TINA/Spice/LMP8481: Missing LMP8481 PSpice model

John, and any interested readers,
The forum did not provide any useful answer to "how to make use of models from the TI WEBENCH as subcircuits in third-party Spice simulators", but Google found this excellent TI Application Report - which is exactly what I was looking for:

www.ti.com/lit/an/sloa070/sloa070.pdf

Cheers,
Bob P.
R. Peruzzi Consulting, Inc.

Bob,

There are a couple of things to note about our Spice-type models, and how they are structured & posted for download.

For signal chain parts - amplifiers & MUX's for example - our default simulators are TINA and Pspice.
If a TINA and/or Pspice model has been posted, either will have a model netlist you can download and use in a third-party simulator.
The models are posted to the device product folders and to the model selector page given in the previous message.

If you are unfamiliar with TINA, it is a free Spice simulator you can download from ti.com/tool/tina-ti .
TINA models are posted in the device product folders as zipped model files and as schematics.
If you have installed TINA on your desktop/laptop, you can open the schematic by clicking on the associated Reference Design link.
Or you can download the schematic file, which has a *.TSC extension.

The TINA model downloads & unzips into three files:
1. *.TSM is the TINA model, which includes the netlist and TINA schematic symbol information.
      You can insert the model into a schematic using the Insert/Macro command in an active TINA session.
2. *.LIB is the stand-alone model netlist, which is what you were looking for. 
     The TINA .LIB file uses Pspice-compatible syntax, so you can usually import the TINA netlist into Pspice, and it will run fine.
     It will often work in other third-party simulators as well.
3. The *.TLD file is used if you want to add the model to TINA's internal library.

You can import model netlists into TINA as well. That is the subject of an app note:
www.ti.com/.../litabsmultiplefilelist.tsp

Our Pspice models are posted as standalone model netlists or entire Pspice projects.
The standalone model netlist files have *.LIB, *.CIR, *.MOD, or *.TXT extensions, and may be posted as zipped or unzipped files. 
Either will work in Pspice, and most will also work in other third-party simulators.
You may have to change the file extension for some simulators to recognize the file.

If the model is part of a zipped Pspice project, it will contain the model netlist file and supporting schematic files.
The model netlist will have a *.LIB extension.
So if a model is posted as a Pspice project, you can download & unzip the project files and extract & use the model netlist in your simulator of choice.

I hope this helps. Please let me know if you have any more questions.

Regards,
John

John,

Thank you very much for your guidance.  I downloaded and used the lmp8481_S.lib file in LTSpice.  I am guessing that Tina Spice has an algorithm that LTSpice does not have,  to deal with stepped analog signals (voltage and current) in its solver.

I checked out the lmp8481_s by ramping up VCC.  As it reaches a threshold, a conditional (IF statement) VCVS attempts to jump from zero volts to some other voltage in zero time.  The solver takes finer and finer time steps until it gives up and fails.  The solution for me was to copy the model into another name and create a new symbol for it with the new name.  In the new .lib file, edit the "E" source and some "G" source lines too.  I sacrificed power supply self-checks for convergence.

In Verilog-AMS I know how to avoid discontinuities using exponential transient functions.  I'm sure a similar approach can be taken in SPICE.  On the other hand, maybe it's not a problem with Tina Spice.

Granted, your models are provided freely, as is, with no guarantees and I'm happy to use them.  Mine is just a suggestion your model designers could use to add value to what you provide.  Even if free, it does carry the TI brand.

Cheers,

Robert Peruzzi.  R. Peruzzi Consulting, Inc.