• State TI Thinks Resolved
  • Locked Locked
  • Replies 10 replies
  • Answers 3 answers
  • Subscribers 50 subscribers
  • Views 412 views
  • Users 0 members are here
Support feedback
Options
Options
Similar topics

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.

AMC3330: Error when starting simulation in PSpice for TI

Alex U.
Prodigy 25 points
Part Number: AMC3330
Other Parts Discussed in Thread: AMC3302, TINA-TI

Hello Technical Support,

for quite a while I have been looking for a solution to this problem, but I have not found one.
I even checked this forum, but couldn't find an answer, which is why I decided to share the problem here.
It's about the AMC3330 ±1-V input, precision voltage sensing isolated amplifier.
When simulating with PSpice for TI, I get certain error messages every time (see figure).

Error Messages
This figure is from the OrCAD PSpice Simulator window under the "Output Window" pane. U3 is the current label of the AMC3330.
If I simulate the AMC3302 ±50-mV input, precision current sensing isolated amplifier, I do not get these error messages.
I simulated both ICs with LTSpice before, and they also worked, but I had other problems, which is why I switched to PSpice for TI.
The demo project I used to test the AMC3330 can be found at the bottom. I used the circuit example from chapter 9 from the datasheet for this.
I would like to thank you in advance for your support.

Important informations:
PSpice for TI Version:
23.1-2024 S001
Model Library Version:
2024-02-22T07:01:18-06:00
AMC3330 and AMC3302 Version:
9.3.200.277 SF-TI from 04/21/2022
Operating System:
Microsoft Windows 10 Pro

Kind Regards

amc3330_test.zip

  • 0
    TI__Expert 4955 points

    Hi Alex,

    What is U1 in your model? I think either that or the AMC3330 could be your invalid device. I think this error could happen if there is a missed connection. If not though, I will reach out to someone on my team!

    Alternatively, you could consider using the TINA-TI simulation program and AMC33xx model in the meantime.

    Best regards,

    Eva

  • 0 in reply to Eva Mason
    Prodigy 25 points

    Hello Eva,

    thank you for your reply.
    In this model there is no U1 directly, as I have separated this part from a larger main circuit in order to test it more thoroughly. U1 is most likely the component in the PSpice subcircuit AMC3330_Amp_0 from the PSpice model of the AMC3330. I can't say exactly, because I'm not versed in writing PSpice models.

    The migration to TINA-TI is not so easy, because the main circuit consists of much more than just the AMC3330 and AMC3302, but I will give it a try.

    Kind Regards

  • 0 in reply to Alex U.
    TI__Expert 4955 points

    Hi Alex,

    I see, I will check with my team what they advise.

    Best regards,

    Eva

  • 0 in reply to Alex U.
    TI__Expert 4955 points

    Hi Alex,

    My team says the problem is caused by a single '.' character that has been left in the AMC3330.lib file. The error message is found after this '.' line in "bias.out.1" file of your project:

    ------------------------------------------------------------------------------------------------------------------------

    .

    $
    ERROR(ORPSIM-16364): Invalid device in subcircuit

    ------------------------------------------------------------------------------------------------------------------------

    Hope this helps!


    Best regards,

    Eva

  • 0 in reply to Eva Mason
    Prodigy 25 points
    Hello Eva,

    I noticed this sign too, which is why I deleted it, but then the following error messages appeared.
    It was also no longer possible to restart the simulation, which is why a reboot was necessary every time.
    That's why I classed the character as essential.

    I have tried a few things, but the problem remains.

    Kind Regards
  • 0 in reply to Alex U.
    TI__Expert 3400 points

    Hi Alex,

    I'm moving the thread to the PSPICE for TI team.  There may be some issue with the model's compatibility with the 2024 PSPICE version.

  • 0 in reply to Saleh Ahmad
    TI__Genius 16830 points

    Hi Saleh and Eva,

    What line is the extra '.' in the amc3330.lib file?

    It sounds like the model needs to be corrected, and then released. 

    Just deleting the extraneous '.' will result in the libsig file no longer matching the .lib file. Then, all the models appear as imported models, triggering soft landing.

    Regards,

    David

  • 0 in reply to David Larkin
    Prodigy 25 points
    Hello David,

    the character "·" can be found in line 1130, directly below the two lines of code:
    .Param VthH={Vthres+Vhyst}
    .Param VthL={Vthres-Vhyst}
    All these lines are part of the HYSTCOMPG_THLRF subcircuit.

    Kind Regards
  • 0 in reply to Alex U.
    TI__Genius 16830 points

    This behavior has been confirmed by Cadence and they have opened a CCR to look into a solution.

    If this is urgent, I'd suggest updating the model (remove that darned line 1130 character), and release the model again.

    That'll get a new libsig so that PSpice for TI doesn't have issues not recognizing a TI model.

    David

  • 0 in reply to David Larkin
    TI__Genius 16830 points

    Cadence has an answer. The newest version recognizes accented characters which were previously ignored.

    This points to the solution, which is to revise the model to remove that special character. Unintended consequences of expanding capability.

    David