• State Resolved
  • Locked Locked
  • Replies 3 replies
  • Subscribers 38 subscribers
  • Views 455 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.

Floating Point Overflow Error during Transient Simulation on a TDK LAN Transformer SPICE model

Satish Acharya
Prodigy 230 points
Other Parts Discussed in Thread: TINA-TI

Hi,

I created a simple transformer circuit in TINA-TI using the spice model downloaded from TDK website ALT4532M-201-T001 : Detailed Information | Transformers - Pulse Transformers and Modules for LAN | TDK Product Center. Attached is the circuit schematics from TINA-TI. The same link also has a .pdf file describing the circuit used for the spice model.

AC Transfer Characteristics seems to run fine along with some of the other analyses. However, transient simulation terminates with a Floating Point Overflow Error right at the start. Can someone please help to identify if this is due to an error in the SPICE model, or an issue with TINA simulator or if I need to change some TINA simulation parameter settings for it to run successfully?

I can run transient simulation fine of much more elaborate circuits using TI opamp models on TINA-TI. I think I am using the latest version of the simulator: Version 9.3.200.277 SF-TI

Thanks,

TDK_LAN_Xfrmr_0.TSC

Satish

  • +1
    TI__Guru 71526 points

    Hello Satish,   

    Thank you for your inquiry about TINA-TI.  Since TINA-TI is a DesignSoft/TINA program, questions are handled by using the DesignSoft support page: http://www.tina.com/technical-support/  . 

    The DesignSoft/TINA team is very helpful and this is the most direct way for TINA support.  Please advise by Reply to this case when the issue has been resolved.    

    Regards, 

    ~Leonard  

  • 0 in reply to LeonardEllis
    Prodigy 230 points

    The response I got from DesignSoft is below. TI does not offer version 12 yet. So, I need to find a solution myself.

    It's some kind of numerical instability in Tina-TI when you run this particular model. I tried to find a modified parameter set but without success. My only suggestion is upgrading to Tina 12 In Tina 12 this circuit is running nicely.

    Regards
    Tibor Horvath
  • 0 in reply to Satish Acharya
    Prodigy 230 points

    Just for the benefit of others....

    So, I removed all the surrounding caps, resistors and inductors from the transformer model and kept only the 4 core inductors and their mutual inductances. Yet, the simulation failed.

    With more experiments, it turns out there is some issue with modelling of transformer (center tap on both sides) that TINA simulator cannot handle. One can replicate the issue with just the 4 inductors.

    Following fails with floating point error:

    K112 L111 L112 9.99740000E-01
    K113 L111 L113 9.99740000E-01
    K114 L111 L114 9.99840000E-01
    K123 L112 L113 9.99840000E-01
    K124 L112 L114 9.99740000E-01
    K134 L113 L114 9.99740000E-01

    L111 12 51 9.10000000E-05
    L112 22 61 9.10000000E-05
    L113 51 32 9.10000000E-05
    L114 61 42 9.10000000E-05

    while the following works fine with loss of some modelling accuracy in mutual inductance (only difference  between the two is specification of identical mutual inductance for all inductors in a single line)

    K112 L111 L112 L113 L114 9.99740000E-01

    L111 12 51 9.10000000E-05
    L112 22 61 9.10000000E-05
    L113 51 32 9.10000000E-05
    L114 61 42 9.10000000E-05

    I do not understand the rationale and I'm not fluent in spice syntax or simulator internals but the change seems to work for me.

    Regards,

    Satish