Home > Community > Forums > PCB Design > Extracting Multiple Nets from PCB Editor into SigXplorer

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: *

 Extracting Multiple Nets from PCB Editor into SigXplorer 

Last post Thu, Jan 24 2008 7:52 AM by archive. 8 replies.
Started by archive 24 Jan 2008 07:52 AM. Topic has 8 replies and 1968 views
Page 1 of 1 (9 items)
Sort Posts:
  • Thu, Jan 24 2008 7:52 AM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,930
    Extracting Multiple Nets from PCB Editor into SigXplorer Reply

    I hope that this question is appropriate for this forum

    I am using the "L" version of PCB Performance and SigXplorer and am still somewhat new to them.

    I am trying to use the Topology Extract feature to extract a net into SigXplorer. The net is actually divided into 2 individual nets with 2 net names. Net #1 is routed from the driving source to one side of a series terminating resistor. Net #2 connects the other side of the term. resistor to the receiver.

    Using Topology Extract, I can only seem to extract one net or the other (including the resistor) into SigXplorer. How do I specify that I want to extract the entire net (from source to receiver)?

    Thank You

    Nick


    Originally posted in cdnusers.org by nipri
    • Post Points: 0
  • Thu, Jan 24 2008 8:19 AM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,930
    RE: Extracting Multiple Nets from PCB Editor into SigXplorer Reply

    Hi,
    the SQuest & SigExp must recognize the net as xnet, for that you need to assign a SI model to the serie resistor.
    Doron.


    Originally posted in cdnusers.org by darmoni
    • Post Points: 0
  • Thu, Jan 24 2008 8:38 AM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,930
    RE: Extracting Multiple Nets from PCB Editor into SigXplorer Reply

    Hi and thanks for the reply!

    The resistor is part of a resistor pack to which I have created / assigned an IBIS device model. I assigned all of my IBIS models through the Setup Adviser.

    How are Xnets created? Is this done through the Constraint Manager? My installation of 16.0 seems to have some problems with the help files!

    Nick


    Originally posted in cdnusers.org by nipri
    • Post Points: 0
  • Thu, Jan 24 2008 9:22 AM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,930
    RE: Extracting Multiple Nets from PCB Editor into SigXplorer Reply

    if you created it right then it should work.
    you either didn't creat a valid part or didn't assign it in the advisor,
    make sure that the value field is a number only (10 not 10R or such).
    also i think that it should be a spice model device not ibis model.
    good luck.
    Doron.


    Originally posted in cdnusers.org by darmoni
    • Post Points: 0
  • Thu, Jan 24 2008 9:40 AM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,930
    RE: Extracting Multiple Nets from PCB Editor into SigXplorer Reply

    You have to assign a dml model to the rpack and the rpack has to have the property of being a discrete for this to work correctly. SourceLink has a good example of an Rpack with common pins and the create e spice model will do standard rpacks automatically.


    Originally posted in cdnusers.org by Kalevi2
    • Post Points: 0
  • Thu, Jan 24 2008 11:18 AM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,930
    RE: Extracting Multiple Nets from PCB Editor into SigXplorer Reply

    >>You have to assign a dml model to the rpack<<

    Actually, I used the IBIS file generator in Model Integrity to make an Ibis model for the resistor pack which has 8 isolated resistors (not bussed, no common pin) I then converted the Ibis device model to DML and assigned it to each resistor pack in my design through the Adviser. The value field is set to the value of the resistor (47) with no other chars.

    When I extract either net into SigXplorer, the resistor also ports in with the correct pins on the resistor pack that the nets are connected to and the correct R value (47) also ports in. It's only the other net and its driver or receiver that doesn't port in.

    >>the rpack has to have the property of being a discrete<<
    Where do I set this?

    >>SourceLink has a good example of an Rpack with common pins<<
    Im in the process of looking for this now.

    Nick


    Originally posted in cdnusers.org by nipri
    • Post Points: 0
  • Fri, Jan 25 2008 6:20 AM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,930
    RE: Extracting Multiple Nets from PCB Editor into SigXplorer Reply

    You can change a device type in Logic - Parts List but if you have correctly assigned an espice model to the rpack, this should not be a problem.


    Originally posted in cdnusers.org by Kalevi2
    • Post Points: 0
  • Fri, Jan 25 2008 10:53 AM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,930
    RE: Extracting Multiple Nets from PCB Editor into SigXplorer Reply

    Extracting through the resistor should work (eventually!). Make sure you have PinConnections.

    When all else fails, you can extract the two nets separately and then use the File -> Append feature to glue them together. That feature is powerful yet simple, and works quite well.

    Donald


    Originally posted in cdnusers.org by Donald Telian
    • Post Points: 0
  • Mon, Feb 11 2008 10:34 PM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,930
    RE: Extracting Multiple Nets from PCB Editor into SigXplorer Reply

    Hi,

    I've seen cases in the L version of the tools where you need to run Tools, Database check inside the PCB Editor in order for it to recognize the xnet after assigning espice models to resistors - so try that.

    Best regards,
    Ole


    Originally posted in cdnusers.org by ejlersen
    • Post Points: 0
Page 1 of 1 (9 items)
Sort Posts:
Started by archive at 24 Jan 2008 07:52 AM. Topic has 8 replies.