Wolfspeed Power Applications Forum

Wolfspeed Technical Community:

SpeedFit™ Design Simulator

Simulate and evaluate the performance of SiC-based power circuits and determine the right SiC device in seconds.

Start a Simulation

Categories

LTspice model body diode characteristics differ significantly from datasheet

Options
KiliB
KiliB Contributor Level 1
edited May 12 in Module Products

Hi,

I noticed that the Vds-Ids characteristics in LTspice of the CAB760M12HM3 module differs quite a bit from the datasheet values. The first plot shows the module characteristics using the LTspice model. The break in the body diode curve is not in the model, I just did not collect datapoints below 200A. The second plot uses data from the plecs XML file (which is way closer to the datasheet). Especially the fact that the diode temperature curves are swapped (150°C is above the 25°C) is not possible in reality.

Wolfspeed_Vds-Ids_LTspice_FAIL.png
Wolfspeed_Vds-Ids.png

Not only the body diode behaves very strange in LTspice, also the Rdson seems a little different. Did anyone else observe this behavior?

Thanks

Tagged:

Comments

  • Forum_Moderator
    Forum_Moderator Wolfspeed Employee - Contributor Level 5
    Options

    Thank you for your post, it has been approved and we will respond as soon as possible.

  • BlakeNelson
    BlakeNelson Wolfspeed Employee - Contributor Level 3
    Options

    Hello KiliB,

    I agree, something is definitely strange about that plot! At first I was a bit confused because I had not seen that behavior in the models and I was getting a different result in my testing than you are showing, e.g.

    image.png

    Which came from this simulation:

    {B5C63DC7-6701-4C76-89B8-4B1C92235811}.png

    I also saw similar behavior in a transient simulation:

    {BC519161-4A48-45E0-9E25-DB012AE1DCAD}.png
    image.png


    I was playing around with things and then stumbled into this simulation:

    {79911B9C-2B07-4A2E-A523-1C4B4C180580}.png

    Which at first seems to replicate your simulations behavior:

    image.png

    But upon further inspection I realized, I was seeing a large jump due to my poor choice of x-axis. Upon switching my dc sweep to ".dc oct I1 0.01 1 100", I got the much more reasonable,

    image.png

    So I my best guess at this moment is that we're seeing a simulator issue / setup issue, but I'd be happy to help you with your SPICE simulation directly if you're able to share the file. You are also welcome to start a private message if you would rather not post it publicly.

    Please let me know if this addresses your question!

    Blake

  • KiliB
    KiliB Contributor Level 1
    Options

    Hi Blake,

    thank you for your answer. Unfortunately, I can not see which trace in your plots is which parameter-set without legend. Also, I'm sorry I did not mention that I used the CAB760M12HM3 module-model.

    My setup uses the double pulse test bench you provide as an example and I adapted it for PWM operation. It looks like this:

    image.png

    The diagram was created using a Matlab script, that automatically adjusts the parameters Itest and Temperature . I only added the .step param command for explanation now. Please find the model attached.

    The body diode voltage was then obtained by measuring Vds at time t_off_BD = 674.97e-6 s. Then it looks like this for example:

    image.png

    So still the diode shows a positive temperature coefficient (should be negative) and the Rdson also shows a positive coefficient.

    PWM_HB.asc

  • BlakeNelson
    BlakeNelson Wolfspeed Employee - Contributor Level 3
    Options

    Thanks for following up!

    Looking at my simulations again, I am also getting the inverted temperature dependence of the body diode model. Unfortunately, while I have identified that this problem is not isolated to the CAB760M12HM3 model, I'll need to continue working on it to discover the root cause and resolve it.

    In an ideal world, I will get back to you this week, but in the meantime I wanted to make sure you know that I see the problem and am looking for a solution.

    Blake

    KiliB
  • BlakeNelson
    BlakeNelson Wolfspeed Employee - Contributor Level 3
    Options

    Hi KiliB,

    I have finally tracked down the source of the error (the third quadrant parameters that were creating during the fitting process were getting altered before the model was created, so the the final model was not matching behavior I was expecting) and have generated a new CAB760M12HM3 model:

    image.png

    This issue affects several other models in our library, so I'll be working to publish a fixed version of our library to our website soon. In the meantime I have this set of files with the fixed CAB760M12HM3 model:

    Fixed CAB760 2026-05-08.zip

    If there are any other SPICE models you need immediately, please let me know and I'll get them to you. If you have any feedback or run into any issues with this new model I'd be happy to review them for you.

    Thank you for reaching out and taking the time to explain this issue!
    Blake

  • KiliB
    KiliB Contributor Level 1
    Options

    Hi Blake,

    thank you very much for clarification! The new one seems to work fine in my setup. I also had a look on a bare die model (EM40120-026JS0), but that seems to work fine, at least from the temperature behavior. Would be great if you could leave a short message here, as soon as you have exchanged the whole library :)

    Best Regards,

    Kilian

    BlakeNelson
This discussion has been closed.