single ended line which is
> intrinsic to that line only and can't be changed by changing differential
> impedance actually it is other way around, once you have set the
> characteristic impedance of your single ended line then differential
> impedance between two lines depends on characteristic impedance(Z0) of lines
(Continue reading)

Permalink | Reply | 2 comments |
headers
Havermann, Gert | 1 Jul 2011 13:12

AW: Re: Differential Pair - Impedance Question

Jayasuryan,

the coupling between individual traces of a differential pair is a function of distance. The wider you put
the traces apart, the lower the coupling. In your case with 45Ohm individual and 90 Ohm differential
impedance, you will go for zero coupling, thus the traces need to be far away.
For stripline, as a rule of thumb, 1.5 times the Signal Plane to GND Plane distance (prepreg thicknes) would
be a good starting point for zero coupling.

Just couriosity, why do you need 45 Ohm single ended impedance? In many differential applications a
tighter coupling is beneficial.

BR
Gert

--------------------------------------------------------------------------
Absender ist HARTING Electronics GmbH & Co. KG; Sitz der Gesellschaft: Espelkamp; Registergericht: Bad
Oeynhausen; Register-Nr.: HRA 5596; persönlich haftende Gesellschafterin: HARTING Electronics
Management GmbH; Sitz der Komplementär-GmbH: Espelkamp; Registergericht der Komplementär-GmbH:
Bad Oeynhausen; Register-Nr. der Komplementär-GmbH: HRB 8808; Geschäftsführer: Edgar-Peter
Duening, Torsten Ratzmann, Dr. Alexander Rost
-----Ursprüngliche Nachricht-----

Von: si-list-bounce@...
[mailto:si-list-bounce@...] Im Auftrag von Jayasuryan KG
Gesendet: Freitag, 1. Juli 2011 10:05
An: Rohit MISHRA
Cc: si-list@...
Betreff: [SI-LIST] Re: Differential Pair - Impedance Question

Dear Rohit,
(Continue reading)

Permalink | Reply | 0 comments |
headers
Rohit MISHRA | 1 Jul 2011 13:34

Re: Differential Pair - Impedance Question

Jayasuryan,

Well I assume you are talking about pcb traces. 

There are two sets of tools which is used in industry for calculating & measuring characteristic and
differential impedance. Field solver can be used on pcb layout before pcb manufacturing while TDR or VNA
is used on manufactured pcb.

Since characteristic impedance and hence differential impedance depends on geometry(space, width,
thickness ) of traces, These geometry information you get from pcb fabricator guy, when you provide him
impedance information. PCB layout engineer job is to use this geometry information and make a layout. 

Once layout is ready, use field solver to calculate impedance and use TDR or VNA to measure & ensure that pcb
traces are manufactured with correct impedance.

Hope it helps.

Rgds,
Rohit

-----Original Message-----
From: si-list-bounce@...
[mailto:si-list-bounce@...] On Behalf Of steve weir
Sent: Friday, July 01, 2011 1:51 PM
To: si-list@...
Subject: [SI-LIST] Re: Differential Pair - Impedance Question

Use a field solver.

Steve.
(Continue reading)

Permalink | Reply | 1 comment |
headers
J_Dong | 1 Jul 2011 16:50
Favicon

Re: Differential Pair - Impedance Question

Here you can estimate the impedance of microstrip-type pcb:
http://www.microwaves101.com/encyclopedia/calmstrip.cfm

and stripline-type pcb:
http://www.microwaves101.com/encyclopedia/calsstrip.cfm

and coplanar-type pcb:
http://www.microwaves101.com/encyclopedia/calcpw.cfm

Note that all those calculations are approximated. If your parameters are
out of their range (e.g. dielectric constant too high, pcb too thick etc),
you have to use some full-wave simulators. Here is a free solution for that:
http://www.feko.info/ Their evaluation version of the software allows
simulation with limited number of unknowns, which should be more than enough
to handle this sort of problems.

-----------------------------------------------------

Junwei Dong, Ph.D.

Research Scientist

Microwave Engineering Corporation (MEC)

1551 Osgood Street, North Andover, MA 01845

Tel:  +1-978-685-2776 (Ext.12)

Fax: +1-978-975-4363
(Continue reading)

Permalink | Reply | 0 comments |

Gmane