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.

  • Resolved

OPA2209: OPA2209

Prodigy 190 points

Replies: 4

Views: 70

Part Number: OPA2209

I was using Tina TI to build a filter circuit using the OPA2209. I used the macro in the Tina library and my circuit was working fine. I was on line and I noticed a new PSpice file for the OPA2209 called OPA209. I downloaded the file and imported the Macro. Now when I analyze my circuit (transient analysis), it has a 1.5vdc offset (not good). So, I my question is, did I do something bad when I imported the file? Also, when I used the Macro, it came up with an error in which the very last line had a ".P" in it. Tina, did not like that apparently, so I made it a comment. After I did that, the macro came to life and I could analyze my circuit.

I did this with several op amps. If I use the one in the library, it works. If I use the PSpice model you provide and import it, I get the error and the offset. What am I doing wrong.

  • Hi Glenn,

    Sorry you ran into a problem with our OPA209 simulation model. The first model that you mention is an older, but well vetted OPA209/OPA2209 simulation model that was released sometime in the 2010 timeframe. It has been included in the TINA-TI op amp selection for a long time and should provide you with accurate filter response. The OPA209 model retrieved from the web page is a newer, 2019 version of the model that provides additional enhancements. Unfortunately, in some cases a few bugs have found their way into some of the revised models.

    I would go ahead and use the OPA2209 model provided with TINA-TI. You should see good simulation results from it. If you want to send me your TINA circuit file that uses the newer OPA209 model version, I can try and replicate the problem your are seeing when you attempt a transient analysis. If I can replicate the problem, I can file a bug report and have it added to the model repair queue.

    Regards, Thomas

    Precision Amplifiers Applications Engineering

  • In reply to Glenn Varnon52:

    HI Glenn,

    Thank you for providing your OPA2209 TINA schematic. That allowed me to run some simulations and gain some perspective into the problem you observed.

    When I take your ground fault filter circuit which had a dc input battery of +300 mV and replace with a dc voltage source that could be swept from 0 V to a higher positive voltage an interesting difference was observed between the original TINA-TI OPA2209 model and the newer website OPA209 models. You can see the results of the sweeps here:

    Observe that in the righthand image the OPA2209 model output begins to change with the dc input level as low as about +175 mV. The output begins to go nonlinear with an input level of +2.3 V. By comparison, the newer webpage OPA209 output doesn't begin to change until the input voltage is +1.5 V and then continues to follow at least to +3.7 V as the graph shows.

    This points out an important issue with your circuit. The OPA209/OPA2209 common-mode input voltage (VCM) range is specified as (V–) + 1.5 to (V+) – 1.5 V. Since you have the V- supply in your circuit set to ground, or 0 V, the minimum VCM is +1.5 V; the same voltage that is received from the newer webpage OPA209 model. Therefore, it appears that the older TINA-TI OPA2209 model is not providing correct common-mode behavior.

    If you are to use the newer OPA209 model and operating it within the correct VCM range, I do expect it would provide your with correct filter response. I ran an ac sweep with a 2.5 V dc source included in series with an ac input source.I obtained the following low-pass amplitude responses with SW-SPST2 opened and closed. I expect the responses are correct for the component values used in the filter.

    Do use the newer webpage OPA209 simulation model for your analysis.

    Regards, Thomas

    Precision Amplifiers Applications Engineering

  • In reply to Thomas Kuehl:

    Thanks.

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.