1. Welcome to our site! Electro Tech is an online community (with over 170,000 members) who enjoy talking about and building electronic circuits, projects and gadgets. To participate you need to register. Registration is free. Click here to register now.
    Dismiss Notice

Can LTSpice use pspice models

Discussion in 'Circuit Simulation & PCB Design' started by PickyBiker, Nov 6, 2017.

  1. PickyBiker

    PickyBiker New Member

    Joined:
    Nov 1, 2017
    Messages:
    9
    Likes:
    0
    I'm new to LTSpice and have trouble understanding how to import 3rd party simulation models. I saw some online comments that say you can use Pspice models, but no clear instructions on how to use them in LTSpice.

    If I could get help with this example, I would probably understand how to import others.
    Using Windows 10
    LTSpice XVII
    Part of interest Infineon IPP080N06
    Downloaded the PSpice simulation file for this part
    The folder is 01_OptiMOS and it contains several files, the .lib file is OptiMOS_60V.lib

    So now what needs to happen?
     
  2. MikeMl

    MikeMl Well-Known Member Most Helpful Member

    Joined:
    Mar 17, 2009
    Messages:
    11,099
    Likes:
    562
    Location:
    AZ 86334
    Post your .lib file, and I will show you how to incorporated it into a running sim...
     
  3. PickyBiker

    PickyBiker New Member

    Joined:
    Nov 1, 2017
    Messages:
    9
    Likes:
    0
    Here is the .lib file. I added .txt to get it to upload.
     

    Attached Files:

  4. dave

    Dave New Member

    Joined:
    Jan 12, 1997
    Messages:
    -
    Likes:
    0


     
  5. MikeMl

    MikeMl Well-Known Member Most Helpful Member

    Joined:
    Mar 17, 2009
    Messages:
    11,099
    Likes:
    562
    Location:
    AZ 86334

    This is not going to be easy. Optimos uses a non-standard five pin symbol for its devices (instead of three, like everybody else), where in addition to the standard three "drain, gate, source" pins, they add two "non-physical" pins to send in Tj (junction temperature) and Tcase (case temp). You will have to create a new symbol for LTSpice with five pins.

    I have no idea how they "communicate" with those extra pins???
     
  6. PickyBiker

    PickyBiker New Member

    Joined:
    Nov 1, 2017
    Messages:
    9
    Likes:
    0
    Not sure I understand the problem.
    This chip uses 3 pins in a standard T0220 package.
    Manufacturer Part#:
    IPP080N06
    Product Category: FETs - Single
    Manufacturer: INFINEON
    Description: MOSFET N-CH 60V 80A TO-220
     
  7. eTech

    eTech Active Member

    Joined:
    Apr 25, 2012
    Messages:
    567
    Likes:
    49

    Attached is symbol per AN2014-02 and a test circuit for LTspice.
    The Tj terminal is an output used to monitor Junction temperature.
    The Tcase terminal is an input and models ambient temperature (1V=1C).
    See Infineon application note "Application Note AN 2014-02".

    eT
     

    Attached Files:

    • Like Like x 1
  8. PickyBiker

    PickyBiker New Member

    Joined:
    Nov 1, 2017
    Messages:
    9
    Likes:
    0
    Okay eTech, I see that you have the part and symbol working in LTSpice. But I do not see how you got from A to B (where A is where I am and B is where you are).

    Here is what I did to try to create an LTSpice schematic using the same part:
    created a new folder called My Test
    created the My Test schematic and named the mosfet IPB080N06N
    inserted the op command: .inc OptiMOS_60V.lib.txt
    copied the files OptiMOS_60V.lib.txt and nmos_Infineon.asy into that folder​

    When I run it, the error message says "m1: Can't find the definition of model "ipb080n06n"".

    What else do I need to do to make this work and where did nmos_Infineon.asy come from?


    Here is the My Test folder folder:
    https://www.dropbox.com/s/amm892lsvfxgcgb/My Test.zip?dl=0
     
    Last edited: Nov 7, 2017
  9. eTech

    eTech Active Member

    Joined:
    Apr 25, 2012
    Messages:
    567
    Likes:
    49

    Good.

    Don't use the native mosfet symbol.
    Copy the symbol and .txt file I gave you into the folder. Then use the component selector to browse to the folder and select the symbol.
    Rht-clk the symbol and set the property "value" to IPB080N06N

    If placed on the schematic...Good
    I usually place the directive on the schematic then rht-clk and browse to the file.
    This way I'm sure LTspice will find it.

    Bad. correct action, wrong timing :)

    Follow the above comments. Then it should work.

    eT
     
    • Like Like x 1
  10. PickyBiker

    PickyBiker New Member

    Joined:
    Nov 1, 2017
    Messages:
    9
    Likes:
    0
    eTech......... BINGO, it works! Thankk you.

    One last question, I know where the .lib.txt file came from but where did the nmos_Infineon.asy come from?

    In any case, thanks so much for the help. It is appreciated.
     
  11. eTech

    eTech Active Member

    Joined:
    Apr 25, 2012
    Messages:
    567
    Likes:
    49
    I made a custom LTspice symbol based on the Infineon App note AN 2014-02.
     
    • Like Like x 1
  12. PickyBiker

    PickyBiker New Member

    Joined:
    Nov 1, 2017
    Messages:
    9
    Likes:
    0
    Okay, thank you. I'll read up on that App note.
     
  13. eTech

    eTech Active Member

    Joined:
    Apr 25, 2012
    Messages:
    567
    Likes:
    49
    Just to clarify how I made the symbol:

    1. Place the native nmos symbol on the schematic.
    2. ctrl-rht-clk the nmos symbol then click the "open symbol" button.
    3. Select "File->Save As" from the menu bar, browse to the new folder, TYPE A NEW SYMBOL FILE NAME, then click "Save".
    4. The symbol is now saved with the new symbol file name in the new folder and is currently being edited.
    5. Finish modifying the symbol as desired.

    Note - Be aware that it is important not to use a symbol name that is already a file name used for a native symbol.
    The native symbol will override the new symbol.

    Hope that helps...

    eT
     
    • Like Like x 1
  14. PickyBiker

    PickyBiker New Member

    Joined:
    Nov 1, 2017
    Messages:
    9
    Likes:
    0
    It indefinably does help.

    You have made the confusing problem I had understandable. Thank you again.
     

Share This Page