• State Resolved
  • Locked Locked
  • Replies 10 replies
  • Answers 2 answers
  • Subscribers 49 subscribers
  • Views 605 views
  • Users 0 members are here
Support feedback
Options
Options
Similar topics

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.

Original question:

TLV2381 Op Amp TINA Library?

TLV2381: Spice model

Alberto Burani
Intellectual 345 points
Part Number: TLV2381
Other Parts Discussed in Thread: TLV9042, TINA-TI

is it possible to have a pspice model of TLV2381?

Thank you

  • 0
    TI__Genius 17587 points

    Hey Alberto, 

    There is currently no existing model for this part and has a deprioritized development since it was released 19 years ago. 
    For evaluation purposes, I suggest sampling the part and evaluating it in person. 

    A better solution I believe would be to suggest a newer part that has a model already available. 
    What are your system needs?

    All the best,
    Carolina

  • 0 in reply to Caro Walter
    Intellectual 345 points

    Hi Carolina,

    my needs are:

    low power (20  microamps max)

    Highest possible slew rate

    power supply range from 2.7 to  5V

    RRO

    no phase reversal for out of rail input

    no bga

    Thanks for your suppport

  • 0 in reply to Alberto Burani
    TI__Genius 17587 points

    Hey Alberto, 

    I believe that TLV9042 will be a better fit here. There is a TINA and Pspice available for the part. 

    All the best,
    Carolina

  • 0 in reply to Caro Walter
    Intellectual 345 points

    Hi,

    I've placed the model of the tlv9402 into my circuit in pspice but it doens not work, I get the rerror:

    **** EXPANSION OF SUBCIRCUIT X_U4.XCLAWp ****
    X_U4.XCLAWp.G1 X_U4.25 X_U4.VCC_B TABLE {ABS(V(0#,1#))} 0 1.00E-05 36
    + 1.50E-05 37.5 2.50E-04 40 1.75E-03 40
    -------------------------------------$
    ERROR(ORPSIM-16049): Values must be monotonic increasing

    With many other models I don't have any kind of issue. Is there a new model available? Do you know something about this issue?

    Thank you

  • 0 in reply to Alberto Burani
    TI__Genius 17587 points

    Hey Alberto, 

    Have you tried using the TLV9042 from Pspice for TI? Have you had similar issues from TINA-TI?

    All the best,
    Carolina 

  • 0 in reply to Caro Walter
    Intellectual 345 points

    Hi Carolina,

    no I tried with PSPICE A/D 17.4 which is the same of PSPICE for TI.

    The reference design in tina TI is working but this does not help me because i need a PSPICE model.

    I've also tried to copy the model of the TINA ref design in to my model but the issue is allways the same.

    Thanks for your help

  • 0 in reply to Alberto Burani
    TI__Genius 17587 points

    Hey Alberto, 

    I will try to run your attached files and compare against the working model that I have to try to nail down what causes convergence issues. I will report back when I have more details. 

    All the best,
    Carolina

  • 0 in reply to Caro Walter
    TI__Genius 17587 points

    Hey Alberto, 

    It would seem that PSpice is much less forgiving in terms of netlists than TINA. The error that is showing up is from the claw portion of the model that is a piecewise: "Values must be monotonic increasing" is complaining about these lines: 

    .SUBCKT VCCS_LIM_CLAW+_0 VC+ VC- IOUT+ IOUT-
    G1 IOUT+ IOUT- TABLE {ABS(V(VC+,VC-))} =
    +(0, 1.00E-05)
    +(36, 1.50E-05)
    +(37.5, 2.50E-04)
    +(40, 1.75E-03)
    +(40, 1.94E-03)
    +(40, 2.05E-03)
    +(41, 3.35E-03)
    .ENDS
    *

    In which the value 40 is assigned three different values, I have gone ahead and edited this to be: 

    .SUBCKT VCCS_LIM_CLAW+_0 VC+ VC- IOUT+ IOUT-
    G1 IOUT+ IOUT- TABLE {ABS(V(VC+,VC-))} =
    +(0, 1.00E-05)
    +(36, 1.50E-05)
    +(37.5, 2.50E-04)
    +(40, 1.75E-03)
    +(40.1, 1.94E-03)
    +(40.2, 2.05E-03)
    +(41, 3.35E-03)
    .ENDS
    *

    It will take some time until this fix is live on the web, until then please use the attached lib file

    TLV9042_Edit.lib
    This video shows how to import models, remember to configure your simulation profile to the lib file, does not have to be Pspice for TI: training.ti.com/pspice-ti-3rd-party-model-import

    All the best,
    Carolina 

  • 0 in reply to Caro Walter
    Intellectual 345 points

    Hi thanks for your response.

    I've tried the new model but I've faced a convergence issue. To fix it I did this:

    1) cheked the flag edit simulation profile->analysis->SKIPBP

    2) edit simulation profile->options->RELTOL=0.01

    3) edit simulation profile->options->GMIN=1e-10

    the i had to change the model to have a gmin>10e-9 so I've changed:

    * MODEL DEFINITIONS:
    .model BB_SW VSWITCH(Ron=50 Roff=10G Von=700e-3 Voff=0)
    .model ESD_SW VSWITCH(Ron=50 Roff=10G Von=250e-3 Voff=0)

    and

    .MODEL S_VSWITCH_1 VSWITCH (RON=50 ROFF=10G VON=500M VOFF=450M)

    .MODEL S_VSWITCH_2 VSWITCH (RON=50 ROFF=10G VON=500M VOFF=450M)
    .MODEL S_VSWITCH_3 VSWITCH (RON=50 ROFF=10G VON=500M VOFF=450M)
    .MODEL S_VSWITCH_4 VSWITCH (RON=50 ROFF=10G VON=500M VOFF=450M)
    .MODEL S_VSWITCH_5 VSWITCH (RON=10M ROFF=10G VON=10M VOFF=0)
    .MODEL S_VSWITCH_6 VSWITCH (RON=10M ROFF=10G VON=10M VOFF=0)
    .MODEL S_VSWITCH_7 VSWITCH (RON=1M ROFF=10G VON=500M VOFF=100M)
    .MODEL S_VSWITCH_8 VSWITCH (RON=50 ROFF=10G VON=500M VOFF=100M)
    .MODEL S_VSWITCH_9 VSWITCH (RON=50 ROFF=10G VON=500M VOFF=100M)

    Now the model is running fast and stable.

    Thank you and have anice day