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.

[FAQ] TINA/Spice: Note about encrypted models and importing models from one simulator to another

Other Parts Discussed in Thread: TINA-TI

Tool/software: TINA-TI or Spice Models

I am using a simulator for which TI does not provide a model. How can I import TI's existing model to my target simulator? 

  • Many "Power" related models provided by Texas Instruments are encrypted and will only run in the simulator in which they are encrypted. For example, a PSpice encrypted model will only run in PSpice 15.7 and up. A TINA-TI encrypted model will only run in TINA-TI (which is a free Spice simulator provided by TI).

    You can not use a model that is encrypted in one simulator in another simulator. If you want to import TI's models from one simulator to another, you will need the unencrypted model. Instructions on how to find out whether a model is encrypted or unencrypted can be found here.


    Importing unencrypted models into TINA-TI: 

    You can refer to either this video or this document, both of which describe the procedure to import unencrypted PSpice models provided by TI into TINA-TI. 

    Importing unencrypted models into HSPICE:

    Please refer to the following post on some guidelines to import unencrypted PSpice/TINA-TI models to HSpice.

    Importing unencrypted models into other tools:

    Spice models developed by TI are targeted for PSpice and TINA-TI simulators. PSpice is available from Cadence and required the purchase of a license from them, whereas TINA-TI is a free spice simulator provided by TI and can be downloaded from

    While TI does not guarantee that its models can be used outside PSpice and TINA-TI, here are some tips to help you import these models into other simulators if you wish to do so.

    Steps to import unencrypted models into other simulators

    1. The 1st step would be to make sure that your target simulator is compatible with PSpice.

    2. TI tries to make its model as generic as possible so that it allows for portability between PSpice compatible simulators. However, even if other simulators claim to be PSpice compatible, please note that they may not be 100% compatible and support all nuances in PSpice.

    3. Things to look out for when importing TIs models into other simulators include syntax incompatibilities and convergence issues. Some common issues while importing are listed below. Note again that these may not be all encompassing, but are a good starting point for debugging when your import does not work.

    Syntax Incompatibilities

    1. Check for the “^” symbol in a logical statement. PSpice considers this an exclusive OR statement, however, other simulators see this as a bitwise OR statement.

    2. In some cases, PSpice will netlist out multiple PARAMS or empty PARAMS in the sub circuit call. An example is shown below. This will be flagged as an error in most simulators except PSpice. Simply remove the extra PARAMS from the statement.

    X_U4_U14         U4_N13787296 V5FILT d_d1 PARAMS:

    3. If an equation is used for raising to a power, use **, not ^. PSpice will accept both, however, other simulators will not accept “^”.

    4. ‘+’ or ‘-’ signs in node names causes a lot of grief in some simulators. The only way to fix this is to replace all the nodes with “_P” or “_M” for plus and minus. This can be dangerous since +/- are used in equations as well.

    5. PSpice encloses all behavioral modeling equations in parenthesis. In some cases, PSpice will netlist multiple parenthesis (duplicates) which is ok in PSpice but not in other simulators. Simply remove the extra parenthesis while making sure not to modify the structure of the behavioral equations.

    E_U9_ABM33         U9_TESTUP 0 VALUE { {IF(V(U9_N15480822) > 0.5,0,0.1m)}    }

    6. Check the syntax for the initial conditions on nodes and components. Make sure it follows the approved syntax in your simulator.

    Convergence Issues

    1. We do not provide the simulation parameters with the unencrypted PSpice models as these are very simulator specific. Many simulator default parameter values can cause convergence errors with power models. Since this is very simulator specific, we are relying on the user to understand their simulator and how it works.

    2. If your circuit fails to converge, please adjust the appropriate simulation parameters in your simulator depending on the type of convergence error.

    3. Also make sure that if you have any initial conditions in the external circuit that these values are given correctly. Incorrect initial condition or contradictory initial conditions can cause convergence issues in simulators.

    4. In many cases when providing an input to the model like VIN, try to ramp up the input from 0V to its final value if possible. Starting with a DC source directly can lead to convergence errors. While some simulators try this automatically based on their algorithms, others may not do so.

    If your import does not work, a safer alternative is to try to run the simulation in TINA-TI. TINA-TI models can be downloaded from the product folder directly or you can search them from Use the keyword “TINA” in the search box. If a TINA-TI model is not available for a product and you have access to the unencrypted model, you can import it into TINA-TI using the instructions listed above in this post. If you do run into issues while importing unencrypted models into TINA-TI, please submit your feedback on this E2E Forum.