Tina Ti model for Log112

Hello Murali,

I spent much time converting and testing the LOG112 simulation model from the PSpice version listed on the web-page to a TINA-TI Spice version. Oddly, I had found a already existing LOG112 symbol in the TINA symbol library, but no corresponding model. That is usually not a good sign. Once I had the TINA version running I found that the simulation model did not produce correct output results. I suspect one the DesignSoft folks, the TINA-TI developers, originally tested the LOG112 model and found the same problem. They would have had to build a symbol to test the model, but wouldn't have included a broken model in the library. Thus, I suspect that the PSpice model listed on the web-page may be faulty as well because it and a TINA version can use the same PSpice model file.

Fixing the model usually isn't a quick project because the models are very involved and finding the problem can take much time. Is their any possibility you can use the LOG114 simulation model in your circuit? That model was built a few years ago and I know that it simulates well and is accurate. The LOG114 is quite similar to the LOG112, but with more versatility.

Regards, Thomas

PA - Linear Applications Engineering

Hello Thomas,

Thank you for trying it and replying immediately. I'll try the simulation with LOG114. 

Regards,

Murali

Thomas,

I am currently using NI's Multisim Education Edition Version 10.1.1 (10.1.372) to simulate the LOG112. I downloaded the model from your website and created a component, with schematic and PCB representations, and it seems to work as advertised in my simple test circuits, but each time I run the simulation, it gives me this error:

------ Checking SPICE netlist for Probe_B_and_Band - 2012-05-25 09:05:50 ------
SPICE Netlist Warning in schematic RefDes 'u22', element 'ql112':  Duplicate parameter 'itf' found, overwriting old value with '10e-3'
======= SPICE Netlist check completed, 0 error(s), 1 warning(s) =======

I have no experience building SPICE models, but it appears to be from a section of code where the variable ITF is defined twice, first as ITF=0.01 and then in the next line as ITF=10E-3. Is this an error, or part of how the model works?

Thank you,

Henry Wroblewski

University of Iowa Physics Department

Hello Henry,

Yes, I see the issue you are mentioning; for the LOG112 logging transistor (QL112) two values are being assigned to the ITF parameter; first 0.01, and then 0.001. Only one value should be assigned and that is being detected by your MultiSim simulator resulting in the warning message. Then, MultiSim simply overwrites the first value with the second value and it is able to proceed using the second value.

This appears to be an error in the model, but not a fatal error. ITF is the bipolar transistor base transit time parameter. It is used in the transit time capacitance calculation. The value of parameters such as ITF were established by the original model builder and I don't know which setting is correct. When I review the forward transient time (tF) equation ITF is a minor factor. I suspect the effect of ITF being one value, or the other, has miniml affect on the LOG112 electrical behaviors.

You probably have the ability in MultiSim to edit the Spice syntax. I would simply set ITF to one value, remove the other ITF setting, and compare the simulation results. I believe the simulation differences will be quite small, but if you do find the results are noticeably different it may justify reworking the model.

Regards, Thomas

PA - Linear Applications Engineering