Home > Community > Forums > PCB Design > xnets not generated properly

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: *

 xnets not generated properly 

Last post Thu, Nov 15 2007 9:49 AM by archive. 6 replies.
Started by archive 15 Nov 2007 09:49 AM. Topic has 6 replies and 1683 views
Page 1 of 1 (7 items)
Sort Posts:
  • Thu, Nov 15 2007 9:49 AM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,930
    xnets not generated properly Reply

    I'm using 15.7 and I have resistor networks 0603x4. I'm not able to properly generate xnets through these resistors. Is there such an issue or I'm not doing it properly?


    Originally posted in cdnusers.org by mihai
    • Post Points: 0
  • Thu, Nov 15 2007 10:28 AM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,930
    RE: xnets not generated properly Reply

    First thing to check with xnet generation is the models create/assigned to the discrete devices - make sure the Res Pack has a espice model assigned to it. Res Pack models do not get created automatically when using the auto setup or auto generate button (back-end or front-end), so they need to be created seperately.

    make sure the Res Pack is of CLASS = DISCRETE, and the pins are PIN_TYPE=UNSPEC


    Originally posted in cdnusers.org by andrewjw
    • Post Points: 0
  • Thu, Nov 15 2007 10:44 AM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,930
    RE: xnets not generated properly Reply

    so how do I choose or create an espice model for my resistor packs?


    Originally posted in cdnusers.org by mihai
    • Post Points: 0
  • Thu, Nov 15 2007 11:06 AM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,930
    RE: xnets not generated properly Reply

    I think I figure it out.
    This is a sample of my resistor pack model.

    ("RESNETX4_RNX4_68_68"
    ("ESpice"
    ".subckt RESNETX4_RNX4_68_68 1 2 3 4 5 6 7 8
    R1 1 2 68
    R2 3 4 68
    R3 5 6 68
    R4 7 8 68
    .ends RESNETX4_RNX4_68_68
    ")
    ("PinConnections"
    ("1" "2")
    ("2" "1")
    ("3" "4")
    ("4" "3")
    ("5" "6")
    ("6" "5")
    ("7" "8")
    ("8" "7")
    )
    )


    Originally posted in cdnusers.org by mihai
    • Post Points: 0
  • Thu, Nov 15 2007 11:22 AM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,930
    RE: xnets not generated properly Reply

    I guess you are using Allegro PCB and not DEHDL (schematic)?

    Easiest way to create a Espice model for the Res Packs in Allegro PCB is to to use:-

    Analyze->SI/EMI Sim->Model (if using XL or SI Model Setup from Tools->Setup Advisor)
    Click on RefDes Pins tab
    Find the Res Pack and select it
    Click on Create Model and create a Espice model


    Originally posted in cdnusers.org by andrewjw
    • Post Points: 0
  • Thu, Nov 15 2007 12:39 PM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,930
    RE: xnets not generated properly Reply

    I tried that, but then when I looked at the output I realized that something went wrong.
    What it did it created all the possible combination on the resistor pack. I just needed the combinations like 1-2 and 2-1. I don't know if that makes sense. Either way thanks for your help.


    Originally posted in cdnusers.org by mihai
    • Post Points: 0
  • Thu, Nov 15 2007 2:44 PM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,930
    RE: xnets not generated properly Reply

    To create a resistor pack in the SI Model Assignment form;
    Consitering a 8-pin pack;
    with mapping of: 1-2, 3-4, etc. enter the pin numbers in order as 1 2 3 4 5 6 7 8
    with mapping of: 1-8, 2-7, etc. enter the pin numbers as 1 8 2 7 3 6 4 5
    With a common pin 8: enter 8 in the common pin field and the rest as 1 2 3 4 5 6 7
    With common pins 1 and 8: enter the pin numbers as 1 2 1 3 1 4 1 5 1 6 1 7 8 2 8 3 8 4 8 5 8 6 8 7

    After creating the model select the device and then Edit Model. Review the pin mapping in the Pin Connections section of the model, it should be obvious if anything is incorret.


    Originally posted in cdnusers.org by djs
    • Post Points: 0
Page 1 of 1 (7 items)
Sort Posts:
Started by archive at 15 Nov 2007 09:49 AM. Topic has 6 replies.