Home > Community > Forums > PCB Design > DP extraction for SI-crosstalk as coupled microstrip line

Email

* Required Fields

Recipients email * (separate multiple addresses with commas)

Your name *

Your email *

Message *

Contact Us

* Required Fields
First Name *

Last Name *

Email *

Company / Institution *

Comments: *

 DP extraction for SI-crosstalk as coupled microstrip line 

Last post Thu, Sep 25 2008 1:26 AM by MAAC. 5 replies.
Started by MAAC 09 Sep 2008 04:04 AM. Topic has 5 replies and 4192 views
Page 1 of 1 (6 items)
Sort Posts:
  • Tue, Sep 9 2008 4:04 AM

    • MAAC
    • Top 25 Contributor
    • Joined on Thu, Jul 17 2008
    • Bangalore, Karnataka
    • Posts 195
    • Points 3,620
    DP extraction for SI-crosstalk as coupled microstrip line Reply

    Hi,

    Has any body tried to extract the Differential pairs to SI to anlayze as a single Microstrip line. The measurement can be EMI or crosstalk.

    The topolgogy should be like the one which is attached. But it should be directly extracted from the board.

    If yes can u explain with some design as the reference.

     

    Thanks,


    • Post Points: 20
  • Tue, Sep 9 2008 10:16 PM

    • Khurana
    • Top 25 Contributor
    • Joined on Thu, Aug 14 2008
    • Posts 238
    • Points 3,315
    Re: DP extraction for SI-crosstalk as coupled microstrip line Reply

     Yes, I have, however, I am not sure what your question is.  To be able to extract an unrouted or routed differential from the board (Allegro) into SigXplorer topology canvas, the pins that the two nets (that make up the differential pair) are attached to, should be defined as "mate pins" in the IBIS Device Model Editor for the model being reference by that footprint (this is accomplished in the Signal Model Assignment window).  Then invoke the Probe command and if one net is selected then both nets are automatically selected and extracted when the View Topology button is clicked.

    • Post Points: 20
  • Wed, Sep 10 2008 9:26 AM

    • Ejlersen
    • Top 10 Contributor
    • Joined on Mon, Jul 28 2008
    • Aalborg, Copenhagen
    • Posts 569
    • Points 10,080
    Re: DP extraction for SI-crosstalk as coupled microstrip line Reply

    Hi,

    In this case, there are several things to look for.

    1. The 2 nets should be defined as a differential pair.
    2. The pins on the component should have ibis models with 'mate' pins assigned. (check model for this)
    3. In the Analyze, SI/EMI SIM, Preferences, InterconnectModels check that Differential pair extraction mode is enabled. Also check what the 'minimum coupled length' is - if it is larger than the length the traces are coupled then you'll see 2 microstrips or striplines instead of a coupled pair.

     

    Best regards Ole
    • Post Points: 20
  • Thu, Sep 11 2008 3:15 AM

    • MAAC
    • Top 25 Contributor
    • Joined on Thu, Jul 17 2008
    • Bangalore, Karnataka
    • Posts 195
    • Points 3,620
    Re: DP extraction for SI-crosstalk as coupled microstrip line Reply

    Hi All,

    I tried all ur suggestions but still couldnot extract the DP.

    Sometimes i get this warning

    WARNINGS:
    Diff pair DP1 is not defined by a signal model so only one member of the diff pair will be extracted.

    Should i make any settings in cross-section like differential mode and set the coupling type to edge....something like that which i say in some seminar..

    Can somebody explain me with some sample design file....

    i have assigned the 2 pins as shown in the pic with their corresponding mate pins.....is this correct

     


    • Post Points: 20
  • Thu, Sep 11 2008 4:37 AM

    • Ejlersen
    • Top 10 Contributor
    • Joined on Mon, Jul 28 2008
    • Aalborg, Copenhagen
    • Posts 569
    • Points 10,080
    Re: DP extraction for SI-crosstalk as coupled microstrip line Reply

    Hi,

     I'm sorry but I cannot send out any samples of this. But the message tells me that the problem is within the IBIS models.

    Have you assigned IBIS models to your devices (Analyze, SI/EMI SIM, Models)

    If you have done so, It's beacuse no 'Mate' pins are assigned for differential pairs. 

    I have a movie that shows whats wrong, but cannot upload files of size more than 750Kb - but in the models dialog, select the component then edit model

    Click the pin and set the type to inverting/non-inverting and set the correct mate pin.

     

    Best regards Ole
    • Post Points: 20
  • Thu, Sep 25 2008 1:26 AM

    • MAAC
    • Top 25 Contributor
    • Joined on Thu, Jul 17 2008
    • Bangalore, Karnataka
    • Posts 195
    • Points 3,620
    Re: DP extraction for SI-crosstalk as coupled microstrip line Reply

    Hi all,

    I could extract the topology for DP from the board but the buffer assigned at input are something like combined one.. so i`m not able to simulate for crosstalk.. The topology is attached for the ref...

     Any suggestions...

     

    thanks,


    • Post Points: 5
Page 1 of 1 (6 items)
Sort Posts:
Started by MAAC at 09 Sep 2008 04:04 AM. Topic has 5 replies.