• State Resolved
  • Locked Locked
  • Replies 2 replies
  • Subscribers 39 subscribers
  • Views 1391 views
  • Users 0 members are here
Support feedback
Options
Options
Related

This thread has been locked.

If you have a related question, please click the "Ask a related question" button in the top right corner. The newly created question will be automatically linked to this question.

Supported Circuit Elements / Is LTRA Supported

Anthony F. Seely
Guru 69070 points

Other Parts Discussed in Thread: TINA-TI

Hi, I'm trying to model a differential driver / receiver pair with a lossy transmission line in between the two.

I've read  http://e2e.ti.com/support/development_tools/webench_design_center/f/234/t/234485.aspx

and downloaded the model.  But when I copy / paste the lossy model into my testbench, I get errors about the receiver side of the transmission line floating.

I've tried to make a new macro subcircuit that includes the LTRA device:

* LTRA Subcircuit - 120 Ohm Zo, 1 Meter
.SUBCKT LTRA_Z120_1M 1001 1002 1003 1004
* PINOUT ORDER        N1    N2   N3   N4
* Port 1 Nodes are N1,N2.  Port 2 Nodes are N3, N4
*///////////////////////////////////////////////////////////
.MODEL XLINE LTRA R=5m L=1.28n C=18.2p LEN=39
O1 1001 1002 1003 1004 XLINE
.ENDS LTRA_Z120_1M

But when Tina crunches this in the create new macro wizard, it reports:  "Invalid syntax element LTRA, Line: #6.


I'm thinking that maybe the Tina-TI package does not support the LTRA component,  but I can't find any clear documentation on this.  In fact the component help indicates that there is a transmission line schematic symbol which doesn't show up on the component toolbar in the program.

Version I'm using is Version 9.3.50.40 SF-TI     

Thanks,

Anthony

  • 0
    TI__Mastermind 39210 points

    Hi Anthony,

    TINA-TI accepts standard PSpice formats. This is an excerpt from the PSpice manual for transmission lines. Please try using this syntax instead. This is similar to what is given in the post that you were referring to. Please make sure that you have made all connection properly in your schematic. It is a 4 terminal device so please do not leave any node floating.

    General form

    T<name> <A port (+) node> <A port (-) node>
    + <B port (+) node> <B port (-) node>
    + [ <model name> [electrical length value] ]
    + LEN=<value> R=<value> L=<value>
    + G=<value> C=<value>


    Examples

    T1 1 2 3 4 Z0=220 TD=115ns
    T2 1 2 3 4 Z0=220 F=2.25MEG
    T3 1 2 3 4 Z0=220 F=4.5MEG NL=0.5
    T4 1 2 3 4 LEN=1 R=.311 L=.378u G=6.27u C=67.3p
    T5 1 2 3 4 TMOD 1

    Model form .MODEL <model name> TRN [model parameters]

    Best regards,

  • 0 in reply to Nikhil Gupta (Product Folder Models)
    TI__Guru 69070 points

    Hi Nikhil,

    Thanks for the quick reply - you got me unstuck!

    I wound up doing the following:

    .SUBCKT TRANLINE_Z120 1 2 3 4 5
    *T1 1 2 3 4 Z0=120 TD=6n
    T1 1 2 3 4 LEN=1 R=5m L=39 G=5u C=18.2p
    R1 1 5 1Meg
    R2 2 5 1Meg
    R3 3 5 1Meg
    R4 4 5 1Meg
    .END

    Adding a 5th port to GND and the 1Meg resistors.   Without this, I got the errors about ports 3 and 4 floating,  just like with the symbol from the previous post.

    Also the above didn't work with the 2nd T1 line uncommented.  I got a "Model Error" with this form.

    The first form of the transmission line with Z0 and TD worked though.

    Thanks and Best Regards,

    Anthony