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.

TINA/Spice/LMV771: Changing the parameter values in the .lib file of LMV771

Part Number: LMV771
Other Parts Discussed in Thread: TINA-TI, , TLV771

Tool/software: TINA-TI or Spice Models

Hello,

Is it possible to change the offset voltage, V_os and bias current, I_b values in the LMV771.lib file. I tried changing the values and saved the file with a different name. I wanted to simulate this model in Orcad Pspice, when I add the part to the library there, but I think the model is still being taken from LMV771.lib since the subckt model name is still LMV771. I'm not able to change that, could you please help me out with this ?

  • Hi Akshata,

    Please read the below FAQ. Please share the PSPICE project so we can have a look.

    Regards,

    Karthik

  • Hi Akshata,

    The short answer is yes, it's possible to change the VOS and IB values on this model.
    Make sure you change the following lines:
    V_OS 39 40 -97.13U
    I_OS ESDn MID 5P
    I_B 40 MID 10P

    If you change the model into different file name, I would recommend that you create a new symbol from scratch rather than reusing TLV771 symbol to avoid confusion. For instance, you can call your new file name as TLV771NEW and then by going to Model Editor -> Export to Part Library that will create a new symbol called TLV771NEW. This will to ensure that your TLV771NEW is interlinked with TLV771NEW.LIB

    If you don't want any headache in dealing with symbol what I usually do is simply comment out the lines within the TLV771 file such as this:

    *V_OS 39 40 -97.13U
    V_OS 39 40 -500U

    *I_OS ESDn MID 5P
    I_OS ESDn MID 8P

    *I_B 40 MID 10P
    I_B 40 MID 11P

    Hope this helps,
    Herman